User’s Manual CNC Pilot 4290 NC Software 625 952-xx V7.
Data input keypad Machine operating panel Manual control operating mode Cycle start Automatic operating mode Cycle stop Programming modes (DIN PLUS, simulation, TURN PLUS) Feed rate stop Organization modes (parameter, service, transfer) Spindle STOP Display error status Spindle on - M3/M4 direction Call the info system Spindle jog - M3/M4 direction (The spindle turns until you press the key.
Data input keypad Page up, Page down (PgUp/PgDn) Change to previous/next screen page Change to previous/next screen dialog box Switches between input windows Enter – Confirmation of input 4 Machine operating panel Touchpad with right and left mouse key
CNC PILOT 4290, Software and Functions This manual describes functions that are available in the CNC PILOT 4290 with NC software number 625 (Release 7.1). For programming the B and Y axes, please refer to the User's Manual “CNC PILOT 4290 with B and Y Axes”. It is not described in this manual. The machine manufacturer adapts the features offered by the control to the capabilities of the specific lathe by setting machine parameters.
Contents 1 2 3 4 5 6 7 8 9 10 11 Introduction and Fundamentals Basics of Operation Manual Control and Automatic Modes ISO Programming Graphic Simulation TURN PLUS Parameters Operating Resources Service and Diagnosis Transfer Tables and Overviews HEIDENHAIN CNC PILOT 4290 7
1 Introduction and Fundamentals ..... 29 1.1 The CNC PILOT ..... 30 Programming ..... 30 The C axis ..... 31 The Y axis ..... 32 Full-surface machining ..... 33 The B axis ..... 34 1.2 The Modes of Operation ..... 35 1.3 Expansion Stages (Options) ..... 37 1.4 Fundamentals ..... 39 Position encoders and reference marks ..... 39 Axis designations and coordinate system ..... 40 Machine reference points ..... 40 Absolute and incremental workpiece positions ..... 41 Units of measure ..... 42 1.
3.2 Manual Control Mode ..... 61 Entering the machine data ..... 62 M commands in Manual Control mode ..... 63 Manual turning operations ..... 64 Handwheel ..... 65 Spindle and manual direction keys ..... 65 Slide/spindle change key ..... 66 3.3 Table for Tools and Chucking Equipment ..... 67 Setting up a tool list ..... 68 Comparing a tool list with an NC program ..... 70 Transferring the tool list from an NC program ..... 71 Simple tools ..... 71 Tool life management .....
4 DIN Programming ..... 107 4.1 DIN Programming ..... 108 Introduction ..... 108 DIN PLUS screen ..... 109 Linear and rotary axes ..... 110 Units of measurement ..... 111 Elements of a DIN program ..... 111 4.2 Programming Notes ..... 113 Configuring the DIN editor ..... 113 Parallel editing ..... 114 Selecting submenus, positioning the cursor ..... 114 Making, editing and deleting NC blocks ..... 115 Search functions ..... 116 Conversational or free editing ..... 117 Geometry and machining commands .....
4.4 Program Section Code ..... 135 PROGRAM HEAD section ..... 136 TURRET section ..... 137 CHUCKING EQUIPMENT section ..... 142 CONTOUR section ..... 143 BLANK section ..... 143 FINISHED PART section ..... 143 AUXILIARY CONTOUR section ..... 144 FRONT section ..... 144 REAR SIDE section ..... 144 SURFACE section ..... 144 MACHINING section ..... 144 END code ..... 144 ZUORDNUNG [ASSIGNMENT] instruction $.. ..... 144 SUBPROGRAM section ..... 145 RETURN code ..... 145 CONST code ..... 145 4.
4.10 Front and Rear Face Contours ..... 172 Starting point of front/rear face contour G100-Geo ..... 172 Line segment in front/rear face contour G101-Geo ..... 172 Circular arc in front/rear face contour G102/G103-Geo ..... 173 Bore hole on front/rear face G300-Geo ..... 174 Linear slot on front/rear face G301-Geo ..... 175 Circular slot on front/rear face G302/G303-Geo ..... 175 Full circle on front/rear face G304-Geo ..... 176 Rectangle on front/rear face G305-Geo .....
4.15 Tool-Tip and Cutter Radius Compensation ..... 196 G40: Switch off TRC/MCRC ..... 197 G41/G42: Switch on TRC/MCRC ..... 197 4.16 Zero Point Shifts ..... 198 Zero point shift G51 ..... 199 Parameter-dependent zero offset G53, G54, G55 ..... 199 Additive zero point shift G56 ..... 200 Absolute zero point shift G59 ..... 201 Mirror/shift contour G121 ..... 202 4.17 Oversizes ..... 204 Switch off oversize G50 ..... 204 Axis-parallel oversize G57 ..... 204 Contour-parallel oversize (equidistant) G58 .....
4.22 Thread Cycles ..... 239 Thread switch G933 ..... 239 Thread cycle G31 ..... 240 Simple thread cycle G32 ..... 242 Thread single path G33 ..... 244 4.23 Drilling Cycles ..... 246 Drilling cycle G71 ..... 246 Boring, countersinking G72 ..... 248 Tapping G73 ..... 249 Tapping G36 ..... 250 Deep-hole drilling G74 ..... 251 4.24 C-Axis Commands ..... 253 No. of C axis G119 ..... 253 Reference diameter G120 ..... 253 Zero point shift, C axis G152 ..... 254 Standardize C axis G153 ..... 254 4.
4.28 Assignment, Synchronization, Workpiece Transfer ..... 282 Converting and mirroring G30 ..... 282 Spindle with workpiece G98 ..... 283 Workpiece group G99 ..... 284 One-sided synchronization G62 ..... 284 Synchronization marking G162 ..... 285 Synchronous start of slides G63 ..... 285 M97 Synchronous function ..... 286 Spindle synchronization G720 ..... 286 C-angle offset G905 ..... 287 Measuring angular offset during spindle synchronization G906 ..... 288 Traversing to a fixed stop G916 .....
4.32 Other G Functions ..... 302 Period of dwell G4 ..... 302 Precision stop G7 ..... 302 Precision stop off G8 ..... 302 Precision stop G9 ..... 302 Move rotary axis G15 ..... 303 Switch off protection zone G60 ..... 303 Chucking equipment in simulation G65 ..... 304 Component position G66 ..... 305 Waiting for time G204 ..... 305 Update nominal values G717 ..... 305 Move lag error G718 ..... 306 Actual values in variables G901 ..... 306 Zero-point shift in variables G902 .....
4.35 Conditional Block Run ..... 322 Program branching IF..THEN..ELSE..ENDIF ..... 322 WHILE..ENDWHILE program repeat ..... 323 SWITCH..CASE—program branching ..... 324 Skip level /.. ..... 326 Slide code $.. ..... 326 4.36 Subprograms ..... 327 Subprogram call: L"xx" V1 ..... 327 Dialog texts in subprogram call ..... 328 Help graphics for subprogram calls ..... 329 4.37 M Commands ..... 330 M commands for program-run control ..... 330 Machine commands ..... 331 4.38 Lathes with Multiple Slides .....
5 Graphic Simulation ..... 361 5.1 Simulation Mode of Operation ..... 362 Screen layout, soft keys ..... 363 Graphic elements ..... 364 Displays ..... 364 Zero point shifts ..... 366 Path display ..... 367 Simulation window ..... 368 Setting the simulation window ..... 369 Configuring the simulation ..... 370 Adjusting the section (zoom function) ..... 371 Errors and warnings ..... 372 How to activate the simulation function ..... 372 Simulation mode ..... 373 5.2 Contour Simulation .....
6 TURN PLUS ..... 389 6.1 TURN PLUS Mode of Operation ..... 390 TURN PLUS concept ..... 390 TURN PLUS files ..... 391 TURN PLUS program management ..... 391 Operating notes ..... 392 6.2 Program Head ..... 393 Generating programs for automatic lathes ..... 394 6.3 Workpiece Description ..... 396 Entering the workpiece blank contour ..... 396 Entering the finished part contour ..... 397 Superimposing form elements ..... 398 Integrating overlay elements ..... 399 Entering contours machined with the C axis ...
6.8 C-Axis Contours ..... 421 Position of a front or rear face contour ..... 421 Position of a lateral surface contour ..... 421 Milling depth ..... 421 Entering the C-axis contour dimensions ..... 422 Front or rear face: Starting point ..... 422 Front or rear face: Linear element ..... 423 Front or rear face: Circular element ..... 424 Front or rear face: Single hole ..... 426 Front or rear face: Circle (full circle) ..... 428 Front or rear face: Rectangle ..... 429 Front or rear face: Polygon .....
6.11 Manipulating Contours ..... 461 Editing the contours of a blank part ..... 461 Deleting contour elements ..... 462 Editing contour elements or form elements ..... 462 Adding a contour or contour element ..... 463 Closing the contour ..... 464 Resolving a contour ..... 464 Trimming – Linear element ..... 465 Trimming – Length of contour ..... 466 Trimming – Radius of arc ..... 466 Trimming – Diameter of linear element ..... 467 Transformations – Fundamentals ..... 467 Transformations – Shifting .....
6.13 Preparing a Machining Process ..... 482 Preparing a machining process – Fundamentals ..... 482 Chucking a workpiece at the spindle ..... 483 Chucking a workpiece at the tailstock ..... 483 Defining the cutting limit ..... 484 Deleting the chucking data ..... 484 Rechuck – Standard machining ..... 485 Rechuck – 1st setup after 2nd setup ..... 486 Parameters for two-jaw, three-jaw or four-jaw chucks ..... 488 Collet chuck parameters ..... 489 Parameters for face drivers (“without chuck”) .....
6.14 Interactive Working Plan Generation (IWG) ..... 494 Working plan exists ..... 495 Generating a work block ..... 496 Calling a tool ..... 497 Cutting data ..... 497 Cycle specification ..... 498 Overview of roughing operations ..... 499 Roughing longitudinal (G810) ..... 500 Roughing transverse (G820) ..... 501 Roughing contour-parallel (G830) ..... 502 Residual roughing – longitudinal ..... 503 Residual roughing – transverse ..... 504 Residual roughing – contour-parallel .....
6.17 Configuring TURN PLUS ..... 549 General settings ..... 549 Configuring windows (views) ..... 550 Configuring the control graphics ..... 550 Setting the coordinate system ..... 551 6.18 Machining Information ..... 552 Tool selection, turret assignment ..... 552 Contour recessing, recess turning ..... 553 Drilling ..... 553 Cutting data, coolant ..... 553 Hollowing ..... 554 Inside contours ..... 555 Drilling ..... 556 Shaft machining ..... 557 Multi-slide machines ..... 559 Full-surface machining .....
7.6 Machining Parameters ..... 585 1 – Global parameters for finished parts ..... 585 2 – Global technology parameters ..... 586 3 – Centric predrilling ..... 588 4 – Roughing ..... 591 5 – Finishing ..... 594 6 – Recessing and contour recessing ..... 597 7 – Thread cutting ..... 599 8 – Measuring ..... 600 9 – Drilling ..... 600 10 – Milling ..... 602 Load monitoring ..... 603 20 – Direction of rotation for rear-side machining ..... 604 21 – Name of the subroutines .....
9 Service and Diagnosis ..... 645 9.1 The Service Mode of Operation ..... 646 9.2 Service Functions ..... 647 Access authorization ..... 647 System service ..... 648 Fixed-word lists ..... 649 9.3 Maintenance System ..... 650 Maintenance dates and intervals ..... 651 Displaying maintenance actions ..... 652 9.4 Diagnosis ..... 655 Information and display ..... 655 Log files and network settings ..... 656 Software update ..... 657 10 Transfer ..... 659 10.1 The Transfer Mode of Operation .....
11 Tables and Overviews ..... 683 11.1 Undercut and Thread Parameters ..... 684 Undercut DIN 76, Parameters ..... 684 Undercut DIN 509 E, Parameters ..... 686 Undercut DIN 509 F, Parameters ..... 686 Thread Parameters ..... 687 Thread pitch ..... 688 11.2 Pin Layouts and Connecting Cables for the Data Interfaces ..... 694 RS-232-C/V.24 interface for HEIDENHAIN devices ..... 694 Non-HEIDENHAIN devices ..... 695 RS-422/V.11 interface ..... 696 Ethernet interface RJ45 socket ..... 696 11.
Introduction and Fundamentals HEIDENHAIN CNC PILOT 4290 29
1.1 The CNC PILOT 1.1 The CNC PILOT The CNC PILOT is a contouring control designed for complex lathes and turning centers. In addition to turning operations, the control can also perform milling, drilling and boring operations. The C, Y and B axes enable you to drill and mill on the front and rear faces, the lateral surface and oblique planes. And as always, the CNC PILOT supports full-surface machining with dual-spindles.
1.1 The CNC PILOT The graphic simulation feature enables you to subject your NC programs to a realistic test. The CNC PILOT displays the machining of up to four workpieces in the working space. The simulation shows workpiece blanks and finished parts, chucking equipment and tools to scale. When working with the tilted B axis, the working plane is also shown tilted. This enables you to see, without distortion, the holes and milling contours to be machined.
1.1 The CNC PILOT The Y axis With a Y axis you can drill and mill a workpiece on its front, back and lateral surfaces. During use of the Y-axis, two axes interpolate linearly or circularly in the given working plane, while the third axis interpolates linearly. This enables you to machine slots or pockets, for example, with plane floors and perpendicular edges. By defining the spindle angle, you can determine the position of the milling contour on the workpiece.
1.1 The CNC PILOT Full-surface machining Functions like angle-synchronous part transfer with rotating spindle, traversing to a stop, controlled parting, and coordinate transformation ensures efficient machining as well as simple programming of fullsurface machining. The functions for full-surface machining are available in: DIN PLUS TURN PLUS contour definition TURN PLUS working plan generation The CNC PILOT supports full-surface machining for all common machine designs.
1.1 The CNC PILOT The B axis The B axis makes it possible to drill, bore and mill in oblique planes. To make programming easy, the coordinate system is tilted in such a way that you can define the drilling patterns and milling contours in the YZ plane. The actual drilling or milling operation is then performed in the tilted plane. During work on the tilted plane, the tool is perpendicular to the plane. The tilting angle of the B axis and the angle of the tilted plane are identical.
1.2 The Modes of Operation 1.2 The Modes of Operation Operating modes Manual mode: In the Manual Control mode you set up the machine and move the axes manually. Automatic mode: NC in Automatic mode, NC programs are executed from start to end. You control and monitor the machining of the workpieces. DIN PLUS programming mode: You write the structured NC programs in DIN PLUS. First you define the geometry of the blank and finished part, and then program the machining of the workpiece.
1.2 The Modes of Operation Operating modes Service organization mode: In Service you log in for password-protected functions, select the conversational language and make system settings. This operating mode also provides diagnostic functions for commissioning and checking the system. Transfer organization mode: In Transfer, you exchange data with other systems, organize your programs and back-up your data. The actual control is not accessible to the machinist.
1.3 Expansion Stages (Options) 1.3 Expansion Stages (Options) The machine manufacturer configures the CNC PILOT according to the capabilities of the specific lathe.
1.
1.4 Fundamentals 1.4 Fundamentals Position encoders and reference marks The machine axes are equipped with position encoders that register the positions of the slide or tool. When a machine axis moves, the corresponding position encoder generates an electrical signal. The control evaluates this signal and calculates the precise actual position of the machine axis. XMP If there is a power interruption, the calculated position will no longer correspond to the actual position of the machine slide.
1.4 Fundamentals Axis designations and coordinate system Coordinate system The meanings of the coordinates X, Y, Z, B, C are specified in DIN 66 217. +Y The coordinates entered for the principle axes X and Z are referenced to the workpiece zero point. The angular data for the rotary axes B and C are given with respect to the zero point of the respective rotary axis. +X +B On lathes, C axis movements are realized by turning the workpiece and B axis movements by tilting the tool (swivel head).
1.4 Fundamentals Absolute and incremental workpiece positions If the coordinates of a position are referenced to the workpiece zero point, they are referred to as absolute coordinates. Each position on a workpiece is clearly defined by its absolute coordinates. Incremental coordinates: Incremental coordinates are given with respect to the last programmed position. They specify the distance from the last active position and the subsequent position.
1.4 Fundamentals Units of measure You can program the CNC PILOT either in the metric or inch system. The units of measurement listed in the table below apply to all inputs and displays.
1.5 Tool Dimensions 1.5 Tool Dimensions The CNC PILOT requires information on the specific tools for a variety of tasks, such as calculating the cutting radius compensation or the proportioning of cuts. Tool dimensions:All position values that are programmed and displayed are referenced to the distance between the tool tip and workpiece zero point.
1.
Basics of Operation HEIDENHAIN CNC PILOT 4290 45
2.1 User Interface 2.1 User Interface Screen displays 1 Operating mode bar: Shows the status of the operating modes. The active mode is shown with a dark-gray background. Programming and organization operating modes: The selected mode of operation is shown at right next to the symbol. Additional information such as the selected program, submode, etc. are shown below the operating mode symbol. 2 Menu bar and pull-down menu enable you to select functions.
2.1 User Interface Controls and displays Operating elements of the CNC PILOT: Screen with Horizontal and vertical soft keys: The meaning is shown above or next to the soft keys. Auxiliary key 1: Acts as the Esc key Auxiliary key 2: Acts as the Insert key Auxiliary keys 3: PLC keys Keyboard with Alphabetic keyboard with integrated numeric keypad Keys for operating mode selection Touchpad: For cursor positioning (menu or soft key selection, selection from lists, selecting edit boxes, etc.
2.1 User Interface Selecting the operating mode Keys for operating mode selection Manual control operating mode Automatic operating mode Programming modes Organization modes You can usually switch operating mode at any times. In some situations, you cannot switch operating modes when a dialog box is open. In this case, close the dialog box before changing operating modes. After the change, the new mode starts in the function in which it was last exited.
2.1 User Interface When you press the OK button, the control accepts the data entered or edited. As an alternative you can press the Ins key to confirm the data, regardless of the cursor position. If you leave the input window by pressing the “Cancel” button or the ESC key, entries or changes will be lost. If the dialog consists of more than one input window, you already confirm the data when pressing the PgUp/PgDn key. Note: Instead of selecting the OK or Cancel button, you can press the Ins or Esc key.
2.2 Info and Error System 2.2 Info and Error System The info system The info system calls excerpts from the User's Manual to the screen. The header shows the selected topic. You'll usually find information on the current operating situation (context-sensitive help). if no context-sensitive help is available for a specific situation look for the topics in the following sources: The table of contents The subject index The search functions Cross references are marked in the text.
2.2 Info and Error System Navigating in the info system: U You navigate by touchpad as is usual in Windows programs. If the topic of information exceeds the window size: U Navigate with the up/down cursor keys and PgUp/ PgDn keys through the displayed topic. Prerequisite: The cursor must be located in the topic window and not in the Content/Index window. Moving the cursor: U Press the soft keys. The cursor switches between the topic window and the Content/Index window.
2.2 Info and Error System Context-sensitive help You'll usually find information on the current operating situation (context-sensitive help). if no context-sensitive help is available for a specific situation look for the topics in the following sources: The table of contents The subject index The search functions Direct error messages The CNC PILOT uses a direct error message whenever immediate error correction is possible. Confirm the message and correct the error.
2.2 Info and Error System Error display If during the system start or program run or other operation an error occurs, it is indicated in the date box, displayed in the status line, and saved in the error display. The date and time remain highlighted in red until all of the errors have been canceled. Information of the error message: Error description: Explains the error Error number: For service questions Channel number: Slide for which the error occurred.
2.2 Info and Error System Additional information on error messages When an error message occurs, press the info key, or place the cursor on the error message in the error display and then press the info key, to get further information on the respective error. Meaning of the soft keys: U Information on the next error message. U Information on the previous error message.
2.3 Data Backup 2.3 Data Backup The CNC PILOT stores NC programs, operating-resource data and parameters on the hard disk. Since the possibility of damage to the hard disk due to excessive vibration or shock cannot be eliminated, HEIDENHAIN recommends making regular backup copies of your programs, operating resource data and parameters on a PC or on USB memory media. You can use DataPilot 4290, the WINDOWS “Explorer” or other suitable programs for backing up your data on a PC.
2.4 Explanation of Terms 2.4 Explanation of Terms MP: With machine parameters (MP) the control is interfaced to the machine, settings are made, etc. Cursor: In lists, or during data input, a list item, an input field or a character is highlighted. This “highlight” is called a cursor. Cursor keys: You can move the cursor with the arrow keys, PgUp, PgDn of the touchpad.
Manual Control and Automatic Modes HEIDENHAIN CNC PILOT 4290 57
3.1 Switch-On, Switch-Off, Reference Run 3.1 Switch-On, Switch-Off, Reference Run Switch-on In the header, the CNC PILOT displays the individual steps of the system start and then prompts you to select an operating mode. Whether the reference run is necessary depends on the encoders installed: EnDat encoder: Reference run is not necessary. Distance-coded encoders: The position of the axes is ascertained after a short reference run. Standard encoder: The axes move to known, machine-based points.
3.1 Switch-On, Switch-Off, Reference Run Reference jog for single axis Select Ref > Reference jog. The “Status of reference run approach” dialog box informs you of the current status. Set slides and axes (“Reference jog” dialog box) The reference run is conducted for as long as the Cycle Start key stays pressed. To interrupt the reference run, release the key. “Cycle stop” interrupts the reference run.
3.1 Switch-On, Switch-Off, Reference Run Switch-off “Shutdown” is available in the programming and organization modes if no operating mode is selected. U Press the soft key to switch off the CNC PILOT. U Confirm the security query with OK. After a few seconds, the CNC PILOT requests you to switch off the machine. Proper switch-off is recorded in the error log file.
3.2 Manual Control Mode 3.2 Manual Control Mode The Manual Control mode offers various functions for setting up the machine, for measuring tool dimensions and for manually machining workpieces. Options of operation: Manual mode: With the “machine keys” and the handwheel, you can control the spindle and move the axes to machine the workpiece. Setup mode: Here you enter the tools to be used, set the workpiece datum, the workpiece change point, the protection zone dimensions etc.
3.2 Manual Control Mode Entering the machine data Setting the feed rate In the menu group F you define a feed rate per revolution or per minute. Setting the feed per revolution: U U Select F > Feed per revolution Enter the feed rate in mm/rev (or inches/rev) Setting the feed rate per minute: U U Select F > Feed per minute Enter the feed rate in mm/min (or inches/min) and press OK.
3.2 Manual Control Mode Insert the nominal tool U Select T. Enter the turret position, or U the next turret position, or U the previous turret position, or Functions of the tool change: Move the tool into position Calculate “new” tool dimensions Display “new” actual values in the position display M commands in Manual Control mode In the menu group M you either type in the M function to be run or you select the desired function from the menu.
3.2 Manual Control Mode Manual turning operations The “manual” menu group includes G functions, simple longitudinal and transverse turning, and manual NC programs written by the machine tool builder. Simple longitudinal and transverse turning operations: U U U Select Manual > Constant feed Select the direction of feed (“Constant feed” dialog box) Control the feed rate with the cycle keys With “constant speed,” a feed rate per revolution must be defined.
3.2 Manual Control Mode Handwheel U Assign the handwheel to a principal axis or C axis (“Handwheel axes” dialog box U Define the feed rate or angle of rotation per handwheel increment (“Handwheel axes” dialog box). U The cancel the handwheel assignment, press the “Handwheel” soft key with opened dialog box. The handwheel assignment and speed ratio are shown in the machine display (the axis letter and the decimal place of the handwheel traverse ratio are marked).
3.2 Manual Control Mode Slide/spindle change key On lathes with multiple slides the following keys, functions and displays refer to the selected slide: Manual direction keys Setup functions (for example workpiece zero point setting, set tool change point) Slide-dependent display elements of the machine display Display of the “selected slide”: Machine display The “selected slide” is listed in the “slide display” (see “Machine Display” on page 97).
3.3 Table for Tools and Chucking Equipment 3.3 Table for Tools and Chucking Equipment The tool list (turret table) indicates the current tool carrier assignment. To set up a tool list, enter the ID numbers of the tools. You can use the entries in the TURRET section of the NC program to set up the tool list. The “Compare list” and “Accept list” functions refer to the NC program last interpreted in automatic mode.
3.3 Table for Tools and Chucking Equipment Setting up a tool list In “Setup tool list” you can declare the tool list independently from the data of an NC program. Entering a tool Select Setting up > Tool list > Compile list Select the tool location. Entering the tool directly: Press ENTER (or the INS key). The CNC PILOT opens the “Setup” dialog box Enter the ID number and click OK to close the dialog box.
3.3 Table for Tools and Chucking Equipment Deleting a tool Select Setting up > Tool list > Compile list Select the tool location. Use the soft key, or Press the DEL key to delete the tool Changing the tool location Select Setting up > Tool list > Compile list Select the tool location. Deletes the tool and saves it in the “ID number clipboard” Select a new tool location. Take the tool from the “ID number clipboard” If the location was occupied, the previous tool is taken into the clipboard.
3.3 Table for Tools and Chucking Equipment Comparing a tool list with an NC program The CNC PILOT compares the current tool list with the entries in the NC program last translated in automatic mode. The entries in the TURRET section are considered to be nominal tools. The CNC PILOT shows the following tools marked: Actual tool not equal to nominal tool Actual tool not occupied, nominal tool occupied Tool locations that are not assigned in the NC program cannot be selected.
3.3 Table for Tools and Chucking Equipment Transferring the tool list from an NC program The CNC PILOT transfers the new tool assignment from the TURRET section (reference: the NC program last interpreted in Automatic mode). Depending on the previous turret assignment, the following might occur: Tool not used: The CNC PILOT enters the new tools in the tool list. Positions that were occupied in the old tool list, but are not used in the new list, are retained. Delete the tool, if required.
3.3 Table for Tools and Chucking Equipment Tool life management The tool life management allows you to define the sequence of exchange and declare the tool to be ready for use. The tool life/ quantity is defined in the tool database. Apart from ID numbers and tool type descriptions, the tool list includes data for tool life management: Status: Shows the remaining tool life/quantity.
3.3 Table for Tools and Chucking Equipment Entering the tool life parameters Select Setting up > Tool list > Tool life management The CNC PILOT displays the entered tools Select the tool location. Press ENTER. The CNC PILOT opens the “Tool life management” dialog box. Enter the replacement tool and the other tool life parameters. Press the “New cutting edge” button: The CNC PILOT sets the tool life/quantity to the value programmed in the database and sets the tool to ready for use.
3.3 Table for Tools and Chucking Equipment Setting up the chucking table The chucking table is evaluated by the concurrent graphics. To switch to the chucking assignment of further spindles, press the PgUp/PgDn keys. Parameters for “spindle x” (main spindle, spindle 1, ..
3.4 Setup Functions 3.4 Setup Functions Setting the tool changing point With G14, the slide moves to the tool change point. Always program the tool change point as far from the workpiece as possible to allow the turret to rotate to any position. The tool change point is entered and displayed as distance between machine zero point and tool carrier zero point. Since these values are not displayed, it is advisable to move to the tool change point and “teach-in” the position.
3.4 Setup Functions Shifting the workpiece zero point The shift is referenced to the machine zero point. You can move the workpiece zero point for all principal axes. The workpiece zero point is a setup parameter. Specify the workpiece datum For more than one slide: Define the desired slide Move the tool into position Select Setting up > Shift zero point The “displace zero point” dialog box displays the new workpiece zero point.
3.4 Setup Functions Defining the protection zone Protection zone parameters: Serve for protection zone monitoring—not as software limit switches Given with respect to the machine zero point X values are radius dimensions 99999/-99999 means no monitoring of this protection zone side The protection zone parameters are managed in the parameters MP 1116, 1156 and following. Defining the protection zone Insert any tool (except T0).
3.4 Setup Functions Setting up machine dimensions This function takes into account the machine dimensions 1 to 9 and the “configured axes” per dimension. You can use the machine dimensions in the NC program. Machine dimensions are managed in MP 7. Machine dimensions are given with respect to the machine zero point. Define machine dimensions Select Setting up > Machine dimensions Enter the “machine dimension number” Teach in a single machine dimension Select the input field.
3.4 Setup Functions Tool measurement You specify the type of tool measurement in MP 6: 0: Touch-off 1: Measurement with probes 2: Measurement using optical measuring systems You move according to the measurement method to a certain position in the working space that is known to the system. Using that dimension, the CNC PILOT calculates the setting dimensions of the tool. The entries in the “Enter measured value” dialog box are given with respect to the workpiece zero point.
3.4 Setup Functions Measure tools with an optical gauge Select the X/Z input field Align the tool point in the X/Z direction with the cross hairs.
Overview of soft keys in Automatic mode In Automatic mode, the data are entered and displayed according to control parameter 1 either in meters or in inches. The setting in the “program head” of the NC program governs the execution of the NC part program. It has no influence on operation or display.
3.5 Automatic Mode Program selection The CNC PILOT interprets the NC program before it can be activated with Cycle Start. “#-Variables” are entered during the translation process. A “restart” prevents a new translation, while a “new start” forces a new translation. If the “turret table” of the NC program is not the currently valid table, there is a warning. The name of the NC program is retained until you select another program, even if the lathe was switched off in the meantime.
3.5 Automatic Mode Start again Select “Prog > New start” The NC program is loaded and converted. (Use for starting an NC program containing # variables.) From DIN PLUS Select “Prog > From DIN PLUS” The NC program selected in DIN PLUS is loaded and converted.
3.5 Automatic Mode Finding a start block In the start block search: Starting at program start, the CNC PILOT complies with the technology commands but does not conduct a tool change. The CNC PILOT allows no positioning. Danger of collision If the start block includes a T command, the CNC PILOT first rotates the turret. The first traversing instruction is executed from the current tool position. Select a suitable start block on all slides before you press the Accept soft key.
3.5 Automatic Mode Modifying the program run Skip level The NC blocks with skip levels are not executed when the skip level is active. The “Skip levels” display field marks the (active) skip levels detected by the “block execution.“ The CNC PILOT accounts for activated/deactivated skip levels after approx. 10 blocks (reason: block scan during the execution of NC blocks). Activating/deactivating a skip level Select “Process > Skip level.” Activating a skip level Enter the “Level no.
3.5 Automatic Mode V variables Working with V variables: The “V variables” dialog box serves for input and display of variables. V variables are defined at the beginning of the NC program. The meaning is specified in the NC program. To check or enter a V variable: Select “Process > V variables” The CNC PILOT displays the defined variables in the NC program. Change the variable: Press the Edit button Single-block mode In single-block mode, only one NC command (basic block) is executed at a time.
3.5 Automatic Mode Feed rate override F% The programmed feed rate changes with the programmed feed rate (range of 0 % to 150 %). The machine display shows the current feed rate override. Adjusting the feed rate override Adjust the desired override with the override knob (in the machine operating panel) Spindle speed override With the spindle speed override you can deviate from the programmed feed rate (range of 50 % to 150 %). The machine display shows the current spindle speed override.
3.5 Automatic Mode Additive compensation U Select “Comp > Tool compensation values” U Enter the compensation values (901 to 916). The CNC PILOT displays the valid compensation values. U Enter the compensation values. U Values entered here are added to the existing compensation values.
3.5 Automatic Mode Inspection mode For the inspection mode, interrupt the program run, check or correct the active tool, or change the cutter. Resume the NC program at the point of interruption. When the tool is retracted, the CNC PILOT stores the first five traverse movements. Each change in direction corresponds to a path of traverse. Notes on the inspection mode: During the inspection process you can turn the turret, press the spindle keys, etc. The return motion program inserts the “correct” tool.
3.5 Automatic Mode 2. Inspection – Check the cutting edge Inspect the tool; if necessary, replace it. Conclude the inspection process. The CNC PILOT loads the return motion program (_SERVICE). The “Tool compensation” dialog box appears. Enter the tool compensation. If you are using a new cutting edge, modify the tool compensation so that the tool—when returning—comes to a stop before the point of interruption. If necessary, activate the spindle. 3.
3.5 Automatic Mode 3.1 Return the tool and “scrambled takeoff” Start the return motion program. The “Scrambled takeoff on restart?” dialog box appears. Enter 1 (=yes) Takeoff from IP: The “Start from point of interruption (IP)” dialog box appears. Enter 0 (= to IP) The return motion program positions the tool from/before the interruption point and continues the program without stopping. Takeoff before IP: The “Start from point of interruption (IP)” dialog box appears.
3.5 Automatic Mode 3.2 Return the tool and stop Start the return motion program. The “Scrambled takeoff on restart?” dialog box appears. Enter 0 (=no) Takeoff from IP: The “Start from point of interruption (IP)” dialog box appears. Enter 0 (=from IP) The return motion program positions the tool on/before the interruption point and stops. Takeoff before IP: The “Start from point of interruption (IP)” dialog box appears.
3.5 Automatic Mode If the NC program stops before the interruption point, the “Distance from the interruption point” comes into play: If the entered distance is greater than the distance between the start of the NC block and the interruption point, program sequence begins at the start of the interrupted NC block. If the entered distance is less than the distance between the start of the NC block and the interruption point, the CNC PILOT takes the distance into account.
3.5 Automatic Mode Graphic display The “Automatic graphics” function displays the programmed blank and finished part and the paths of traverse. This enables process control of non-visible areas during production and provides an oversight of production status, etc. All machining operations, including milling, are depicted in the turning window (XZ view). U Activate the graphics. If the graphic was already active, the screen is adapted to the current machining status.
3.5 Automatic Mode Enlargement, reduction, and selecting a section Zoom settings by keyboard: U Activate the magnify function The red rectangle indicates the new section. U Adjust the section: To magnify, use the PgDn key To reduce, use the PgUp key To move the frame, use the arrow keys U Exit the zoom function.
3.5 Automatic Mode Post-process measuring status Post-process measuring means that the workpiece is measured outside the lathe and that the results are transferred to the CNC PILOT. The “PPM Info” dialog box contains information on the status of the measured values, displays the transferred results, and allows initialization of communication with the measuring device.
3.6 Machine Display 3.6 Machine Display Switching the display The machine display of the CNC PILOT can be configured. Per slide, you can configure up to 6 displays in Manual mode and Automatic mode (starting with control parameter 301). Switching the display U Switch to the next configured display. U Switch to the display of the next slide. U Switch to the display of the next spindle.
3.
3.
3.7 Load Monitoring 3.7 Load Monitoring The load monitoring function of the CNC PILOT compares the current torque, or the values for the work of the drives, with the values from a reference run. If “torque limit 1” or the “work limit” is exceeded, the CNC PILOT marks the tool as worn out. If torque limit 2 is exceeded, the CNC PILOT assumes tool breakage and stops the machining process (feed stop). Violations of limit values are reported as error messages.
3.7 Load Monitoring Machining using load monitoring During use of the load monitor, a worn tool should require significantly more torque than a sharp one. As a rule, drives that are subjected to considerable loads should be monitored. That usually means the spindle. Due to the relatively small torque variations, it is difficult to monitor machining operations with small cutting depths. A decrease in torque cannot be identified.
3.7 Load Monitoring Reference machining The reference machining cycle (registration of nominal values) determines the maximum permissible torque and work of each monitoring zone. These values are used as reference values! CNC PILOT executes a reference machining cycle if: There are no monitoring parameters You select “yes” in the reference machining dialog box (after program selection).
3.7 Load Monitoring Production using load monitoring If you wish to use the load monitoring function for your machining processes, you must activate it in the NC program (G996). Display torque values and limit values: U Select Disp(lay) > Load monitoring > Display “Load monitoring > Display” submenu: “Curves” menu item In curves 1 to 4 you assign the input field to the drives. Line graphic: A curve Bar graphic: Up to four bars With “Display grid” you influence the accuracy of the depiction.
3.7 Load Monitoring Editing the load parameters The “Display and adjust load parameters” dialog box displays the parameters of one component of one monitoring zone, which can then be edited. The bar graphic shows all components of the monitoring zone (the larger bar displays the values for performance; the smaller bar displays the values for work). The selected component is highlighted. Enter the monitoring zone and select the component. The CNC PILOT displays the reference values.
3.7 Load Monitoring “Analyzer (file display)” submenu: Set cursor: Position the cursor with the left/right arrow keys or to the Beginning of file Next beginning zone Maximum in zone Display menu item: Select the component from the “Display file” dialog box. Setting - Zoom: Set the zoom factor. (Small values increase the accuracy of the display and reduce the step size of the cursor.
3.7 Load Monitoring Control parameter 8 “Load monitoring settings” Factor for torque limit value 1, 2 Factor for work limit value Limit value = reference value * factor for limit value Minimum torque [% of rated torque]: Reference values below this value are raised to this minimum torque value. This prevents that limit values are exceeded as a result of minor torque differences.
DIN Programming HEIDENHAIN CNC PILOT 4290 107
4.1 DIN Programming 4.1 DIN Programming Introduction The CNC PILOT supports both conventional DIN programming and DIN PLUS programming. Conventional DIN/ISO programming: You program the basic contour with line segments, circular arcs and simple turning cycles. For conventional DIN programming, the simple tool description is sufficient. “DIN PLUS” (ISO) programming: The geometrical description of the workpiece and the machining process are separated.
4.1 DIN Programming DIN PLUS screen Screen layout: 1 2 3 4 5 Menu bar NC program bar with the name of the loaded NC programs. The selected program is marked. Full, double or triple editing window. The selected window is marked. Contour display or machine display Soft keys Parallel editing: You can edit up to eight NC program/subprograms in parallel. The CNC PILOT displays NC programs as desired in either a full, double, or triple window.
4.1 DIN Programming Linear and rotary axes Principal axes: Coordinates of the X, Y and Z axes refer to the workpiece zero point.
4.1 DIN Programming Units of measurement You write NC programs in metric or inch values. The unit of measure is defined in the “Unit” box (see “PROGRAM HEAD section” on page 136). Once the unit of measure has been defined, it cannot be edited any longer.
4.1 DIN Programming Examples: Permissible combination: N10 G1 X100 Z2 M8 Non-permissible combination: N10 G1 X100 Z2 G2 X100 Z2 R30 (same address letters are used more than once) or N10 M3 M4—opposing functionality NC address parameters The address parameters consist of 1 or 2 letters followed by A value A mathematical expression A question mark (VGP simplified geometry programming) A letter “i” to designate incremental address parameters (examples: Xi..., Ci..., XKi..., YKi..., etc.
4.2 Programming Notes 4.2 Programming Notes Configuring the DIN editor The following properties of the DIN editor can be configured in the main menu: Display/do not display a help graphic next to the dialog box Number of editing windows Font size You save and load these settings. Help graphic: U U Select Config > Help graphic. The editor opens the “Configuration of help graphic” dialog box. Set whether the help graphic should be displayed.
4.2 Programming Notes Parallel editing The CNC PILOT runs up to eight NC program/subprograms in parallel and provides up to three editing windows.
4.2 Programming Notes Making, editing and deleting NC blocks Make NC block: The insertion of new NC blocks varies depending on the program section. Program head U Close the “Editing program head” dialog box: The CNC PILOT automatically creates the blocks of the program head (code “#”). TURRET and CHUCKING EQUIPMENT program sections: U Press the INS key: The CNC PILOT opens the dialog for a new tool or chuck. U The new block is inserted after the dialog is finished.
4.2 Programming Notes Change NC element: U Position the cursor on an element of the NC block (NC block number, G or M command, address parameter, etc.) or the section code. U Press ENTER or double-click with the left mouse key. The CNC PILOT activates a dialog box which displays the block number, the number of the G or M function, or the address parameters of the function, which can then be edited. When editing section codes, you can change the associated parameters (Example: number of the turret).
4.2 Programming Notes Conversational or free editing In free editing you select the NC functions from the menus and edit the address parameters in dialog boxes. In free editing you enter all elements of the NC block. The maximum block length for “free editing,” is 128 characters per line. To select “free” editing: U U Select “Block > New: Free input” in the main menu. The DIN editor inserts an NC block at the cursor position and waits for the entry of a complete NC block.
4.2 Programming Notes Contour programming The “contour follow-up” function and contour-related turning cycles require the previous description of the blank and finished part. For milling and drilling, contour definition is a precondition if you wish to use fixed cycles. Contours for turning Describe a continuous contour. The direction of the contour description is independent of the direction of machining. CNC PILOT closes open contours paraxially.
4.2 Programming Notes Contour Follow-Up The CNC PILOT takes the blank part as a basis and accounts for each cut and each cycle when regenerating the contour. Thus you can inspect the current contour of the workpiece during each machining stage. With the “contour follow-up” function, the CNC PILOT optimizes the paths for approach and departure and avoids noncutting passes. Contour regeneration is available only for turning operations. It also works with auxiliary contours.
4.2 Programming Notes List of G functions If you do not know the G number, the DIN editor supports you with the G function list. U Select G in the geometry or machining menu. The editor opens the G number list. U Place the cursor on the desired G function. U Press ENTER to load the G number. Address parameters Coordinates can be programmed absolutely or incrementally. If you do not make any entry for X, Y, Z, XK, YK, C, the coordinates of the block previously executed will be retained (modal).
4.2 Programming Notes Tool programming The designations of the tool pockets are fixed by the machine tool builder. Each tool holder has a unique T number. In the T command (MACHINING section) you program the tool holder, and therefore the position to which the tool carrier rotates. The CNC PILOT retrieves the assignment of the tools to the tilted position from the TURRET section, or the tool list (in case the T number is not defined in TURRET).
4.2 Programming Notes Subprograms, expert programs Subprograms are used to program the contour or the machining process. In the subprograms, transfer parameters are available as variables. You can fix the designation of the transfer parameter (see “SUBPROGRAM section” on page 145). In every subprogram, the variables #256 to #285 are available for internal calculations. Subprograms can be nested up to six times. Nesting means that a subprogram calls a further subprogram, etc.
4.2 Programming Notes Fixed cycles HEIDENHAIN recommends programming a fixed cycle as follows: Tool change Define the cutting data Position the tool in front of the working area Definition of safety clearance Cycle call Retract the tool Move to tool change position Danger of collision! Remember when omitting cycle programming steps during optimization: A special feed rate remains in effect until the next feed command (for example the finishing feed rate during recessing cycles).
4.3 The DIN PLUS Editor 4.
4.3 The DIN PLUS Editor Overview of geometry menu The Geometry submenu contains G functions and instructions for the BLANK and FINISHED PART sections. With the menu items G, Line and Cir you select basic contour elements: If you know the G number, call G and enter the number of the G function.
4.3 The DIN PLUS Editor Overview of machining menu The Machining submenu contains G, M, T, S and F functions as well as further instructions for the MACHINING section. Selecting the G and M functions: If you know the G or M number, call the G or M menu and then enter the number of the function. If you do not know the G or M number, select the desired function from the G or M menu. T menu items (tool call): U U Select T Enter the T number, or select the tool from the list Menu item F: U Select F.
NC programs contain instructions and information that are configured specially to your lathe and organization. You can combine these data in a starting template and use it to write new programs (see programming example). Such a sample program makes it easier to write a new program and aids in standardizing NC programs. If you do not use the starting template, CNC PILOT makes a new NC program with the standard program section codes.
4.3 The DIN PLUS Editor NC program management Loading the NC program: Load NC program in the next free window: U Select Prog > Load > Main program (or > Subprogram). The CNC PILOT displays the files. U Select and load the NC program or subprogram Load NC program in selected window: U U U Select and activate free editing window Select Prog > Load > Main program (or > Subprogram). The CNC PILOT displays the files.
4.3 The DIN PLUS Editor Graphics window During editing CNC PILOT displays programmed contours in up to two graphic windows. To select the graphic windows: U Select “Graph. > Window” in the main menu U Mark the desired window To activate the contour display/update the contour: In the main menu: Select “Graph. > Graphic ON” U In the submenu: Press the soft key, or U U Select Graphic To activate the machine display: U Select “Graph.
4.3 The DIN PLUS Editor Workpiece-blank programming To describe the workpiece blank, proceed as follows: Standard blank (cylinder, hollow cylinder): U U Select “Geo > Blank> Chuck piece/bar G20” in the main menu. The CNC PILOT Creates an NC block in the BLANK section Switches to the “Geometry” submenu Activates the “Chuck part, cylinder/tube G20” dialog box Casting as blank (the workpiece blank contour is based on the finished part contour): U U Select “Geo > Blank> Casting G21” in the main menu.
4.3 The DIN PLUS Editor Programming instructions Instructions of the geometry menu Below are the contents of the Instr. (instructions) menu group DIN PLUS words: U U Select “Instr. > DIN PLUS words.” The editor opens the selection box. Select the desired instruction for program structuring or the input/ output command. Variable: U U Select “Instr. > Variables.” The editor opens the input line. Enter a variable or mathematical expression. Program section codes: Auxiliary contour: U Select “Instr.
4.3 The DIN PLUS Editor DIN PLUS words: U U Select “Instr. > DIN PLUS words.” The editor opens the selection box. Select the desired section code, instruction for program structuring or the input/output command. Variable: U U Select “Instr. > Variables.” The editor opens the input line. Enter a variable or mathematical expression. Skip level: U U Select “Instr. > / Deletion.” The editor opens the “Skip level” dialog box. Enter skip level [1 to 9]. Slide code: U U Select “Instr. > $ Slide.
4.3 The DIN PLUS Editor Block group menu This function enables NC block groups (several successive NC blocks) to be moved, copied, deleted or exchanged between NC programs. To define an NC block group, highlight the first and last line of the block group. Then select the desired operation on the block group. In order to exchange blocks groups between NC programs, copy the block group to the clipboard. Then read in the block group from the clipboard.
4.3 The DIN PLUS Editor Copying a block group: U U Position the cursor at the target position. Select “Edit > Copy and paste.” The block is inserted at/copied to the target position. The “Cancel” menu item: U Select “Cancel.” The editor removes all marking. The “Insert contour” menu item U Select “Insert contour.
4.4 Program Section Code 4.4 Program Section Code A new DIN program is already provided with section codes. You can add new codes or delete existing ones, depending on your program requirements. A DIN program must contain at least the MACHINING and END section codes. You can select further program section codes under the menu item “PAb” (Program section code) in the main menu, in the “Instr.” menu or in the DIN PLUS Words selection box. The CNC PILOT inserts the section code at the correct position.
4.4 Program Section Code PROGRAM HEAD section Instructions and information of the PROGRAM HEAD: Slide: The NC program is executed only for indicated slides Enter 1 for $1 Enter 12 for $1 and $2 No entry: NC program is run on every slide. Unit: Select dimensional system in millimeters or inches No entry: The unit set in control parameter 1 is used. The other fields contain organizational information and set-up information, which do not influence the machining process.
4.4 Program Section Code TURRET section The TURRET x program section (x: 1 to 6) defines the assignment of the tool carrier x. For every assigned turret pocket: The tool ID number is entered if the tool is in the database. The tool description is entered directly if it is a temporary tool. Temporary tools are not transferred into the database.
4.4 Program Section Code Simple tool description: The tools are suitable only for simple traverse paths and turning cycles (G0...G3, G12, G13; G81...G88). Contour follow-up is not taken into account. The tool radius compensation is conducted. Simple tools are not transferred into the database. If you do not program the TURRET, the tools entered in the tool list will be used. The names _SIM... and _AUTO... are reserved for temporary tools (simple tools and tools without ID number).
4.4 Program Section Code Entering or editing tools: U Select “Head > Turret assignment.” The editor moves the cursor to the TURRET section. Entering a tool: U Position the cursor. U Press the INS key. The editor opens the Tool dialog box. U Edit the Tool dialog box Editing the tool data: U Position the cursor on the entry to be edited. U Press RETURN or double-click with the left mouse key U Edit the Tool dialog box.
4.4 Program Section Code Loading a tool list As of software version 625 952-04: A tool list that has been set up in Machine mode can be loaded into the NC program. U U Place the cursor in the program section (TURRET 1, TURRET 2, PLATE MAGZN., etc.). Select “Head > Load list” in the main menu. The CNC PILOT transfers the selected turret or magazine list into the NC program. If you have already entered tools, they will be deleted after a confirmation prompt.
4.4 Program Section Code Turret assignment as tool list In the “Set up tool list” function, the CNC PILOT provides the turret assignment as a tool list for editing.
4.4 Program Section Code CHUCKING EQUIPMENT section The CHUCKING EQUIPMENT x program section (x: 1 to 4) defines spindle assignment x. Using the identification numbers of chuck, jaws and adapters (lathe center, etc.), you create the chucking equipment table.
4.4 Program Section Code CONTOUR section The CONTOUR program section assigns the following workpiece blank and finished part description to the contour “number x.” The control manages up to four contours (workpieces) in one NC program. A G99 in the machining section assigns the contour to a slide or spindle. Parameters Q Number of the contour (1 to 4) X Zero point shift (diameter value) Z Datum shift V Position of the coordinate system V=0 X X Z Q Z Q=1..
4.4 Program Section Code AUXILIARY CONTOUR section In the AUXILIARY CONTOUR section you describe the auxiliary contours of the turning contour. FRONT section In the FRONT section you describe the contours of the front face. Parameters Z Position of front face contour REAR SIDE section In the REAR SIDE section you describe the contours of the back face. Parameters Z Position of the rear-face contour SURFACE section In the SURFACE section you describe the cylindrical-surface contours.
4.4 Program Section Code SUBPROGRAM section If you define a subprogram within your NC program (within the same file), it is designated with SUBPROGRAM, followed by the name of the subprogram (max. 8 characters). RETURN code The RETURN code concludes the subprogram. CONST code In the CONST section of the program you define constants. You use constants for the definition of: a value a # variable a V variable You enter the value directly or you calculate it.
4.5 Definition of Workpiece Blank 4.5 Definition of Workpiece Blank Chuck piece: bar/tube G20-Geo G20 defines the contour of a cylinder/hollow cylinder. Parameters X Cylinder/hollow cylinder diameter Diameter of circumference of a polygonal blank Z Length of the blank K Right edge (distance between workpiece zero point and right edge) I Inside diameter of hollow cylinders Example: G20-Geo . . . ROHTEIL [WORKPIECE BLANK] N1 G20 X80 Z100 K2 I30 [hollow cylinder] . . .
Starting point of turning contour G0-Geo G0 defines the starting point of a turning contour. Example: G0-Geo Parameters . . . X Contour starting point (diameter value) FERTIGTEIL [FINISHED PART] Z Contour starting point N2 G0 X30 Z0 [starting point of contour] N3 G1 X50 B-2 N4 G1 Z-40 N5 G1 X65 N6 G1 Z-70 . . . Line segment in a contour G1-Geo G1 defines a line segment in a turning contour.
4.6 Basic Contour Elements Example: G1-Geo . . .
4.6 Basic Contour Elements Parameters B Chamfer/rounding. Defines the transition to the next contour element. When entering a chamfer/rounding, program the theoretical end point.
4.6 Basic Contour Elements Example: G2-, G3-Geo . . . FERTIGTEIL [FINISHED PART] N1 G0 X0 Z-10 N2 G3 X30 Z-30 R30 Target point and radius N3 G2 X50 Z-50 I19.8325 K-2.584 Target point and center, incremental N4 G3 XI10 ZI-10 R10 Target point (incremental) and radius N5 G2 X100 Z? R20 Unknown target point coordinate N6 G1 XI-2.5 ZI-15 . . . Circular arc of turning contour G12/G13-Geo G12/G13 defines a circular arc in a contour with absolute center dimensioning.
4.6 Basic Contour Elements Example: G12-, G13-Geo . . . FERTIGTEIL [FINISHED PART] N1 G0 X0 Z-10 . . . N7 G13 XI-15 ZI15 R20 Target point (incremental) and radius N8 G12 X? Z? R15 Only the radius is known N9 G13 X25 Z-30 R30 B10 Q1 Rounding arc in transition and selection of intersections N10 G13 X5 Z-10 I22.3325 K-12.584 Target point and center, absolute . . .
4.7 Contour Form Elements 4.7 Contour Form Elements Recess (standard) G22-Geo G22 defines a recess on the previously programmed paraxial reference element.
4.7 Contour Form Elements Example: G22-Geo . . . FERTIGTEIL [FINISHED PART] N1 G0 X40 Z0 N2 G1 X80 N3 G22 X60 I70 KI-5 B-1 R0.2 Recess on face, depth is incremental N4 G1 Z-80 N5 G22 Z-20 I70 K-28 B1 R0.2 Longitudinal recess, width is absolute N6 G22 Z-50 II-8 KI-12 B0.5 R0.3 Longitudinal recess, width is incremental N7 G1 X40 N8 G1 Z0 N9 G22 Z-38 II6 K-30 B0.5 R0.2 Longitudinal recess, inside . . .
4.7 Contour Form Elements Parameters B Outside radius/chamfer at corner near the starting point (default: 0) B>0: Rounding radius B<0: Chamfer width P Outside radius/chamfer at corner far from the starting point (default: 0) P>0: Radius of the rounding arc P<0: Chamfer width R Inside radius in both corners of recess (default: 0) The CNC PILOT refers the recess depth to the reference element. The recess base runs parallel to the reference element.
4.7 Contour Form Elements Example: G23-Geo . . . FERTIGTEIL [FINISHED PART] N1 G0 X40 Z0 N2 G1 X80 N3 G23 H0 X60 I-5 K10 A20 B-1 P1 R0.2 Recess on face, depth is incremental N4 G1 Z-40 N5 G23 H1 Z-15 K12 U70 A60 B1 P-1 R0.2 Longitudinal recess, width is absolute N6 G1 Z-80 A45 N7 G23 H1 X120 Z-60 I-5 K16 A45 B1 P-2 R0.4 Longitudinal recess, width is incremental N8 G1 X40 N9 G1 Z0 N10 G23 H0 Z-38 I-6 K12 A37.5 B-0.5 R0.2 Longitudinal recess, inside . . .
4.7 Contour Form Elements Example: G24-Geo . . . FERTIGTEIL [FINISHED PART] N1 G0 X40 Z0 N2 G1 X40 B-1.5 Starting point for thread N3 G24 F2 I1.5 K6 Z-30 Thread with undercut N4 G1 X50 Next transverse element N5 G1 Z-40 . . . Undercut contour G25-Geo G25 generates the following undercut contours in paraxial inside contour corners. Program G25 after the first axis-parallel element. You specify the undercut type in parameter H.
4.7 Contour Form Elements Undercut DIN 509 E (H=0.5) Parameters H Undercut type DIN 509 E: H=0 or H=5 I Undercut depth (radius) K Width of undercut R Undercut radius (in both corners of the undercut) W Undercut angle The CNC PILOT uses the diameter to calculate the parameters that you do not define. Example: Call G25-Geo DIN 509 E . . . N.. G1 Z-15 [longitudinal element] N.. G25 H5 [DIN 509 E] N.. G1 X20 [transverse element] . . .
4.7 Contour Form Elements Undercut DIN 76 (H=7) Parameters H Undercut type DIN 76: H=7 I Undercut depth (radius) K Width of undercut R Undercut radius in both corners of the undercut (default: R=0.6*I) W Undercut angle (default: 30°) Example: Call G25-Geo DIN 76 . . . N.. G1 Z-15 [longitudinal element] N.. G25 H7 I1.5 K7 N.. G1 X20 [DIN 76] [transverse element] . . . Undercut type H (H=8) If you do not enter W, the angle will be calculated on the basis of K and R.
4.7 Contour Form Elements Undercut type K (H=9) Parameters H Undercut type K: H=9 I Undercut depth R Undercut radius—no value: The circular element is not machined W Undercut angle A Angle to longitudinal axis (default: 45°) Example: Call G25-Geo type K . . . N.. G1 Z-15 [longitudinal element] N.. G25 H9 I1 R0.8 W40 N.. G1 X20 [type K] [transverse element] . . .
4.7 Contour Form Elements Thread (general) G37-Geo G37 defines the different types of thread. Multi-start threads and concatenated threads are possible. Threads are concatenated by programming several G01/G34 blocks after each other.
4.7 Contour Form Elements Before G37, program a linear contour element as a reference. Machine the thread with G31. For standard threads, the parameters P, R, A and W are defined by the CNC PILOT. Use Q=12 if you wish to use individual parameters. Danger of collision! The thread is generated to the length of the reference element. Another linear element without undercut is to be programmed as overrun.
4.7 Contour Form Elements Hole (centric) G49-Geo G49 defines a single hole with countersink and thread at the turning center (front or rear face). The G49 hole is a form element, not part of the contour.
4.8 Attributes for Contour Description 4.8 Attributes for Contour Description Overview of attributes for contour description G7 Precision stop ON Page 164 G8 Precision stop OFF Page 164 G9 Precision stop blockwise Page 164 G10 Influences the finishing feed rate for basic contour elements of the entire contour.
4.8 Attributes for Contour Description Precision stop Precision stop ON G7-Geo G7 switches precision stop on. It is a modal function. The block with G7 is run with precision stop. The CNC PILOT does not run the following block until the tool reaches the position tolerance window around the end point (for more on the tolerance window, see MP 1106, 1156, ...). Precision stop is used for basic contour elements that are executed with G890 or G840. Precision stop OFF G8-Geo G8 switches precision stop off.
4.8 Attributes for Contour Description Feed rate reduction factor G38-Geo G38 activates the special feed rate for the finishing cycle G890. The “special feed rate” applies only to basic contour elements. Parameters E Special feed factor (default: 1) Special feed rate = active feed rate * E (0 < E <= 1) G38 is a non-modal function. Program G38 before the contour element for which it is intended. G38 replaces another special feed rate or programmed surface roughness.
4.8 Attributes for Contour Description Use surface roughness (V, RH), finishing feed rate (F) and special feed rate ("E") alternately! G39 is a non-modal function. Program G39 before the contour element for which it is intended. G50 preceding a cycle (MACHINING section) cancels a finishing oversize programmed for that cycle with G39. Blockwise oversize G52-Geo G52 defines an equidistant oversize that is taken into consideration in G810, G820, G830, G860 and G890.
4.8 Attributes for Contour Description Additive compensation G149-Geo G149 followed by a D number activates/deactivates an additive compensation function. The CNC PILOT manages the 16 toolindependent compensation values in the setup parameter10. Parameters D Additive compensation (default: D900) D=900: Deactivates the additive compensation D=901 to 916: Activates the additive compensation D Note the direction of contour description.
4.9 C-Axis Contours—Fundamentals 4.9 C-Axis Contours— Fundamentals Milling contour position Define the reference plane or the reference diameter in the section code. Specify the depth and position of a milling contour (pocket, island) in the contour definition: With depth P programmed in the previous G308 cycle. Alternatively on figures: Cycle parameter depth P.
G309 defines the end of a reference plane. Every reference plane defined with G308 must be ended with G309 (see “Milling contour position” on page 168). Example for G308/G309 . . . FERTIGTEIL [FINISHED PART] . . .
4.9 C-Axis Contours—Fundamentals Slot centerline as reference and normal position Programming: Pattern center = center of curvature Pattern radius = curvature radius Normal position These commands arrange the slots at the distance of the pattern radius about the pattern center. Example: Slot centerline as reference, normal position N.. G402 Q4 K30 A0 XK0 YK0 H0 Circular pattern, normal position N..
4.9 C-Axis Contours—Fundamentals Center of curvature as reference and normal position Programming: Pattern center <> center of curvature Pattern radius = curvature radius Normal position These commands arrange the slots at the distance of the pattern radius plus curvature radius about the pattern center. Example: Center of curvature as reference, normal position N.. G402 Q4 K30 A0 XK5 YK5 H0 Circular pattern, normal position N..
4.10 Front and Rear Face Contours 4.10 Front and Rear Face Contours Starting point of front/rear face contour G100-Geo G100 defines the starting point of a front or rear face contour.
4.10 Front and Rear Face Contours Circular arc in front/rear face contour G102/ G103-Geo G102/G103 defines a circular arc in a front or rear face contour.
4.10 Front and Rear Face Contours Bore hole on front/rear face G300-Geo G300 defines a hole with countersinking and thread in a front or rear face contour.
4.10 Front and Rear Face Contours Linear slot on front/rear face G301-Geo G301 defines a linear slot in a contour on the front face/rear face. Parameters XK Center in Cartesian coordinates YK Center in Cartesian coordinates A Angle to XK axis (default: 0°) K Slot length B Slot width P Depth/height (default: “P” from G308) P<0: Pocket P>0: Island Circular slot on front/rear face G302/G303-Geo G302/G303 defines a circular slot in a contour on the front face/rear face.
4.10 Front and Rear Face Contours Full circle on front/rear face G304-Geo G304 defines a full circle in a contour on the front face/rear face. Parameters XK Center in Cartesian coordinates YK Center in Cartesian coordinates R Radius P Depth/height (default: “P” from G308) P<0: Pocket P>0: Island Rectangle on front/rear face G305-Geo G305 defines a rectangle in a contour on the front face/rear face.
4.10 Front and Rear Face Contours Eccentric polygon on front/rear face G307-Geo G307 defines a polygon in a contour on the front face/rear face.
4.10 Front and Rear Face Contours Circular pattern on front/rear face G402-Geo G402 defines a circular hole pattern or figure pattern on the front or rear face. G402 is effective for the hole/figure defined in the following block (G300 to 305, G307).
4.11 Lateral Surface Contours 4.11 Lateral Surface Contours Starting point of lateral surface contour G110-Geo G110 defines the starting point of a lateral-surface contour. Parameters Z Starting point C Starting point (starting angle) CY Starting point as linear value; reference: unrolled reference diameter Program either Z, C or Z, CY. Line segment in a lateral surface contour G111-Geo G111 defines a line segment in a lateral-surface contour.
4.11 Lateral Surface Contours Circular arc in lateral surface contour G112-/ G113-Geo G112/G113 defines a circular arc in a lateral-surface contour. Direction of rotation: See help graphic Parameters Z End point C End point (end angle) CY End point as linear value; reference: unrolled reference diameter R Radius K Center point in Z direction W Angle of the center point J Angle of the center point as a linear value B Chamfer/rounding. Defines the transition to the next contour element.
4.11 Lateral Surface Contours Hole on lateral surface G310-Geo G310 defines a hole with countersink and thread in a lateral surface contour.
4.11 Lateral Surface Contours Linear slot on lateral surface G311-Geo G311 defines a linear slot in a lateral-surface contour.
4.11 Lateral Surface Contours Full circle on lateral surface G314-Geo G314 defines a full circle in a lateral-surface contour. Parameters Z Center C Center (angle) CY Center as linear value; reference: unrolled reference diameter R Radius P Pocket depth (default: “P” from G308) Rectangle on lateral surface G315-Geo G315 defines a rectangle in a lateral-surface contour.
4.11 Lateral Surface Contours Eccentric polygon on lateral surface G317-Geo G317 defines a polygon in a lateral-surface contour.
4.11 Lateral Surface Contours Linear pattern on lateral surface G411-Geo G411 defines a linear hole or figure pattern on the lateral surface. G411 is effective for the hole/figure defined in the following block (G310.0.315, G317).
4.11 Lateral Surface Contours Circular pattern on lateral surface G412-Geo G412 defines a circular hole or figure pattern on the lateral surface. G412 is effective for the hole/figure defined in the following block (G310.0.315, G317).
4.12 Tool Positioning 4.12 Tool Positioning Rapid traverse G0 G0 moves at rapid traverse along the shortest path to the target point. Parameters X Target point (diameter) Z Target point Programming X, Z: Absolute, incremental or modal Setting the tool change position G14 G14 moves the slide at rapid traverse to the tool change position. In setup mode, define permanent coordinates for the tool change position. Parameters Q Sequence.
4.12 Tool Positioning Rapid traverse to machine coordinates G701 G701 moves at rapid traverse along the shortest path to the target point. Parameters X End point (diameter) Z End point X, Z refer to the machine zero point and the slide zero point.
4.13 Simple Linear and Circular Movements 4.13 Simple Linear and Circular Movements Linear path G1 G1 moves the tool on a linear path at the feed rate to the “end point.” Parameters X End point (diameter) Z End point A Angle (angular direction: see help graphic) Q Point of intersection. End point if the line segment intersects a circular arc (default: 0): Q=0: Near point of intersection Q=1: Far point of intersection B Chamfer/rounding. Defines the transition to the next contour element.
4.13 Simple Linear and Circular Movements Circular path G2/ G3 G2/G3 moves the tool in a circular arc at the feed rate to the “end point.” The center dimensioning is incremental.
4.13 Simple Linear and Circular Movements Circular path G12/ G13 G12/G13 moves the tool in a circular arc at the feed rate to the “end point.” The center dimensioning is absolute. Direction of rotation (see help graphic): G12: In clockwise direction G13: In counterclockwise direction Parameters X End point (diameter) Z End point R Radius (0 < R <= 200 000 mm) I Absolute center point (radius) K Absolute center point Q Point of intersection.
4.14 Feed Rate and Spindle Speed 4.14 Feed Rate and Spindle Speed Rotational speed limiting G26 G26: Main spindle; Gx26: Spindle x (x: 1...3) The speed limitation remains in effect until the end of the program or until a new value is programmed for G26/Gx26. Parameters S (Maximum) speed Example: G26 . . . N1 G14 Q0 N1 G26 S2000 N2 T3 G95 F0.25 G96 S200 M3 N3 G0 X0 Z2 Actual S > “absolute maximum speed” (MP 805, ff), applies to the parameter value.
G64 interrupts the programmed feed for a short period of time. G64 is a modal function. Parameters E Pause duration (0.01 s < E < 99.99 s) F Feed duration (0.01 s < E < 99.99 s) For switch-on, program G64 with E and F. For switch-off, program G64 without parameters. Example: G64 . . . N1 T3 G95 F0.25 G96 S200 M3 N2 G64 E0.1 F1 [interrupted feed on] N3 G0 X0 Z2 N4 G42 N5 G1 Z0 N6 G1 X20 B-0.5 N7 G1 Z-12 N8 G1 Z-24 A20 N9 G1 X48 B6 N10 G1 Z-52 B8 N11 G1 X80 B4 E0.
4.14 Feed Rate and Spindle Speed Feed per tooth Gx93 Gx93 (x: spindle 1...3) defines the drive-dependent feed rate with respect to the number of teeth of the cutter. Parameters F Feed per tooth in mm/tooth or inch/tooth The actual value display shows the feed rate in mm/rev. Example: G193 . . . N1 M5 N2 T1 G197 S1010 G193 F0.08 M104 N3 M14 N4 G152 C30 N5 G110 C0 N6 G0 X122 Z-50 N7 G... N8 G... N9 M15 . . . Constant feed rate G94 (feed per minute) G94 defines the feed rate independent of drive.
4.14 Feed Rate and Spindle Speed Constant surface speed Gx96 G96: Main spindle; Gx96: Spindle x (x: 1...3) The spindle speed is dependent on the X position of the tool tip or on the diameter of the driven tools. Parameters S Cutting speed in m/min or ft/min Example: G96, G196 . . . N1 T3 G195 F0.25 G196 S200 M3 N2 G0 X0 Z2 N3 G42 N4 G1 Z0 N5 G1 X20 B-0.5 N6 G1 Z-12 N7 G1 Z-24 A20 N8 G1 X48 B6 N9 G1 Z-52 B8 N10 G1 X80 B4 E0.08 N11 G1 Z-60 N12 G1 X82 G40 . . .
4.15 Tool-Tip and Cutter Radius Compensation 4.15 Tool-Tip and Cutter Radius Compensation Tool-tip radius compensation (TRC) If TRC is not used, the theoretical tool tip is the reference point for the paths of traverse. This might lead to inaccuracies when the tool moves along non-paraxial paths of traverse. The TRC function corrects programmed paths of traverse. The TRC (Q=0) reduces the feed rate for circular arcs if the shifted radius < the original radius.
G40 is used to deactivate TRC/MCRC. Please note: The TRC/MCRC remains in effect until a block with G40 is reached. The block containing G40, or the block after G40 only permits a linear path of traverse (G14 is not permissible). Function of the TRC/MCRC . . . N.. G0 X10 Z10 N.. G41 G0 Z20 Path of traverse: from X10/Z10 to X10+TRC/ Z20+TRC N.. G1 X20 The path of traverse is “shifted” by the TRC N.. G40 G0 X30 Z30 Path of traverse from X20+TRC/Z20+TRC to X30/ Z30 . . .
4.16 Zero Point Shifts 4.16 Zero Point Shifts You can program several zero point shifts in one NC program. The relationships of the coordinates (for blank/finished part, auxiliary contours) are retained by the zero offset description. G920 temporarily deactivates zero point shifts—G980 reactivates them.
4.16 Zero Point Shifts Zero point shift G51 G51 shifts the workpiece zero point by Z (or X). The shift is referenced to the workpiece zero point defined in setup mode. Parameters X Shift (radius) Z Shift Even if you shift the zero point several times with G51, it is always referenced to the workpiece zero point defined in setup mode. The zero point shift is valid until program end, or until it is canceled by other zero point shifts. Example: G51 . . . N1 T3 G95 F0.
4.16 Zero Point Shifts Additive zero point shift G56 G56 shifts the workpiece zero point by Z (or X). The shift is referenced to the currently active workpiece zero point. Parameters X Shift (radius value) – (default: 0) Z Shift If you shift the workpiece zero point more than once with G56, the shift is always added to the currently active zero point. Example: G56 . . . N1 T3 G95 F0.25 G96 S200 M3 N2 G0 X62 Z5 N3 G810 NS7 NE12 P5 I0.5 K0.
4.16 Zero Point Shifts Absolute zero point shift G59 G59 sets the workpiece zero point to X, Z. The new zero point remains in effect to the end of the program. Parameters X Shift (radius) Z Shift G59 cancels all previous zero point shifts (with G51, G56 or G59). Example: G59 . . . N1 G59 Z256 [zero point shift] N2 G14 Q0 N3 T3 G95 F0.25 G96 S200 M3 N4 G0 X62 Z2 . . .
4.16 Zero Point Shifts Mirror/shift contour G121 G121 mirrors and/or shifts the blank and finished part contours. The contour is mirrored at the X axis and shifted in Z direction. The workpiece zero point is not affected. Parameters H Type of transformation (default: 0) H=0: Contour shift, not mirroring H=1: Contour shift, mirroring and reversing the direction of the contour description Q Mirroring the Z axis of the coordinate system (default: 0) Q=0: Do not mirror Q=1: Mirror Z Shift.
4.16 Zero Point Shifts Contour shift, mirroring the coordinate system N.. . . . Rear side machining on the opposing spindle N.. G121 H1 Q1 Z.. D1 Shifts and mirrors the contour; mirrors the coordinate system. N.. . . . Shift contour, do not mirror N.. . . . Rear side machining on the opposing spindle N.. G121 H0 Q0 Z.. D1 Shifts the contour N.. . . . Contour mirroring and shifting N.. . . . Rear-face machining with one spindle (manual rechucking) N.. G121 H1 Q0 Z..
4.17 Oversizes 4.17 Oversizes Switch off oversize G50 G50 switches off oversizes defined with G52/G39 Geo for the following cycle. Program G50 before the cycle. To ensure compatibility the G52 code is also supported for switching off the oversizes. HEIDENHAIN recommends using G50 for new NC programs. Axis-parallel oversize G57 G57 defines different oversizes for X and Z. Program G57 before the cycle call.
4.17 Oversizes Contour-parallel oversize (equidistant) G58 G58 defines an equidistant oversize. Program G58 before the cycle call. A negative oversize during finishing is permitted with G890. Parameters P Oversize G58 is effective in the following cycles. After cycle run, the oversizes are deleted: G810, G820, G830, G835, G860, G869, G890 not deleted: G83 If an oversize is programmed with G58 and in the cycle, the oversize from the cycle is used. Example: G58 . . . N1 T3 G95 F0.
4.18 Safety Clearances 4.18 Safety Clearances Safety clearance G47 G47 defines the safety clearance for the turning cycles: G810, G820, G830, G835, G860, G869, G890. the drilling cycles G71, G72, G74. the milling cycles G840...G846. Parameters P Safety clearance G47 without parameters activates the parameter values (machining parameters 2, ... – safety clearances). G47 replaces the safety clearance set in the machining parameters or that set in G147.
4.19 Tools, Types of Compensation 4.19 Tools, Types of Compensation Tool call – T The CNC PILOT displays the tool assignment defined in the TURRET section. You can enter the T number directly or select it from the tool list (switch with the CONTINUE soft key).
4.19 Tools, Types of Compensation (Changing the) tool edge compensation G148 G148 defines the values compensating for wear. DX, DZ become effective after program start and after a T command. Parameters Q Selection (default: 0) O=0: DX, DZ active—DS inactive O=1: DS, DZ active—DX inactive O=2: DX, DS active—DZ inactive The recessing cycles G860, G866, G869 automatically take the “correct” wear compensation into account. Example: G148 . . . N1 T3 G95 F0.25 G96 S160 M3 N2 G0 X62 Z2 N3 G0 Z-29.
The CNC PILOT manages 16 tool-independent compensation values. One G149 followed by a D number activates the additive compensation function. G149 D900 deactivates the additive compensation function. Example: G149 . . . N1 T3 G96 S200 G95 F0.
4.19 Tools, Types of Compensation Compensation of right-hand tool tip G150 Compensation of left-hand tool tip G151 G150/G151 defines the tool reference point for recessing and button tools. G150: Reference point is on right tip G151: Reference point is on left tip. G150/G151 is effective from the block in which it is programmed and remains in effect up to the next tool change program end. The displayed actual values always refer to the tool tip defined in the tool data.
4.19 Tools, Types of Compensation Adding tool dimensions G710 When a T command is programmed, the CNC PILOT replaces the previous tool dimensions with new tool dimensions. When you activate the adding function with G710 Q1, the dimensions of the new tool are added to the dimensions of the previous tool. Parameters Q Adding tool dimensions Q=0: Off Q=1: On Application example For full-surface machining, the workpiece is transferred to a rotating gripper after having been machined on the front face.
4.20 Contour-Based Turning Cycles 4.20 Contour-Based Turning Cycles Working with cycles Finding the block references: Activate the contour view: U Press the soft key or select the menu item “Graphic.” U Place cursor in NS or NE input field Switch to graphic window: Press the CONTINUE soft key U Select the contour element: Use the horizontal arrow keys to select the contour element U U Use the vertical arrow keys to switch between contours (also face contours, etc.).
4.20 Contour-Based Turning Cycles Parameters E Approach behavior E=0: Descending contours are not machined.
4.20 Contour-Based Turning Cycles Parameters B Slide lead with 4-axis machining B=0: Both slides work at the same diameter—at double feed rate B<>0: Distance to the leading slide (the approach). The slides work on different diameters with the same feed rate. B<0: Slide with larger number leads B>0: Slide with smaller number leads The CNC PILOT uses the tool definition to distinguish between external and internal machining. Program at least NS or NS, NE and P.
4.20 Contour-Based Turning Cycles Use as 4 axis cycle Same diameter: Both slides start simultaneously. Differing diameters: The second slide starts when the leading slide has reached lead B. This is synchronized at every step. Each slide advances by the calculated depth of cut. If the slides do not have to execute the same number of cuts, the leading slide executes the last cut. With constant surface speed, the cutting speed depends on the speed of the leading slide.
4.
4.20 Contour-Based Turning Cycles Program at least NS or NS, NE and P. The tool radius compensation: is active. A G57 oversize Enlarges the contour (also inside contours) A G58 oversize >0: Enlarges the contour <0: Is not offset G57/G58 oversizes are deleted after cycle end. Cycle run 1 Calculates the areas to be machined and the cutting segmentation. 2 Approaches workpiece for first pass from starting point, taking the safety clearance into account (first in X direction, then in Z).
4.20 Contour-Based Turning Cycles Contour-parallel roughing G830 G830 machines the area parallel to the contour from NS to NE as defined by NS, NE. If required, the area to be machined is divided into several sections (example: with contour valleys). X Z Parameters NS Starting block number (beginning of contour section) NE End block number (end of contour section) NE not programmed: The contour element NS is machined in the direction of contour definition.
4.20 Contour-Based Turning Cycles Parameters D Omit elements. The following undercuts, relief turns and recesses are not run (default: 0): G22 G23 H0 G23 H1 G25 H4 G25 H5/6 G25 H7 to H9 D=0 • • • • • • D=1 • • • – – – D=2 • • – • • • D=3 • • – – – – D=4 • • – • • – “•”: Do not machine the elements The CNC PILOT uses the tool definition to distinguish between external and internal machining. Program at least NS or NS, NE and P.
4.20 Contour-Based Turning Cycles Contour-parallel with neutral tool G835 G835 machines the contour area defined by NS, NE parallel to the contour and bidirectionally. If required, the area to be machined is divided into several sections (example: with contour valleys). X W Parameters NS Starting block number (beginning of contour section) NE End block number (end of contour section) NE not programmed: The contour element NS is machined in the direction of contour definition.
4.20 Contour-Based Turning Cycles Parameters D Omit elements. The following undercuts, relief turns and recesses are not run (default: 0): G22 G23 H0 G23 H1 G25 H4 G25 H5/6 G25 H7 to H9 D=0 • • • • • • D=1 • • • – – – D=2 • • – • • • D=3 • • – – – – D=4 • • – • • – “•”: Do not machine the elements The CNC PILOT uses the tool definition to distinguish between external and internal machining. Program at least NS or NS, NE and P.
4.20 Contour-Based Turning Cycles Recessing G860 G860 machines the contouring area axially/radially from NS to NE as defined by NS, NE. The contour to be machined can contain various valleys. If required, the area to be machined is divided into several sections (example: with contour valleys).
4.20 Contour-Based Turning Cycles Program at least NS or NS, NE. Number of cutting passes: Maximum offset = SBF * cutting width (SBF: See Machining Parameter 6) The tool radius compensation: is active. A G57 oversize enlarges the contour (also inside contours). A G58 oversize >0: Enlarges the contour <0: Is not offset G57/G58 oversizes are deleted after cycle end. Cycle run (where Q=0 or 1) 1 Calculates the areas to be machined and the cutting segmentation.
4.20 Contour-Based Turning Cycles Recessing cycle G866 G866 generates a recess defined by G22-Geo. The CNC PILOT uses the tool definition to distinguish between external and internal machining, or between radial and axial recesses.
G869 machines the contouring area axially/radially from NS to NE as defined by NS, NE. The workpiece is machined by alternate recessing and roughing movements. The machining process requires a minimum of retraction and infeed movements. The contour to be machined can contain various valleys. If required, the area to be machined is divided into several sections.
4.20 Contour-Based Turning Cycles Parameters V Identifier beginning/end (default: 0) A chamfer/rounding arc is machined: V=0: At start and end V=1: At start V=2: At end V=3: No machining O Recessing feed rate (default: active feed rate) E Finishing feed rate (default: active feed rate) B Offset width (default: 0) The CNC PILOT uses the tool definition to distinguish between radial and axial recesses. Program at least NS or NS, NE and P.
4.20 Contour-Based Turning Cycles Cycle run (where Q=0 or 1) 1 Calculates the areas to be machined and the cutting segmentation. 2 Approaches workpiece for first pass from starting point, taking the safety clearance into account. Radial recess: First Z, then X direction Axial recess: First X, then Z direction 3 Executes the first cut (recessing). 4 Machines perpendicularly to recessing direction (turning). 5 Repeats 3 to 4 until the complete area has been machined.
4.20 Contour-Based Turning Cycles Finish contour G890 G890 finishes the contour area defined by NS, NE in one pass and takes chamfers/rounding arc into account. The operation proceeds from NS to NE.
4.20 Contour-Based Turning Cycles Parameters H Type of retraction (default: 3) Tool backs off at 45° against the machining direction and moves as follows to the position I, K: H=0: Diagonal H=1: First X, then Z direction H=2: First Z, then X direction H=3: Remains at safety clearance H=4: No traverse—tool remains on the end coordinate X Cutting limit (diameter value)—(default: no cutting limit) Z Cutting limit (default: no cutting limit) D Omit elements (default: 1).
4.20 Contour-Based Turning Cycles Automatic feed rate reduction for chamfers/rounding arcs: Peak-to-valley height or feed rate with G95-Geo are programmed: No automatic feed reduction. Surface roughness or feed rate are not programmed: Automatic feed rate reduction; the chamfer/rounding arc is machined with at least 3 revolutions For chamfers/rounding arcs which, as a result of their size, are machined with at least three revolutions, the feed rate is not reduced automatically.
4.21 Simple Turning Cycles 4.21 Simple Turning Cycles End of cycle G80 G80 concludes a fixed cycle. Simple longitudinal roughing G81 G81 roughs the contour area defined by the current tool position and X, Z. If you wish to machine an oblique cut, you can define the angle with I and K.
4.21 Simple Turning Cycles Cycle run 1 Calculates the number of cutting passes. 2 Approaches workpiece for first pass from starting point on paraxial path. 3 Moves at feed rate to target point Z. 4 Depending on algebraic sign of I: <0: Machines contour outline I>0: Retracts by 1 mm at 45° 5 Returns at rapid traverse and approaches for next pass. 6 Repeats 3 to 5 until target point X has been reached.
4.21 Simple Turning Cycles Cycle run 1 Calculates the number of cutting passes (infeeds). 2 Approaches workpiece for first pass from starting point on paraxial path. 3 Moves at feed rate to target point X. 4 Depending on algebraic sign of K: K<0: Machines contour outline K>0: Retracts by 1 mm at 45° 5 Returns at rapid traverse and approaches for next pass. 6 Repeats 3 to 5 until target point Z has been reached.
4.21 Simple Turning Cycles Simple contour repeat cycle G83 G83 carries out the functions programmed in the following blocks (simple traverses or cycles without a contour definition) more than once. G80 ends the machining cycle.
4.21 Simple Turning Cycles Danger of collision! After each pass, the tool returns on a diagonal path before it advances for the next pass. If required, program an additional rapid traverse path to avoid a collision. Undercut cycle G85 With the function G85, you can machine undercuts according to DIN 509 E, DIN 509 F and DIN 76 (thread undercut). The CNC PILOT determines the type of undercut using K.
4.
4.21 Simple Turning Cycles Parameters K Radial recess: Recess width K>0: Recess width No input: Recess width = tool width Axial recess: Oversize K>0: Oversize (roughing and finishing) K=0: No finishing E Dwell time (for chip breaking)—(default: length of time for one revolution) With finishing oversize: Only for finishing Without finishing oversize: For every recess “Oversize” programmed: First roughing, then finishing G86 machines chamfers at the sides of the recess.
4.21 Simple Turning Cycles Radius cycle G87 G87 machines transition radii at orthogonal, paraxial inside and outside corners. The direction is taken from the position/machining direction of the tool. Parameters X Corner point (diameter) Z Corner point B Radius E Reduced feed rate (default: active feed) A preceding longitudinal or transverse element is machined if the tool is located at the X or Z coordinate of the corner before the cycle is executed. The tool radius compensation: is active.
4.22 Thread Cycles 4.22 Thread Cycles Overview of threading cycles G31 machines simple threads, successions of threads and multistart threads with G24, G34 or G37 Geo (see “Thread cycle G31” on page 240). G31 does not switch the velocity feedforward. If you want to work without velocity feedforward you can switch it off before the thread cycle. G32 cuts a simple thread in any desired direction and position (see “Simple thread cycle G32” on page 242). G32 is used to deactivate velocity feedforward.
4.22 Thread Cycles Thread cycle G31 G31 machines simple threads, successions of threads and multi-start threads with G24-, G34- or G37-Geo. The CNC PILOT uses the tool definition to distinguish between external and internal threads. Parameters NS Block number (reference to basic element G1 Geo for successions of threads: block number of the first basic element) I Maximum infeed B Run-in length—no input: Run-in length is calculated from adjacent undercuts or recesses.
4.22 Thread Cycles You can calculate the minimum run-in and run-out length with the following equation. Smooth threading switched off Run-in length: B = 0.75 * (F*S)² / a + 0.15 Run-out length: P = 0.75 * (F*S)² / e + 0.15 Smooth threading switched on Run-in length: B = 0.75 * (F*S)² / a * 0.66 + 0.15 Run-out length: P = 0.75 * (F*S)² / e * 0.66 + 0.15 F: Thread pitch in mm/revolution S: Speed in revolutions/second a, e: Acceleration in mm/s² (see “Acceleration at block start/block end” in MP 1105, .
4.22 Thread Cycles Cycle run 1 Calculates the number of cutting passes. 2 Returns diagonally to the internal starting point at rapid traverse. This point lies in front of the “starting point of thread” by the runin length B. With H=1 (or 2, 3) the current offset is taken into account for calculating the internal starting point. The internal starting point is calculated on the basis of the tool tip. 3 Accelerates to feed rate (line B). 4 Executes a thread cut. 5 Decelerates (line P).
4.22 Thread Cycles Parameters H Type of offset for smoothing the thread flanks (default: 0) H=0: Without offset H=1: Offset from left H=2: Offset from right H=3: Tool is offset alternately from the right and left The cycle calculates the thread from the thread end point, thread depth and the tool position. The main machining direction of the tool determines whether an internal or an external thread will be machined. First infeed = Remainder of the division of thread depth/cutting depth.
4.22 Thread Cycles Thread single path G33 G33 conducts a single thread cut. The direction of the single thread path is as desired (longitudinal, tapered or transverse threads; internal or external threads). You can make successive threads by programming G33 several times in succession. Position the tool in front of the thread by the run-in length B if the slide must accelerate to the feed rate. And remember the run-out length P before the end point of thread if the slide has to be decelerated.
4.22 Thread Cycles Run-in length: B = 0.75 * (F*S)² / a * 0.66 + 0.15 Run-out length: P = 0.75 * (F*S)² / e * 0.66 + 0.15 F: Thread pitch in mm/revolution S: Speed in revolutions/second a, e: Acceleration in mm/s² (see “Acceleration at block start/block end” in MP 1105, ...) Starting angle C: At the end of the “run-in path B” the spindle is at the “starting angle C” position. Feedforward: G31 does not switch the feedforward off.
4.23 Drilling Cycles 4.23 Drilling Cycles Drilling cycle G71 G71 is used for axial and radial holes using driven or stationary tools for: Single hole without contour description Hole with contour description (single hole or hole pattern) Parameters NS Block number of contour Reference to the contour of the hole (G49-, G300- or G310Geo) No input: Single hole without contour description NF Reference from which the cycle reads the hole positions [1 to 127].
4.
4.23 Drilling Cycles Boring, countersinking G72 G72 is used for holes with contour definition (individual hole or hole pattern). Use G72 for the following axial and radial drilling functions using driven or stationary tools: Boring Countersinking Reaming NC centering Centering Parameters NS Block number of contour.
4.23 Drilling Cycles Tapping G73 G73 cuts axial/radial threads using driven or stationary tools. G73 is used for holes with contour definition (individual hole or hole pattern). Parameters NS Block number of contour.
4.23 Drilling Cycles Cycle run 1 Moves at rapid traverse to the starting point: K not programmed: Retracts directly to the starting point K programmed: Moves to the position K and then to the starting point 2 Moves along run-in length B feed rate (synchronization of spindle and feed drives). 3 Cuts the thread. 4 Retracts with return speed S: K not programmed: To the starting point K programmed: To the position K Tapping G36 G36 cuts axial/radial threads using driven or stationary tools.
4.23 Drilling Cycles Type of taps: Stationary tap: Main spindle and feed drive are synchronized. Driven tap: Driven tool and feed drive are synchronized. “Cycle STOP” becomes effective at the end of the tapping operation. Feed rate override is not effective. Do not use spindle override! Use a floating tap holder if the driven tool is not controlled, e.g. by a ROD encoder. Deep-hole drilling G74 G74 is used for axial and radial holes in several stages using driven or stationary tools.
4.23 Drilling Cycles The cycle is used for: Single hole without contour description Hole with contour description (single hole or hole pattern) “1st drilling depth P” is used for the first pass. MANUALplus then automatically reduces the drilling depth with each subsequent pass by the reduction value I, however, without falling below the minimum drilling depth J. After each pass, the tool is retracted either by retraction distance B or to the starting point of the hole.
4.24 C-Axis Commands 4.24 C-Axis Commands No. of C axis G119 Use G119 if several C axes are available and the active C axis is switched during machining. With G119 without Q, deselect the old assignment and assign the C-Axis to the slide with G119 Q... Parameters Q Number of the C axis (default: 0) Q=0: Cancel assignment of C axis to slide Q>0: Assign the C axis to the slide Reference diameter G120 G120 determines the reference diameter of the unrolled lateral surface.
4.24 C-Axis Commands Zero point shift, C axis G152 G152 defines an absolute zero point for the C axis (reference: MP 1005, .. “Reference point, C axis”). The zero point is valid until the end of the program. Parameters C Angle (spindle position) of the new C-axis zero point Example: G152 . . . N1 M5 N2 T7 G197 S1010 G193 F0.08 M104 N3 M14 N4 G152 C30 N5 G110 C0 N6 G0 X122 Z-50 N7 G71 X100 N8 M15 . . .
4.25 Front/Rear-Face Machining 4.25 Front/Rear-Face Machining Rapid traverse on front/rear face G100 G100 moves at rapid traverse along the shortest path to the end point.
4.25 Front/Rear-Face Machining Linear segment on front/rear face G101 G101 moves the tool on a linear path at the feed rate to the “end point.” Parameters X End point (diameter) C End angle—for angle direction, see help graphic XK End point (Cartesian) YK End point (Cartesian) Z End point (default: current Z position) Programming: X, C, XK, YK, Z: Absolute, incremental or modal Program either X–C or XK–YK Example: G101 . . . N1 T7 G197 S1200 G195 F0.
4.25 Front/Rear-Face Machining Circular arc on front/rear face G102/G103 G102/G103 moves the tool in a circular arc at the feed rate to the “end point.” The direction of rotation is shown in the graphic support window.
4.26 Lateral Surface Machining 4.26 Lateral Surface Machining Rapid traverse, lateral surface G110 G110 moves at rapid traverse along the shortest path to the end point. G110 is recommneded for positioning the C axis to a defined angle (programming: N.. G110 C...). Parameters Z End point C End angle CY End point as linear value (referenced to unrolled reference diameter G120) X End point (diameter) Programming: Z, C, CY: Absolute, incremental, or modal Program either Z–C or Z–CY Example: G110 .
4.26 Lateral Surface Machining Line segment on lateral surface G111 G111 moves the tool on a linear path at the feed rate to the “end point.” Parameters Z End point C End angle—for angle direction, see help graphic CY End point as linear value (referenced to unrolled reference diameter G120) X End point (diameter value)—(default: current X position) Programming: Z, C, CY: Absolute, incremental, or modal Program either Z–C or Z–CY Example: G111 . . . [G111, G120] N1 T8 G197 S1200 G195 F0.
4.26 Lateral Surface Machining Circular arc on lateral surface G112/G113 G112/G113 moves the tool in a circular arc at the feed rate to the “end point.
4.27 Milling Cycles 4.27 Milling Cycles Contour milling G840—Fundamentals G840 mills or deburrs open or closed contours (figures or “free contours”). Depending on the cutter, select vertical plunging or predrilling and then milling. Plunge strategies: Depending on the cutter you are using, select one of the following strategies: Vertical plunge: The cycle moves the tool to the starting point; the tool plunges and mills the contour. Calculate positions, predrill, mill.
4.27 Milling Cycles G840 – Calculating hole positions “G840 A1 ..” calculates the hole positions and stores them at the reference specified in “NF.” Program only the parameters given in the following list. See also: G840—Fundamentals: Page 261 G840—Milling: Page 263 Parameters – Calculating hole positions Q Cycle type (= milling location) Open contour. If there is any overlapping, Q defines whether the first area (as of starting point) or the entire contour is to be machined.
4.27 Milling Cycles Parameters – Calculating hole positions D Starting element number for partial figures The direction of contour definition for figures is counterclockwise. The first contour element for figures: Circular slot: The larger arc Full circle: The upper semicircle Rectangles, polygons and linear slots: The position angle points to the first contour element.
4.27 Milling Cycles Parameters – milling Q Cycle type (= milling location). Open contour. If there is any overlapping, Q defines whether the first area (as of starting point) or the entire contour is to be machined. Q=0: Milling center on the contour (without TRC) Q=1: Machining at the left of the contour. If there is overlapping, G840 machines only the first area of the contour. Q=2: Machining at the right of the contour. If there is overlapping, G840 machines only the first area of the contour.
4.27 Milling Cycles Parameters – milling R Radius of approaching/departing arc (default: 0) R=0: Contour element is approached directly; feed to starting point above the milling plane, then vertical plunge. R>0: Tool moves on approaching/departing arc that connects tangentially to the contour element. R<0 for inside corners: Tool moves on approaching/ departing arc that connects tangentially to the contour element.
4.27 Milling Cycles Approach and departure: For closed contours, the point of the surface normal from the tool position to the first contour element is the point of approach and departure. If no surface normal intersects the tool position, the starting point of the first element is the point of approach and departure. For figures, use D and V to select the approach/depart. Cycle run for milling 1 Starting position (X, Z, C) is the position before the cycle begins. 2 Calculates the milling depth infeeds.
Direction of tool rotation TRC Up-cut milling (H=0) Mx04 Inside Climb milling (H=1) Inside Outside (Q=2) Cycle type Cutting direction Inside Direction of tool rotation TRC Up-cut milling (H=0) Mx03 Right Left (Q=3) Up-cut milling (H=0) Mx04 Left Right Left (Q=3) Climb milling (H=1) Mx03 Left Right Right (Q=3) Climb milling (H=1) Mx04 Right Cycle type Cutting direction Left Right (Q=3) Mx03 Left Climb milling (H=1) Mx04 Up-cut milling (H=0) Mx03 HEIDENHAIN CNC PILOT 42
4.27 Milling Cycles G840 – Deburring G840 deburrs when you program chamfer width B. If there is any overlapping of the contour, specify with Q whether the first area (as of starting point) or the entire contour is to be machined. Program only the parameters given in the following list. Parameters – deburring Q Cycle type (= milling location) Open contour Q=0: Milling center on the contour. Q0 deburrs the slot in one pass on the previously open or closed contour.
4.27 Milling Cycles Parameters – deburring R Radius of approaching/departing arc (default: 0) R=0: Contour element is approached directly; infeed to starting point above the milling plane, then vertical plunge. R>0: Tool moves on approaching/departing arc that connects tangentially to the contour element. R<0 for inside corners: Tool moves on approaching/ departing arc that connects tangentially to the contour element.
4.27 Milling Cycles Approach and departure: For closed contours, the point of the surface normal from the tool position to the first contour element is the point of approach and departure. If no surface normal intersects the tool position, the starting point of the first element is the point of approach and departure. For figures, use D and V to select the approach/departure element. Cycle run for deburring 1 Starting position (X, Z, C) is the position before the cycle begins.
4.27 Milling Cycles G845 – Calculating hole positions “G845 A1 ..” calculates the hole positions and stores them at the reference specified in “NF.” The cycle takes the diameter of the active tool into account when calculating the hole positions. Therefore, you need to insert the drill before calling “G845 A1 ..”. Program only the parameters given in the following list.
4.27 Milling Cycles G845 – Milling You can change the milling direction with the cutting direction H, the machining direction Q and the direction of tool rotation (see following table). Program only the parameters given in the following list.
4.27 Milling Cycles Parameters—Milling Plunge at pre-drilled position O=1: If “NF” is programmed: The cycle positions the milling cutter above the first pre-drilled hole; the tool plunges and mills the first area. If applicable, the cycle positions the tool to the next pre-drilled hole and mills the next area, etc. If “NF” is not programmed: The tool plunges at the current position and mills the area. If applicable, position the tool to the next pre-drilled hole and mill the next area, etc.
4.27 Milling Cycles Parameters—Milling Plunge in a reciprocating circular motion O=6, 7: The tool plunges at the plunging angle “W” and mills a circular arc of 90°. The cycle then mills along this path in the opposite direction. As soon as it reaches the milling depth “P,” the cycle switches to face milling. “WE” defines the arc center, “WB” the arc radius. O=6 – manually: The tool position corresponds to the center of the circular arc. The tool moves to the arc starting point and plunges.
4.27 Milling Cycles Cycle run 1 Starting position (X, Z, C) is the position before the cycle begins. 2 Calculates the number of cuts (infeeds to the milling planes, infeeds in the milling depths) and the plunging positions and paths for reciprocating or helical plunges. 3 Approaches to safety clearance and, depending on O, feeds to the first milling depth or approaches helically or on a reciprocating path, . 4 Mills a plane.
4.27 Milling Cycles Pocket milling, finishing G846 You can change the milling direction with the cutting direction H, the machining direction Q and the direction of tool rotation (see following table). Machining parameters – finishing NS Block number – reference to contour description P (Maximum) milling depth (infeed in the working plane) R Radius of approaching/departing arc (default: 0) R=0: Contour element is approached directly.
4.27 Milling Cycles Cycle run 1 Starting position (X, Z, C) is the position before the cycle begins. 2 Calculates the number of cutting passes (infeeds to the milling planes, infeeds in the milling depths). 3 Moves to the safety clearance and feeds to the first milling depth. 4 Mills a plane. 5 Retracts by the safety clearance, returns and cuts to the next milling depth. 6 Repeat steps 4 and 5 until the complete surface is milled. 7 Returns to retraction plane J.
4.27 Milling Cycles Thread milling, axial G799 Starting with software version 625 952-05: G799 mills a thread in existing holes. The cycle positions the tool on the end point of the thread within the hole. Then the tool approaches on "approaching radius R" and mills the thread. During this, the tool advances by the thread pitch F. Following that, the cycle retracts the tool and returns it to the starting point.
4.27 Milling Cycles Engraving on front face G801 G801 engraves character strings in linear or polar layout on the front face. The text to be engraved is entered in the “ID” box as a character string. Parameters ID Text. Text to be engraved () NS Character number. ASCII code of the character to be engraved X Starting diameter (polar coordinates) C Starting angle (polar coordinates) XK Starting point in Cartesian coordinates YK Starting point in Cartesian coordinates Z Milling floor.
4.27 Milling Cycles Engraving on lateral surface G802 G802 engraves character strings aligned linearly on the lateral surface. The text to be engraved is entered in the “ID” box as a character string. Parameters ID Text. Text to be engraved () NS Character number. ASCII code of the character to be engraved Z Starting point C Starting angle CY Starting angle as line dimension (reference: unrolled reference diameter) X Milling diameter. X position, infeed depth during milling.
Capital letters NS Character NS Character Numerals, diacritics NS Character 97 a 65 A 48 0 32 98 b 66 B 49 1 37 % Per cent sign 99 c 67 C 50 2 40 ( Opening parenthesis Special characters NS Character Meaning Blank space 100 d 68 D 51 3 41 ) Closing parenthesis 101 e 69 E 52 4 43 + Plus character 102 f 70 F 53 5 44 , Comma 103 g 71 G 54 6 45 – Minus sign 104 h 72 H 55 7 46 .
4.28 Assignment, Synchronization, Workpiece Transfer 4.28 Assignment, Synchronization, Workpiece Transfer Multichannel systems The CNC PILOT controls one slide per NC channel. Lathes with two or more slides are referred to as multichannel systems. Examples: Machines for full-surface machining with opposing spindles Multiple slide working on one workpiece Two or more workpieces machine in one working space. Such operations are programmed in one NC program.
4.28 Assignment, Synchronization, Workpiece Transfer Application: For full-surface machining, you describe the complete contour, machine the front face, rechuck the workpiece using an expert program, and then machine the rear face. To enable you to program rear-face machining in the same way as front-face machining (Z-axis orientation, arc rotational direction, etc.). Includes the expert program commands for converting and mirroring. Mirror the traverse paths and tool lengths in separate G30 commands.
4.28 Assignment, Synchronization, Workpiece Transfer Workpiece group G99 For two or more contours (workpieces) in one NC program, use CONTOUR Q.. (see “CONTOUR section” on page 143). G99 assigns the “Contour Q” to the following operations. The slide code before the NC block defines the slides that machine this contour. If G99 was not yet programmed (for example at the start of the program), all slides on contour 1.
. . . $1 N.. G62 Q2 H5 Slide $1 waits until slide $2 reaches the mark 5 . . . $2 N.. G62 Q1 H7 X200 Slide $2 waits until slide $1 reaches the mark 7 and the position X200 . . . Synchronization marking G162 G162 sets a synchronous mark. (Another slide programmed with G62 waits until the mark has been crossed.) The slide continues executing the NC program without a pause.
4.28 Assignment, Synchronization, Workpiece Transfer M97 Synchronous function Slides for which M97 is programmed wait until all slides have reached this block. Program run then continues. For complex machining operations (e.g. machining of several workpieces), M97 is programmed with parameters.
. . . N.. G397 S1500 M3 Speed of direction of rotation of master spindle N.. G720 C180 S4 H2 Q2 F-1 Synchronization of master spindle and slave spindle. The slave spindle precedes the master spindle by 180°. Slave spindle: Direction of rotation M4; rotational speed 750 $2 N.. G1 X.. Z.. . . . . . . C-angle offset G905 G905 measures the angular offset of workpiece transfer with rotating spindle. The sum of angle C and the angle offset goes into effect as the zero point shift of C axis.
4.28 Assignment, Synchronization, Workpiece Transfer Measuring angular offset during spindle synchronization G906 G906 writes the angular offset between the master spindle and the slave spindle into variable V921. Programming: Program G906 only for active angular synchronization – both chucks must be closed. Program G906 in a separate NC block. Program a G909 (interpreter stop) before processing V921.
4.28 Assignment, Synchronization, Workpiece Transfer Programming “traverse to a fixed stop”: U U U U Position the slide at a sufficient distance before the fixed stop. Use a moderate feed rate (< 1000 mm/min) Program G916 or G916 Hx D1 in the G1 positioning block Program G1 .. as follows: Target position is behind the fixed stop Move only one axis Activate a per-minute feed rate (G94) Example of traversing to a fixed stop: . . . $2 N.. G94 F200 $2 N.. G0 Z20 Pre-position slide 2 $2 N..
4.28 Assignment, Synchronization, Workpiece Transfer Example of tailstock function . . . $2 N.. G94 F800 $2 N.. G0 Z20 Pre-position slide 2 $2 N.. G916 H250 D1 G1 Z-10 Activate the tailstock function—contact force 250 daN . . . $2 N.. G916 D2 G1 Z100 As of software version 625 952-04: Check whether the end point is reached: G916 D3 On reaching the fixed stop, the CNC PILOT stops the slide and saves the stop position in the variables V901 to V918.
4.28 Assignment, Synchronization, Workpiece Transfer Controlled parting using lag error monitoring G917 G917 monitors the path of traverse. The controlled parting function (cut-off control) prevents collisions caused by incomplete parting processes. Application Parting control Move the workpiece in the positive Z direction after it has been cut off. If a lag error occurs, the workpiece is defined as no cut-off.
4.28 Assignment, Synchronization, Workpiece Transfer Programming: Program G917 and G1 in one block Program G1 .. as follows: For controlled parting: Path > 0.
4.28 Assignment, Synchronization, Workpiece Transfer Programming: Program constant surface speed G96 Program G991 and G1 (path before the parting operation or return path) in one block. Result in V300: 0: Not cut off 1: Cut off Parting control with G917 is preferable to G991. Tool breakage results in speed differences which in turn might affect the monitoring result. It is therefore advisable to monitor the reverse path too.
4.29 Contour Follow-Up 4.29 Contour Follow-Up Automatic contour follow-up is not possible with program branches or repetitions. In these cases you control the contour follow up with the following commands. Saving/loading contour follow-up G702 G702 saves the current contour or loads a saved contour. Program G702 for one slide. Parameters Q Save/load contour Q=0: Saves the current contour. The contour follow-up is not affected. Q=1: Loads the saved contour.
4.29 Contour Follow-Up K default branch G706 During program conversion it is unknown which branch of an IF or SWITCH instruction will be run. The initialization of global information such as contour follow-up, rotational speed, incremental positions, etc. is therefore suspended. With G706 you define the default branch of an IF or SWITCH instruction. This branch is then used to initialize the global information.
4.30 In-process and Post-process Measuring 4.30 In-process and Post-process Measuring In-process measuring A touch-trigger probe is a prerequisite. Application example: With in-process measurement you can monitor tool wear. If you use the tool life monitoring, worn-out tools are identified as such and the CNC PILOT replaces it. Example: In-process measuring . . . N.. T.. Insert the touch probe N.. G910 Activate in-process measurement N.. G0 .. Pre-position the touch probe N.. G912 N.. G1 ..
4.30 In-process and Post-process Measuring Actual value capture for in-process measurement G912 With G912, when the probe stylus is deflected, the CNC PILOT stops and writes the position into variables V901 to V920. The remaining path of traverse is deleted. You can use Q to influence the reaction to “touch probe not triggered.
4.30 In-process and Post-process Measuring Post-process measurement G915 Post-process measuring means that the workpiece is measured outside the lathe and that the measurement results are transferred to the CNC PILOT. Prerequisites: The measuring device and the CNC PILOT are connected by serial interface Communications protocol: 3964-R The measuring device determines whether measured values or compensation values are transferred. The measurement results are evaluated by the NC program.
4.30 In-process and Post-process Measuring Example: Using a measuring result as compensation value . . . N2 T1 Finish the outside contour . . . N49 ... End the workpiece machining N50 G915 H1 Request the measurement results... N51 IF {V940==1} ...if there are any results N52 THEN N53 V {D1 [X] = D1 [X] + V941} Add result to compensation value D1 N54 ENDIF . . . Example: Monitoring for tool breakage . . . N2 T1 Rough the outside contour . . . N49 ...
4.31 Load Monitoring 4.31 Load Monitoring Fundamentals of load monitoring The load monitoring function checks the performance and work values of the drives and compares them to limit values which have been determined during a reference machining cycle. The CNC PILOT considers two limit values: If the first limit value is exceeded, the tool is marked as worn out and the tool life monitoring inserts the replacement tool (see “Tool programming” on page 121).
4.31 Load Monitoring Specifying the monitoring zone G995 G995 defines the monitoring zone and the axes to be monitored.
4.32 Other G Functions 4.32 Other G Functions Period of dwell G4 With G4, the CNC PILOT interrupts the program run for the time F before executing the next program block. If G4 is programmed together with a path of traverse in the same block, the dwell time only becomes effective after the path of traverse has been executed. Parameters F Dwell time [sec] (0 < F <= 999) Precision stop G7 G7 switches precision stop on. It is a modal function.
G15 tilts the rotary axis to the given angle and moves at feed rate to the programmed position. Parameters A, B Angle – end point of rotary axis X, Y, Z End point of principal axis (X diameter value) U, V, W End point of secondary axis B Y Z Z Y X X Use G15 to move to position, not to machine Switch off protection zone G60 G60 is used to cancel protection zone monitoring. G60 is programmed before the traversing command to be monitored or not monitored.
4.32 Other G Functions Chucking equipment in simulation G65 G65 displays the selected chucking equipment in the simulation graphics. G65 needs to be programmed separately for each chuck. G65 H.. without X, Z cancels the chuck in the simulation graphics.
4.32 Other G Functions Component position G66 The simulation can only depict tool positions and movements if the X and Z position, or the X, Y and Z position, is known. For slides that move in only one direction (for example a parting slide), add the missing coordinates with G66. In “Shift” you can include a zero point shift. On the basis of these data, the CNC PILOT simulates slides with one axis.
4.32 Other G Functions Move lag error G718 G718 prevents the automatic updating of nominal control position values with the axis position data (e.g. when traversing to a fixed stop, or after canceling and re-enabling a controller release). Parameters Q On / Off Q=0: Off Q=1 on, the servo lag stays saved Application: Before activating a master-slave axis coupling. Use G718 only in “expert programs.
4.32 Other G Functions Feed rate override 100% G908 G908 sets the feed override for traverse paths (G0, G1, G2, G3, G12, G13) block by block to 100%. Program G908 and the traverse path in the same NC block. Interpreter stop G909 The CNC PILOT pre-interprets approx. 15 to 20 NC blocks. If variables are assigned shortly before the evaluation, “old values” would be processed. G909 stops the pre-interpretation. The NC blocks are processed up to G909. Only after G909, are the subsequent NC blocks processed.
4.32 Other G Functions Deactivate zero-point shifts G920 G920 deactivates the workpiece zero point and zero-point shifts. Traverse paths and position values are referenced to the distance tool tip – machine zero point. Deactivate zero-point shifts, tool lengths G921 G921 deactivates the workpiece zero point, zero point shifts and tool dimensions. Traverse paths and position values are referenced to the slide reference point – machine zero point. T no.
4.32 Other G Functions Transferring magazine compensation values G941 G941 writes in the following variables the compensation values of the magazine tool to be deposited and to be fetched. The compensation values describe the deviations of the individual magazine pockets from the standard dimensions. In V800, write the number of the tool to be deposited, and use G940 to find the tool to be fetched before you program G941.
4.32 Other G Functions Activate zero-point shifts, tool lengths G981 G981 activates the workpiece zero point, all zero-point shifts and the tool dimensions. Traverse paths and position values are referenced to the distance of the tool tip to the workpiece zero point, while taking the zero point shifts into consideration. Sleeve monitoring G930 G930 activates/deactivates the sleeve monitoring. When the monitoring is activated, the maximum contact force for one axis is defined.
4.32 Other G Functions Shaft speed with V constant G922 Available as of software version 625 952-05. With constant surface speed (V constant), the spindle speed depends on the X position of the tool tip. With G922 you program whether this procedure should apply to G0 paths, as well. G922 applies to the spindle assigned to the slide.
4.33 Data Input and Data Output 4.33 Data Input and Data Output Output window for # variables WINDOW WINDOW (x) opens an output window with x lines. The window is opened as a result of the first input/output. WINDOW (0) closes the window. Syntax: WINDOW(line number) (0 <= line number <= 10) Example: . . . N.. WINDOWS(8) . . . N.. INPUT(input diameter: ,#1) The standard window comprises 3 lines. You do not need to program it. . . . N.. PRINT(output diameter: ,#1) . . .
4.33 Data Input and Data Output Output of # variables PRINT PRINT can be used to output texts and variable values during program interpretation. You can program a succession of several texts and # variables. Syntax: PRINT(text,variable, text,variable, ..) V variable simulation V variables and all data input/output are included during simulation. The V variables can be assigned values. Thus all branches of your NC program can be tested.
4.33 Data Input and Data Output Input of V variables INPUTA With INPUTA you program the input of V variables that are evaluated during program interpretation. Syntax: INPUTA(Text,variable) You define the input text and the number of the variable. The CNC PILOT requests the input of the variable value during the execution of the command. The input is assigned to the variable and the program run continues. The CNC PILOT displays the input after having completed the INPUT command.
4.34 Programming with Variables 4.34 Programming with Variables The CNC PILOT supports NC programs before the program run. The system therefore differentiates between two types of variables: Syntax Mathematical functions # variables are evaluated during NC program interpretation. V variables (or events) are evaluated during NC program run.
4.34 Programming with Variables # variables The CNC PILOT uses value ranges to define the scope of variables: #0 to #29 Channel-dependent, global variables can be used for each slide (NC channel). Identical variable numbers on different slides are no problem. The variables are retained after the program has been completed and can be processed by the following NC program. #30 to #45 Channel-independent, global variables are available once within the control.
4.34 Programming with Variables NC information in # variables #787 Reference diameter for lateral surface machining (G120) #788 Spindle holding the workpiece (G98) #790 Oversize G52-Geo 0: Do not include 1: Include #791..#792 G57 oversizes X, Z #793 G58 oversize P #794..
4.
4.34 Programming with Variables Requests and assignments Interrogating sequential events: Syntax: V{Ex[1]} x = event: 20 to 59, 90 20: Life of this tool has expired (global information) 21 to 59: Tool life of this tool has expired 90: Start block search (0=not active; 1=active) Interrogate external events: Syntax: V{Ex[y]} x = slide 1 to 6 y = bit: 1 to 16 Interrogates bit of the event for 0 or 1. The meaning of the external event is determined by the machine manufacturer.
4.34 Programming with Variables Sequential events and tool life monitoring The tool life monitoring function and the function for searching the start block trigger sequential events. Assign this clock event to the tool ("tool life management"—Manual control mode). When a tool is worn-out, event 20 (global information) and event 1 are triggered. Event 1 identifies the worn-out tool. When the last tool of an tool interchange chain is worn out, event 2 is also triggered.
4.34 Programming with Variables Information in V variables V901 to V920 G901, G902, G903, G912 and G916 write the positions into the variables: V901 to V903: Axis X, Z, Y of slide 1 V904 to V906: Axis X, Z, Y of slide 2 V907 to V909: Axis X, Z, Y of slide 3 V910 to V912: Axis X, Z, Y of slide 4 V913 to V915: Axis X, Z, Y of slide 5 V916 to V918: Axis X, Z, Y of slide 6 V919: C axis 1 V920: C axis 2 X values are saved as radius values.
4.35 Conditional Block Run 4.35 Conditional Block Run Program branching IF..THEN..ELSE..ENDIF A conditional branch consists of the elements: IF, followed by a condition. The condition includes a variable or mathematical expression on either side of the relational operator. THEN. If the condition is fulfilled, the THEN branch is executed ELSE. If the condition is not fulfilled, the ELSE branch is executed ENDIF concludes the conditional program branch.
4.35 Conditional Block Run WHILE..ENDWHILE program repeat A program repeat consists of the elements: WHILE, followed by a condition. The condition includes a variable or mathematical expression on either side of the relational operator. ENDWHILE concludes the conditional program repeat. NC blocks programmed between WHILE and ENDWHILE are executed repeatedly for as long as the condition is fulfilled.
4.35 Conditional Block Run SWITCH..CASE—program branching The switch statement consists of the elements: SWITCH, followed by a variable. The content of the variables is interrogated in the following CASE instruction. CASE x: The CASE branch is run with the variable value x. CASE can be programmed repeated times. DEFAULT: This branch is executed if no CASE instruction matched the variable value. DEFAULT can be omitted.
BREAK N.. ENDSWITCH 4.35 Conditional Block Run N.. . . . N.. N.. DEFAULT G0 XI30 . . . N.. BREAK N.. ENDSWITCH . . .
4.35 Conditional Block Run Skip level /.. An NC block with prepended skip level is not executed if the skip level is active. Activate/deactivate the skip levels in Automatic mode. In addition, you can use the skip cycle (deletion cycle) (set-up parameter 11: deletion level/cycle). Skip cycle x activates the skip level every xth time. Example: /1 N 100 G... N100 .. is not executed with active skip cycle 1. Slide code $.. An NC block preceded by a slide code is executed only for the indicated slide.
4.36 Subprograms 4.36 Subprograms Subprogram call: L"xx" V1 The subprogram contains the following elements: L: Identifying letter for subprogram call "xx": Name of the subprogram – file name for external subprograms (max. 8 letters or numbers) V1: Identification code for external subprograms—omitted for local subprograms Note on using subprograms: External subprograms are defined in a separate file. They are called from any main program, other subprograms, or from TURN PLUS.
4.36 Subprograms Dialog texts in subprogram call You can define up to 19 parameter descriptions that precede/follow the input fields in an external subprogram. The CNC PILOT automatically sets the unit of measure for parameter values to the metric system or inches. pn: Parameter designations (la, lb, ...) n: Conversion number for units of measurement The parameter descriptions can be positioned within the subprogram as desired. 0: Non-dimensional 1: mm or inches 2: mm/rev or in.
4.36 Subprograms Help graphics for subprogram calls With help graphics you illustrate the calling parameters of subprograms. The CNC PILOT places the help graphics to the left next to the dialog box of the subprogram call. As of software version 625 952-04: If you append an underscore _ and the input field name to the name of the help graphic, the CNC PILOT will display a separate graphic for that input field.
4.37 M Commands 4.37 M Commands M commands for program-run control The effect of machine commands depends on the configuration of your machine. On your lathe, other M commands may apply for the listed functions. Refer to your machine manual. Overview: M commands for program-run control M00 Program stop The program run stops. Cycle start resumes the program run. M01 Selectable stop If the “Selectable stop” soft key is active in Automatic mode, the program run stops with M01.
4.37 M Commands Machine commands The effect of machine commands depends on the configuration of your machine. The following table lists the M commands used on most machines. M commands as machine commands M03 Main spindle on (cw) M04 Main spindle on (ccw) M05 Main spindle stop M12 Lock main spindle brake M13 Release main spindle brake M14 C axis on M15 C axis off M19..
4.38 Lathes with Multiple Slides 4.38 Lathes with Multiple Slides Multi-slide programming Multiple slide programming see: Assignments Program head Page 136 The “slide” input field has the following meaning: No entry: The NC program is run on every slide. One slide number: The NC program is run on this slide. Two or more slide numbers: The NC program is run on the given slides. Enter the slide numbers in succession and without separators.
see: End of program Every active slide has to execution an M30/M99 to end the NC program. We recommend programming M30/M99 without slide designation. Subroutines Page 327 Subprogram call: The subprogram is called for the slide whose designation is programmed. Subprogram end: The calling slide must conclude the subprogram with RETURN. We recommend programming the RETURN without slide designation.
4.38 Lathes with Multiple Slides Program run Block display: You can configure the block display for multiple slides. The cursor displays the active NC block for each slide. Start-block search for multi-slide programs: U U U U U U Activate the block display for all slides involved (channels). Select the start block for the first slide. Use the slide-switch key to switch to the block display of the next slide. Select the start block for this slide. “Accept” the start blocks. Start the machining.
4.38 Lathes with Multiple Slides . . .
4.38 Lathes with Multiple Slides DIN subprogram for steady-rest positioning %LUE_POS.NCS $2 N 1 G0 Z#__LA Position the steady rest $2 N 2 M300 Close the steady rest . . . Further steady rest commands as required $2 RETURN DIN subprogram for steady-rest parking %LUE_PARK.NCS $2 N 1 M301 Open the steady rest $2 N 2 G701 Z1200 Steady rest to park position . . . Further steady rest commands as required $2 RETURN Traveling steady rest The tool and the steady rest are pre-positioned (N3 to N17).
4.38 Lathes with Multiple Slides DIN program for a traveling steady-rest %LUENETTE.NC PROGRAMMKOPF [PROGRAM HEAD] #SCHLITTEN $1$2 [SLIDE] Slide 1: tool carrier; slide 2: steady rest . . . REVOLVER 1 [TURRET] T 2 ID"111-80-080.1" T 4 ID"121-55-040.1" . . . BEARBEITUNG [MACHINING] N 1 G59 Z1000 . . . $1$2 N 2 M97 Synchronize slides 1 and 2 ZUORDNUNG $1 [ASSIGNMENT] N 3 G14 Q0 Slide 1: Prepare operation N 4 T4 N 5 G95 F0.5 G96 S200 M4 N 6 G0 X300 Z10 . . .
4.38 Lathes with Multiple Slides Two slides work simultaneously In a first roughing operation the workpiece is machined to the point at which it can be recess turned. The recessing (N26 to N34) is conducted parallel to further roughing operations (N20 to N25) Slide 1 defines the cutting speed. For this reason it is moved after the roughing operation to a parking position that allows an adequate cutting speed.
4.38 Lathes with Multiple Slides DIN program with dual-slide machining %12GLEICH.NC #SCHLITTEN $1$2 [SLIDE] . . . REVOLVER 1 [TURRET] T 2 ID"111-80-040.1" Roughing tool . . . REVOLVER 2 [TURRET] T 4 ID"151-0.15-0.5" Recessing tool . . . ROHTEIL [WORKPIECE BLANK] N 1 G20 X30 Z80 K2 FERTIGTEIL [FINISHED PART] N 2 G0 X0 Z0 N 3 G1 X16 B-2 N 4 G1 Z-20 N 5 G1 X28 B1 N 6 G1 Z-50 N 7 G22 Z-40 II-4 K-45 B-0.5 R0.2 . . .
4.38 Lathes with Multiple Slides N 21 G820 NS3 NE3 P2 I0.5 K0.3 V3 N 22 G47 P3 N 23 G810 NS4 NE6 P4 I0.5 K0.3 Q2 N 24 M109 N 25 G0 X60 Z10 ZUORDNUNG $2 [ASSIGNMENT] Slide 1: Waiting position (provides cutting speed) Slide 2: Recessing parallel to roughing N 26 T4 N 27 G95 F0.2 N 28 G0 X32 Z-44 N 29 M108 N 30 G47 P3 N 31 G866 NS7 I0.
4.38 Lathes with Multiple Slides DIN program with two consecutive slides %12NACH.NC PROGRAMMKOPF [PROGRAM HEAD] #SCHLITTEN $1$2 [SLIDE] . . . REVOLVER 1 [TURRET] T 2 ID"111-80-040.1" Roughing tool . . . T 4 ID"121-55-040.1" Finishing tool . . . N 1 G20 X30 Z80 K2 FERTIGTEIL [FINISHED PART] N 2 G0 X0 Z0 N 3 G1 X16 B-2 N 4 G1 Z-20 N 5 G1 X28 B1 N 6 G1 Z-50 . . .
4.38 Lathes with Multiple Slides $1$2 N 21 M97 Slide 2 waits for slide 1 ZUORDNUNG $2 [ASSIGNMENT] Slide 2: Finishing N 22 G59 Z200 N 23 T4 N 24 G95 F0.
4.38 Lathes with Multiple Slides FERTIGTEIL [FINISHED PART] N 2 G0 X0 Z0 N 3 G1 X50 B8 N 4 G1 Z-150 B6 N 5 G1 X100 B5 N 6 G1 Z-200 . . . BEARBEITUNG [MACHINING] $1$2 N 7 M97 Synchronize slides 1 and 2 ZUORDNUNG $1$2 [ASSIGNMENT] Both slides: Tool change and pre-positioning N 8 G14 Q0 N 9 T1 N 10 G59 Z300 N 11 G0 X120 Z5 G95 F1 $1$2 N 12 M97 $1 Synchronize slides 1 and 2 N 13 G96 S300 M4 N 14 G810 NS4 NE5 P5 I0.5 K0.
4.39 Full-surface machining 4.39 Full-surface machining Fundamentals of full-surface machining In "full-surface machining," the front and rear ends can be machined in one NC program. The CNC PILOT supports full-surface machining for all common machine designs. The features include angle-synchronous part transfer with rotating spindle, traversing to a stop, controlled parting, and coordinate transformation. This ensures efficient fullsurface machining and simple programming.
4.39 Full-surface machining Programming of full-surface machining When programming a contour on the rear face, be sure to consider the orientation of the XK axis (or X axis) and rotational direction of arcs. Insofar as you use drilling and milling cycles, there are no special aspects to rear-face machining, since these cycles refer to predefined contours. For rear-face machining with the basic commands G100 to G103 the same conditions apply as for rear-face contours.
4.39 Full-surface machining Full-surface machining with opposing spindle G30: The expert program activates the mirroring of the Z axis and the conversion of the arcs (G2, G3, ..). The arcs must be converted for turning operations and operations with the C axis. G121: The expert program shifts the contour and mirrors the coordinate system (Z axis). Further programming of G121 is normally not required for machining the rear face after rechucking.
4.39 Full-surface machining Full-surface machining on machines with opposing spindles PROGRAMMKOPF [PROGRAM HEAD] #SCHLITTEN $1$2 [SLIDE] . . . REVOLVER 1 [TURRET] T1 ID “512-600.10“ T2 ID “111-80-080.1” T3 ID “514-600.10” T4 ID “121-55-040.1” T6 ID “115-80.080” T8 ID “125-55.
4.39 Full-surface machining $1 N29 G65 H2 X100 Z-99 D1 Q4 $1 N30 G14 Q0 $1 N31 G26 S2500 $1 N32 T2 . . . $1 N62 G126 S4000 Milling – contour – outside – front face $1 N63 M5 $1 N64 T1 $1 N65 G197 S1485 G193 F0.05 M103 $1 N66 M14 $1 N67 M107 $1 N68 G0 X36.0555 Z3 $1 N69 G110 C146.31 $1 N70 G147 I2 K2 $1 N71 G840 Q0 NS15 NE18 I0.5 R0 P1 $1 N72 G0 X31.
4.39 Full-surface machining Full-surface machining with single spindle G30: Normally not required G121: The expert program mirrors the contour. Further programming of G121 is normally not required for machining the rear face after rechucking. Example: Describes the machining of the front and rear face, using one NC program. The workpiece is first machined on the front face; then it is rechucked manually. The rear face is machined subsequently.
4.39 Full-surface machining N24 G103 XK-8 YK3.8038 R6 I-5 B0 N25 G101 XK-12 YK-10 N26 G309 BEARBEITUNG [MACHINING] N27 G59 Z233 Zero point shift for 1st setup N28 G65 H1 X0 Z-135 D1 Display chucking equipment of 1st setup N29 G65 H2 X100 Z-99 D1 Q4 . . .
4.40 DIN PLUS Program Example 4.40 DIN PLUS Program Example Example of a subprogram with contour repetitions Contour repetitions, including saving of the contour PROGRAMMKOPF [PROGRAM HEAD] #SCHLITTEN $1 [SLIDE] REVOLVER 1 [TURRET] T2 ID “121-55-040.1“ T3 ID “111-55.080.1” T4 ID “161-400.2” T8 ID “342-18.0-70” T12 ID “112-12-050.1” BLANK N1 G20 X100 Z120 K1 FERTIGTEIL [FINISHED PART] N2 G0 X19.2 Z-10 N3 G1 Z-8.5 B0.35 N4 G1 X38 B3 N5 G1 Z-3.05 B0.2 N6 G1 X42 B0.5 N7 G1 Z0 B0.2 N8 G1 X66 B0.5 N9 G1 Z-10 B0.
4.40 DIN PLUS Program Example N18 G14 Q0 N19 T8 N20 G97 S2000 M3 N21 G95 F0.2 N22 G0 X0 Z4 N23 G147 K1 N24 G74 Z-15 P72 I8 B20 J36 E0.1 K0 N25 G14 Q0 N26 T3 N27 G96 S300 G95 F0.35 M4 N28 G0 X72 Z2 N29 G820 NS8 NE8 P2 K0.2 W270 V3 N30 G14 Q0 N31 T12 N32 G96 S250 G95 F0.22 N33 G810 NS7 NE3 P2 I0.2 K0.1 Z-12 H0 W180 Q0 N34 G14 Q2 N35 T2 N36 G96 S300 G95 F0.
4.40 DIN PLUS Program Example N56 G1 Z-10 B0.5 N57 G1 X17 N58 G0 X72 N59 G0 X80 Z-10 G40 Turn TRC off N60 G14 Q0 N61 G56 Z-14.
4.41 DIN PLUS Templates 4.41 DIN PLUS Templates A template is a predefined NC code block that is adapted to your lathe and is integrated in the NC program. That reduces the programming effort while helping you to standardize. The CNC PILOT differentiates between: The starting template for making a new NC program. Structure templates, which support you when programming complex processes. The templates are saved in the NCPS directory under the name DINSTART.BEV or VORLAGEx.BEV (x: 1 to 9).
4.41 DIN PLUS Templates Design of structure templates When you call a structure template, the NC blocks of the template are loaded into the NC program. The blocks of the template have been designed in such a way that you can influence the NC program by adding or omitting entries. This is done by using transfer parameters. In addition, the CNC PILOT adds the block numbers.
4.41 DIN PLUS Templates Editing structure templates U U U U Log in as “System Manager” Select “Prog > Load > Template” in the main menu. Choose Vorlagex from the template list. Edit the template using the free editing function and then save. Help graphics for structure templates Help graphics illustrate the transfer parameters of structure templates. The CNC PILOT places the help graphics to the left next to the dialog box. The help graphic is named after the template it illustrates.
4.41 DIN PLUS Templates Template example Example VORLAGEx.BEV %VORLAGEX.BEV Work block for slide 1 [//] Declare transfer parameters [/LB; S=TOOL TO SPINDLE0 ;E=S0/] [/LC; S=TOOL TO SPINDLE3 ;E=S0/] [/LF; S=G FUNCTION [/LH; S=MAKE SP [/J; S=SP NAME /] ;E=G/] yes/no decision G function ;E=S0/] Transfer the entered text [//] [[#__LH]] [===== SUBPROGRAM ====] [[#__LH]] UNTERPROGRAMM “#__J“ [SUBPROGRAM] [[#__LB]] G714 ID ““ [TOOL] Slide 1 to spindle 0 [[#__LB]] G96 S100 G95 F0.
4.41 DIN PLUS Templates From this data, the CNC PILOT generates the following program sequence: [===== SUBPROGRAM ====] UNTERPROGRAMM “SCHRU1“ [SUBPROGRAM] Call the subprogram with the entered SP name N 2 G714 ID ““ [TOOL] Slide 1 to spindle 3 N 3 G396 S100 G395 F0.05 M303 [TECHNOLOGY] N 4 G0 [APPROACH POSITION] N 5 M107 [COOLANT ON] N 6 G47 P3 [SAFETY CLEARANCE] N 7 G810 NS.. NE.. ...
4.42 Connection between Geometry and Machining Commands 4.
4.42 Connection between Geometry and Machining Commands C-axis machining – front/rear face Function Geometry Machining Individual elements G100 to G103 G840 Contour milling G845/G846 Pocket milling, roughing/finishing Figures G301 Linear groove G302/G303 Circular slot G304 Full circle G305 Rectangle G307 Eccentric polygon G840 Contour milling G845/G846 Pocket milling, roughing/finishing Hole G300 G71 Simple drilling cycle G72 Counterboring, countersinking, etc.
Graphic Simulation HEIDENHAIN CNC PILOT 4290 361
5.1 Simulation Mode of Operation 5.1 Simulation Mode of Operation The Simulation mode shows a graphic representation of programmed contours, the paths of traverse and cutting operations. The CNC PILOT shows the working space, tools and chucking equipment true to scale. Check machining operations with the C axis in the supplementary windows (front/surface and side view windows). For complex NC programs with branches, variable calculations, external events, etc.
5.
5.1 Simulation Mode of Operation Graphic elements Coordinate systems: The zero point of the coordinate system corresponds to the workpiece zero point. The arrows of the X and Z axes point in the positive direction. If the NC program is machining more than one workpieces, the coordinate systems of all required slides are displayed. Workpiece blank depiction Programmed: Programmed blank Not programmed: standard blank from control parameter 23.
5.
5.1 Simulation Mode of Operation Displays for contours: If several contours are defined in the NC program, the simulation displays the corresponding contour symbols. Contour symbols Information of the contour symbols: Qn (n: 1..4): Contour n Position of the coordinate system The symbol of the selected contour is marked The simulation window displays the coordinate system of the selected contour. Selection of a contour U U Select “Setup > Contour selection.
5.1 Simulation Mode of Operation Path display Rapid paths are shown as a broken white line. Feed paths are displayed either as a line or as a cutting trace, depending on the soft-key setting: Line display: A solid line describes the path of the theoretical tool tip (wire-frame graphics) The wire frame display is particularly convenient if you only need a quick overview of the proportioning of cuts. The path of the theoretical tool tip, however, is not identical with the contour of the workpiece.
5.1 Simulation Mode of Operation Simulation window With the simulation windows described in the following you check not only the turning work but also the drilling and milling operations. Turning window: The turning contour is depicted in the XZ coordinate system. Front window: The contour and traverse paths are shown in the XY plane, taking the spindle position into account. The spindle position 0° is located on the positive X-axis (designation: XK).
5.1 Simulation Mode of Operation Setting the simulation window Window selection dialog box: U Select “Set up > Window”: The CNC PILOT opens the dialog box for the settings listed below. Set: The window combination The path display in the supplementary windows: The front window, surface window, and side view are considered supplementary windows. The following setting specifies whether the simulation depicts traverse paths in the windows.
5.1 Simulation Mode of Operation Configuring the simulation Slide setting: U Select “Set up > Slide”: The CNC PILOT opens the “slide settings” dialog box for the settings listed below. Path display for all slides: The simulation shows the paths of all slides. Path display for current slide: The simulation shows the paths of the selected slide. Slide position of slide x: The simulations shows the paths of the slide in front of / behind the workpiece.
5.1 Simulation Mode of Operation Adjusting the section (zoom function) In the stopped condition, you can magnify/reduce the detail section with the zoom function Zoom settings by keyboard: U Activate the magnify function The red rectangle indicates the new section. If several simulation windows are open: U Choose the window. U Adjust the section: To magnify, use the PgDn key To reduce, use the PgUp key To move the frame, use the arrow keys U Exit the zoom function.
5.1 Simulation Mode of Operation Errors and warnings Warnings that occur during the interpretation of an NC program are displayed in the header. You see these warnings during a simulation stop or after the simulation: U Select “Set up > Warnings” U If there are two or more: Press ENTER to switch to the next message The CNC PILOT deletes a warning after you have confirmed the corresponding message with ENTER. The system stores a maximum of 20 warnings.
5.1 Simulation Mode of Operation Simulation mode You can set by soft key whether the simulation will be run continuously or blockwise. U Single block: Stop after every NC source block U Basic block Contour simulation: Stop after every contour element Machining or motion simulation: Stop after every traverse path U Without stop (single block and basic block soft keys are not pressed): The simulation is conducted without stop. U Menu item “Stop”: The simulation stops.
5.2 Contour Simulation 5.2 Contour Simulation Functions of the contour simulation Contour simulation presupposes that the blank or finished part contour (blank or finished part definition, auxiliary contours) is programmed. If the blank or finished part contours have not yet been completely programmed, they are displayed as completely as possible. The contour-simulation function allows you to: Select between “section” or “view” graphics.
5.2 Contour Simulation Contour dimensioning Position the cursor: For element or point dimensioning, position the cursor (small red square) as follows: U Cursor left/right: Changes to the next contour point U Cursor up/down: Changes the contour (for example, between blank and finished contour) U Changes to the next simulation window (prerequisite: there are contours on the reference planes). Element dimensioning U Select “Dimension. > Element dimension.
5.3 Machining Simulation 5.3 Machining Simulation Checking the workpiece machining The machining simulation function allows you to: Check the traverse paths of the tool Check the number of cutting passes Measure the machining time Monitor protection zone and limit switches Display and set variables Save the machined contour You can change the speed of the machining simulation with control parameter 27.
5.3 Machining Simulation Protection zone and limit switch monitoring (machining simulation) You set the monitoring of protection zones and limit switch as follows: U U U “Set up > Protection zone > Monitoring off”: The protection zones/ limit switches are not monitored. Select “Set up > Protection zone > Monitoring with warning”: The CNC PILOT registers protection-zone or limit-switch violations and treats them as warnings. The NC program is simulated up to the end of program.
5.3 Machining Simulation Contour checking With the functions of the “Contour” menu you can adapt the contour to the progress of machining, or switch to contour dimensioning or 3D view. Contour follow-up: U Select “Contour > Contour follow-up”: The simulation deletes all previously depicted traverse paths and updates the contour according to the simulated progress of machining. The CNC PILOT takes the blank part as a basis and accounts for each cut.
5.3 Machining Simulation Displaying the tool tip reference point In the machining simulation, the simulation depicts the tool tip reference point with very high magnification. You can also derive the tool orientation from it.
5.4 Motion Simulation 5.4 Motion Simulation Real-time simulation The motion simulation depicts the workpiece blank material as a “filled surface” and “machines” it during simulation by “erasing” the material (erasing graphics). The tools move at the programmed feed rate (program-run graphics). You can interrupt the motion simulation at any time, even during simulation of an NC block. The display below the simulation window indicates the target position of the current path.
5.4 Motion Simulation Protection zone and limit switch monitoring (motion simulation) You set the monitoring of protection zones and limit switch as follows: U U U “Set up > Protection zone > Monitoring off”: The protection zones/ limit switches are not monitored. Select “Set up > Protection zone > Monitoring with warning”: The CNC PILOT registers protection-zone or limit-switch violations and treats them as warnings. The NC program is simulated up to the end of program.
5.5 3-D View 5.5 3-D View Influencing the 3-D view In the 3-D view the CNC PILOT shows the workpiece in its simulated condition. If you call the 3-D view from the main menu or from the contour simulation, the finished part is depicted. The 3-D view includes contours machined by turning, but not for C or Y or B operations.
5.6 Debugging Functions 5.6 Debugging Functions Simulation with starting block If a start block is defined, the simulation converts the NC program without displaying the traverse to the starting block. Setting the start block: U Select “Debug > Set starting block”: The simulation opens the “Set start block” dialog box. U Enter the block number U Select “New”: The CNC PILOT simulates the NC program up to the starting block and stops. U Select “Continue”: The CNC PILOT resumes the simulation.
5.6 Debugging Functions Displaying variables Permanent variables display: Instead of the NC source block, the simulation shows four “selected variables” below the simulation window. Select the variables: U Select Debug > Display variables > Set display: The simulation opens the “Selection of display” dialog box.
5.6 Debugging Functions Editing variables For complex NC programs with branches, variable calculations, events, etc., you simulate all inputs and events to test all program branches.
5.7 Checking Multi-channel Programs 5.
Time Calculation During machining or motion simulation, the CNC PILOT calculates the productive and non-productive times. The display appears in the “time calculation” table The table shows the simulation of the machining times, idle times and total times (green: machining times; yellow: idle times). Each line represents the use of a new tool (for each tool call with T). If there are more table entries than fit on a screen page, you can call further time data with the arrow keys and PgUp/PgDn.
5.8 Time Calculation, Synchronous Point Analysis Synchronous point analysis The synchronous point analysis shows the chronological history of machining and the interdependency of the slides. This helps you to organize and optimize a multi-channel program.
TURN PLUS HEIDENHAIN CNC PILOT 4290 389
6.1 TURN PLUS Mode of Operation 6.1 TURN PLUS Mode of Operation TURN PLUS enables you to describe the workpiece blank and finished part in a graphic-interactive environment. Then you can have the working plan generated fully automatically or generate it yourself interactively. The result is a commented and structured NC program.
6.1 TURN PLUS Mode of Operation You can use part of the functions and continue working in DIN PLUS (example: Define a contour using TURN PLUS and program the machining operation in DIN PLUS). Alternately, you can optimize the DIN PLUS program generated by TURN PLUS. The working plan generation uses the tool/chucking equipment and the technological information contained in the respective database. Therefore, make sure that the database contains a correct description of the operating resources.
6.1 TURN PLUS Mode of Operation To generate a DIN PLUS program: U U U Select “Program > Save > NC program”. TURN PLUS displays the existing DIN PLUS programs and presents the currently active program for saving. Check/correct the file name. TURN PLUS generates the DIN PLUS program when saving the file. Saving TURN PLUS programs: U U Select “Program > Save > Complete (or Workpiece, ..)”. TURN PLUS displays the existing files of the directory and presents the currently active program for saving.
6.2 Program Head 6.2 Program Head The PROGRAM HEAD comprises: Material: For determining the cutting values. Assignment of spindle to slide for 1st setup Assignment of spindle to slide for 2nd setup: For full-surface machining, enter the spindle and the slide for machining the setup. If more than one slide is used, enter the slide numbers one after the other (for example: “12” = $1 and $2).
6.2 Program Head Generating programs for automatic lathes Use the following settings to generate a DIN PLUS program for automatic lathes by using TURN PLUS: U Set the “Program for automatic lathe” program head entry to YES Prerequisite: The templates “turnvor1.bev” to “turnvor5.bev” are provided in the “/ep90/ncps” directory. The templates are prepared by the machine tool builder and used for generating DIN PLUS programs.
6.
6.3 Workpiece Description 6.3 Workpiece Description You program a contour by entering individual contour elements one after the other in the correct sequence. You define the contour elements using absolute, incremental, Cartesian or polar coordinates. You can usually program a contour with the dimensions given in the workpiece drawing. TURN PLUS automatically calculates all missing coordinates, points of intersection, center points, etc. that can be derived mathematically.
6.3 Workpiece Description Entering the finished part contour The finished part contour includes: Turning contour, consisting of Basic contour Form elements (chamfers, rounding arcs, undercuts, recesses, threads, centric holes) C-Axis Contours Y-axis contours The turning contour must be a closed contour. Describe first the basic contour and then superimpose the form elements.
6.3 Workpiece Description Superimposing form elements Form elements are superimposed on the basic contour. They remain independent elements that can be edited or deleted. If required, TURN PLUS generates a special machining cycle for the form elements.
6.3 Workpiece Description Integrating overlay elements You describe contour trains in the same way as a finished part contour and superimpose them. Alternatively, you can use the following standard overlay elements (see “Overlay Elements” on page 418): Circular arc Wedge Pontoon These elements superimpose existing linear or circular supporting contour elements. Integrated overlay elements are part of the contour. Integrating a contour train: Select “Program > Load > Contour train”.
6.3 Workpiece Description Entering contours machined with the C axis You define standard forms with figures; regular linear or circular figures or holes in patterns. To define complex contours, use the basic elements “line” and “arc.
6.3 Workpiece Description Defining a C-axis contour Select “Workpiece > Finished part > Pattern > xx”. (xx: pattern type or single hole). Select “Workpiece > Finished part > Figure > xx”. (xx: figure type or free contour). Select the front/rear face or lateral surface. Specify the reference plane (plane on the front/rear face or lateral surface) and enter the reference dimension/diameter. TURN PLUS opens the corresponding dialog box. Define the pattern, figure, single hole or contour.
6.4 Contours of Workpiece Blanks 6.4 Contours of Workpiece Blanks Bar This function defines the contour of a cylinder (chuck or bar). Parameters X Diameter Diameter of circumference of a polygonal blank Z Blank length, including transverse oversize K Transverse oversize Tube This function defines the contour of a hollow cylinder.
6.4 Contours of Workpiece Blanks Cast blank (or forged blank) This function generates the workpiece blank from an existing finished part. Parameters Surface Cast blank Forged blank With bore Yes No K Equidistant oversize for the complete part I Single oversize (for individual elements or contour sections) First enter the “single oversize” and then select the contour element/the contour section.
6.5 Contours of Finished Parts 6.5 Contours of Finished Parts Notes on defining contours Parameters that TURN PLUS knows are not requested. The input boxes are locked. Example: On horizontal or vertical lines, only one of the coordinates changes and the angle is defined by the direction of the element. You set the type of dimensioning by soft key.
6.5 Contours of Finished Parts Linear elements This function defines a line segment. Parameters X End point in Cartesian coordinates Z End point in Cartesian coordinates Xi Distance from starting point to end point Zi Distance from starting point to end point a End point in polar coordinates (reference: positive Z axis) P End point in polar coordinates W Angle of the line (for reference see illustration) WV Counterclockwise angle to the preceding element.
6.5 Contours of Finished Parts Circular element This function defines a circular arc.
6.5 Contours of Finished Parts Defining a circular element: Call the arcs menu. Select the direction of rotation. Enter the arc dimensions and define the transition to the next element.
6.6 Form Elements 6.6 Form Elements Chamfer This form element defines a chamfer. Parameters B Chamfer width Rounding This form element defines a rounding.
6.6 Form Elements Undercut type E This form element defines an undercut type E. TURN PLUS suggests the parameters based on the diameter (see “Undercut DIN 509 E, Parameters” on page 686). Parameters K Undercut length I Undercut depth (radius) R Undercut radius in both corners of the undercut W Approach angle (undercut angle) Undercut type F This form element defines an undercut type F. TURN PLUS suggests the parameters based on the diameter (see “Undercut DIN 509 F, Parameters” on page 686).
6.6 Form Elements Undercut type H This form element defines an undercut type H. Parameters K Undercut length I Undercut depth (radius) R Undercut radius W Approach angle Undercut type K This form element defines an undercut type K. Parameters I Undercut depth R Undercut radius W Angular length A Approach angle, angle to longitudinal axis (default: 45°) Undercut type U This form element defines an undercut type U.
6.6 Form Elements Recess general This form element defines an axial or radial recess on a linear reference element. The recess is assigned to the selected reference element. Parameters X Reference point Z Reference point K Recess width without chamfer/rounding arc I Recess depth U Diameter of recess base (only for axial recess) A Recess angle, angle between the recess edges (0° <= A < 180°) 1.
6.6 Form Elements Recess type D (sealing ring) This form element defines an axial or radial recess on the outside or inside of the contour. The recess is assigned to the previously selected reference element.
6.6 Form Elements Relief turn (type FD) This form element defines an axial or radial relief turn on a linear reference element. The relief turn is assigned to the previously selected reference element. Parameters X Reference point Z Reference point K Recess width I Recess depth U Diameter of recess base (only for axial recess) A Recess angle (0° < A <= 90°) R Inside radius in both corners of the recess The CNC PILOT refers the recess depth to the reference element.
6.6 Form Elements Thread This function defines the different types of thread.
6.
6.
6.
6.7 Overlay Elements 6.7 Overlay Elements Select the standard overlay elements arc, wedge or pontoon, define the element and superimpose it after the definition. When you are superimposing a contour train, TURN PLUS uses the last active contour train or the last overlay element defined (see “Integrating overlay elements” on page 399).
6.7 Overlay Elements Pontoon Reference point: Center of base element Parameters XF Reference point shift ZF Reference point shift R R>0: Rounding radius R=0: No rounding A Angular length LS Length of wedge sides (projecting element parts are cut at the “points of overlay”) B Width of base element W Angle of rotation: The overlay contour is rotated by the “angle of rotation.
6.7 Overlay Elements Circular superimposition (“circular overlay”) The direction of rotation according to which the overlay contours are arranged corresponds to the direction of rotation of the supporting contour element. The reference point of the contour to be superimposed is positioned on the “point of overlay.
6.8 C-Axis Contours 6.8 C-Axis Contours Position of a front or rear face contour TURN PLUS takes the selected reference plane and suggests it as reference dimension. Change the parameter, if required. Parameters Z Reference dimension Position of a lateral surface contour TURN PLUS takes the selected reference plane and suggests it as reference diameter. Change the parameter, if required.
6.8 C-Axis Contours Entering the C-axis contour dimensions Press the soft key for the type of dimensioning you want to use for the contour element, figure or pattern (see “Notes on defining contours” on page 404). When defining lateral surface contours, enter either the angle or the “linear dimension.” The linear dimension is given with respect to the unrolled surface at the “reference diameter.
6.8 C-Axis Contours Front or rear face: Linear element This function defines a line segment on the front/rear face.
6.8 C-Axis Contours Front or rear face: Circular element This function defines a circular arc on the front/rear face.
6.8 C-Axis Contours Parameters Other parameters R Arc radius Tangential/nontangential: Specify the transition to the next contour element WA Angle between positive XK axis and tangent in starting point of arc WE Angle between positive XK axis and tangent in end point of arc WV Counterclockwise angle between preceding element and tangent in starting point of arc. If the preceding element is an arc: Angle to the tangent.
6.8 C-Axis Contours Front or rear face: Single hole This function defines a single hole on the front/rear face.
6.
6.8 C-Axis Contours Front or rear face: Circle (full circle) This function defines a full circle on the front/rear face.
6.8 C-Axis Contours Front or rear face: Rectangle This function defines a rectangle on the front/rear face.
6.8 C-Axis Contours Front or rear face: Polygon This function defines a polygon on the front/rear face.
6.8 C-Axis Contours Front or rear face: Linear slot This function defines a linear slot on the front/rear face.
6.8 C-Axis Contours Front or rear face: Circular slot This function defines a circular slot on the front/rear face.
6.8 C-Axis Contours Front or rear face: Linear hole or figure pattern This function defines a linear hole or figure pattern on the front/rear face.
6.8 C-Axis Contours Front or rear face: Circular hole or figure pattern This function defines a circular hole or figure pattern on the front/rear face.
6.8 C-Axis Contours Lateral surface: Starting point This function defines the starting point of a “free contour” on the lateral surface.
6.8 C-Axis Contours Lateral surface: Linear element This function defines a line segment on a lateral surface. Parameters Z End point of the line P End point of the line – polar CY End point of the line – angle as “linear dimension” C End point – angle W Angle of the line (for reference see illustration) WV Counterclockwise angle to the preceding element. If the preceding element is an arc: Angle to the tangent. WN Counterclockwise angle to the following element.
6.8 C-Axis Contours Lateral surface: Circular element This function defines a circular arc on a lateral surface.
6.8 C-Axis Contours Lateral surface: Single hole This function defines a single hole on the lateral surface.
6.
6.8 C-Axis Contours Lateral surface: Circle (full circle) This function defines a full circle on the lateral surface.
6.8 C-Axis Contours Lateral surface: Rectangle This function defines a rectangle on the lateral surface.
6.8 C-Axis Contours Lateral surface: Polygon This function defines a polygon on the lateral surface.
6.8 C-Axis Contours Lateral surface: Linear slot This function defines a linear slot on the lateral surface.
6.8 C-Axis Contours Lateral surface: Circular slot This function defines a circular slot on the lateral surface.
6.8 C-Axis Contours Lateral surface: Linear hole or figure pattern This function defines a linear hole or figure pattern on the lateral surface.
6.8 C-Axis Contours Lateral surface: Circular hole or figure pattern This function defines a linear hole or figure pattern on the lateral surface.
6.9 Help Functions 6.9 Help Functions Unresolved contour elements Contour elements that cannot be calculated are referred to as “unresolved elements.” TURN PLUS displays these elements on the right side of the screen. Each unresolved element is depicted by a symbol. TURN PLUS additionally lists all the parameters that are already known. If a contour element is not sufficiently defined, TURN PLUS reports the error.
6.9 Help Functions Selections Contour points or contour elements are first selected and then superimposed by form elements.
6.9 Help Functions Selecting a single contour point/contour element Single selection by touch pad Place the cursor on the contour point or contour element. Press the left mouse button – the contour point/element is selected. Single selection by soft key Go to the contour point. Go to the contour element. Select the contour point/contour element. Selecting more than one contour point/element Multiple selection by touch pad Activate multiple selection of contour points.
6.9 Help Functions Multiple selection by soft key Go to the first contour point. Mark the contour point and activate multiple selection. Go to the first contour element. Mark the contour element and activate multiple selection. For each contour point/element you want to select: Go to the contour point. Go to the contour element. Mark the contour point/contour element. Conclude the selection.
6.9 Help Functions Selecting a contour area Area selection by touch pad Place the cursor on the first element. Activate area selection. Place the cursor on the last element. Press the left mouse button: Area is selected in the direction of contour definition Press the right mouse button: Area is selected opposite to the direction of contour definition Area selection by soft key Go to the beginning of the area. Mark the beginning of the area and activate area selection. Go to the end of the area.
6.9 Help Functions Zero point shift Example: If the workpiece dimensions refer to different sides, you start by defining the contour elements whose dimensions are referenced to the right-hand side. Then shift the zero point and define the contour elements whose dimensions are referenced to the lefthand side. Activate zero point shift: U Select “Zero point > Shift” in the finished part menu. TURN PLUS opens the “Shift zero point” dialog box. U Enter the zero point shift.
6.9 Help Functions Copying a contour section in circular series With this function, you can define a contour section and append it to the existing contour any number of times. U U U U U Select “Copy > Row > Circular” in the finished part menu. TURN PLUS marks the last element. Select the contour section (you can only select the last contour elements entered). TURN PLUS opens the “Copy in circular series” dialog box. Enter the number of copies and the radius.
6.9 Help Functions Calculator You can use an online pocket calculator for example for standard calculations, calculation of fit tolerances, and calculation of the core hole diameter for inside threads. Calculate: U Position the cursor on the input field of the dialog box U Call the calculator. The value of the input box is loaded. U Perform the calculation. “OK” closes the calculator and applies the values. “Cancel” closes the calculator without applying the values.
6.9 Help Functions Digitizing With the digitizing feature, you determine the input values using the quadruple arrow (cross hairs) and transfer them to the input field. TURN PLUS displays the coordinates of the cross-hairs position. U Activate digitizing mode with the dialog box open. U Position the cross hairs by arrow keys or touch pad. U Exit the digitizing mode: ENTER key: Values are applied. ESC key: Values are not applied.
6.9 Help Functions Checking contour elements (inspector) The “inspector function” can be used to check contour elements, form elements, figures and patterns. It is not possible to edit the displayed data. Select the desired window (reference plane). Activate the magnify function. Call the “inspector.” Place the cursor on the contour element, form element, figure or pattern. Confirm the position. TURN PLUS shows the entered parameters.
6.9 Help Functions Error messages If the actual error message shows the characters “>>,” TURN PLUS can display further information on the error, if desired. U Display additional information on the error.
6.10 Importing of DXF Contours 6.10 Importing of DXF Contours Fundamentals for DXF import Contours that exist in DXF format can be imported into TURN PLUS. DXF contours describe Workpiece blanks Finished parts Contour trains Milling contours For workpiece blank and finished-part contours as well as for contour trains, DXF layers should contain only one contour. Milling contours can contain and import multiple contours.
6.10 Importing of DXF Contours Configuring the DXF Import In the starting point automatic configuration parameter you specify the behavior of TURN PLUS when entering the finished part contour. U U Select “Configuration > Change > Settings” from the main menu. TURN PLUS opens the “Settings” dialog box. Set the “Starting point automatic” parameter: Yes: Upon calling the finished part contour entry, TURN PLUS immediately branches to the entry of the contour starting point.
6.10 Importing of DXF Contours DXF parameters: Maximum gap: There might be small gaps between contour elements in the DXF drawing. With this parameter you specify how large the distance between two contour elements may be. Maximum gap is not exceeded: The following element is seen as being part of the “current” contour. Maximum gap is exceeded: The following element is an element of the “new” contour. Starting point: The DXF import analyzes the contour and determines the starting point.
6.11 Manipulating Contours 6.11 Manipulating Contours Note when editing contours: For contour elements that are superimposed by form elements, the indicated end points or the end points to be entered are given with respect to the “theoretical” end point. When contour elements are modified, the system automatically adjusts chamfers, rounding arcs, threads and undercuts to the new position. Sequence, starting point and end point of a contour element are determined by the direction of definition.
6.11 Manipulating Contours Deleting contour elements Deleting contour elements or form elements: U Select “Manipulate > Delete > Element (or Form element)” in the finished part menu. U Select the element to be deleted. U TURN PLUS deletes the selected contour/form element. Deleting all form elements: U Select “Manipulate > Delete > All form elements” in the finished part menu. U TURN PLUS deletes all existing form elements.
6.11 Manipulating Contours Editing a form element: U Select “Manipulate > Change > Form element” in the finished part menu. U Select the form element you want to edit. TURN PLUS opens the corresponding dialog box for editing. U Change parameters. U TURN PLUS applies the changes. Editing a C-axis contour: U U U U U Select the front-face, rear-face or lateral-surface window. Select “Manipulate > Change > Pattern/Figure/Pocket” in the finished part menu. Select the figure, pattern, contour element, etc.
6.11 Manipulating Contours Closing the contour Close an open contour: U U Select “Manipulate > Connect” in the finished part menu. TURN PLUS closes the contour by inserting a line segment. Resolving a contour With the “Resolve” function, TURN PLUS transforms form elements, figures or patterns into separate contour elements. Turning contour: Form elements (also chamfers and rounding arcs) are transformed into linear segments and arcs.
6.11 Manipulating Contours Trimming – Linear element With this function you change the length of a linear element. The starting point of the contour element remains unchanged. Closed contours: The manipulated element is recalculated and the position of the subsequent element is adapted. Open contours: The manipulated element is recalculated and the subsequent contour train is shifted.
6.11 Manipulating Contours Trimming – Length of contour With this function you change the length of a contour. Select the element to be modified and a “compensation element.” Parameters L Length or end point of the modified linear element. Z Length or end point of the modified linear element. Change length of contour: U Select “Manipulate > Trimming > Length contour” in the finished part menu. U Select the element you want to change. TURN PLUS suggests a compensation element.
6.11 Manipulating Contours Trimming – Diameter of linear element With this function you change the diameter of a horizontal linear element. TURN PLUS recalculates the manipulated element and adjusts the position of the preceding/succeeding element.
6.11 Manipulating Contours Transformations – Shifting This function shifts the contour incrementally or to the given position (reference point: contour starting point). Parameters X Target point Z Target point Xi Target point – incremental Zi Target point – incremental Original (only with C-axis contours): Copy: Original contour is maintained Delete: Original contour is deleted Transformations – Rotating This function rotates the contour at the center of rotation about the angle of rotation.
6.11 Manipulating Contours Transformations – Mirroring This function mirrors the contour. Define the position of the mirror axis by entering the starting point and end point or the starting point and angle.
6.12 Assigning Attributes 6.12 Assigning Attributes After the contour of a blank/finished part has been defined, individual contour elements/contour sections can be assigned attributes. The AWG and IWG evaluate the attributes for generating a working plan. The machining attributes you define are transferred as cycle parameters by the IWG. Attributes for workpiece blanks Attributes for workpiece blanks influence the division into machining areas and the selection of roughing cycles in the AWG.
6.12 Assigning Attributes Attributes – Oversize The attribute defines oversizes for individual contour sections or for the entire contour. The oversize, e.g. grinding allowance, is retained after the machining process has been completed. Parameters I Absolute oversize Ii Relative oversize TURN PLUS differentiates between: Absolute oversize: Is “final,” other oversizes are ignored. Relative oversize: Applies additively to other oversizes.
6.12 Assigning Attributes Attributes – Feed rate The “Feed rate” and “Feed rate reduction” attributes influence the finishing feed rate. Parameters F (Finishing) feed rate Assign the feed-rate attribute: U U U U Select “Attribute > Feed/Peak-to-valley > Feed rate” in the finished part menu. Select the entire contour, a contour section or individual contour elements (see “Selections” on page 448). TURN PLUS opens the “Feed rate” dialog box. Define the feed rate.
6.12 Assigning Attributes Attributes – Additive compensation With this attribute, you can assign an additive compensation value to the entire contour, a contour section or individual contour elements. The CNC PILOT manages 16 tool-independent additive compensation values. In the attribute, you enter the number of the additive compensation value. The compensation value is defined by parameter.
6.12 Assigning Attributes Machining attributes – Threading The machining attribute defines the details of a thread cutting operation. Parameters B Starting length No input: The CNC PILOT automatically determines the length from adjacent undercuts or recesses. No input, no undercut/recess: The CNC PILOT uses the thread starting length from machining parameter 7. P Overrun length No input: The CNC PILOT automatically determines the length from adjacent undercuts or recesses.
6.12 Assigning Attributes Machining attributes – Drill – Retraction plane The machining attribute defines the retraction plane of a drilling operation. The drill moves to the retraction plane (hole on lateral surface: diameter) before/after the drilling operation. Parameters K Retraction plane. Position of the drill before/after machining. Assign the “Retraction plane” machining attribute: U Select “Attribute > Machining attribute > Drill > Retraction plane” in the finished part menu.
6.12 Assigning Attributes Machining attributes – Contour milling The attribute defines the contour milling operation and the associated machining parameters for the selected figure or for a “free” open or closed contour.
6.12 Assigning Attributes Machining attributes – Area milling The attribute defines the area milling operation and the associated machining parameters for the selected figure or for a “free” closed contour. Parameters H Cutting direction 0: Up-cut milling 1: Climb milling D Milling diameter for selecting suitable tool. K Retraction plane. Cutter position before/after milling (lateral surface: diameter).
6.12 Assigning Attributes Machining attributes – Deburring The attribute defines the deburring operation and the associated machining parameters for the selected figure or for a “free” open or closed contour. Parameters H Cutting direction 0: Up-cut milling 1: Climb milling B Width W Angle for the tool selection (default 45°) K Retraction plane. Cutter position before/after milling (lateral surface: diameter).
6.12 Assigning Attributes Machining attributes – Engraving The attribute defines the engraving operation and the associated machining parameters for the selected figure or for a “free” open or closed contour. Parameters B Width W Angle for the tool selection (default 45°) K Retraction plane. Cutter position before/after milling (lateral surface: diameter). Assign the “Engraving” machining attribute: U Select “Attribute > Machining attribute > Mill > Engraving” in the finished part menu.
6.12 Assigning Attributes Machining attributes – Separation point The attribute defines a position on the contour as the separation point. Separation points are used for shaft machining and for machining with more than one setup. Parameters Position Delete: Deletes the existing separation point. The separation of the contour elements is maintained. 1. At target point: Separation point is end point of element 2. On element: Separation point is on the element.
6.12 Assigning Attributes Assigning the “Exclusion from machining” attribute to the elements of the turning contour: U Select “Attribute > Feed/Peak-to-valley > Exclusion from machining” in the finished part menu. U Select the entire contour, a contour section or individual contour elements (see “Selections” on page 448). U TURN PLUS assigns the attribute. Assigning the “Exclusion from machining” attribute to a C/Y-axis contour: U U U U Activate the front-face, rear-face or lateral-surface window.
6.13 Preparing a Machining Process 6.13 Preparing a Machining Process Preparing a machining process – Fundamentals The “Prepare” function defines the chucking equipment, the position of the chucking equipment, and TURN PLUS specific turret assignments. For chucking a workpiece, TURN PLUS determines the following data: Inside and outside cutting limit. Zero point shift. The value is transferred to the NC program as a G59 command.
6.13 Preparing a Machining Process Chucking a workpiece at the spindle Clamp the workpiece: U U U U Select “Prepare > Chucking > Clamp > Spindle side.” Select the type of chuck (drop-down menu). TURN PLUS opens one of the following dialog boxes: Two-jaw chuck Three-jaw chuck Four-jaw chuck Collet chuck Without chuck (face driver) Three-jaw chuck indirect (face driver with jaws) Define the chuck and jaws as well as the clamping form and clamp range.
6.13 Preparing a Machining Process Defining the cutting limit TURN PLUS finds the cutting limit on the outside and inside of the contour when the workpiece is chucked at the spindle. Edit the cutting limit: U U Select “Prepare > Chucking > Clamp > Cutting limitation.” TURN PLUS opens the “Cutting limitation for AWG” dialog box. Define the cutting limit. The cutting limit is displayed as a red line.
6.13 Preparing a Machining Process Rechuck – Standard machining Use “Rechuck – Standard machining” for front-face and rear-face machining with separate NC programs. TURN PLUS Mirrors the workpiece (blank and finished part) and shifts the zero point by “Nvz.” Rotates lateral surface contours or contours of the YZ plane by “Wvc.” Deletes the chucking equipment used for the first setup. Rechuck: U U Select “Prepare > Chucking > Rechuck > Standard machining.
6.13 Preparing a Machining Process Rechuck – 1st setup after 2nd setup The “Rechuck – 1st setup after 2nd setup” function initiates the machining operation for the second setup. First define the chucking equipment. TURN PLUS then activates an expert program from machining parameter 21. Which expert program is activated depends on the spindle entries specified for “1st setup ..” and “2nd setup ..
6.13 Preparing a Machining Process Parameters (example) LD Pick-up position in Z 0: Pick-up position at machine dimension 1 1 to 6: Pick-up position at machine dimension 1 to 6 ¼ 0 to 6: Pick-up position. TURN PLUS calculates a default value. LE Working position in Z (proposed value: zero point offset of Z axis $1) I Minimum feed path No traverse to fixed stop: Safety clearance on the workpiece to be transferred (proposed value: “Safety clearance on blank part” from machining parameter 2).
6.13 Preparing a Machining Process Parameters for two-jaw, three-jaw or four-jaw chucks Parameters ID number chuck Jaw type and steps Clamp form (see table below) ID number jaw Clamp length TURN PLUS calculates the clamp length from the jaw and the clamp form. Correct this value if the clamping length is different. Clamping pressure The entry is transferred to the program head. TURN PLUS does not evaluate this parameter.
6.13 Preparing a Machining Process Collet chuck parameters Parameters ID number chuck Clamp diameter Free length (distance between front edge of collet and right edge of blank) Clamping pressure The entry is transferred to the program head. TURN PLUS does not evaluate this parameter. Parameters for face drivers (“without chuck”) Parameters ID number Indentation depth Approximate depth to which the grippers press into the material. TURN PLUS uses this value to position the face driver graphics.
6.13 Preparing a Machining Process Parameters for face drivers with jaws (“Threejaw chuck indirect”) Parameters ID number chuck Type of jaw ID number jaw ID of face driver Indentation depth Approximate depth to which the grippers press into the material. TURN PLUS uses this value to position the face driver graphics. Clamping pressure The entry is transferred to the program head. TURN PLUS does not evaluate this parameter.
6.13 Preparing a Machining Process Setting up tools Select “Setting up > Tool list > Set up turret > Set up turret n.” Select the tool location. Entering the tool directly: Press ENTER (or the INS key). The CNC PILOT opens the ““Tool” dialog box. Enter the ID number, define the relevant coolant circuits and close the dialog box. Select the tool from the database: List the tools by type mask or List the tools by ID number mask Place the cursor on the nominal tool. Insert the tool.
6.13 Preparing a Machining Process Deleting a tool Select “Setting up > Tool list > Set up turret > Set up turret n.” Select the tool location. Use the soft key, or Press the DEL key to delete the tool Changing the tool location Select “Setting up > Tool list > Set up turret > Set up turret n.” Select the tool location. Deletes the tool and saves it in the “ID number clipboard.” Select a new tool location.
6.13 Preparing a Machining Process Managing tool lists Functions for turret assignment: Load saved tool list: Loads a saved tool list (“Load file” selection box). Load tool list of machine: Loads the current turret assignment of the machine. Save list: Saves the current turret assignment. Delete list: Deletes the selected file. Loading a tool list from the file Select “Prepare > Tool list > Load list > Saved tool list.” TURN PLUS opens the “Load file” selection box. Select and load the tool list.
6.14 Interactive Working Plan Generation (IWG) 6.14 Interactive Working Plan Generation (IWG) In the IWG, you define the work blocks. You do this by selecting the tool and the cutting values and determining the fixed cycle. The semiautomatic mode of the IWG generates a complete work block. In special machining (SM) you add paths of traverse, subprogram calls or G/M functions (example: use of tool handling systems).
6.14 Interactive Working Plan Generation (IWG) Working plan exists If a working plan exists, the IWG starts up with the “Working plan exists” dialog. Set: Working plan – new (reject an existing working plan and create a new one) Working plan – continue Working plan – edit Working plan – view Select IWG. TURN PLUS opens the “Working plan exists” dialog box. Creating a new working plan: Select New. TURN PLUS deletes the existing working plan.
6.14 Interactive Working Plan Generation (IWG) Generating a work block A work block is defined as follows: 1. 2 3. 4. 5. 6. 7. 8. 9. Select the machining mode. Select the tool. Check or optimize the cutting data. Define the machining range by area selection (see “Selections” on page 448). Check or optimize the cycle parameters. If required: Define the approach position and/or retraction position. If required: Move to the tool change point. Check the work block with the simulation function.
6.14 Interactive Working Plan Generation (IWG) Calling a tool The “Tool” menu item is only available after you have selected the machining mode. The submenu items have the following meanings: Manually via turret assignment: Select a tool positioned on the turret. Manually via tool type: Select a tool from the database and position it on the turret. From last machining process: The IWG selects the tool used for the last machining operation.
6.14 Interactive Working Plan Generation (IWG) Cycle specification In the “Cycle” drop-down menu, define the cycle parameters and the strategies for approach and departure: Machining range: Define the area to be machined and the machining direction by area selection. Selection by soft key: The sequence of selection defines the machining direction. Selection by touch pad – left mouse button: Machine in direction of contour definition.
6.14 Interactive Working Plan Generation (IWG) Overview of roughing operations The IWG presents the following roughing operations for selection (“Roughing” drop-down menu): Longitudinal roughing: see “Roughing longitudinal (G810)” on page 500 Transverse roughing: see “Roughing transverse (G820)” on page 501 Contour-parallel roughing: see “Roughing contour-parallel (G830)” on page 502 Automatic roughing: TURN PLUS generates the work blocks for all roughing operations.
6.14 Interactive Working Plan Generation (IWG) Roughing longitudinal (G810) The IWG generates the cycle G810 for the selected contour area.
6.14 Interactive Working Plan Generation (IWG) Roughing transverse (G820) The IWG generates the cycle G820 for the selected contour area.
6.14 Interactive Working Plan Generation (IWG) Roughing contour-parallel (G830) The IWG generates the cycle G830 for the selected contour area.
6.14 Interactive Working Plan Generation (IWG) Residual roughing – longitudinal The IWG generates the cycle G810 for removing residual material.
6.14 Interactive Working Plan Generation (IWG) Residual roughing – transverse The IWG generates the cycle G820 for removing residual material.
6.14 Interactive Working Plan Generation (IWG) Residual roughing – contour-parallel The IWG generates the cycle G830 for removing residual material.
6.14 Interactive Working Plan Generation (IWG) Roughing hollowing – neutral tool (G835) The IWG generates the cycle G835 for the selected contour area.
6.
6.14 Interactive Working Plan Generation (IWG) Contour recessing radial/axial (G860) The IWG generates the cycle G860 for the form elements “Recess general” and “Relief turn” (recess type F) and for freely defined recesses.
6.14 Interactive Working Plan Generation (IWG) Recessing radial/axial (G866) The IWG generates the cycle G866 for the form elements “Recess type D” (sealing ring) and “Recess type S” (guarding ring). If an oversize has been specified, TURN PLUS first rough-machines and then finish-machines the recess.
6.14 Interactive Working Plan Generation (IWG) Recess turning radial/axial (G869) The IWG generates the cycle G869 for the selected contour area (machining with alternating recessing and roughing passes). The parameters for radial and axial recess turning are identical, except for the reference axis of the approach and departure angles.
6.
6.14 Interactive Working Plan Generation (IWG) Parting For parting, the AWG activates the expert program entered in machining parameter 21 – “SP 100098.” TURN PLUS determines the parameters as far as possible and enters them as default values. Check, edit or enter the values. Parameters LA Bar diameter LB Starting point in Z. TURN PLUS uses the position that you defined when selecting the machining range.
6.14 Interactive Working Plan Generation (IWG) Parting and workpiece transfer For parting with workpiece transfer, TURN PLUS activates an expert program from machining parameter 21. Which expert program is activated depends on the spindle entries specified for “1st setup ..” and “2nd setup ..” in the program head: Same spindle (manual rechucking): Entry from “SP-ABHAND.” Different spindles (workpiece transfer to opposing spindle): Entry from “SP-UMKOMPLA.
6.14 Interactive Working Plan Generation (IWG) Expert program “UMKOMPLA” The expert program entered in SP-UMKOMPLA (machining parameter 21) parts the workpiece and transfers it to the opposing spindle. TURN PLUS entered the calculated parameters as proposed values. Check, edit or enter the values.
6.14 Interactive Working Plan Generation (IWG) Expert program “ABHAND” The expert program entered in SP-ABHAND (machining parameter 21) parts the workpiece and supports the manual rechucking of the workpiece for machining the rear face on machines with one spindle. TURN PLUS entered the calculated parameters as proposed values. Check, edit or enter the values.
6.
6.14 Interactive Working Plan Generation (IWG) Centric predrilling (G74) The IWG generates the cycle G74 for the selected contour area (predrilling at turning center using stationary tools). Select the machining range: Select all contour elements encompassing the bore hole. If required, the bore hole can be limited with “drilling limitation Z.
6.
6.
6.
The IWG presents the following finishing operations for selection (“Finishing” drop-down menu): Finishing using cycle G890: Contour machining Residual-contour machining Finishing hollowing (neutral tool) Finishing using special functions: Clearance turning: see “Finishing – Clearance turning” on page 524 Undercuts: see “Finishing – undercut” on page 524 Parameters X Cutting limit Z Cutting limit L Depending on the soft-key setting: Longitudinal oversize Constant oversize (generates “O
6.14 Interactive Working Plan Generation (IWG) Parameters H Type of retraction. The tool retracts at 45° in the opposite direction to the machining direction.
6.
6.14 Interactive Working Plan Generation (IWG) Finishing – Clearance turning TURN PLUS executes a measuring cut on the selected contour element. Precondition: The contour element was assigned the “Measure” attribute (see “Machining attributes – Measure” on page 473). Parameters I Oversize for measuring cut K Length of measuring cut Q Measuring loop counter (every nth workpiece is measured) Clearance turning is performed by the expert program SP-MEAS01 (machining parameter 21).
6.14 Interactive Working Plan Generation (IWG) Thread machining (G31) The IWG generates the cycle G31 for the selected thread. Parameters B Run-in length No input: The CNC PILOT automatically determines the length from adjacent undercuts or recesses. No input, no undercut/recess: The CNC PILOT uses the thread starting length from machining parameter 7. P Overrun length No input: The CNC PILOT automatically determines the length from adjacent undercuts or recesses.
6.
6.14 Interactive Working Plan Generation (IWG) Contour milling – Roughing/Finishing (G840) The IWG generates the cycle G840, including the following parameters, for the selected open or closed contour.
6.14 Interactive Working Plan Generation (IWG) Parameters L Oversize The oversize “shifts” the contour depending on the cutter position Q (generates “Oversize G58” before the milling cycle): Q=0: Oversize will be ignored For closed contours: Q=1: Reduces the contour Q=2: Enlarges the contour For open contours: Q=1: Shift to the left Q=2: Shift to the right Effects of “cutter position, cutting direction and direction of tool rotation:” see “Contour milling G840— Fundamentals” on page 261.
6.14 Interactive Working Plan Generation (IWG) Deburring (G840) The IWG generates the cycle G840, including the following parameters, for the selected open or closed contour.
6.14 Interactive Working Plan Generation (IWG) Engraving (G840) The IWG generates the cycle G840, including the following parameters, for the selected open or closed contour.
6.
6.14 Interactive Working Plan Generation (IWG) Special machining (SM) “Special machining” defines a work block that is integrated in the working plan. In special machining you add paths of traverse, subprogram calls or G/M functions (example: use of tool handling systems). Soft keys Simultaneous Defining tool paths at feed rate or rapid traverse First X, then Z direction Select “Special machining > Free input” in the IWG menu. First Z, then X direction Press “Tool.” Select and position the tool.
6.14 Interactive Working Plan Generation (IWG) Defining a subprogram call Select “Special machining > Free input > Single block > Technology” in the IWG menu. Select “Subprogram.” TURN PLUS opens the selection box with the available subprograms. Select the desired subprogram and define the transfer parameters. Select “G and M functions.” Define the target position and strategy for the path of traverse (see soft key table). Select “Cutting data.” Check/optimize the cutting data suggested by TURN PLUS.
6.15 Automatic Working Plan Generation (AWG) 6.15 Automatic Working Plan Generation (AWG) The AWG generates the work blocks of the working plan in the sequence defined in “Machining sequence.” Machining parameters define details of machining. TURN PLUS automatically finds all the elements of a work block. An existing part machining can be continued with the AWG. Use the machining sequence editor to specify the machining sequence.
6.15 Automatic Working Plan Generation (AWG) Generating a working plan block by block: Select “AWG > Blockwise.” TURN PLUS generates the working plan block by block and displays it in the control graphics. After generation you can accept or reject the work block. After generation you can accept or reject the working plan. Machining sequence – Fundamentals TURN PLUS analyzes the contour in the sequence defined in “Machining sequence.
6.15 Automatic Working Plan Generation (AWG) The AWG does not generate the work blocks if any required preparatory step is missing, or if the appropriate tool is not available, etc. TURN PLUS skips machining operations/machining sequences that do not make sense in the machining process. You initiate rear-face machining with the main machining and submachining operation “Parting – Full-surface machining” or “Rechucking – Full-surface machining.
6.15 Automatic Working Plan Generation (AWG) Editing a machining sequence Select “AWG > Machining sequence > Change.” TURN PLUS activates the machining sequence editor. Select the position. Position the cursor. Enter a new machining operation (the new machining operation is inserted in front of the cursor). TURN PLUS opens the “Machining sequence – editor” dialog box. Use the arrow keys to select the main machining and submachining operation and the location. Confirm the setting with ENTER.
6.15 Automatic Working Plan Generation (AWG) Overview of machining sequences Special machining has no significance for the AWG.
Main machining Submachining Location (Roughing) Hollowing Execution Contour analysis: Using the “inward copying angle (EKW),” you can determine recess areas (undefined recesses). The machining operation is performed with one or two tools.
6.15 Automatic Working Plan Generation (AWG) Machining sequence for contour machining (finishing) Main machining Submachining Location Contour machining (finishing) Execution Contour analysis: Dividing the contour into areas for outside and inside machining.
Main machining Submachining Location Recess turning Execution Contour analysis: Without previous roughing operation: The complete contour, including recess areas (undefined recesses), is machined. With previous roughing: Recess areas (undefined recesses) are determined and machined according to the “inward copying angle (EKW).
6.15 Automatic Working Plan Generation (AWG) Machining sequence for contour recessing Main machining Submachining Location Contour recessing Execution Contour analysis: Recess areas (recesses) are determined and machined according to the “inward copying angle (EKW).
Main machining Submachining Location Undercuts Description Contour analysis/machining: Determining the “Undercuts” form elements: Type H – Machining using single paths of traverse; copying tool (type 22x) Type K – Machining using single paths of traverse; copying tool (type 22x) Type U – Machining using single paths of traverse; recessing tool (type 15x) Type G – Machining using cycle G860 Sequence: First outside, then inside machining; first radial, then axial machining – – All recess types;
6.15 Automatic Working Plan Generation (AWG) Machining sequence for drilling Main machining Submachining Location Drilling Execution Contour analysis: Determining the “Hole” form elements.
Main machining Submachining Location Milling Execution Contour analysis: Determining the milling contours.
6.15 Automatic Working Plan Generation (AWG) Machining sequence for engraving Main machining Submachining Location Engraving Execution Contour analysis: Determining milling contours with “Engraving” attribute.
6.16 Control Graphics 6.16 Control Graphics During contour definition, TURN PLUS displays all contour elements that can be displayed. The IWG and AWG permanently display the finished part contour and graphically depict the cutting operations. The workpiece blank takes on a contour during machining. Adjusting the section (zoom function) The zoom function can be used to isolate a detail and magnify it. Zoom settings by keyboard: U Activate the magnify function The red rectangle indicates the new section.
6.16 Control Graphics Setting the control graphics You can select the display of the tool paths and the simulation mode in the configuration (see “Configuring the control graphics” on page 550) or by soft key. Window size If several windows are displayed on screen: U Press the “.” key. The control graphics toggles between full-screen and tiled display.
6.17 Configuring TURN PLUS 6.17 Configuring TURN PLUS With the “configuration” you change and manage the display and input variants. General settings Selection: U U Select “Configuration > Change.” Press “Settings.” TURN PLUS opens the “Settings” dialog box. “Settings” dialog box Zoom behavior: Dynamic: Adapts the contour graphics to the window size. Static: Adapts the contour graphics to the window size when the contour is loaded; this setting is maintained.
6.17 Configuring TURN PLUS Configuring windows (views) Define the views that TURN PLUS is to depict besides the main view (XZ plane). Selection: U U Select “Configuration > Change.” Press “Views.” TURN PLUS opens the “Window configuration” dialog box.
6.17 Configuring TURN PLUS Setting the coordinate system With the configuration of the “Coordinate system,” you define the dimensions of the control graphics window and the position of the workpiece zero point. Selection: U U Select “Configuration > Change.” Select “Coordinates > Main view” (“.. > Front face”, “.. > Rear side” or “.. > Lateral surface”). TURN PLUS opens the “Coordinate system” dialog box.
6.18 Machining Information 6.18 Machining Information Tool selection, turret assignment The tool selection is determined by: Machining direction Contour to be machined Machining sequence If the ideal tool is not available, TURN PLUS First looks for a replacement tool, Then for an emergency tool. If necessary, TURN PLUS adapts the machining cycle to the requirements of the replacement or emergency tool. If more than one tool is suitable for a machining operation, TURN PLUS uses the optimal tool.
6.18 Machining Information Contour recessing, recess turning The cutting radius must be smaller than the smallest inside radius of the recess contour, but >= 0.2 mm. TURN PLUS determines the width of the recessing tool from the recess contour: Recess contour includes paraxial base elements with radii on both sides: SB <= b + 2*r (if radii differ: smallest radius).
6.18 Machining Information Coolant: Depending on the workpiece material, cutting material and machining operation, define in the technology database whether coolant is used. If you have specified that coolant is to be used, the AWG activates the coolant circulation for the respective machining block. If high-pressure coolant circulation is used, the AWG generates a corresponding M function. The IWG controls coolant circulation in the same way as the AWG.
6.18 Machining Information Inside contours TURN PLUS machines continuous inside contours up to the transition from the “deepest point” to a greater diameter. The end position for drilling, roughing and finishing operations depends on: Cutting limit, inside Overhang length, inside ULI (machining parameter 4) Prerequisite: The usable tool length must be sufficient for the machining operation. If it is not, then this parameter defines the inside machining operation.
6.18 Machining Information Roughing limit behind cutting limit Example 2: The roughing limit (SU) is located behind the cutting limit, inside (SBI).
6.18 Machining Information Shaft machining For shafts, TURN PLUS supports rear-face machining of outside contours in addition to standard machining processes. This enables shafts to be completely machined using one setup. TURN PLUS does not support retracting the tailstock and does not check the setup used. Precondition for shaft machining: The workpiece is clamped at spindle and tailstock.
6.18 Machining Information Protective zones for drilling and milling operations TURN PLUS machines drilling and milling contours on transverse surfaces (front/rear face) if: (Horizontal) distance to transverse surface > 5 mm, or Distance between chucking equipment and drilling/milling contour is > SAR (SAR: See machining parameter 2). If jaws are used for clamping the shaft at the spindle, TURN PLUS accounts for the cutting limitation (SB).
6.18 Machining Information Multi-slide machines On machines with more than one slide, you can influence the tool selection and program generation through the following parameters: Program head: In the “1st setup: Spindle .. With slide ..” box, specify the slides you want to use for the machining operation. Enter the slide numbers one after the other, without separators (see illustration). This also applies to the second setup.
6.18 Machining Information Full-surface machining You describe the geometry of the blank and finished part, and TURN PLUS generates the working plan for the complete workpiece. Preconditions for full-surface machining: In the program head the spindle and the slide for the second setup are defined (“2nd setup ..” input boxes). In the machining sequence the main machining operation “Rechucking”“ or “Parting” is entered after the machining of the front face.
6.18 Machining Information Note on machining the rear face For contours on the rear side (C/Y axis machining) remember the orientation of the XK or X axis and the orientation of the C axis. Designations (see figure at right): Front side (“V”): The side toward the working space Rear side (“R”): The side away from the working space These designations also apply to workpieces clamped at the opposing spindle, or to workpieces rechucked for rear-side machining in lathes with one spindle.
6.19 Example 6.19 Example On the basis of the production drawing, the working steps for defining the contour of the blank and finished part, the setup procedures and automatic working plan generation are explained. Workpiece blank: Ø60 X 80; Material: Ck 45 Undefined chamfers: 1x45° Undefined radii: 1 mm Creating a program U U U U U U Select “Program > New”. TURN PLUS opens the “New program” dialog box.
6.19 Example Defining the workpiece blank U U U Select “Workpiece > Blank > Bar.” TURN PLUS opens the “Bar” dialog box. Inputs: Diameter = 60 mm Length = 80 mm Oversize = 2 mm TURN PLUS displays the workpiece blank. U Press the ESC key to return to the main menu. Defining the basic contour U U U Select “Workpiece > Finished part (> Contour).
6.19 Example Defining form elements Chamfer at corner of threaded shank: U U U Select “Form > Chamfer.” Select the corner of the threaded shank. “Chamfer” dialog box: Chamfer width = 3 mm Rounding arcs: U U U Select “Form > Rounding.” Select the corners for the rounding arcs. “Rounding” dialog box: Rounding radius = 2 mm Undercut: U U U Select “Form > Undercut > Undercut type G.” Select the corner for the undercut. “Undercut type G” dialog box: Undercut length = 5 mm Undercut depth = 1.
6.19 Example Preparing the machining process, chucking U U U U Select “Prepare > Chucking > Clamp.” Select “Spindle side > Three-jaw chuck.” “Three-jaw chuck” dialog box: Select the “ID number chuck.” Enter the type of jaw. Enter the clamp form. Select the “ID number jaw.” Check/enter the clamp length and clamping pressure. Define the clamp range: Select a contour element touched by the jaws. TURN PLUS displays the selected chucking equipment and the cutting limit.
6.
Parameters HEIDENHAIN CNC PILOT 4290 567
7.1 The Parameter Mode of Operation 7.1 The Parameter Mode of Operation The parameters of the CNC PILOT are grouped as follows: Machine parameters: These are used to adapt the control to the requirements of the machine (e.g. parameters for components, assemblies, the assignment of axes, slides and spindles, etc.). Control parameters: These are used to configure the control system (machine display, interfaces, measuring system used, etc.).
7.2 Editing Parameters 7.2 Editing Parameters Current parameters This drop-down menu presents an overview of frequently used parameters so that you can select them without having to know the parameter number. Edit parameter U If required, log on as system manager (Service mode). U Select the parameter from the “Cur.Para > ..” dropdown menu. The CNC PILOT presents the parameter for editing. U Make the required changes and close the dialog box.
7.2 Editing Parameters Editing configuration parameters In the “Config” drop-down menu, all parameter groups are presented for selection. The procedure is identical with that described in this section. The CNC PILOT checks whether the user is authorized to change a parameter. Log on as system manager if you wish to edit protected parameters. Otherwise, you are only authorized to read parameters. Parameters that influence the production of a workpiece cannot be edited in automatic mode.
7.3 Machine Parameters (MP) 7.3 Machine Parameters (MP) Value ranges of machine parameters: 1..200: General machine configuration 201..500: Slides 1 to 6 (50 positions per slide) 501..800: Tool carriers 1 to 6 (50 positions per tool carrier) 801..1000: Spindles 1 to 4 (50 positions per spindle) 1001..1100: C-axes 1 to 2 (50 positions per C axis) 1101..2000: Axes 1 to 16 (50 positions per axis) 2001..
7.3 Machine Parameters (MP) General machine parameters 18 Control configuration PLC is to perform counting of workpieces: 0: CNC is to perform counting of workpieces 1: PLC is to perform counting of workpieces M0/M1 for all NC channels 0: M0/M1 triggers a STOP on programmed channels. 1: M0/M1 triggers a STOP on all channels. Interpreter stop upon tool change 0: No interpreter stop 1: Interpreter stop.
211, 261, .. Position of the touch probe or optical gauge To define the position of the probe, enter its external coordinates (reference: machine zero point). To define the position of the optical measuring system, enter the position of the cross hairs (+X/+Z). Position of touch probe/optical gauge in +X Position of touch probe in –X Position of touch probe/optical gauge in +Z Position of touch probe in –Z 511..542, 561..592, ..
7.3 Machine Parameters (MP) Spindle parameters 807, 857, .. Measuring the angle offset (G906) for spindle Evaluation: G906 Measuring angular offset during spindle synchronization Maximum permissible change in position: Tolerance window for the change of position offset after the spindles have gripped the workpiece at both ends during synchronized operation. If the offset change exceeds the maximum value, an error message appears. A normal fluctuation of approx. 0.5° must be considered.
1010, 1060, .. Load monitoring for C axis Evaluation: Load monitoring Start-up time for monitoring [0..1000 ms]: The load monitoring function is not activated if the nominal acceleration of the spindle exceeds the limit value (limit value = 15% of acceleration ramp / brake ramp). As soon as nominal acceleration falls below the limit value, the monitoring function is activated after the start-up time for monitoring has elapsed. The parameter is only evaluated if “Omit paths of rapid traverse” is active.
7.3 Machine Parameters (MP) Parameters for linear axes 1110, 1160, .. Load monitoring for linear axis Evaluation: Load monitoring Start-up time for monitoring [0..1000 ms]: The load monitoring function is not activated if the nominal acceleration of the spindle exceeds the limit value (limit value = 15% of acceleration ramp / brake ramp). As soon as nominal acceleration falls below the limit value, the monitoring function is activated after the start-up time for monitoring has elapsed.
General control parameters General control parameters 1 Settings Suppressing printer output: With the PRINTA command in the NC program you can output data to a printer (see also control parameter 40). 0: Suppress the output 1: Enable the output Metric / Inches: Setting for the unit of measure. 0: Metric 1: Inches Format of the position displays (actual value displays). 0: Format 4.3 (4 integral, 3 decimal places) 1: Format 3.
7.4 Control Parameters General control parameters 11 FTP parameters Evaluation: Data transfer using FTP (file transfer protocol) User name: Name of one's own station Passcode Address/name of FTP server: Address/name of communications partner Use FTP 0: No 1: Yes Note: The parameters can also be set using the transfer functions. 40 Assignment to the interfaces The interface parameters are saved in the parameters 41 to 47.
7.4 Control Parameters Control parameters for simulation Parameters for simulation 20 Time counting for general simulation These times are used as nonmachining times for the time calculation function. Evaluation: Time calculation (Simulation mode) Tool change time [sec] Gear shifting time [sec] Time allowance for M functions [sec]: All M functions are rated with this time. If an M function is also specified in control parameter 21, the time allowances entered here are added.
7.4 Control Parameters Parameters for simulation 24 Simulation: Color table for feed travel The feed travel of a tool is displayed in the color assigned to the respective turret location. Evaluation: Simulation mode Color for turret position n (n: 1..
7.
7.
7.5 Set-Up Parameters 7.5 Set-Up Parameters Recommendation: Use “Cur. Para > Set-up (menu) – ... ” to edit the parameters. In the other menu items the parameters are listed without the axes. Set-up parameters Workpiece datum Datum position, main spindle X, Y, Z - Slide 1 Datum position, main spindle X, Y, Z - Slide 2 . . . Datum position, main spindle X, Y, Z - Slide 1 Datum position, main spindle X, Y, Z - Slide 2 . . .
7.5 Set-Up Parameters Set-up parameters Tool life monitoring Tool life switch (tool life monitoring/quantity monitoring) 0: Off 1: On Load monitoring 0: Off 1: On Additive compensation Compensation 901..916 in X Compensation 901..916 in Z The CNC PILOT manages 16 compensation values (X and Z) that can be activated/deactivated in the NC program (see G149, G149 Geo). If an additive compensation value is changed in Automatic mode, this parameter is changed accordingly.
7.6 Machining Parameters 7.6 Machining Parameters Machining parameters are used by the work plan generation (TURN PLUS) and various machining cycles.
7.6 Machining Parameters 2 – Global technology parameters Global technology parameters – Tools Tool selection, tool change, speed limitation Tool off .. [WD] When selecting the tool, TURN PLUS considers the following data: 1: Current turret assignment 2: Primarily the current turret assignment and, additionally, the tool database.
7.
7.6 Machining Parameters 3 – Centric predrilling Centric predrilling – Tool selection Tool selection 1. 1st drilling diameter limit [UBD1] 1.
7.6 Machining Parameters Centric predrilling – Oversizes Oversizes Point angle tolerance [SWT] If the drilling limitation element is a diagonal element, TURN PLUS prefers using a twist drill with suitable point angle. If no suitable twist drill is available, an indexable-insert drill is selected for the predrilling operation. SWT defines the permissible point angle tolerance. Drilling oversize – Diameter [BAX] Machining oversize on drilling diameter (X direction – radius value).
7.6 Machining Parameters Centric predrilling – Safety clearances Safety Clearances Safety clearance on blank part [SAB] Internal safety clearance [SIB] Retraction distance for deep-hole drilling (“B” for G74). Centric predrilling – Machining Machining Drilling depth ratio [BTV] TURN PLUS checks the 1st and 2nd drilling steps. The predrilling step is performed with: BTV <= BT / dmax Drilling depth factor [BTF] 1.
7.6 Machining Parameters 4 – Roughing Roughing – Tool standards Furthermore: Roughing cycles are primarily executed with standard roughing tools. Alternatively, tools that allow full-surface machining are used.
7.
7.6 Machining Parameters Roughing – Machining analysis TURN PLUS uses the PLVA/PLVI parameters to define whether a roughing area is to be rough-machined longitudinally or transversely.
7.6 Machining Parameters Fixed cycles Cutting depth reduction factor [SRF] For rough-machining with tools machining opposite to the main machining direction, the infeed value (cutting depth) is reduced. Infeed (P) for roughing cycles (G810, G820): P = ZT * SRF (ZT: Infeed value from technology database) 5 – Finishing Finishing – Tool standards TURN PLUS uses the tool angle and point angle to select the tools according to machining location and main machining direction (MMD).
7.6 Machining Parameters Finishing – Machining standards Machining standards Standard/Full-surface – external/longitudinal [FAL] Standard/Full-surface – internal/longitudinal [FIL] Standard/Full-surface – external/transverse [FAP] Standard/Full-surface – internal/transverse [FIP] Machining of contour areas: 0 – Full-surface finishing cycle: TURN PLUS looks for an optimum tool for machining the complete contour area.
7.6 Machining Parameters Finishing – Tool tolerances Approach and departure are in rapid traverse (G0).
7.6 Machining Parameters 6 – Recessing and contour recessing Recessing, contour recessing – Approach and departure Approach and departure are in rapid traverse (G0).
7.6 Machining Parameters Tool selection, oversizes Equidistant or longitudinal [KSLA] Equidistant oversize or longitudinal oversize None or transverse [KSPA] Transverse oversize The oversizes are accounted for when machining contour valleys with a contour-recessing operation. Standardized recesses such as recess types D, S, A are completed in one machining cycle. A division into roughmachining and finish-machining is only possible in DIN PLUS.
7.6 Machining Parameters 7 – Thread cutting Thread cutting – Approach and departure Approach and departure are in rapid traverse (G0).
7.6 Machining Parameters 8 – Measuring The measuring parameters are assigned to the fit elements as an attribute. Measurement procedure Measurement type [MART] 1: Manual measurement – calls expert program Measuring loop counter [MC] Defines the measurement/loop intervals. Current consumption [mA] Oversize still applied to the element to be measured. Measuring cut length [MSL] 9 – Drilling Drilling – Approach and departure Approach and departure are in rapid traverse (G0).
7.6 Machining Parameters Drilling – Safety clearances Safety Clearances Internal safety clearance [SIB] Retraction distance for deep-hole drilling (“B” for G74). Driven drills [SBC] Safety clearance for driven tools on end face and lateral surface. Stationary drills [SBCF] Safety clearance on end face and lateral surface for tools that are not driven. Driven taps [SGC] Safety clearance for driven tools on end face and lateral surface.
7.6 Machining Parameters 10 – Milling Milling – Approach and departure Approach and departure are in rapid traverse (G0).
7.6 Machining Parameters Load monitoring 11 – Load monitoring – General switches Load monitoring – General switches Load monitoring ON/OFF 0 – OFF: TURN PLUS does not generate any commands for load monitoring 1 – ON: TURN PLUS generates commands for load monitoring Component positions Corresponds to the parameter Q of G996: 0: Monitoring not active 1: Do not monitor rapid traverse 2: Monitor rapid traverse 12..
7.
7.6 Machining Parameters 21 – Name of the subroutines TURN PLUS uses expert programs for functions such as workpiece transfer for full-surface machining. In this parameter you can define which expert programs (subprograms) are to be used. Enter the subprogram names.
7.6 Machining Parameters 23 – Template management Available as of software version 625 952-05. Select whether constants are to be output when templates are used. Template management Output of constants with templates 0: Without output of constants 1: With output of constants 24 – Parameter of the rechucking subroutines Available as of software version 625 952-05. With this parameter you influence the transfer parameters of the rechucking subroutines.
Operating Resources HEIDENHAIN CNC PILOT 4290 607
8.1 Tool Database 8.1 Tool Database The CNC PILOT stores up to 999 tool descriptions which are managed via the tool editor. Data exchange and data backup: The CNC PILOT supports data exchange and data backup of operating resources (tools, chucking equipment, technology data) and the associated fixed-word list (see “Parameters and Operating Resources” on page 674). Tools that do not fit into any of the standard tool type groups are assigned to special turning/drilling/milling tools.
8.1 Tool Database Describing the new tool (entering the tool type directly) Select “New direct.” The tool type is known: Enter the “Tool type”. The tool type is not known: Press the soft key and define the tool type by entering the following data: Main group Subgroup Machining direction Enter the tool data. Describing the new tool (selecting the tool type) Select “New menu.” Select the tool type from the menu. Enter the tool data.
8.1 Tool Database Tool lists Use the tool lists as a starting point for editing, copying or deleting entries. Abbreviations in the header of the tool list: rs: Cutting radius db: Drill diameter df: Cutter diameter ew: Tool angle bw: Drill angle fw: Cutter angle T no.: T number of the turret list Calling a tool list The editor lists the current tool carrier assignments. Soft keys Delete tool entry The editor lists the entries sorted by tool type.
8.1 Tool Database Editing the tool list Place the cursor on the tool you want to edit. Copy the entry. Deleting an entry Press the soft key or Enter key. The CNC PILOT presents the tool data for editing. Copying tools: You can only copy “similar” tools. The “new” tool is assigned a new ID number. Displaying the tool graphic The CNC PILOT generates the displayed tool from the parameters. The graphic enables you to check the entered data. Changes become effective as soon you exit the input box.
8.1 Tool Database Overview of tool types Special tools are tools that do not fit into any other type. They are not used for contour cycles and are not used by TURN PLUS.. Lathe tools Roughing tool (type 11x) Finishing tool (type 12x) Threading tool, standard (type 14x) Recessing tool (type 15x) Parting tool (type 161) Button tool (type 21x) Copying tool (type 22x) – TURN PLUS uses copying tools only for undercut types H and K.
8.
8.1 Tool Database Tool parameters The use of the tool parameters is indicated by the following letters: G: Basic data S: Depicting the tool during simulation/control graphics TP: Information for TURN PLUS (tool selection) Parameters for turning tools Example: Tool type 111 Parameters in dialog box 1 G S TP ID: Tool ID number • • • X, Z, Y dim. (xe, ze, ye): Setting dimensions • – – Tool an. (ew): Tool angle • • • Tip an.
G S TP T hold. DIN: Type of tool holder – • – T hold. heig. (wh): Height of tool holder – • – T hold. brea. (wb): Width of tool holder – • – Breadth (dn): Tool width (tool tip to shank back) – • – Shank d (sd): Shank diameter – • – Design (A) • • • • • • Pitch: Thread pitch • – • Available: Physical availability – – • Picture no. – • – Cutting material – – • CSP comp.: Compensation factor for cutting speed – – • FDR comp.
8.1 Tool Database Drilling tool parameters Example: Tool type 311 Parameters in dialog box 1 G S TP ID: Tool ID number • • • X, Z, Y dim. (xe, ze, ye): Setting dimensions • – – Diamet. (db): Drill diameter • • • Bor.ang. (bw): Drill angle • • • Tip an. W (sw): Point angle • • • Shnk.di. (d1): Shank diameter • • • Shnk.ln. (l1): Shank length • • • Pos.ang. (rw): Position angle • • – X, Z, Y comp. (DX, DZ, DY): Compensation values (maximum +/– 10 mm) • – – Dir.rot.
G S TP T hold. DIN: Type of tool holder – • – T hold. heig. (wh): Height of tool holder – • – T hold. brea. (wb): Width of tool holder – • – Chck.di. (fd): Diameter of chuck – • – Chck.he. (fh): Height of chuck – • – Sali.lg.(ax): Salient length – • – Pitch (hb): Thread pitch • – • Fit qual(ity): H6, H7, H8, H9, H10, H11, H12 or H13 – – • Available: Physical availability – – • Picture no. – • – Cutting material – – • CSP comp.
8.1 Tool Database Milling cutter parameters Example: Tool type 611 Parameters in dialog box 1 G S TP ID: Tool ID number • • • X, Z, Y dim. (xe, ze, ye): Setting dimensions • – – Diamet. (df): Cutter diameter, end • • • Diamet. (d1): Cutter diameter • • • Width (fb): Cutter width • • • Angle (fw): Cutter angle • • • Dep.imm. (et): Maximum infeed depth • • – Pos.ang. (rw): Position angle • • – X, Z, Y comp.
G S TP T hold. DIN: Type of tool holder – • – T hold. heig. (wh): Height of tool holder – • – T hold. brea. (wb): Width of tool holder – • – Chck.di. (fd): Diameter of chuck – • – Chck.he. (fh): Height of chuck – • – Sali.lg.(ax): Salient length – • – Pitch (hf): Thread pitch • – – Threads per unit length (gb) for multiple threads – – – Tooth type: – – • Available: Physical availability – – • Picture no. – • – Cutting material – – • CSP comp.
8.1 Tool Database Parameters for workpiece handling systems and encoders Example: Tool type 811 Parameters in dialog box 1 G S TP ID: Tool ID number • • • X, Z, Y dim. (xe, ze, ye): Setting dimensions • – – Available: Physical availability • – – Shank d (sd): Shank diameter – • – Multi.
8.1 Tool Database Parameters in dialog box 3 M ID: Identification number of the following cutter of a multipoint tool Mon(itoring) type of tool life monitoring (see “Tool programming” on page 121) None Tool life monitoring Quantity, monitoring for number of parts produced Tool life total: Tool life of the cutting edge Tool life rem.
8.1 Tool Database Data input for multipoint tools For the primary cutting edge: U Parameter input (dialog boxes 1 and 2). U Switch to dialog box 3 by pressing the “Page Up” key. U “Multi. tool” input box: Enter the Main (cutting edge). U “M ID” input box: Enter the ID number of the next secondary cutting edge. U Conclude the dialog box by pressing OK. For each secondary cutting edge: U U U U U U Enter the ID number (ID number specified in “M-ID” of the previous cutting edge).
8.1 Tool Database Compensation values (DX, DY, DZ, DS): Compensation for the wear of the cutting edge. For recessing and button tools, DS stands for the compensation value of the third side of the tool (away from the tool reference point). Cutting length (sl): Length of the cutting edge The contour-based cycles check whether the tool can execute the required machining operation. “sl” influences the tool selection of TURN PLUS.
8.1 Tool Database Mount type: If different tool mounts exist, the tool and the tool location must have the same mount type (see MP 511, ...). Influences the tool selection and tool placement in TURN PLUS. The “Set up tool table” functions check whether the tool can be used at the specified turret position. Angle of orientation (rw): Defines the deviation from the main machining direction in the mathematically positive direction of rotation (–90° < rw < +90°) – see illustration.
8.
8.1 Tool Database Holder group 4 X5 driven, axial Holder group 5 X6 driven, radial X7 driven, special holder Adapter When an adapter is used, the values entered for tool height (wh) and tool width (wb) refer to the height/width of the adapter and the holder.
8.1 Tool Database Tool mounting position The mounting position is fixed by the machine tool builder (see MP 511, ...) Depending on the turret location, the CNC PILOT determines the tool mounting position: AP=0: axial mount – left turret side AP=1: radial mount – left turret side AP=2: radial mount – right turret side AP=3: axial mount – right turret side When the tool is mounted radially in the middle of the turret, “AP=1” is used.
8.2 Database for Chucking Equipment 8.2 Database for Chucking Equipment The CNC PILOT stores up to 999 chucking equipment descriptions which are managed via the chucking equipment editor. Chucking equipment is used in TURN PLUS mode and displayed in the simulation/control graphics. The chuck parameters can be omitted provided that you do not use TURN PLUS, or do not wish chucks to be displayed in the simulation graphics. ID number: Each chuck has its own ID number (up to 16 numbers/ letters).
8.2 Database for Chucking Equipment Chucking equipment lists The CNC PILOT lists the chucking equipment according to identification numbers or chuck types. The chucking equipment list serves as starting point for editing, copying or deleting entries. The header of the list indicates the entered mask, the number of chucks found, the number of chucks stored, and the maximum number of chucks. Calling the chucking equipment list The editor lists the entries sorted by chuck type.
8.2 Database for Chucking Equipment Chucking equipment data Overview of chuck types Primary chucking equipment Chucking equipment Model Chuck Chuck jaws 21x Chucking equipment Collet chuck 220 Chuck Model Mandrel 23x Collet chuck 110 Face driver 24x Two-jaw chuck 120 Rotating gripper 25x Three-jaw chuck 130 Dead center 26x Four-jaw chuck 140 Lathe center 27x Face chuck 150 Centering cone 28x Special chuck 160 Adapters for chuck type 21x Adapters for chuck types 23x..
8.2 Database for Chucking Equipment Chuck Example: Three-jaw chuck (type 130) Parameters, chuck (type 1x0) ID: Chuck identification number Available: Physical availability (fixed-word list) Jaw con.: Code for jaw adapter d: Chuck diameter l: Chuck length max.cl.dia. (d1): Maximum clamping diameter min.cl.dia. (d2): Minimum clamping diameter dz: Centering diameter max.
8.2 Database for Chucking Equipment Code for jaw adapter: When specific combinations of chuck and jaws are required, enter the appropriate jaw adapter code. For both the chuck and the required chuck jaws, enter the same code. Jaw con.=0: All chuck jaws are permitted.
8.2 Database for Chucking Equipment Chuck jaws Example: Chuck jaw (type 211) Parameters, chuck jaws (type 21x) ID: Chuck identification number Available: Physical availability (fixed-word list) Jaw con.: Code for jaw adapter – must correspond to the jaw adapter code of the chuck L: Width of jaws H: Height of jaws G1: Dimension, step 1 in Z direction G2: Dimension, step 2 in Z direction S1: Dimension, step 1 in X direction S2: Dimension, step 2 in X direction min.cl.dia. (d2): Minimum clamping diameter max.
8.
8.
8.2 Database for Chucking Equipment Mandrel Example: Mandrel (type 231) Parameters, mandrel (type 23x) ID: Chuck identification number Available: Physical availability (fixed-word list) Mandril length LD: Total length DF: Flange diameter BF: Flange width max.cl.dia.: Maximum clamping diameter min.cl.dia.
8.2 Database for Chucking Equipment Face driver Example: Face driver (type 241) Parameters, face driver (type 24x) ID: Chuck identification number Available: Physical availability (fixed-word list) ds: Tip diameter ls: Tip length DK: Body diameter BK: Body width DF: Flange diameter BR: Flange width d1: Maximum clamping diameter d2: Minimum clamping diameter Rotating gripper Parameters, rotating gripper (type 25x) ID: Chuck identification number Available: Physical availability (fixed-word list) Nom.dia.
8.
8.
8.
8.3 Technology Database 8.3 Technology Database The CNC PILOT saves the technology data (cutting values) in a threedimensional table depending on the following information: Material (of the workpiece) Cutting material (material of the tool's cutting edge) Machining operation The types of machining are specified. Define the workpiece material and cutting material by fixed-word list and assign them to the table (see figure). The cutting data is managed in the technology editor.
8.3 Technology Database Editing the technology data The technology database contains the following data: Specific cutting effort for the material: The parameter is for information only; it is not evaluated. Cutting speed Main feed rate [mm/rev] for the main machining direction Auxiliary feed rate [mm/rev] for the secondary machining direction Depth of cut With/without coolant: The automatic working plan generation (AWG) uses this parameter to determine whether coolant is used.
8.3 Technology Database Cutting-value tables Call the technology editor: U Select “Tech(nology data)” in the Parameter mode. Calling the cutting-value tables Select “Tab. material.” The “List by materials” dialog box appears. Specify the machining method and cutting material. The CNC PILOT lists the technology data, sorted by material. Select “Tab. cut material.” The “List by cutting materials” dialog box appears. Specify the material and machining method.
8.
Service and Diagnosis HEIDENHAIN CNC PILOT 4290 645
9.1 The Service Mode of Operation 9.1 The Service Mode of Operation The Service mode of operation features: Service functions: User registration and user management, language switching and different system settings Diagnostic functions: Functions for system inspection and support when searching for errors Maintenance system: Reminds the machine user about necessary maintenance and repair tasks.
9.2 Service Functions 9.2 Service Functions Access authorization Functions such as editing important parameters are reserved for privileged users. The control permits access when the correct password is entered. The access authorization remains in effect until the user logs off or until a second user logs on correctly. The password consists of a 4-digit number. It is entered “masked” (not visible).
9.2 Service Functions System service “Sys.srv.” (System service) drop-down menu Date/Time: Error messages are recorded together with the date and time they occurred. Since all errors are stored in a log file for a long period of time, you should always ensure that the date and time are correctly set. These data facilitate the fault diagnosis in case you require field service. Language switching: Select the language with the soft key “>>” and press “OK”.
9.2 Service Functions Fixed-word lists Material/Cutting material: The CNC PILOT manages the designations of workpiece materials and cutting materials in fixedword lists. Use them to adapt the technology database to your requirements (see “Technology Database” on page 641). Fit: The parameter “Fit” is included for the delta drill and reamer tools. Specify the desired fit qualities in the “0WZPASSU” fixed-word list.
9.3 Maintenance System 9.3 Maintenance System The CNC PILOT reminds the machine user of the required maintenance and repair tasks. Each action is described in brief form (assembly, maintenance interval, responsible person, etc.). This information is shown in the “maintenance and repair jobs“ list. A comprehensive description of the maintenance action is provided if desired. As soon as you acknowledge a completed maintenance measure, the maintenance interval restarts.
9.3 Maintenance System Maintenance dates and intervals Dates and intervals (see illustration): I – interval: Time period of the maintenance interval, specified by the machine manufacturer. During the on-time of the control, the current maintenance interval is continuously reduced. The maintenance system displays the remaining time in the “When” column. D – duration: Time period between “due” and “overdue,” specified by the machine manufacturer.
9.3 Maintenance System Displaying maintenance actions Information on maintenance actions Call the maintenance system: U Select “Maintenance” in the Service mode. The maintenance system displays the “Maintenance and repair actions” list. U Change to part 2 of the list. U Change to part 1 of the list. U The vertical arrow keys and the Page Up/Dn keys move the cursor within the list. U Return to Service mode.
9.3 Maintenance System The entries in the Maintenance actions list have the following meanings: Type: See the “Type of maintenance action” table.
9.3 Maintenance System Special maintenance action lists Call lists according to the “Type” or “Status” of maintenance actions: U Switch to the soft-key row “Type/status of actions”. U Call the “All repair actions” list or another special list (see soft-key table). U Return to the general maintenance system. Call the list of acknowledged maintenance actions: U Call the “Acknowledged actions” list.
9.4 Diagnosis 9.4 Diagnosis Information and display Call the Diagnosis submenu: U Select “Diag(nosis)” in the Service - Maintenance mode. U Return to Service mode. The “Diagnosis” submenu provides information, test and control functions that help you with troubleshooting. “Info” menu item: Provides information on the software modules being used. As of software version 625 952-02: Information about OEM data is also displayed, if available.
9.4 Diagnosis Log files and network settings “Log files” drop-down menu: Errors, system events, and data exchange between different system components are recorded in log files. Display error log: Displays the most recent error message. To view further entries, press the PgUp/PgDn keys. Save error log file: Makes a copy of the error log file (file name: error.log; Directory: Para_Usr). Existing "error.log" files are overwritten.
9.4 Diagnosis Software update A software update provides new system functions or installs bug fixes released by HEIDENHAIN. To update the software, proceed as follows: U Log on in the System Manager user class. U Select “Controls > Software Update > User Update“ in the Diagnosis menu. The CNC PILOT opens the “Software Update” dialog box. U In this dialog box, the CNC PILOT offers to make a backup copy of the current software. HEIDENHAIN recommends making this backup.
9.
Transfer HEIDENHAIN CNC PILOT 4290 659
10.1 The Transfer Mode of Operation 10.1 The Transfer Mode of Operation The Transfer mode is used for data backup and data exchange with other data processing systems. The transferred files contain NC programs (DIN PLUS or TURN PLUS), *DXF files, parameter files, or files with information for service personnel (oscilloscope data, log files, etc.). The Transfer mode also includes organizational functions such as copying, deletion, renaming, etc.
10.1 The Transfer Mode of Operation Function overview of the Transfer mode of operation: Network: Activates the WINDOWS network and shows the “masked” files of the CNC PILOT and the communications partner. Serial: Activates serial data transmission and displays the “masked” files of the CNC PILOT. FTP: Activates the FTP network and shows the “masked” files of the CNC PILOT and the communications partner. USB storage media: The CNC PILOT supports Windows XP compatible USB mass storage devices.
10.1 The Transfer Mode of Operation USB interfaces: The CNC PILOT is prepared for the connection of standard storage media with USB interface. Serial: You transfer program or parameter files via serial interface – without protocol. Ensure that your communications partner complies with the defined interface parameters (baud rate, word length, etc.). Printer: The CNC PILOT does not control the printer directly.
10.1 The Transfer Mode of Operation Configuring Windows networks HEIDENHAIN recommends configuration of the Windows networks by the authorized personnel of your machine manufacturer. Configuring a network As of software version 625 952-04: You configure the network and edit the settings in the Windows dialog box.
10.1 The Transfer Mode of Operation Call the Security window: U U U Press CTRL+ALT+DEL. Windows opens the Security window. Use Log-off to log the current Windows user off. Log on with another Windows user name (with network configuration privileges, for example). If you have to restart the operating system after changing operatingsystem settings, for example, you should shut down the system and switch off the control before restarting.
10.1 The Transfer Mode of Operation Changing the computer name Computer name: You must be logged on as an “Administrator” in Windows XP before the computer name can be changed. U Select “Network Connections > Advanced > Network Identification”. U Enter the new computer name. Set the workgroup or domain Selection: U Select “Setting > Network” in the Transfer mode.
10.1 The Transfer Mode of Operation Configuring the serial interface or “printer” Configure serial interface U U U Logon as “System Manager” Select “Setting > Serial” in the Transfer mode. The CNC PILOT opens the “Serial setting” dialog box. Enter the parameters of the serial interface. Define the interface parameters in consultation with the communications partner. Baud rate (in bits per second): The baud rate is defined according to the local condition (cable length, interference, etc.).
10.1 The Transfer Mode of Operation Configure “printer” U U U Log in as “System Manager” Select “Setting > Printer” in the Transfer mode. The CNC PILOT opens the “Printer setting” dialog box. Enter “FILE” in the “Device name” field. The other parameters have no effect. The printout is prepared and output to a file named “PRINT_xx.txt” (xx: 00 to 19) in the “Data” directory. Maximum file size: 1 MB For DataPilot, you can also use the “STD” entry for the Windows standard printer.
10.2 Data Transfer 10.2 Data Transfer Enabling, file types Shared directories of the CNC PILOT: see table. Computer systems in the network can access the files located in the shared directories of the CNC PILOT. For security reasons, however, HEIDENHAIN recommends initiating the data exchange from the control. The network rules of WINDOWS XP apply when accessing shared directories. ..\NCPS NC main programs and subprograms, template files ..
10.2 Data Transfer Basics of operation Window contents: In the left window File transfer: CNC PILOT-specific files Parameters/operating resources: Files in “internal format” In the right window File transfer: Files of the communications partner Parameters/operating resources: Files in ASCII format (PARA_USR or BACKUP directory) Mark files: When using data transfer and organization functions, you mark the file(s) you want to transfer or edit.
10.2 Data Transfer Enter the mask: “*”: Any desired (number of) characters can be specified at this position. “?”: Any desired character can be specified at this position. The CNC PILOT automatically adds an asterisk * to the mask you have defined, and displays the current mask setting below the menu line. Position the cursor Horizontal arrow keys: Move from left to right window and vice versa.
10.2 Data Transfer Transmitting and receiving files When you select “Network” or “FTP”, the CNC PILOT will display an error message if the communications partner does not respond within a specific time. The parameters and operating resource data need to be converted before transfer, and vice versa (see “Parameters and Operating Resources” on page 674). Data exchange using USB storage media: Enter “D:\” as the transfer directory (dialog box: “Network Settings”).
10.2 Data Transfer Ethernet-based transfer Select “Network” (or “FTP”) in the Transfer menu. Define a mask to limit the number of files displayed. Transmit files: Place the cursor in the left window. Mark the files you want to transfer. Press the soft key. The CNC PILOT transfers the marked files to the communications partner. Receive files: Place the cursor in the right window. Mark the files you want to load. Press the soft key. The CNC PILOT transfers the marked files from the communications partner.
10.2 Data Transfer Transfer via serial interface Select “Serial” in the Transfer menu. The CNC PILOT displays its own files in the left window and the selected interface in the right window. Define a mask to limit the number of files displayed. Transmit files: Mark the files you want to transfer. Press the soft key. The CNC PILOT transfers the marked files over the serial interface. Receive files: Press the soft key. The CNC PILOT changes to readyto-receive state and receives the transferred data.
10.3 Parameters and Operating Resources 10.3 Parameters and Operating Resources The CNC PILOT saves parameters and operating resource data in “internal formats.” Before data is transferred or backed up, it is converted to ASCII format. Vice versa, i.e. when loading or restoring, the CNC PILOT converts the received parameters/operating resource data back to the “internal format” and integrates it in the active parameter/operating resource files in the control.
10.3 Parameters and Operating Resources Transmitting parameters/operating resources Place the cursor in the left window. Transmit a complete file: Select the parameter group or operating resource group. Transmit individual parameters/operating resources: Place the cursor on the parameter group or operating resource group. Press the soft key. The CNC PILOT lists all the parameters/operating resources of this group. Mark the parameter/operating resource you want to convert. Press the soft key.
10.3 Parameters and Operating Resources Loading parameters/operating resources The CNC PILOT expects the parameters/operating resource data to be located in the PARA_USR directory. The CNC PILOT recognizes the parameter group or operating resource group by the file name extension. This is why the file name can be changed on external systems—but not the extension.
10.3 Parameters and Operating Resources Backing up and restoring data Create a data backup: Backing up all parameters and operating resources is performed in two steps: U Select “Backup” to create backup files. U Use the standard transfer functions to transfer the backup files to an external system.
10.3 Parameters and Operating Resources Restore a data backup: Restoring is performed in two steps: U Use the standard transfer functions to transfer the backup files from the external system to the BACKUP directory. U Select “Restore” to convert and integrate the backup files. Restore downloads all backup files in the BACKUP directory (except maintenance system files). Restore Log in as “System Manager” Select “Parameter conversion > Backup/Restore” in the Transfer menu.
10.3 Parameters and Operating Resources Viewing parameter, operating-resource or backup files Select “Parameter conversion > Save/Load” (or “.. > Backup/ Restore“) in the Transfer menu. In the right window, place the cursor on a parameter/operating resource file or on a backup file. Press ENTER; the CNC PILOT displays the file contents. Close the file: Press ENTER again (or press the ESC key). Press the ESC key to return to the Transfer main menu.
10.4 File Organization 10.4 File Organization Fundamentals for file organization You can organize NC program files and parameter files with the Copy, Delete and Rename functions. The Print function is additionally available for ASCII files.
10.4 File Organization Managing files Manage CNC PILOT files Select “Org(anization)” in the Transfer menu. Define a mask to limit the number of files displayed. Place the cursor on the parameter or operating resource file. Mark the required files. Press ENTER. The CNC PILOT displays the file contents. Press the soft key. The CNC PILOT deletes the marked files. Press the soft key and enter the new file name. The CNC PILOT renames the file. Press the soft key and enter the name of the new file.
10.4 File Organization Manage CNC PILOT files and external files Log on as System Manager (or higher). Select “Network” in the Transfer menu. Press the soft key. The CNC PILOT activates the organization functions for its own files and for those of the communications partner. Place the cursor in the left or right window. Place the cursor on the parameter or operating resource file. Mark the required files. Press ENTER. The CNC PILOT displays the file contents. Press the soft key.
Tables and Overviews HEIDENHAIN CNC PILOT 4290 683
11.1 Undercut and Thread Parameters 11.1 Undercut and Thread Parameters Undercut DIN 76, Parameters TURN PLUS determines the parameters for the thread undercut (undercut DIN 76) from the thread pitch. The undercut parameters are in accordance with DIN 13 for metric threads. External thread Thread pitch I K R W External thread Thread pitch I K R W 0.2 0.3 0.7 0.1 30° 1.25 2 4.4 0.6 30° 0.25 0.4 0.9 0.12 30° 1.5 2.3 5.2 0.8 30° 0.3 0.5 1.05 0.16 30° 1.75 2.6 6.
I K R W Internal thread Thread pitch I K R W 0.2 0.1 1.2 0.1 30° 1.25 0.5 6.7 0.6 30° 0.25 0.1 1.4 0.12 30° 1.5 0.5 7.8 0.8 30° 0.3 0.1 1.6 0.16 30° 1.75 0.5 9.1 1 30° 0.35 0.2 1.9 0.16 30° 2 0.5 10.3 1 30° 0.4 0.2 2.2 0.2 30° 2.5 0.5 13 1.2 30° 0.45 0.2 2.4 0.2 30° 3 0.5 15.2 1.6 30° 0.5 0.3 2.7 0.2 30° 3.5 0.5 17.7 1.6 30° 0.6 0.3 3.3 0.4 30° 4 0.5 20 2 30° 0.7 0.3 3.8 0.4 30° 4.5 0.5 23 2 30° 0.75 0.
11.1 Undercut and Thread Parameters Undercut DIN 509 E, Parameters Diameter I K R W <=1.6 0.1 0.5 0.1 15° > 1.6 – 3 0.1 1 0.2 15° > 3 – 10 0.2 2 0. 2 15° > 10 – 18 0.2 2 0.6 15° > 18 – 80 0.3 2.5 0.6 15° > 80 0.4 4 1 15° The undercut parameters are determined from the cylinder diameter. Where: I: Undercut depth K: Undercut width R: Undercut radius W: Undercut angle Undercut DIN 509 F, Parameters Diameter I K R W P A <=1.6 0.1 0.5 0.1 15° 0.1 8° > 1.
11.1 Undercut and Thread Parameters Thread Parameters To determine the thread parameters, the CNC PILOT uses the following table; Where: F: Thread pitch. Where an asterisk “*” is given in the table, the thread pitch is calculated from the diameter, depending on the thread type (see “Thread pitch” on page 688) . P: Thread depth R: Thread width A: Thread angle, left W: Thread angle, right Calculation formula: Kb = 0.26384*F – 0.
11.1 Undercut and Thread Parameters Thread type Q F P R A W Internal * 0.54127*F F 30° 30° External * 0.61343*F F 30° 30° Internal * 0.54127*F F 30° 30° Q=15 UNEF U.S. extra-fine-pitch thread External * 0.61343*F F 30° 30° Internal * 0.54127*F F 30° 30° Q=16 NPT U.S. taper pipe thread External * 0.8*F F 30° 30° Internal * 0.8*F F 30° 30° External * 0.8*F F 30° 30° Q=14 UNF US fine-pitch thread Q=17 NPTF U.S. taper dryseal pipe thread Internal * 0.
11.1 Undercut and Thread Parameters Q = 8 Cylindrical round thread Diameter Thread pitch 12 2.54 14 3.175 40 4.233 105 6.35 200 6.35 Q = 9 Cylindrical Whitworth thread Thread designation Diameter (in mm) Thread pitch Thread designation Diameter (in mm) Thread pitch 1/4“ 6.35 1.27 1 1/4“ 31.751 3.629 5/16“ 7.938 1.411 1 3/8“ 34.926 4.233 3/8“ 9.525 1.588 1 1/2“ 38.101 4.233 7/16“ 11.113 1.814 1 5/8“ 41.277 5.08 1/2“ 12.7 2.117 1 3/4“ 44.452 5.08 5/8“ 15.
11.1 Undercut and Thread Parameters Q = 11 Whitworth pipe thread Thread designation Diameter (in mm) Thread pitch Thread designation Diameter (in mm) Thread pitch 1/8“ 9.728 0.907 2“ 59.614 2.309 1/4“ 13.157 1.337 2 1/4“ 65.71 2.309 3/8“ 16.662 1.337 2 1/2“ 75.184 2.309 1/2“ 20.995 1.814 2 3/4“ 81.534 2.309 5/8“ 22.911 1.814 3“ 87.884 2.309 3/4“ 26.441 1.814 3 1/4“ 93.98 2.309 7/8“ 30.201 1.814 3 1/2“ 100.33 2.309 1“ 33.249 2.309 3 3/4“ 106.68 2.
11.1 Undercut and Thread Parameters Q = 14 UNF U.S. fine-pitch thread Thread designation Diameter (in mm) Thread pitch Thread designation Diameter (in mm) Thread pitch 0.06“ 1.524 0.3175 3/8“ 9.525 1.058333333 0.073“ 1.8542 0.352777777 7/16“ 11.1125 1.27 0.086“ 2.1844 0.396875 1/2“ 12.7 1.27 0.099“ 2.5146 0.453571428 9/16“ 14.2875 1.411111111 0.112“ 2.8448 0.529166666 5/8“ 15.875 1.411111111 0.125“ 3.175 0.577272727 3/4“ 19.05 1.5875 0.138“ 3.5052 0.
11.1 Undercut and Thread Parameters Q = 16 NPT U.S. taper pipe thread Thread designation Diameter (in mm) Thread pitch Thread designation Diameter (in mm) Thread pitch 1/16“ 7.938 0.94074074 3 1/2“ 101.6 3.175 1/8“ 10.287 0.94074074 4“ 114.3 3.175 1/4“ 13.716 1.411111111 5“ 141.3 3.175 3/8“ 17.145 1.411111111 6“ 168.275 3.175 1/2“ 21.336 1.814285714 8“ 219.075 3.175 3/4“ 26.67 1.814285714 10“ 273.05 3.175 1“ 33.401 2.208695652 12“ 323.85 3.175 1 1/4“ 42.
11.1 Undercut and Thread Parameters Q = 19 NPFS U.S. cylindrical pipe thread without lubricant Thread designation Diameter (in mm) Thread pitch Thread designation Diameter (in mm) Thread pitch 1/16“ 7.938 0.94074074 1/2“ 21.336 1.814285714 1/8“ 10.287 0.94074074 3/4“ 26.67 1.814285714 1/4“ 13.716 1.411111111 1“ 33.401 2.208695652 3/8“ 17.145 1.
11.2 Pin Layouts and Connecting Cables for the Data Interfaces 11.2 Pin Layouts and Connecting Cables for the Data Interfaces RS-232-C/V.24 interface for HEIDENHAIN devices The interface complies with the requirements of EN 50 178 for “low voltage electrical separation.” Please note that pins 6 and 8 of the connecting cable 274 545 are bridged.
Pin Assignment Socket Color Pin Adapter block 363 987-02 Socket Pin Socket Color Socket 1 Do not assign 1 Red 1 1 1 1 Red 1 2 RXD 2 Yellow 2 2 2 2 Yellow 3 3 TXD 3 White 3 3 3 3 White 2 4 DTR 4 Brown 4 4 4 4 Brown 6 5 Signal GND 5 Black 5 5 5 5 Black 5 6 DSR 6 Violet 6 6 6 6 Violet 4 7 RTS 7 Gray 7 7 7 7 Gray 8 8 CTR 8 White/Green 8 8 8 8 White/Green 7 9 Do not assign 9 Green 9 9 9 9 Green 9 Hsg. Ext.
11.2 Pin Layouts and Connecting Cables for the Data Interfaces RS-422/V.11 interface Only non-HEIDENHAIN devices are connected to the RS-422 interface. The interface complies with the requirements of EN 50 178 for “low voltage electrical separation.” The pin layouts on connection X28 (main computer) and on the adapter block are identical.
Specifications CNC PILOT 4290 – Specifications Basic version Contouring control with integrated motor control and integrated inverter 2 closed-loop axes X1 and Z1 on slide 1 1 feedback-controlled spindle Expandable to Maximum 10 control loops Maximum 6 slides Maximum 4 drives Maximum 2 C axes Components MC 420 or MC 422C main computer CC 422 or CC424 controller unit Operating panel 15-inch TFT color flat-panel display with soft keys Program memory Hard disk Input resolution and dis
11.
CNC PILOT 4290 TURN PLUS (option 1) TURN PLUS comprises: Programming with graphic support Graphically supported, interactive sequential programming with DIN PLUS program generation Automatic DIN PLUS program generation with DIN PLUS program generation TURN PLUS is used for: Turning C-axis machining (option 1.1) Y-axis machining Full-surface machining with opposing spindles (option 1.
11.3 Technical Information Standard functions CNC PILOT 4290 TURN PLUS – Sequential programming with interactive graphics Sequential programming for individual machining steps with: TURN PLUS – Automatic sequential programming Automatic working plan generation with: Automatic tool selection Automatic turret assignment Automatic calculation of cutting data Automatic generation of machining sequence in all working planes (also for C-axis machining (with option 1.
? – Simplified geometry programming ... 120 /.. Skip level ... 326 # variables In NC program conversion ... 122 Programming ... 316 # variables input ... 312 # variables output ... 313 $.. Slide code ... 326 SYMBOLE 3-D view ... 382 4-axis machining Cycle G810 ... 215 Cycle G820 ... 217 9-field box ... 49 A Absolute coordinates ... 41 Acceleration (slope) G48 ... 192 Access authorization ... 647 Active tool ... 320 Actual value display, display settings ... 571 Actual values in variables G901 ...
Index Circular slot DIN PLUS Front/rear face G302-/G303Geo ... 175 Lateral surface G312-/G313Geo ... 182 In circular patterns ... 169 TURN PLUS Front/rear face ... 432 Lateral surface ... 444 Comments Fundamentals ... 112 Input in geometry menu ... 125 Input in machining menu ... 126 Compensation Additive compensation G149 ... 209 Additive compensation G149Geo ... 167 Enter the compensation values. ... 87 Compensation of right/left-hand tool tip G150/G151 ... 210 Compensation values ...
D display ... 98 D display (display element) ... 97 Data backup Transfer mode ... 660 Data exchange (transfer) ... 660 Data input/output (NC program) ... 312 Data interfaces ... 694 Data transfer ... 660 Data transfer methods ... 661 DataPilot ... 660 Date, setting ... 648 Debug ... 374, 376, 380 Deburring DIN PLUS cycle G840 ... 268 TURN PLUS machining attribute ... 478 Deep-hole drilling G74 ... 251 Default value ... 56 Define tool position G712 ... 723 Delete Contour elements, deleting (TURN PLUS) ...
Index F Face roughing G820 ... 215 Feed per minute Linear axes G94 ... 194 Manual control ... 62 Rotary axes G192 ... 193 Feed per revolution G95 ... 194 Feed rate Constant G94 ... 194 Feed per minute for rotary axes G192 ... 193 Feed rate override 100% G908 ... 307 Feed rate reduction factor G38Geo ... 165 Feed-rate override, Automatic mode ... 87 In Manual Control mode ... 62 Interrupted feed G64 ... 193 Per revolution G95-Geo ... 166 Per revolution Gx95 ... 194 Per tooth Gx93 ... 194 Rotary axes G192 ..
HEIDENHAIN CNC PILOT 4290 G192 Feed per minute for rotary axes ... 193 G2 Circular path ... 190 G204 Wait for moment ... 305 G26 Speed limitation ... 192 G3 Circular path ... 190 G30 Converting and mirroring ... 282 G31 Thread cycle ... 240 G32 Simple thread cycle ... 242 G33 Thread single path ... 244 G36 Tapping ... 250 G4 Period of dwell ... 302 G40 Switch off TRC/MCRC ... 197 G41 Switch on TRC/MCRC ... 197 G42 Switch on TRC/MCRC ... 197 G47 Safety clearance ... 206 G48 Acceleration (slope) ...
Index G913 Switch off in-process measuring ... 296 G914 Switch off probe monitoring ... 296 G915 Post-process measuring ... 298 G916 Traversing to a fixed stop ... 288 G917 Controlled parting ... 291 G918 Velocity feedforward ... 307 G919 Spindle override 100% ... 307 G920 Deactivating zero shifts ... 308 G921 Deactivating zero-point shifts, tool lengths ... 308 G922 shaft speed with V constant ... 311 G93 Feed per tooth ... 194 G930 Sleeve monitoring ... 310 G933 Thread switch ...
M M ... 331 M commands In Manual Control mode ... 63 M97 Synchronous function ... 286 M99 program end with return jump ... 330 TURN PLUS program head ... 393 M commands in DIN PLUS programming ... 330 M commands, TURN PLUS ... 497 HEIDENHAIN CNC PILOT 4290 Machine commands ... 331 Machine Data ... 62 Machine datum ... 40 Machine display Adjusting/switching ... 97 Display elements ... 97 Fundamentals ... 46 Parameters for machine display ... 580 Machine operating panel ... 47 Machine parameters (MP) ...
Index Mirroring DIN PLUS Converting and mirroring G30 ... 282 Mirror/shift contour G121 ... 202 TURN PLUS Copying a contour section by mirroring ... 453 Transformations – Mirroring ... 469 Modal address parameters ... 120 Modal G functions ... 120 Monitoring zone definition G995 ... 301 Motion simulation ... 380 Mount type ... 622 Multipoint tools Tool parameters ... 620 Tool programming ... 121 Multi-slide programming Example of dual-slide machining ... 338, 340 Example of positioning the steady rest ...
HEIDENHAIN CNC PILOT 4290 Post-process measuring Cycle G915 ... 298 Status ... 96 Precision stop DIN PLUS attribute for contour description ... 164 DIN PLUS machining commands ... 302 TURN PLUS attribute ... 479 Predrilling (IWG) ... 517 Preparing a machining process (TURN PLUS) ... 482 Chucking a workpiece at the spindle ... 483 Chucking a workpiece at the tailstock ... 483 Defining a cutting limitation ... 484 Deleting the chucking data ... 484 Fundamentals ... 482 Rechuck – 1st setup after 2nd setup ...
Index Rear-side machining DIN PLUS Section code ... 144 TURN PLUS Machining sequence ... 536 Preconditions for full-surface machining ... 560 Recess turning DIN PLUS cycle G869 ... 225 TURN PLUS IWG recess turning radial/axial ... 510 Recessing DIN PLUS Contour based recessing G860 ... 222 Recess contour (general) G23Geo ... 153 Recess contour (standard) G22Geo ... 152 Recessing cycle G866 ... 224 Recessing G860 ... 222 Simple G86 ... 236 Simple G866 ... 224 TURN PLUS Form element, general recess ...
HEIDENHAIN CNC PILOT 4290 Simulation 3-D view ... 382 Checking multi-channel programs ... 386 Chucking equipment depiction ... 364 Contour generation during simulation ... 378 Contour Simulation ... 374 Dimensioning ... 375 Display ... 364 Errors and warnings ... 372 Front window ... 368 Line and trace display ... 367 Machining simulation ... 376 Motion simulation ... 380 Operating mode .. ... 362 Screen contents ... 363 Side view (YZ) ... 368 Surface window ... 368 Synchronous point analysis ...
Index Start pocket/island G308-Geo ... 168 Starting length (thread) ... 239 Starting point of contour DIN PLUS Display ... 129 Front/rear face G100-Geo ... 172 Lateral surface G110-Geo ... 179 Turning contour G0-Geo ... 147 TURN PLUS Basic contour ... 404 Front/rear face ... 422 Lateral surface ... 435 Starting template ... 354 Step drill ... 612 Stopper tool ... 613 Structure template ... 354 Structured DIN PLUS program ... 108 Subprogram Call ... 327 Fundamentals ... 122 Section code ...
HEIDENHAIN CNC PILOT 4290 IWG Cutting data ... 497 Cycle specification ... 498 Finishing ... 521 Interactive working plan generation ... 494 Milling ... 526 Special machining tasks ... 532 Thread machining ... 525 Tool call ... 497 Machining information Cutting parameters ... 553 Drilling ... 556 Full-surface machining ... 560 Hollowing ... 554 Inside contours ... 555 Shaft machining ... 557 Tool selection ... 552 Turret assignment ... 552 Preparing a machining process Defining a cutting limitation ...
V Values for controlled parting G992 ... 293 Variables # variables ... 316 As address parameters ... 120 Assignment ... 320 Calculations ... 315 Scope (# variables ) ... 316 Scope (V variables) ... 318 Variable display ... 136 Velocity feedforward G918 ... 307 View of contour (simulation) ... 374 W Wait for moment G204 ... 305 Warnings (simulation) ... 372 WHILE.. Program repeat ... 323 Width (of tool) ... 622 WINDOW (special output window) ... 312 Window selection Editing window (DIN PLUS) ...
Program section codes Program section codes Program head Workpiece machining PROGRAMMKOPF [PROGRAM HEAD] Page 136 BEARBEITUNG [MACHINING] Page 144 REVOLVER [TURRET] Page 137 ZUORDNUNG [ASSIGNMENT] Page 144 ENDE [END] Page 144 SCHEIBENMAGAZIN [PLATE MAGZN.
Overview of G Commands in the CONTOUR Section Overview of G Commands in the CONTOUR Section G commands for turning contours Turning contour Turning contour Workpiece-blank definition Contour form elements G20-Geo Chuck part, cylinder/tube Page 146 G34-Geo Thread (standard) Page 159 G21-Geo Cast part Page 146 G37-Geo Thread (general) Page 160 G49-Geo Bore hole at turning center Page 162 Basic Contour Elements G0-Geo Starting point of contour Page 147 Help commands for contour definitio
C-axis contour G302-Geo Circular slot on face Page 175 G315-Geo Rectangle, lateral surface Page 183 G303-Geo Circular slot on face Page 175 G317-Geo Eccentric polygon, lateral surface Page 184 G304-Geo Full circle, face Page 176 G411-Geo Linear pattern, lateral surface Page 185 G305-Geo Rectangle on face Page 176 G412-Geo Circular pattern, lateral surface Page 186 G307-Geo Eccentric polygon on face Page 177 G401-Geo Linear pattern, face Page 177 G402-Geo Circular pattern, face Page 178
Overview of G Commands in the MACHINING Section Overview of G Commands in the MACHINING Section G commands for turning Turning—Basic functions Turning—Basic functions Tool positioning without machining Zero point shifts G0 Positioning in rapid traverse Page 187 G53 Parameter-dependent zero point shift Page 199 G14 Move to the tool change position Page 187 G54 Parameter-dependent zero point shift Page 199 G701 Rapid traverse to machine coordinates Page 187 G55 Parameter-dependent zero poi
Turning—Basic functions Tool-tip radius compensation (TRC/MCRC) Tools, types of compensation G40 Switch off TRC/MCRC Page 197 T Insert the tool Page 207 G41 TRC/MCRC, left Page 197 G148 (Changing the) cutter compensation Page 208 G42 TRC/MCRC, right Page 197 G149 Additive compensation Page 209 G150 Compensate right tool tip Page 210 Overview: Zero point shifts Page 198 G151 Compensate left tool tip Page 210 G51 Page 199 G710 Adding tool dimensions Page 211 Zero point shifts
Overview of G Commands in the MACHINING Section Synchronization commands Synchronization Synchronization Assigning the contour to the operation Spindle synchronization, workpiece transfer G98 Assignment spindle – workpiece Page 283 G30 Converting and mirroring Page 282 G99 Workpiece group Page 284 G121 Contour mirroring/shifting Page 202 Slide synchronization G720 Spindle synchronization Page 286 G62 One-sided synchronization Page 284 G905 Measuring C-angle offset Page 287 G63 Sy
Variable programming, program branches Variable programming, program branches Programming with variables Data input and data output # variables Evaluation during program conversion Page 316 INPUT Input (# variables) V variable Evaluation during program execution Page 318 WINDOW Open output window (# variables) Page 312 Program branches, program repeats Page 312 PRINT Output (# variables) Page 313 IF..THEN.. Program branching Page 322 INPUTA Input (V variables) Page 314 WHILE..
Overview of G Commands in the MACHINING Section Other G Functions Other G Functions Other G Functions G4 Dwell time Page 302 G907 Block speed monitoring off Page 306 G7 Precision stop ON Page 302 G908 Feed rate override 100% Page 307 G8 Precision stop OFF Page 302 G909 Interpreter stop Page 307 G9 Precision stop (blockwise) Page 302 G918 Feedforward on/off Page 307 G15 Move rotary axes Page 303 G919 Spindle override 100% Page 307 G60 Deactivate protection zone Page 303 G9
Y-axis machining Y-axis machining Working planes Milling cycles G16 Tilting the working plane G841 Area milling - roughing G17 XY plane (front or rear face) G842 Area milling - finishing G18 XZ plane (turning) G843 Centric polygon - roughing G19 YZ plane (side view/lateral surface) G844 Centric polygon - finishing Tool positioning without machining G845 Pocket milling, roughing G0 Positioning in rapid traverse G846 Pocket milling, finishing G14 Move to the tool change position G
Overview of G Commands in the MACHINING Section
DR. JOHANNES HEIDENHAIN GmbH Dr.-Johannes-Heidenhain-Straße 5 83301 Traunreut, Germany { +49 8669 31-0 | +49 8669 5061 E-mail: info@heidenhain.de Technical support | +49 8669 32-1000 Measuring systems { +49 8669 31-3104 E-mail: service.ms-support@heidenhain.de TNC support { +49 8669 31-3101 E-mail: service.nc-support@heidenhain.de NC programming { +49 8669 31-3103 E-mail: service.nc-pgm@heidenhain.de PLC programming { +49 8669 31-3102 E-mail: service.plc@heidenhain.
