User’s Manual MANUALplus 620 NC Software 548430-02 548431-02 English (en) 1/2014
Controls and displays of the MANUALplus Keys on visual display unit Key Function Switches the help graphics between outside and inside machining (only in the cycle programming) Numeric keypad Key 0 9 /+ Escape key: Cancelation of dialogs and next higher menu level Switches to the next menu in the PLC menu Insert key: OK in dialogs and new NC blocks in the editor DEL Function Machine operating modes: Manual Operation Program Run smart.
Operating panel of the MANUALplus
MANUALplus 620, software and features This manual describes functions that are available in the MANUALplus with NC software number 548430-02 and 548431-02. The programming of smart.Turn and DIN PLUS are not included in this manual. These functions are described in the User's Manual for smart.Turn and DIN PLUS Programming (ID 685556-xx). Please contact HEIDENHAIN if you require a copy of this manual.
New functions of software 548328-04 In the program simulation, the current contour description (of workpiece blank and finished part) can be mirrored and saved. In smart.
The spindle synchronization option G720 synchronizes the shaft speeds of two or more spindles so that they rotate synchronously with a gear ratio or a defined offset (see the smart.Turn and DIN Programming User’s Manual) In combination with the synchronization (G720) of main spindle and tool spindle, the new "Hobbing" cycle (G808) is available for milling external teeth and profiles (see the smart.
New functions of software 548328-05 and 54843x-01 In the Organization mode of operation, you can grant or restrict access to the control by using the EXTERNAL ACCESS soft key (see also "Organization mode of operation" on page 520) The pocket calculator can now be activated in each application and also remains active after a change in operating modes.
The new TURN PLUS function automatically generates NC programs for turning and milling operations based on a fixed machining sequence (see smart.Turn and DIN Programming User's Manual). The G940 function now provides a way to calculate the tool lengths in the basic (definition) position of the B axis (see smart.Turn and DIN Programming User's Manual). For machining operations that require rechucking, you can define a separation point on the contour description with G44 (see the smart.
New functions of software 54843x-02 The "Zero point shift" miscellaneous function was introduced in ICP (see also "Zero point shift" on page 375) In ICP contours, fit dimensions and inside threads can now be calculated using an input form (see also "Fits and inside threads" on page 370) The "Copy Linear, Circular and Mirror" miscellaneous functions were introduced in ICP (see also "Copying a contour section in linear series" on page 375) The system time can now be set using an input form (see also "
About this manual About this manual The symbols used in this manual are described below. This symbol indicates that important information about the function described must be considered. This symbol indicates that there is one or more of the following risks when using the described function: Danger to workpiece Danger to fixtures Danger to tool Danger to machine Danger to operator This symbol indicates that the described function must be adapted by the machine tool builder.
About this manual
Contents 1 2 3 4 5 6 7 8 9 10 Introduction and fundamentals Basics of operation Machine mode of operation Cycle programming ICP programming Graphic simulation Tool and technology database Organization mode of operation Tables and overviews Overview of cycles HEIDENHAIN MANUALplus 620 13
1 Introduction and fundamentals ..... 33 1.1 The MANUALplus ..... 34 The MANUALplus for cycle lathes ..... 34 MANUALplus for CNC lathes ..... 34 1.2 Configuration ..... 35 Slide position ..... 35 Tool carrier systems ..... 35 The C axis ..... 35 The Y axis ..... 36 Full-surface machining ..... 37 1.3 Features ..... 38 Configuration ..... 38 Operating modes ..... 38 1.4 Data backup ..... 40 1.5 Explanation of terms ..... 41 1.6 MANUALplus design ..... 42 1.7 Fundamentals .....
2 Basics of operation ..... 49 2.1 General information on operation ..... 50 Operation ..... 50 Setup ..... 50 Programming – Teach-in ..... 50 Programming – smart.Turn ..... 50 2.2 The MANUALplus screen ..... 51 2.3 Operation and data input ..... 52 Operating modes ..... 52 Menu selection ..... 53 Soft keys ..... 53 Data input ..... 54 smart.Turn dialogs ..... 54 List operations ..... 54 Alphanumeric keyboard ..... 55 2.4 Integrated calculator ..... 56 Calculator functions .....
3 Machine mode of operation ..... 71 3.1 Machine mode of operation ..... 72 3.2 Switch-on / Switch-off ..... 73 Switch-on ..... 73 Monitoring EnDat encoders ..... 73 Traversing the reference marks ..... 74 Switch-off ..... 75 3.3 Machine data ..... 76 Input of machine data ..... 76 Machine data display ..... 78 Cycle statuses ..... 81 Axis feed rate ..... 82 Spindle ..... 82 3.4 Setting up a tool list ..... 83 Machine with turret ..... 83 Machine with multifix ..... 83 Tools in different quadrants .....
3.8 Teach-in mode ..... 106 Teach-in mode ..... 106 Programming Teach-in cycles ..... 106 3.9 Program Run mode ..... 107 Loading a program ..... 107 Comparing a tool list ..... 108 Before executing a program ..... 108 Finding a start block ..... 109 Program execution ..... 110 Entering compensation values during program run ..... 111 Program execution in "dry run" mode ..... 114 3.10 Graphic simulation ..... 115 3.11 Program management ..... 116 Program selection ..... 116 File manager .....
4 Cycle programming ..... 121 4.1 Working with cycles ..... 122 Cycle starting point ..... 122 Help graphics ..... 123 DIN macros ..... 123 Graphical test run (simulation) ..... 123 Contour follow-up in Teach-in mode ..... 124 Cycle keys ..... 124 Switching functions (M functions) ..... 125 Comments ..... 125 Cycle menu ..... 126 Addresses used in many cycles ..... 128 4.2 Workpiece blank cycles ..... 129 Bar/tube blank ..... 130 ICP workpiece blank contour ..... 131 4.3 Single cut cycles .....
4.4 Turning cycles ..... 146 Tool position ..... 147 Roughing, longitudinal ..... 149 Cut, transverse ..... 151 Roughing, longitudinal—expanded ..... 153 Roughing, transverse—expanded ..... 155 Finishing cut, longitudinal ..... 157 Finishing cut, transverse ..... 158 Finishing cut, longitudinal—expanded ..... 159 Finishing cut, transverse—expanded ..... 161 Cut, longitudinal plunge ..... 163 Cut, transverse plunge ..... 165 Cut, longitudinal plunging—expanded ..... 167 Cut, transverse plunging—expanded ....
4.5 Recessing cycles ..... 198 Cutting and infeed directions for recessing cycles ..... 198 Undercut position ..... 199 Contour forms ..... 199 Recessing, radial ..... 200 Recessing, axial ..... 202 Recessing, radial—expanded ..... 204 Recessing, axial—expanded ..... 206 Recessing radial, finishing ..... 208 Recessing axial, finishing ..... 210 Recessing radial, finishing—expanded ..... 212 Recessing axial, finishing—expanded ..... 214 ICP recessing cycles, radial ..... 216 ICP recessing cycles, axial .....
4.6 Thread and undercut cycles ..... 257 Thread position, undercut position ..... 257 Handwheel superimposition ..... 258 Feed angle, thread depth, proportioning of cuts ..... 258 Thread run-in / thread run-out ..... 259 Last cut ..... 260 Thread cycle (longitudinal) ..... 261 Thread cycle (longitudinal)—expanded ..... 263 Tapered thread ..... 265 API thread ..... 267 Recut (longitudinal) thread ..... 269 Recut (longitudinal) thread—expanded ..... 271 Recut tapered thread ..... 273 Recut API thread .....
4.9 Drilling and milling patterns ..... 336 Linear drilling pattern, axial ..... 337 Milling pattern linear, axial ..... 339 Drilling pattern circular, axial ..... 341 Milling pattern circular, axial ..... 343 Drilling pattern linear, radial ..... 345 Linear milling pattern, radial ..... 347 Drilling pattern circular, radial ..... 349 Circular milling pattern, radial ..... 351 Examples of pattern machining ..... 353 4.10 DIN cycles ..... 356 DIN cycle .....
5 ICP programming ..... 359 5.1 ICP contours ..... 360 Loading contours ..... 360 Form elements ..... 361 Machining attributes ..... 361 Calculation of contour geometry ..... 362 5.2 ICP editor in cycle mode ..... 363 Editing contours for cycles ..... 363 File organization with the ICP editor ..... 364 5.3 ICP editor in smart.Turn ..... 365 Editing a contour in smart.Turn ..... 366 5.4 Creating an ICP contour ..... 368 Entering an ICP contour ..... 368 Absolute or incremental dimensioning .....
5.9 Contour elements on face ..... 398 Starting point of face contour ..... 398 Vertical lines on face ..... 399 Horizontal lines on face ..... 400 Line at angle on face ..... 401 Circular arc on face ..... 402 Chamfer/rounding arc on the face ..... 403 5.10 Contour elements on lateral surface ..... 404 Starting point of lateral surface contour ..... 404 Vertical lines on lateral surface ..... 406 Horizontal lines on lateral surface ..... 406 Line at angle on lateral surface .....
5.14 Contours in the XY plane ..... 432 Reference data in XY plane ..... 432 Starting point of contour in XY plane ..... 433 Vertical lines in XY plane ..... 433 Horizontal lines in XY plane ..... 434 Line at angle in XY plane ..... 435 Circular arc in XY plane ..... 436 Chamfer/rounding arc in XY plane ..... 437 Circle in XY plane ..... 438 Rectangle in XY plane ..... 439 Polygon in XY plane ..... 440 Linear slot in XY plane ..... 441 Circular slot in XY plane ..... 442 Hole in XY plane .....
6 Graphic simulation ..... 467 6.1 Simulation mode of operation ..... 468 Using the graphic simulation ..... 469 The miscellaneous functions ..... 470 6.2 Simulation window ..... 471 Setting up the views ..... 471 Single-window view ..... 472 Multiple window view ..... 472 6.3 Views ..... 473 Traverse path display ..... 473 Tool depiction ..... 474 Material-removal graphic ..... 474 3-D view ..... 475 6.4 The zoom function ..... 476 Adjusting the visible section ..... 476 6.
7 Tool and technology database ..... 483 7.1 Tool database ..... 484 Tool types ..... 484 Multipoint tools ..... 485 Tool life management ..... 485 7.2 Tool editor ..... 486 Tool list ..... 486 Editing the tool data ..... 487 Tool texts ..... 488 Editing multipoint tools ..... 489 Editing tool-life data ..... 491 Manual change systems ..... 492 7.3 Tool data ..... 497 General tool parameters ..... 497 Standard turning tools ..... 500 Recessing tools ..... 501 Thread-cutting tools .....
8 Organization mode of operation ..... 519 8.1 Organization mode of operation ..... 520 8.2 Parameters ..... 521 Parameter editor ..... 521 List of user parameters ..... 523 Machining parameters (processing) ..... 527 General settings ..... 527 Thread cutting ..... 542 8.3 Transfer ..... 546 Data backup ..... 546 Data exchange with TNCremo ..... 546 External access ..... 546 Connections ..... 547 Ethernet interface (with software 548328-xx) ..... 548 Ethernet interface (with software 54843x-xx) .....
9 Tables and overviews ..... 571 9.1 Thread pitch ..... 572 Thread parameters ..... 572 Thread pitch ..... 573 9.2 Undercut parameters ..... 579 DIN 76—undercut parameters ..... 579 DIN 509 E – undercut parameters ..... 581 DIN 509 F – undercut parameters ..... 581 9.3 Technical information ..... 582 9.4 Compatibility in DIN programs ..... 591 Syntax elements of the MANUALplus 620 .....
10 Overview of cycles ..... 605 10.1 Workpiece blank cycles, single cut cycles ..... 606 10.2 Turning cycles ..... 607 10.3 Recessing and recess-turning cycles ..... 608 10.4 Thread cycles ..... 609 10.5 Drilling cycles ..... 610 10.6 Milling cycles .....
Introduction and fundamentals HEIDENHAIN MANUALplus 620 33
1.1 The MANUALplus 1.1 The MANUALplus The MANUALplus was conceived for CNC lathes. It is suitable for horizontal and vertical lathes. The MANUALplus supports lathes with tool turrets. The tool carrier of horizontal lathes can be located in front of or behind the workpiece. The MANUALplus supports lathes with spindle, one slide (X and Z axis), C axis or positionable spindle, driven tool and machines with a Y axis.
1.2 Configuration 1.2 Configuration In the standard version, the control is equipped with the axes X and Z and a main spindle. Optionally, a C axis, a Y axis, and a driven tool can be configured. Slide position The machine tool builder configures the MANUALplus.
1.2 Configuration The Y axis With a Y axis you can drill and mill a workpiece on its face 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.
1.2 Configuration 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 MANUALplus supports full-surface machining for all common machine designs.
1.3 Features 1.3 Features Configuration Basic version: X and Z axis, spindle Positionable spindle and driven tool C axis and driven tool Y axis and driven tool B axis for machining a tilted plane Digital current and speed control Operating modes Manual operation Manual slide movement through axis-direction keys or electronic handwheels. Graphic support for entering and running Teach-in cycles without saving the machining steps in alternation with manual machine operation.
1.3 Features Graphic simulation Graphic depiction of the sequence of smart.
1.4 Data backup 1.4 Data backup HEIDENHAIN recommends saving new programs and files created on a PC at regular intervals. HEIDENHAIN provides a backup function for this purpose in the data transfer software TNCremoNT. Your machine tool builder can provide you with a copy. You additionally need a data medium on which all machine-specific data, such as the PLC program, machine parameters, etc., are stored. Please contact your machine tool builder.
1.5 Explanation of terms 1.5 Explanation of terms Cursor: In lists, or during data input, a list item, an input field or a character is highlighted. This "highlight" is called a cursor. Entries and operations, like copying, deleting, inserting a new item, etc., refer to the current cursor position. Arrow keys: The cursor is moved with the horizontal and vertical arrow keys and with the PG UP / PG DN keys. Page keys: The PG UP / PG DN keys are also called “Page keys.
1.6 MANUALplus design 1.6 MANUALplus design The dialog between machinist and control takes place via: Screen Soft keys Data input keypad Machine operating panel The entered data can be displayed and checked on the screen. With the soft key directly below the screen, you can select functions, capture position values, confirm entries, and a lot more. With the ERR key you can call error and PLC information.
1.7 Fundamentals 1.7 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.
1.7 Fundamentals Coordinate system The meanings of the coordinates X, Y, Z, and C are specified in DIN 66 217. The coordinates entered for the principal axes X and Z are referenced to the workpiece zero point. The angles entered for the rotary axis (C axis) are referenced to the datum of the C axis. The axis designations X and Z describe positions in a two-dimensional coordinate system.
1.7 Fundamentals Incremental coordinates Incremental coordinates are always given with respect to the last programmed position. They specify the distance from the last active position and the subsequent position. Each position on a workpiece is clearly defined by its incremental coordinates (see figure). Polar coordinates Positions located on the face or lateral surface can either be entered in Cartesian coordinates or polar coordinates.
1.7 Fundamentals Workpiece zero point To machine a workpiece, it is easier to enter all input data with respect to a zero point located on the workpiece. By programming the zero point used in the workpiece drawing, you can take the dimensions directly from the drawing, without further calculation. This point is the workpiece zero point. It is designated with the letter "W" (see figure). Units of measure You can program the MANUALplus either in the metric or inch system.
1.8 Tool dimensions 1.8 Tool dimensions The MANUALplus requires information on the specific tools for a variety of tasks, such as calculating the cutting radius compensation or the proportioning of cuts. Tool length All programmed and displayed position values are given with respect to the distance between the tool tip and workpiece zero point.
1.8 Tool dimensions Tool-tip radius compensation (TRC) The tip of a lathe tool has a certain radius. When machining tapers, chamfers and radii, this results in inaccuracies which the MANUALplus compensates with its cutting radius compensation function. Programmed paths of traverse are referenced to the theoretical tool tip S. With non-paraxial contours, this will lead to inaccuracies during machining.
Basics of operation HEIDENHAIN MANUALplus 620 49
2.1 General information on operation 2.1 General information on operation Operation Select the desired operating mode with the corresponding operating mode key. Within the operating mode, you can change the mode through the soft keys. With the numeric keypad you can select the function within the menus. Dialogs can consist of multiple pages. Besides with the soft keys, dialogs can be concluded positively with "INS" or negatively with "ESC." Changes made in lists are effective immediately.
2.2 The MANUALplus screen 2.2 The MANUALplus screen The MANUALplus shows the data to be displayed in windows. Some windows only appear when they are needed, for example, for typing in entries. In addition, the control shows the type of operation, the soft-key display and the PLC soft key display on the screen. Each function that appears in a field of the soft-key row is activated by pressing the soft key directly below it.
2.3 Operation and data input 2.3 Operation and data input Operating modes The active mode of operation is highlighted in the operating-mode tab. The MANUALplus differentiates between the following operating modes: Machine—with the submodes: Manual (display: "Machine") Teach-in (Teach-in mode) Program Run Programming—with the submodes: smart.
2.3 Operation and data input Menu selection The numerical keypad is used for activating a menu and for entering data. They are displayed differently depending on the operating mode. During setup, Teach-in mode etc., the functions are shown in a 9-field box, the menu window. The meaning of the selected symbol / menu item is described in the footer. In other operating modes, the keypad symbol is shown with the position of the function marked (see figure).
2.3 Operation and data input Data input Input windows comprise several input fields. You can move the cursor to the desired input field with the vertical arrow keys. The MANUALplus shows the function of the selected field in the footer of the window. Place the highlight on the desired input field and enter the data. Existing data are overwritten. With the horizontal arrow keys, you can move the cursor within the input field and place it on the position where you want to delete, copy or add characters.
2.3 Operation and data input Alphanumeric keyboard You enter letters and special characters with the screen keypad or (if available) with a PC keyboard connected over the USB port. Enter the text with the screen keyboard Press the "Alphabetic keyboard" soft key or the GOTO key to enter a text, for example a program name. The MANUALplus opens the "text entry" window. Just as on a cell phone, you press the numerical keys a few times to get the desired letters or special characters.
2.4 Integrated calculator 2.4 Integrated calculator Calculator functions The calculator can be selected only from open dialogs in cycle programming or smart.Turn programming. You can use the calculator in the following three views (see figures at right): Scientific Standard Equation editor. Here you can type in multiple calculations in immediate sequence (for example 17*3+5/9). The calculator remains in effect even after a change in operating modes. Press the END soft key to close the calculator.
Shortcut (soft key) Sine SIN Cosine COS Tangent TAN Powers of values X^Y Square root SQRT Inversion 1/x pi (3.
2.4 Integrated calculator Adjusting the position of the calculator You can move the calculator as follows: Shift the soft-key menu until the Additional functions soft key appears. Select "additional functions." Position the calculator with the soft keys (see table at right).
The MANUALplus supports the following programs/contours: Program type Folders Extension Teach-in programs (cycle programs) are used in the "Teach in" mode of operation. smart.Turn and DIN main programs are written in the smart.Turn mode of operation. DIN subprograms are written in the smart.Turn operating mode and are used in cycle programs and smart.Turn main programs. ICP contours are generated during Teach-in in the Teach-in or Manual mode of operation.
2.6 The error messages 2.6 The error messages Display of errors The MANUALplus generates error messages when it detects problems such as: Incorrect data input Logical errors in the program Contour elements that are impossible to machine When an error occurs, it is displayed in red type in the header. Long and multi-line error messages are displayed in abbreviated form. If an error occurs in a background mode, the error symbol is shown in the operating mode tab.
2.6 The error messages Detailed error messages The MANUALplus displays possible causes of the error and suggestions for solving the problem: Information on error causes and remedies: Open the error window. Position the cursor on the error message and press the soft key. The MANUALplus opens the window with information on the error cause and corrective action. To exit the info, press the Info soft key again. "Details" soft key The DETAILS soft key supplies information on the error message.
2.6 The error messages Clearing errors Clearing errors outside of the error window: Open the error window. To clear the error/note in the header: Press the CE button. In some operating modes (such as the Editing mode), the CE button cannot be used to clear the error, since the button is reserved for other functions. Clearing more than one error: Open the error window. To delete individual errors: Position the cursor on the error message and press the soft key.
2.6 The error messages Keystroke log file The MANUALplus stores keystrokes and important events (e.g. system startup) in the keystroke log file. The capacity of the keystroke log file is limited. If the log file is full, it switches to the next one, etc. If the last log file is full, the first one is overwritten by a new one, etc. If necessary, switch the log file to see the history. 10 log files are available. Open the keystroke log file. Press the Log file soft key. Open the log file.
2.7 TURNguide context-sensitive help system 2.7 TURNguide context-sensitive help system Application Before you can use the TURNguide, you need to download the help files from the HEIDENHAIN home page (see "Downloading current help files" on page 69). The TURNguide context-sensitive help system includes the user documentation in HTML format.
2.7 TURNguide context-sensitive help system Working with the TURNguide Calling the TURNguide There are several ways to start the TURNguide: Press the Info key if the control is not already showing an error message Click the help symbol at the lower right of the screen beforehand, then click the appropriate soft keys If one or more error messages are waiting for your attention, the control shows the help directly associated with the error messages.
2.7 TURNguide context-sensitive help system Navigating in the TURNguide It’s easiest to use the mouse to navigate in the TURNguide. A table of contents appears on the left side of the screen. By clicking the rightward pointing triangle you open subordinate sections, and by clicking the respective entry you open the individual pages. It is operated in the same manner as the Windows Explorer. Linked text positions (cross references) are shown underlined and in blue.
2.7 TURNguide context-sensitive help system Function Soft key Select the page last shown Page forward if you have used the "select page last shown" function Move up by one page Move down by one page Display or hide table of contents Switch between full-screen display and reduced display. With the reduced display you can see some of the rest of the control window. The focus is switched internally to the control application so that you can operate the control when the TURNguide is open.
2.7 TURNguide context-sensitive help system Subject index The most important subjects in the Manual are listed in the subject index (Index tab). You can select them directly by mouse or with the cursor keys. The left side is active.
2.7 TURNguide context-sensitive help system Downloading current help files You’ll find the help files for your control software on the HEIDENHAIN homepage www.heidenhain.de.
2.
Machine mode of operation HEIDENHAIN MANUALplus 620 71
3.1 Machine mode of operation 3.1 Machine mode of operation The Machine mode of operation includes all functions for machine setup, workpiece machining, and Teach-in program definition. Machine setup: For preparations like setting axis values (defining workpiece zero point), measuring tools or setting the protection zone. Manual mode: Machine a workpiece manually or semiautomatically. Teach-in mode: "Teach-in" a new cycle program, change an existing program, or graphically simulate cycles.
3.2 Switch-on / Switch-off 3.2 Switch-on / Switch-off Switch-on The MANUALplus displays the startup status. When the system has completed all tests and initializations, it switches to the Machine mode of operation. The tool display shows the tool that was last used. If errors are encountered during system start, the control displays the error symbol on the screen. You can check these error messages as soon as the system is ready (see "The error messages" on page 60).
3.2 Switch-on / Switch-off Traversing the reference marks Whether a reference run is necessary depends on the encoders used: 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. As soon as a reference mark is traversed, a signal is transmitted to the control.
3.2 Switch-on / Switch-off Switch-off Proper switch-off is recorded in the error log file. SWITCH-OFF Go to the main level of the Machine mode of operation Activate the error window Press the MORE FUNCTIONS soft key Press the OFF soft key The MANUALplus displays a confirmation request. Press the Enter key or the YES soft key. The software shuts down Wait until the MANUALplus requests you to switch off the machine.
3.3 Machine data 3.3 Machine data Input of machine data In Manual mode, you enter the information for tool, spindle speed and feed rate/cutting speed in the TSF dialog box (Set T, S, F input window). In Teach-in programs the tool information and technology data are included in the cycle parameters, and in smart.Turn programs they are part of the NC program. In the T, S, F dialog box you also define the "maximum speed" and the "stopping angle.
Soft keys for "Set T, S, F" See "Tool compensation" on page 103. Select Set T, S, F (only available in Manual mode) See "Touch off" on page 100. Define the parameters Conclude data input Call the "tool list": Transfer of T number from the tool list: See "Setting up a tool list" on page 83. Transfer of cutting speed and feed rate from the technology data Caution. Depending on the machine, this operation might cause the turret to turn.
3.3 Machine data Machine data display Elements of machine data display Position display X, Y, Z, W: Distance between tool tip and workpiece zero point A black axis letter means the axis is enabled; white means it is not enabled. Handwheel active Clamping active Position display C: Position of the C axis Empty box: C-axis is not active A black axis letter means the axis is enabled; white means it is not enabled.
3.
3.3 Machine data Elements of machine data display Slide display and cycle status Upper field: Setting of the override control Middle field: Programmed feed rate Lower field: Actual feed rate Slide display with rear-face machining If rear-face machining is enabled, the slide number is highlighted in blue.
3.3 Machine data Elements of machine data display Display of quantity: The quantity is incremented after each M30, M99 or M18 programmed counter pulse. MP: Default unit quantity P: Number of finished parts Display of quantity and job time: The quantity is incremented after each M30, M99 or M18 programmed counter pulse.
3.3 Machine data Axis feed rate F is the identification letter for feed data. Depending on which mode of the Feed rate soft key is active, data is entered in: Millimeters per spindle revolution (feed per revolution) Millimeters per minute (feed per minute). On the screen, you can tell the type of feed rate from the unit of measure in the input field. You can change the feed value with the feed compensation controller (feed override) (range: 0 % to 150 %).
3.4 Setting up a tool list 3.4 Setting up a tool list Machine with turret The tools used are listed in the turret list. The ID number of the mounted tool is assigned to every tool holder in the turret. In the Teach-in cycle you program the turret position as T number. The tool ID number is automatically entered under "ID." The turret list can be set up through the TSF menu or directly from the cycle dialogs in the Teach-in mode. T turret pocket number Tool ID (name) is entered automatically.
3.4 Setting up a tool list Tools in different quadrants Example: The principal tool carrier of your lathe is in front of the workpiece (standard quadrant). An additional tool holder is behind the workpiece. When MANUALplus is configured, it is defined for each tool holder whether the X dimensions and the direction of rotation of circular arcs are mirrored. In the above-mentioned example the additional tool holder is assigned the attribute "mirrored.
3.4 Setting up a tool list Filling the turret list from the database The turret list indicates the current assignment of the tool carrier. The turret list can be set up through the TSF menu or directly from the cycle dialogs in the Teach-in mode. Look at the entries in the tool database in order to move entries from the database into the turret assignment list. The MANUALplus displays the database entries in the lower area of the screen. The cursor keys are active in this list.
3.4 Setting up a tool list Filling the turret list The turret assignment indicates the current assignment of the tool carrier. When you set up a turret list, you enter the ID numbers of the tools. The turret list can be set up through the TSF menu or directly from the cycle dialogs in the Teach-in mode. The desired turret pocket is selected through the cursor keys. You can also set up manual changing systems in the turret assignment (see "Setting up the holder for manual change systems" on page 496).
3.4 Setting up a tool list Tool call T is the identification letter for the tool holder. ID designates the tool ID number. The tool is called by "T" (turret pocket number). The ID number ID is shown and automatically filled in the dialogs. A turret list is kept. One tool holder (e.g. multifix): The tool is called by "ID". The pocket number "T" is always 1. No turret list is kept. More than one tool holder (e.g. turret): The tool is called by "T" (turret pocket number).
3.4 Setting up a tool list Tool life monitoring If desired, you can have the MANUALplus monitor tool life or the number of parts that are produced with a specific tool. The tool life monitoring function adds the time a tool is used at feed rate. The quantity monitoring counts the number of finished parts. The count is compared with the entry in the tool data.
3.5 Machine setup 3.5 Machine setup The machine always requires a few preparations, regardless of whether you are machining a workpiece manually or automatically.
3.5 Machine setup Defining the workpiece zero point In the dialog, the distance between the machine zero point and the workpiece zero point (also know as offset) is shown as XN and ZN. If the workpiece zero point is changed, the display values will be changed accordingly. The workpiece datum can now also be set in the direction of the Z axis using a touch probe. When setting the zero point, the control checks which type of tool is currently active.
3.5 Machine setup Homing the axes It is possible to home axes that have already been homed. Here you can select individual axes or all axes simultaneously. REFERENCE RUN Select Setting up Select Set axis values Press the Machine reference soft key Press the Z reference soft key Press the X reference soft key Or press all soft keys Press Cycle start for the control to traverse the reference marks The MANUALplus refreshes the position display.
3.5 Machine setup Setting the protection zone With active protection zone monitoring, the MANUALplus checks for every movement whether the protection zone in –Z direction would be damaged. If it detects such a violation, it stops the axis movement and generates an error message. The "Setting the protection zone" setup dialog shows the distance between the machine zero point and the protection zone in –ZS.
3.5 Machine setup Defining the tool change position With the cycle Move to tool change position or the DIN command G14, the slide moves to the tool change point. Program the tool change point far enough away from the workpiece so that the turret can rotate without collision and the tools do not damage the workpiece during tool change.
3.
3.5 Machine setup Setting up machine dimensions The "Set up machine dimensions" function allows you to save any positions to use these in NC programs.
3.5 Machine setup Calibrating the tool touch probe The "Calibrate the tool touch probe" function enables you to determine the exact position values of the tool touch probe. MEASURING THE TOUCH PROBE POSITION Insert an exactly measured tool or reference tool Select Setting up Select touch probe Select tool touch probe Pre-position the tool for the first direction of measurement Set the positive or negative traverse direction Press the soft key for this direction (e.g. –Z direction) Press Cycle START.
3.5 Machine setup Displaying operating times In the Service menu, you can view different operating times: Operating time Meaning Control on Operating time of the control since being put into service Machine on Operating time of the machine tool since being put into service Program run Duration of controlled operation since being put into service The machine tool builder can provide further operating time displays. The machine manual provides further information.
3.5 Machine setup Setting the system time With the "Adjust system time" function, you can set the date and time on your control. You will need a mouse to navigate the Adjust system time input form. Use the Month and Year soft keys to increment or decrement the respective settings. To use an NTP server for setting the time, select a server from the server list first.
3.6 Tool measurement 3.6 Tool measurement The MANUALplus supports tool calibration By touch-off. The setup dimensions are determined by comparing a tool with an already measured tool. By touch probe (stationary of swiveling in the working space; installed by the machine tool builder). By optical gauge (installed by the machine tool builder). Calibration by touch-off is always available. If a touch probe or an optical gauge is installed, select these measuring methods by soft key.
3.6 Tool measurement Touch off You measure the dimensions relative to a calibrated tool by "touching the tool off.
3.6 Tool measurement Touch probe (tool touch probe) FINDING THE TOOL DIMENSIONS BY USING A TOUCH PROBE In the tool table, enter the tool you want to measure Insert a measured tool and enter the T number in the TSF dialog box Activate Measure tool Activate Touch probe Pre-position the tool for the first direction of measurement Set the positive or negative traverse direction Press the soft key for this direction (e.g. –Z direction) Press Cycle START. The tool moves in the direction of measurement.
3.
3.6 Tool measurement Tool compensation The tool compensation in X and Z as well as the special compensation for recessing tools and button tools compensate for wear of the cutting edge. A compensation value must not exceed +/–10 mm. DEFINING TOOL COMPENSATION Select Set T, S, F (only available in Manual mode) Press the Tool correct.
3.7 "Manual Operation" operating mode 3.7 "Manual Operation" operating mode With manual workpiece machining, you move the axes with the handwheels or manual direction keys. You can also use Teach-in cycles for machining more complex contours (semi-automatic mode). The paths of traverse and the cycles, however, are not stored. After switch-on and traversing the reference marks, the MANUALplus is always in Manual mode. This mode remains active until you select Teach-in or Program Run.
3.7 "Manual Operation" operating mode Manual direction keys With the manual direction keys, you can move the axes at the programmed feed rate or at rapid traverse. Enter the feed rate in the TSF dialog box.
3.8 Teach-in mode 3.8 Teach-in mode Teach-in mode In the Teach-in mode you machine a workpiece step by step with the help of Teach-in cycles. The MANUALplus "memorizes" how the workpiece was machined and stores the working steps in a cycle program, which you can call up again at any time. The Teach-in mode can be switched on by soft key and is displayed in the header. Each Teach-in program is given a name and a short description.
3.9 Program Run mode 3.9 Program Run mode Loading a program In Program Run mode, you use Teach-in and DIN programs for parts production. You cannot change the programs in this mode. The graphic simulation feature, however, allows you to check the programs before you run them. The MANUALplus also offers the Single Block and the Continuous Run mode with which you can machine step by step the first workpiece of a whole batch. The smart.Turn programs are selected as DIN programs (*.nc).
3.9 Program Run mode Comparing a tool list While a program is being loaded, the MANUALplus compares the current tools in the turret with the tool list of the program. If tools are used in the program that are not in the current turret list or are located in another pocket, an error message is displayed. After the error message is confirmed, the program-dependent tool list is shown for checking.
3.9 Program Run mode Finding a start block The MANUALplus must be prepared by the machine tool builder for the mid-program startup function (PLC). Mid-program startup means entering into an NC program at a selected point. In smart.Turn programs you can start the program at any NC block. The MANUALplus starts program run from the cursor position. The starting position is not changed by a previous graphic simulation.
3.9 Program Run mode Program execution The selected Teach-in or DIN program is executed as soon as you press Cycle start. You can interrupt machining at any time by pressing Cycle stop. During program run, the cycle (or DIN block) that is presently being executed is highlighted. With Teach-in programs, the parameters of the cycle currently being run are displayed in the input window. You can influence the program run with the soft keys listed in this table.
3.9 Program Run mode Entering compensation values during program run Tool compensation ENTERING TOOL COMPENSATION VALUES Activate the tool compensation Enter the tool number or select a tool from the tool list Enter the compensation values Press the Save soft key for the valid compensation data to be displayed in the input window and saved Entered values are added to the existing compensation values and are effective immediately.
3.9 Program Run mode Additive compensation The MANUALplus manages 16 additive compensation values. You edit the compensation values in the Program Run mode and activate it with G149 in a smart.Turn program or in ICP finishing cycles.
3.9 Program Run mode DELETING ADDITIVE COMPENSATION Activate the additive compensation Enter the number of the additive compensation Press the Delete soft key—these compensation values are deleted Press the Delete all soft key—all compensation values are deleted Entered values are added to the existing compensation values and are effective immediately. The compensation values are saved in an internal table and are available in any program.
3.9 Program Run mode Program execution in "dry run" mode The dry run mode is used for fast program execution up to a point at which machining is to resume. The prerequisites for a dry run are: The MANUALplus must be prepared by the machine tool builder for dry run. (The function is activated with a keylock switch or a key.) The Program Run mode must be activated. In dry run, all feed paths (except thread cuts) are traversed at the rapid rate.
3.10 Graphic simulation 3.10 Graphic simulation The graphic simulation feature enables you to check the machining sequence, the proportioning of cuts and the finished contour before actual machining. In the Manual Operation and Teach-in modes, this function simulates the execution of a single Teach-in cycle—in Program Run mode it simulates a complete Teach-in cycle or DIN program. A programmed workpiece blank is displayed in the simulation graphics.
3.11 Program management 3.11 Program management Program selection Program Run automatically loads the most recently used program. In the program selection the programs available in the control are listed. You select the desired program, or use the ENTER key to go to the File name input field. In this input field you limit the selection or enter the program name directly. Open the program list. Use the soft keys for program selection and sorting (see following table).
3.11 Program management Soft keys for sorting functions Sort the programs by change date Reverse the sorting direction Open the program for the automatic start Return to program selection dialog File manager With the functions of the program organization you can copy, delete and otherwise manipulate files. You can select the program type (Teach-in programs, smart.Turn or DIN programs) before calling the program organization.
3.11 Program management Soft keys file manager Open the alphabetic keyboard (see "Alphanumeric keyboard" on page 55) Return to program selection dialog Project management You can make your own project folder in the project management so that you can centrally manage associated files. When you create a project, a new folder is set up with the corresponding subfolder structure in the "TNC:\Project\" directory. You can save your programs, contours and drawings to the subfolders.
3.12 Conversion into DIN format 3.12 Conversion into DIN format The Convert to DIN function enables you to convert a Teach-in program to a smart.Turn program with the same functionality. You can then optimize, expand such a smart.Turn program, etc.
3.13 Units of measure 3.13 Units of measure The MANUALplus is operating in either the metric or inch system. The units and decimal places in the displays are given and entries interpreted according to the units of measure. inch Metric Units Coordinates, lengths, path data inch mm Feed rate in./rev or in.
Cycle programming HEIDENHAIN MANUALplus 620 121
4.1 Working with cycles 4.1 Working with cycles Before you can use the cycles, you must set the workpiece zero point and ensure that the tools you are going to use are described. You enter the machine data (tool, feed rate, spindle speed) in Teach-in mode together with the other cycle parameters. In Manual mode, you must program these machine data before calling a cycle. The cutting data can be taken from the technology database using the Proposed technology soft key.
4.1 Working with cycles Help graphics The functions and parameters of the Teach-in cycles are illustrated in the graphic support window. These graphics usually show an external machining operation. The Circle key allows you to switch between the help graphics for internal and external machining.
4.1 Working with cycles Contour follow-up in Teach-in mode The contour follow-up function updates the originally defined workpiece blank with every machining step. The turning cycles take the current contour of the workpiece blank into account for the calculation of infeed and machining paths. Air cuts are avoided and approach paths optimized.
4.1 Working with cycles Switching functions (M functions) The MANUALplus generates all switching functions that are necessary for running a cycle. The direction of spindle rotation must be defined in the tool parameters. Using the tool parameters, the cycles generate spindle trigger functions (M3 or M4). Your machine manual provides further information on automatically triggered switching functions. Comments You may assign a comment to an existing Teach-in cycle. The comment is inserted in brackets "[...
4.1 Working with cycles Cycle menu The main menu shows the cycle groups (see table below). Once a cycle group has been selected, the soft keys for the individual cycles appear. You can use ICP cycles for complex contours, and DIN macros for technologically sophisticated machining operations. In cycle programs, the names of the ICP contours or DIN macros are at the end of the line of the cycle. Some cycles offer optional parameters.
4.1 Working with cycles Soft keys in cycle programming: Depending on the type of cycle, you define the variants of the cycle by soft key (see table below). Soft keys in cycle programming Call the interactive contour input Move to the tool change position Activate spindle positioning (M19) On: Tool returns to the cycle start point Off: Tool remains at cycle end position Switch to the finishing operation Switch to the expanded mode Open the turret list and tool list.
4.1 Working with cycles Addresses used in many cycles Safety clearance G47 Safety clearances are used for approaching and departing paths. If the cycle run takes a safety clearance into account during execution you will find the address "G47" in the dialog. Proposed value: See (safety clearance G47) Page 523. Safety clearances SCI and SCK The safety clearances SCI and SCK are considered for approach and departure paths in drilling and milling cycles.
4.2 Workpiece blank cycles 4.2 Workpiece blank cycles The workpiece blank cycles describe the workpiece blank and the setup used. The workpiece blank cycles do not influence the machining process. The contours of workpiece blanks are shown during the simulation of the machining process.
4.2 Workpiece blank cycles Bar/tube blank Select define the blank Select bar/tube blank The cycle describes the workpiece blank and the setup used. This information is evaluated during the simulation.
4.2 Workpiece blank cycles ICP workpiece blank contour Select define the blank Select ICP workpiece blank contour The cycle integrates the workpiece blank defined with ICP and describes the setup used. This information is evaluated during the simulation.
4.3 Single cut cycles 4.3 Single cut cycles In the single-cut cycles you position the tool at rapid traverse, perform linear or circular cuts, machine chamfers or rounding arcs, and enter M functions.
4.3 Single cut cycles Rapid traverse positioning Call the single-cut menu Select rapid traverse positioning The tool moves at rapid traverse from the starting point to the target point.
4.3 Single cut cycles Approaching the tool change position Call the single-cut menu Select rapid traverse positioning Activate the T-Change approach soft key The tool moves at rapid traverse from the current position to the tool change position (see page 128). After reaching the tool change position, the control switches to the tool indicated in "T.
4.3 Single cut cycles Linear machining, longitudinal Call the single-cut menu Select longitudinal linear machining Off: When the cycle is completed, the tool remains at the cycle end position On: Tool returns to the starting point Linear machining, longitudinal The tool moves from the starting point to the contour end point Z2 at the programmed feed rate and remains at the cycle end position.
4.3 Single cut cycles Linear machining, transverse Call the single-cut menu Select transverse linear machining Off: When the cycle is completed, the tool remains at the cycle end position On: Tool returns to the starting point Linear machining, transverse The tool moves from the starting point to the contour end point X2 at the programmed feed rate and remains at the cycle end position.
4.3 Single cut cycles Linear machining at angle Call the single-cut menu Select linear machining at angle Off: When the cycle is completed, the tool remains at the cycle end position On: Tool returns to the starting point Linear machining at angle The MANUALplus calculates the target position and moves the tool on a straight line from the starting point to the target position at the programmed feed rate. When the cycle is completed, the tool remains at the cycle end position.
4.3 Single cut cycles Contour linear, at angle (with return) The MANUALplus calculates the target position. The tool then approaches the workpiece, executes the linear cut and returns to the starting point at the end of cycle (see figures). Cutter radius compensation is taken into account.
4.3 Single cut cycles Circular machining Call the single-cut menu Select circular machining (counterclockwise) Select circular machining (clockwise) Off: When the cycle is completed, the tool remains at the cycle end position On: Tool returns to the starting point Circular machining The tool moves on a circular path from the starting point X, Z to contour end point X2, Z2 and stops at the end of the cycle.
4.3 Single cut cycles Contour circular (with return) The tool approaches the workpiece, executes the circular cut and returns to the starting point at the end of cycle (see figures). Cutter radius compensation is taken into account.
4.3 Single cut cycles Chamfer Call the single-cut menu Select chamfer Off: When the cycle is completed, the tool remains at the cycle end position On: Tool returns to the starting point Chamfer The cycle produces a chamfer that is dimensioned relative to the corner of the workpiece contour. When the cycle is completed, the tool remains at the cycle end position.
4.3 Single cut cycles Contour chamfer (with return) The tool approaches the workpiece, machines the chamfer that is dimensioned relative to the corner of the workpiece contour and returns to the starting point at the end of cycle. Cutter radius compensation is taken into account.
4.3 Single cut cycles Rounding arc Call the single-cut menu Select rounding Off: When the cycle is completed, the tool remains at the cycle end position On: Tool returns to the starting point Rounding arc The cycle produces a rounding arc that is dimensioned relative to the corner of the workpiece contour. When the cycle is completed, the tool remains at the cycle end position.
4.3 Single cut cycles Contour rounding (with return) The tool approaches the workpiece, machines the rounding that is dimensioned relative to the corner of the workpiece contour and returns to the starting point at the end of cycle. Cutter radius compensation is taken into account.
4.3 Single cut cycles M functions Machine commands (M functions) are not executed until Cycle start has been pressed. With the M list soft key you can open an overview of the available M functions. For the meaning of the M functions, refer to your machine manual.
4.4 Turning cycles 4.4 Turning cycles Turning cycles rough and finish simple contours in basic mode and complex contours in expanded mode. With ICP cutting cycles, you can machine contours defined with ICP. See "ICP contours" on page 360. Proportioning of cuts: The MANUALplus calculates an infeed that is <=infeed depth P. An "abrasive cut" is avoided. Oversizes: Oversizes are considered in "expanded" mode.
4.4 Turning cycles Tool position It is important that you observe the tool positions (starting point X, Z) before executing any of the turning cycles in expanded mode. The rules also apply for all cutting and infeed directions as well as for roughing and finishing (see examples of linear cycles). The starting point must not be located in the shaded area. The area to be machined starts at the starting point X, Z, if the tool is positioned before the contour area.
4.
4.4 Turning cycles Roughing, longitudinal Select cut, longitudinal/transverse Select cut longitudinal The cycle roughs the rectangle described by the starting point and contour starting point X1/contour end point Z2.
4.
4.4 Turning cycles Cut, transverse Select cut, longitudinal/transverse Select cut transverse The cycle roughs the rectangle described by the starting point and contour starting point Z1/contour end point X2.
4.
4.4 Turning cycles Roughing, longitudinal—expanded Select cut, longitudinal/transverse Select cut longitudinal Press the Expanded soft key Taking the oversizes into account, the cycle roughs the area described by the starting point and contour starting point X1/contour end point Z2.
4.
4.4 Turning cycles Roughing, transverse—expanded Select cut, longitudinal/transverse Select cut transverse Press the Expanded soft key Taking the oversizes into account, the cycle roughs the area described by the starting point and the contour starting point Z1/contour end point X2.
4.
4.4 Turning cycles Finishing cut, longitudinal Select cut, longitudinal/transverse Select cut longitudinal Press the Finishing run soft key The cycle finishes the contour area from contour starting point X1 to contour end point Z2. At the end of the cycle, the tool returns to the starting point.
4.4 Turning cycles Finishing cut, transverse Select cut, longitudinal/transverse Select cut transverse Press the Finishing run soft key The cycle finishes the contour area from contour starting point Z1 to contour end point X2. At the end of the cycle, the tool returns to the starting point.
4.4 Turning cycles Finishing cut, longitudinal—expanded Select cut, longitudinal/transverse Select cut longitudinal Press the Expanded soft key Press the Finishing run soft key The cycle finishes the contour area from the contour starting point to the contour end point. When the cycle is completed, the tool remains at the cycle end position.
4.
4.4 Turning cycles Finishing cut, transverse—expanded Select cut, longitudinal/transverse Select cut transverse Press the Expanded soft key Press the Finishing run soft key The cycle finishes the contour area from the contour starting point to the contour end point. When the cycle is completed, the tool remains at the cycle end position.
4.
4.4 Turning cycles Cut, longitudinal plunge Select cut, longitudinal/transverse Select plunge, longitudinal The cycle roughs the area described by the contour starting point, contour end point and plunge angle. The tool plunges with the maximum possible angle, leaving material remaining. The steeper the tool plunges into the material, the greater the feed rate decrease (max. 50 %).
4.
4.4 Turning cycles Cut, transverse plunge Select cut, longitudinal/transverse Select plunge, transverse The cycle roughs the area described by the contour starting point, contour end point and plunge angle. The tool plunges with the maximum possible angle, leaving material remaining. The steeper the tool plunges into the material, the greater the feed rate decrease (max. 50 %).
4.
4.4 Turning cycles Cut, longitudinal plunging—expanded Select cut, longitudinal/transverse Select plunge, longitudinal Press the Expanded soft key The cycle roughs the area described by the contour starting point, contour end point and plunge angle, taking the oversizes into consideration. The tool plunges with the maximum possible angle, leaving material remaining. The steeper the tool plunges into the material, the greater the feed rate decrease (max. 50 %).
4.
4.4 Turning cycles Cut, transverse plunging—expanded Select cut, longitudinal/transverse Select plunge, transverse Press the Expanded soft key The cycle roughs the area described by the contour starting point, contour end point and plunge angle, taking the oversizes into consideration. The tool plunges with the maximum possible angle, leaving material remaining. The steeper the tool plunges into the material, the greater the feed rate decrease (max. 50 %).
4.
4.4 Turning cycles Cut, longitudinal finishing plunge Select cut, longitudinal/transverse Select plunge, longitudinal Press the Finishing run soft key The cycle finishes the contour area from the contour starting point to the contour end point. At the end of the cycle, the tool returns to the starting point. The tool plunges with the maximum possible angle, leaving material remaining. The steeper the tool plunges into the material, the greater the feed rate decrease (max. 50 %).
4.
MFE WP 4.
4.4 Turning cycles Cut, longitudinal finishing plunge—expanded Select cut, longitudinal/transverse Select plunge, longitudinal Press the Expanded soft key Press the Finishing run soft key The cycle finishes the contour area from the contour starting point to the contour end point. When the cycle is completed, the tool remains at the cycle end position. The tool plunges with the maximum possible angle, leaving material remaining.
MFE WP 4.
4.4 Turning cycles Cut, transverse finishing plunge—expanded Select cut, longitudinal/transverse Select plunge, transverse Press the Expanded soft key Press the Finishing run soft key The cycle finishes the contour area from the contour starting point to the contour end point. When the cycle is completed, the tool remains at the cycle end position. The tool plunges with the maximum possible angle, leaving material remaining.
WP 4.
4.4 Turning cycles Cut, ICP contour-parallel, longitudinal Select cut, longitudinal/transverse Select ICP contour-parallel, longitudinal The cycle roughs the defined area on contour-parallel paths. The cycle roughs contour parallel depending on the workpiece blank oversize J and the type of cutting lines H: J=0: the area defined by X, Z and the ICP contour, taking the oversizes into account. J>0: The area defined by the ICP contour (plus oversizes) and the workpiece blank oversize J.
BF A W XA, ZA MT MFS MFE WP 4.4 Turning cycles G47 G14 T ID S F BP Safety clearance (see page 128) Tool change point (see page 128) Turret pocket number Tool ID number Spindle speed/cutting speed Feed per revolution Break duration: Time span for interruption of the feed. The chip is broken by the (intermittent) interruption of the feed. Feed duration: Time interval until the next break. The chip is broken by the (intermittent) interruption of the feed.
4.4 Turning cycles Cut, ICP contour-parallel, transverse Select cut, longitudinal/transverse Select ICP contour-parallel, transverse The cycle roughs the defined area on contour-parallel paths. The cycle roughs contour parallel depending on the workpiece blank oversize J and the type of cutting lines H: J=0: the area defined by X, Z and the ICP contour, taking the oversizes into account. J>0: The area defined by the ICP contour (plus oversizes) and the workpiece blank oversize J.
BF XA, ZA A W MT MFS MFE WP 4.4 Turning cycles G47 G14 T ID S F BP Safety clearance (see page 128) Tool change point (see page 128) Turret pocket number Tool ID number Spindle speed/cutting speed Feed per revolution Break duration: Time span for interruption of the feed. The chip is broken by the (intermittent) interruption of the feed. Feed duration: Time interval until the next break. The chip is broken by the (intermittent) interruption of the feed.
4.4 Turning cycles Cut, ICP contour-parallel, longitudinal finishing Select cut, longitudinal/transverse Select ICP contour-parallel, longitudinal Press the Finishing run soft key The cycle finishes the contour area defined by the ICP contour. When the cycle is completed, the tool remains at the cycle end position. The tool plunges with the maximum possible angle, leaving material remaining.
MFE WP 4.
4.4 Turning cycles Cut, ICP contour-parallel, transverse finishing Select cut, longitudinal/transverse Select ICP contour-parallel, transverse Press the Finishing run soft key The cycle finishes the contour area defined by the ICP contour. When the cycle is completed, the tool remains at the cycle end position. The tool plunges with the maximum possible angle, leaving material remaining.
MFE WP 4.
4.4 Turning cycles ICP cutting, longitudinal Select cut, longitudinal/transverse Select ICP cutting, longitudinal The cycle machines the area defined by the starting point and the ICP contour, taking the oversizes into account. The tool plunges with the maximum possible angle, leaving material remaining. The steeper the tool plunges into the material, the greater the feed rate decrease (max. 50 %).
MT MFS MFE WP 4.4 Turning cycles XA, ZA Starting point of blank (only effective if no blank was programmed): XA, ZA not programmed: The workpiece blank contour is calculated from the tool position and the ICP contour. XA, ZA programmed: Definition of the corner point of the workpiece blank.
4.4 Turning cycles ICP cutting, transverse Select cut, longitudinal/transverse Select ICP cutting, transverse The cycle machines the area defined by the starting point and the ICP contour, taking the oversizes into account. The tool plunges with the maximum possible angle, leaving material remaining. The steeper the tool plunges into the material, the greater the feed rate decrease (max. 50 %).
W MT MFS MFE WP 4.
4.4 Turning cycles ICP longitudinal finishing cut Select cut, longitudinal/transverse Select ICP cutting, longitudinal Press the Finishing run soft key The cycle finishes the contour area defined by the ICP contour. When the cycle is completed, the tool remains at the cycle end position. The tool plunges with the maximum possible angle, leaving material remaining.
MFE WP 4.
4.4 Turning cycles ICP transverse finishing cut Select cut, longitudinal/transverse Select ICP cutting, transverse Press the Finishing run soft key The cycle finishes the contour area defined by the ICP contour. When the cycle is completed, the tool remains at the cycle end position. The tool plunges with the maximum possible angle, leaving material remaining.
MFE WP 4.
4.4 Turning cycles Examples of turning cycles Roughing and finishing an outside contour The shaded area from AP (starting point of contour) to EP (contour end point) is rough-machined with the cycle Plunge longitudinal— expanded, taking oversizes into account. This contour area is to be finished subsequently with the cycle Finishing cut longitudinal— expanded. The rounding arc and the oblique cut at the contour end are also machined in "expanded mode.
4.4 Turning cycles Roughing and finishing an inside contour The shaded area from AP (starting point of contour) to EP (contour end point) is rough-machined with the cycle Plunge longitudinal— expanded, taking oversizes into account. This contour area is to be finished subsequently with the cycle Finishing cut longitudinal— expanded. The rounding arc and the chamfer at the contour end are also machined in "expanded mode.
4.4 Turning cycles Roughing (recess clearance) with plunge cycle The tool to be used cannot plunge at the required angle of 15°. The roughing process for the area therefore requires two steps. First step: The shaded area from AP (starting point of contour) to EP (contour end point) is rough-machined with the cycle Plunge longitudinal— expanded, taking oversizes into account. The starting angle A is defined with 15°, as specified in the workpiece drawing.
4.4 Turning cycles Second step: The area that was left out in the first step (shaded area in the figure) is machined with the cycle Plunge, longitudinal—expanded. Before executing this step, you must change tools. The rounding arcs in the contour valley are also machined in "expanded mode." The parameters for contour starting point X1, Z1 and contour end point X2, Z2 determine the cutting and infeed directions—in this example, external machining and infeed in negative X-axis direction.
4.5 Recessing cycles 4.5 Recessing cycles The recessing cycle group comprises recessing, recess turning, undercut and parting cycles. Simple contours are machined in basic mode, complex contours in expanded mode. ICP recessing cycles machine contours defined with ICP (see "ICP contours" on page 360). Proportioning of cuts: The MANUALplus calculates a constant recessing width that is <=infeed depth P.
4.5 Recessing cycles Undercut position The MANUALplus determines the position of an undercut from the cycle parameters for starting point X, Z (current tool position in Manual mode) and corner point of contour X1, Z1. Undercuts can only be executed in orthogonal, paraxial contour corners along the longitudinal axis.
4.5 Recessing cycles Recessing, radial Call the recessing cycles Select recessing, radial The cycle machines the number of recesses defined in number Qn. The parameters for starting point and end point of contour define the first recess (position, recess depth and recess width). Cycle parameters X, Z Starting point X2, Z2 Contour end point P Recessing width: infeeds <= P (no input: P = 0.
MFE WP 4.
4.5 Recessing cycles Recessing, axial Call the recessing cycles Select axial recessing The cycle machines the number of recesses defined in number Qn. The parameters for starting point and end point of contour define the first recess (position, recess depth and recess width). Cycle parameters X, Z Starting point X2, Z2 Contour end point P Recessing width: infeeds <= P (no input: P = 0.
MFE WP 4.
4.5 Recessing cycles Recessing, radial—expanded Call the recessing cycles Select recessing, radial Press the Expanded soft key The cycle machines the number of recesses defined in number Qn. The parameters for the contour starting point and end point of contour define the first recess (position, recess depth and recess width).
MFE 4.
4.5 Recessing cycles Recessing, axial—expanded Call the recessing cycles Select axial recessing Press the Expanded soft key The cycle machines the number of recesses defined in number Qn. The parameters for the contour starting point and end point of contour define the first recess (position, recess depth and recess width).
WP 4.
4.5 Recessing cycles Recessing radial, finishing Call the recessing cycles Select recessing, radial Press the Finishing run soft key The cycle finishes the number of recesses defined in number Qn. The parameters for starting point and end point of contour define the first recess (position, recess depth and recess width).
WP 4.
4.5 Recessing cycles Recessing axial, finishing Call the recessing cycles Select axial recessing Press the Finishing run soft key The cycle finishes the number of recesses defined in number Qn. The parameters for starting point and end point of contour define the first recess (position, recess depth and recess width).
WP 4.
4.5 Recessing cycles Recessing radial, finishing—expanded Call the recessing cycles Select recessing, radial Press the Expanded soft key Press the Finishing run soft key The cycle machines the number of recesses defined in number Qn. The parameters for the contour starting point and end point of contour define the first recess (position, recess depth and recess width).
MFE WP 4.
4.5 Recessing cycles Recessing axial, finishing—expanded Call the recessing cycles Select axial recessing Press the Expanded soft key Press the Finishing run soft key The cycle machines the number of recesses defined in number Qn. The parameters for the contour starting point and end point of contour define the first recess (position, recess depth and recess width).
MFE WP 4.
4.5 Recessing cycles ICP recessing cycles, radial Call the recessing cycles Select recessing, radial ICP. The cycle machines the number of recesses defined in number Qn with the ICP recessing contour. The starting point defines the position of the first recess. Cycle parameters X, Z Starting point FK ICP finished part: Name of the contour to be machined P Recessing width: infeeds <= P (no input: P = 0.8 * cutting width of the tool) ET Recessing depth by which one cut is fed.
MFE WP 4.
4.5 Recessing cycles ICP recessing cycles, axial Call the recessing cycles Select recessing, axial ICP The cycle machines the number of recesses defined in number Qn with the ICP recessing contour. The starting point defines the position of the first recess. Cycle parameters X, Z Starting point FK ICP finished part: Name of the contour to be machined P Recessing width: infeeds <= P (no input: P = 0.8 * cutting width of the tool) ET Recessing depth by which one cut is fed.
MFE WP 4.
4.5 Recessing cycles ICP recessing, radial finishing Call the recessing cycles Select recessing, radial ICP. Press the Finishing run soft key The cycle finishes the number of recesses defined in number Qn with the ICP recessing contour. The starting point defines the position of the first recess. At the end of the cycle, the tool returns to the starting point.
MFE WP 4.
4.5 Recessing cycles ICP recessing, axial finishing Call the recessing cycles Select recessing, axial ICP Press the Finishing run soft key The cycle finishes the number of recesses defined in number Qn with the ICP recessing contour. The starting point defines the position of the first recess. At the end of the cycle, the tool returns to the starting point.
MFE WP 4.
4.5 Recessing cycles Recess turning The recess turning cycles machine by alternate recessing and roughing movements. The machining process requires a minimum of retraction and infeed movements. To influence recess-turning operations, use the following parameters: Recessing feed rate O: Feed rate for recessing movement Turning operation, unidirectional/bidirectional U: You can perform a unidirectional or bidirectional turning operation.
4.5 Recessing cycles Recess turning, radial Call the recessing cycles Select recess turning Select recess turning, radial The cycle clears the rectangle described by the starting point and contour end point.
4.
MFE WP 4.
4.5 Recessing cycles Recess turning, radial—expanded Call the recessing cycles Select recess turning Select recess turning, radial Press the Expanded soft key Taking the oversizes into account, the cycle clears the area described by the starting point X / contour starting point Z1 and contour end point (see also "Recess turning" on page 224).
MFE WP 4.
4.5 Recessing cycles Recessing turning, axial—expanded Call the recessing cycles Select recess turning Select recess turning, axial Press the Expanded soft key Taking the oversizes into account, the cycle clears the area described by the contour starting point X1 / starting point Z and contour end point (see also "Recess turning" on page 224).
MFE WP 4.
4.5 Recessing cycles Recess turning, radial finishing Call the recessing cycles Select recess turning Select recess turning, radial Press the Finishing run soft key The cycle finishes the contour area defined by the starting point and contour end point (see also "Recess turning" on page 224). With oversizes I, K for the workpiece blank, you define the material to be machined during the finishing cycle. For this purpose, enter the oversizes for recess turning, finishing.
MFE WP 4.
4.5 Recessing cycles Recess turning, axial finishing Call the recessing cycles Select recess turning Select recess turning, axial Press the Finishing run soft key The cycle finishes the contour area defined by the starting point and contour end point (see also "Recess turning" on page 224). With oversizes I, K for the workpiece blank, you define the material to be machined during the finishing cycle. For this purpose, enter the oversizes for recess turning, finishing.
MFE WP 4.
4.5 Recessing cycles Recess turning, radial finishing—expanded Call the recessing cycles Select recess turning Select recess turning, radial Press the Expanded soft key Press the Finishing run soft key The cycle finishes the contour area defined by the contour starting point and contour end point (see also "Recess turning" on page 224). With oversizes I, K for the workpiece blank, you define the material to be machined during the finishing cycle.
MFE WP 4.
4.5 Recessing cycles Recess turning, axial finishing—expanded Call the recessing cycles Select recess turning Select recess turning, axial Press the Expanded soft key Press the Finishing run soft key The cycle finishes the contour area defined by the contour starting point and contour end point (see also "Recess turning" on page 224). With oversizes I, K, you define the material to be machined during the finishing cycle. For this purpose, enter the oversizes for recess turning, finishing.
MFE WP 4.
4.5 Recessing cycles ICP recess turning, radial Call the recessing cycles Select recess turning Select recess turning, radial The cycle clears the defined area (see also "Recess turning" on page 224). If you are machining descending contours, define the starting point—not the starting point of the blank. The cycle clears the area defined by the starting point and the ICP contour, taking the oversizes into account. inclining contours, define the starting point and the starting point of the blank.
MFE WP 4.
4.5 Recessing cycles ICP recess turning, axial Call the recessing cycles Select recess turning Select recess turning, axial The cycle clears the defined area (see also "Recess turning" on page 224). If you are machining descending contours, define only the starting point—not the contour starting point. The cycle clears the area defined by the starting point and the ICP contour, taking the oversizes into account. inclining contours, define the starting point and the contour starting point.
MFE WP 4.
4.5 Recessing cycles ICP recess turning, radial finishing Call the recessing cycles Select recess turning Select recess turning, radial ICP Press the Finishing run soft key The cycle finishes the contour area defined by the ICP contour (see also "Recess turning" on page 224). At the end of the cycle, the tool returns to the starting point. With oversizes I, K for the workpiece blank, you define the material to be machined during the finishing cycle.
MFE WP 4.
4.5 Recessing cycles ICP recess turning, axial finishing Call the recessing cycles Select recess turning Select recess turning, axial ICP Press the Finishing run soft key The cycle finishes the contour area defined by the ICP contour (see also "Recess turning" on page 224). At the end of the cycle, the tool returns to the starting point. With oversizes I, K for the workpiece blank, you define the material to be machined during the finishing cycle.
MFE WP 4.
4.5 Recessing cycles Undercutting type H Call the recessing cycles Select undercutting H The contour depends on the parameters defined. If you do not define an undercut radius R, the oblique cut will be executed up to contour corner Z1 (tool radius = undercut radius). If you do not define the plunging angle, it is calculated from the undercut length and undercut radius. The final point of the undercut is then located at the contour corner.
MFE WP 4.
4.5 Recessing cycles Undercutting type K Call the recessing cycles Select undercut K This cycle performs only one cut at an angle of 45°. The resulting contour geometry therefore depends on the tool that is used.
4.5 Recessing cycles Undercutting type U Call the recessing cycles Select undercutting U This cycle machines an Undercut type U and, if programmed, finishes the adjoining plane surface. The undercut is executed in several passes if the undercut width is greater than the cutting width of the tool. If the cutting width of the tool is not defined, the control assumes that the tool’s cutting width equals the undercut width. Either a chamfer or a rounding arc can be machined.
4.
4.5 Recessing cycles Parting Call the recessing cycles Select parting The cycle parts the workpiece. If programmed, a chamfer or rounding arc is machined on the outside diameter.
4.
4.5 Recessing cycles Examples of recessing cycles Recess outside The machining operation is to be executed first with the Recessing, radial—expanded cycle, taking oversizes into account. This contour area is to be finished subsequently with Recessing, radial finishing, expanded. The rounding arcs in the corners of the contour valley and the oblique surfaces at the contour start and end are also machined in "expanded mode.
4.5 Recessing cycles Recess inside The machining operation is to be executed first with the Recessing, radial—expanded cycle, taking oversizes into account. This contour area is to be finished subsequently with Recessing, radial finishing, expanded. Since the plunge width P is not entered, the MANUALplus plungecuts with 80 % of the plunge-width of the tool. In expanded mode, the chamfers are machined at the start/end of the contour.
4.6 Thread and undercut cycles 4.6 Thread and undercut cycles The thread and undercut cycles machine single or multistart longitudinal and tapered threads, as well as thread undercuts. In Cycle mode you can Repeat the last cut to compensate for tool inaccuracies. Use the Recut function to rework damaged threads (only in Manual mode). Threads are cut with constant rotational speed. At a cycle stop, the tool retracts with the spindle still rotating. The cycle then has to be restarted.
4.6 Thread and undercut cycles Handwheel superimposition If your machine features handwheel superimposition, you can overlap axis movements during thread cutting in a limited area: X direction: Maximum programmed thread depth depending on the current cutting depth Z direction: +/- a fourth of the thread pitch Machine and control must be specially prepared by the machine tool builder for use of this cycle. Refer to your machine tool manual.
4.6 Thread and undercut cycles Thread run-in / thread run-out The slide requires a run-in distance to accelerate to the programmed feed rate before starting the actual thread, and a run-out distance at the end of the thread to decelerate again. If the run-in / run-out length is too short, the thread may not attain the expected quality. In this case, the MANUALplus displays a warning.
4.6 Thread and undercut cycles Last cut After the cycle is finished, the MANUALplus presents the Last cut option. In this way you can enter a tool compensation value and repeat the last thread cut. SEQUENCE OF THE "LAST CUT" FUNCTION Initial situation: The thread cut cycle has been run, and the thread depth is not correct.
4.6 Thread and undercut cycles Thread cycle (longitudinal) Call the thread-cutting menu Select thread cycle On: Internal thread Off: External thread This cycle cuts a single external or internal thread with a thread angle of 30°. Tool infeed is performed in the X axis only. Cycle parameters X, Z Starting point of thread Z2 End point of thread F1 Thread pitch (= feed rate) U Thread depth – No input: I External thread: U=0.6134*F1 Internal thread: U=–0.
4.6 Thread and undercut cycles GH Type of offset 0: Without offset 1: From left 2: From right 3: Alternately left/right Approach (infeed) angle (range: –60° < A < 60°; default 30°) A A<0: Infeed on left thread flank A>0: Infeed on right thread flank Remaining cutting depth only with GV=4 (default 1/100 mm) Number of cuts—the infeed is calculated from IC and U.
4.6 Thread and undercut cycles Thread cycle (longitudinal)—expanded Call the thread-cutting menu Select thread cycle Press the Expanded soft key On: Internal thread Off: External thread This cycle cuts a single or multi-start external or internal thread. The thread starts at the starting point and ends at the end point of thread (without a thread run-in or run-out).
4.6 Thread and undercut cycles GV Type of infeed 0: Constant mach. X-section 1: Constant infeed 2: W/ remaining cutting (with distribution of remaining cuts) 3: W/o remaining cutting (without distribution of remaining cuts) 4: Same as MANUALplus 4110 5: Constant infeed (same as 4290) 6: Constant with distribute.
4.6 Thread and undercut cycles Tapered thread Call the thread-cutting menu Select tapered thread On: Internal thread Off: External thread This cycle cuts a single or multi-start tapered external or internal thread. Cycle parameters X, Z Starting point X1, Z1 Starting point of thread X2, Z2 End point of thread F1 Thread pitch (= feed rate) D Number of thread starts (default: 1 single-start thread) U Thread depth – No input: I External thread: U=0.6134*F1 Internal thread: U=–0.
4.6 Thread and undercut cycles GH Type of offset 0: Without offset 1: From left 2: From right 3: Alternately left/right Approach (infeed) angle (range: –60° < A < 60°; default 30°) A A<0: Infeed on left thread flank A>0: Infeed on right thread flank Remaining cutting depth only with GV=4 (default 1/100 mm) Variable thread pitch (e.g. for manufacturing spiral conveyors or extrusion shafts) No. no load (number of dry runs) Number of cuts—the infeed is calculated from IC and U.
4.6 Thread and undercut cycles API thread Call the thread-cutting menu Select API thread On: Internal thread Off: External thread This cycle cuts a single or multi-start API external or internal thread. The depth of thread decreases at the overrun at the end of thread.
4.6 Thread and undercut cycles GH Type of offset 0: Without offset 1: From left 2: From right 3: Alternately left/right Approach (infeed) angle (range: –60° < A < 60°; default 30°) A R Q MT MFS MFE WP A<0: Infeed on left thread flank A>0: Infeed on right thread flank Remaining cutting depth only with GV=4 (default 1/100 mm) No.
4.6 Thread and undercut cycles Recut (longitudinal) thread Call the thread-cutting menu Select thread cycle Press the Recut soft key On: Internal thread Off: External thread This optional cycle reworks a single-start thread. Since you have already unclamped the workpiece, the MANUALplus needs to know the exact position of the thread.
4.
4.6 Thread and undercut cycles Recut (longitudinal) thread—expanded Call the thread-cutting menu Select thread cycle Press the Expanded soft key Press the Recut soft key On: Internal thread Off: External thread This optional cycle recuts a single or multi-start external or internal thread. Since you have already unclamped the workpiece, the MANUALplus needs to know the exact position of the thread.
4.6 Thread and undercut cycles R Q MT MFS MFE WP Remaining cutting depth only with GV=4 (default 1/100 mm) No.
4.6 Thread and undercut cycles Recut tapered thread Call the thread-cutting menu Select tapered thread Press the Recut soft key On: Internal thread Off: External thread This optional cycle recuts a single or multi-start external or internal taper thread. Since you have already unclamped the workpiece, the MANUALplus needs to know the exact position of the thread.
4.6 Thread and undercut cycles R Q MT MFS MFE WP Remaining cutting depth only with GV=4 (default 1/100 mm) No.
4.6 Thread and undercut cycles Recut API thread Call the thread-cutting menu Select API thread Press the Recut soft key On: Internal thread Off: External thread This optional cycle recuts a single or multi-start external or internal API thread. Since you have already unclamped the workpiece, the MANUALplus needs to know the exact position of the thread.
4.6 Thread and undercut cycles R Q MT MFS MFE WP Remaining cutting depth only with GV=4 (default 1/100 mm) No.
4.6 Thread and undercut cycles Undercut DIN 76 Call the thread-cutting menu Select Undercut DIN 76 Off: When the cycle is completed, the tool remains at the cycle end position On: Tool returns to the starting point The cycle machines a thread undercut according to DIN 76, a thread chamfer, then the cylinder, and finishes with the plane surface. The thread chamfer is executed when you enter at least one of the parameters cylinder 1st cut length or 1st cut radius.
4.
4.6 Thread and undercut cycles Undercut DIN 509 E Call the thread-cutting menu Select undercut DIN 509 E Off: When the cycle is completed, the tool remains at the cycle end position On: Tool returns to the starting point The cycle machines a thread undercut according to DIN 509 type E, a cylinder start chamfer, then the adjoining cylinder, and finishes with the plane surface. You can define a finishing oversize for the area of the cylinder.
4.6 Thread and undercut cycles MFE WP M at end: M function that is executed at the end of the machining step Displays which workpiece spindle is used to process the cycle (machine-dependent) Main drive Opposing spindle for rear-face machining Type of machining for technology database access: Finishing All parameters that you enter will be accounted for—even if the standard table prescribes other values.
4.6 Thread and undercut cycles Undercut DIN 509 F Call the thread-cutting menu Select undercut DIN 509 F Off: When the cycle is completed, the tool remains at the cycle end position On: Tool returns to the starting point The cycle machines a thread undercut according to DIN 509 type F, a cylinder start chamfer, then the adjoining cylinder, and finishes with the plane surface. You can define a finishing oversize for the area of the cylinder.
4.
4.6 Thread and undercut cycles Examples of thread and undercut cycles External thread and thread undercut The machining operation is to be performed in two steps. The thread undercut DIN 76 produces the undercut and thread chamfer. In the second step, the thread cycle cuts the thread. First step The parameters for the undercut and thread chamfer are programmed in two superimposed input windows.
4.6 Thread and undercut cycles Internal thread and thread undercut The machining operation is to be performed in two steps. The thread undercut DIN 76 produces the undercut and thread chamfer. In the second step, the thread cycle cuts the thread. First step The parameters for the undercut and thread chamfer are programmed in two superimposed input windows. The MANUALplus determines the undercut parameters from the standard table. For the thread chamfer, you only need to enter the chamfer width.
4.7 Drilling cycles 4.7 Drilling cycles The drilling cycles allow you to machine axial and radial holes. For pattern machining, see "Drilling and milling patterns" on page 336.
4.7 Drilling cycles Drilling, axial Select drilling Select drilling, axial This cycle drills a hole on the face of the workpiece.
MFE WP 4.
4.7 Drilling cycles Radial drilling Select drilling Select drilling, radial This cycle drills a hole on the lateral surface of the workpiece.
MFE WP 4.
4.7 Drilling cycles Deep-hole drilling, axial Select drilling Select deep-hole drilling, axial The cycle produces a bore hole on the face in several passes. After each pass, the drill retracts and, after a dwell time, advances again to the first pecking depth, minus the safety clearance. You define the first pass with 1st hole depth P. The drilling depth is reduced with each subsequent pass by the reducing value, however, without falling below the minimum drilling depth.
BF MT MFS MFE WP 4.7 Drilling cycles BP Break duration: Time span for interruption of the feed. The chip is broken by the (intermittent) interruption of the feed. Feed duration: Time interval until the next break. The chip is broken by the (intermittent) interruption of the feed.
4.7 Drilling cycles Cycle run 1 2 3 4 5 6 7 Position spindle to spindle angle C (in Manual mode, machining starts from the current spindle angle) If defined, move at rapid traverse to starting point of hole Z1 First pass (pecking depth: P)—drill with reduced feed rate, if defined Retract by retraction length B—or to the hole starting point and advance again to last pecking depth minus safety clearance Next pass (pecking depth: "last depth – IB" or JB).
4.7 Drilling cycles Deep-hole drilling, radial Select drilling Select deep hole, radial The cycle produces a bore hole on the lateral surface in several passes. After each pass, the drill retracts and, after a dwell time, advances again to the first pecking depth, minus the safety clearance. You define the first pass with 1st hole depth P. The drilling depth is reduced with each subsequent pass by the reducing value, however, without falling below the minimum drilling depth.
4.
4.7 Drilling cycles Tapping, axial Select drilling Select tapping, axial This cycle is used to tap a thread on the face of a workpiece. Meaning of retraction length: Use this parameter for floating tap holders. The cycle calculates a new nominal pitch on the basis of the thread depth, the programmed pitch, and the retraction length. The nominal pitch is somewhat smaller than the pitch of the tap. During tapping, the drill is pulled away from the chuck by the retraction length.
4.
4.7 Drilling cycles Tapping, radial Select drilling Select tapping, radial This cycle is used to tap a thread on the lateral surface of a workpiece. Meaning of retraction length: Use this parameter for floating tap holders. The cycle calculates a new nominal pitch on the basis of the thread depth, the programmed pitch, and the retraction length. The nominal pitch is somewhat smaller than the pitch of the tap. During tapping, the drill is pulled away from the chuck by the retraction length.
4.
4.7 Drilling cycles Thread milling, axial Select drilling Select thread milling, axial The cycle mills a thread in existing holes. Use threading tools for this cycle. Danger of collision! Be sure to consider the hole diameter and the diameter of the milling cutter when programming approaching radius R.
4.
4.7 Drilling cycles Examples of drilling cycles Centric drilling and tapping The machining operation is to be performed in two steps. In the first step, the Drilling, axial cycle drills the hole. In the second, the Tapping, axial cycle taps the thread. The drill is positioned at the safety clearance to the workpiece surface (starting point X, Z). The hole starting point Z1 is therefore not programmed. In the parameters "AB" and "V," you program a feed reduction. The thread pitch is not programmed.
4.7 Drilling cycles Deep-hole drilling A hole is to be bored through the workpiece outside the turning center with the cycle Deep-hole drilling, axial. This machining operation requires a traversable spindle and driven tools. The parameters 1st hole depth P and hole depth reduction value IB define the individual passes, and the minimum hole depth JB limits the hole reduction value.
4.8 Milling cycles 4.8 Milling cycles Milling cycles are used to machine axial and radial slots, contours, pockets, surfaces and polygons. For pattern machining, see "Drilling and milling patterns" on page 336. In Teach-in mode these cycles include the activation/deactivation of the C axis and the positioning of the spindle. In Manual mode you can activate the C axis with Rapid traverse positioning and position the spindle before the actual milling cycle.
4.8 Milling cycles Rapid positioning milling Select milling Select rapid traverse positioning The cycle activates the C axis and positions the spindle (C axis) and the tool. Rapid traverse positioning is only required in Manual mode. The C axis is deactivated by a subsequent manual milling cycle.
4.8 Milling cycles Slot, axial Select milling Select slot, axial This cycle mills a slot on the face of the workpiece. The slot width equals the diameter of the milling cutter.
4.
4.
4.
MFE 4.
4.
4.8 Milling cycles ICP contour, axial Select milling Select ICP contour, axial Depending on the parameters, the cycle mills a contour or roughs/ finishes a pocket on the face.
4.
4.8 Milling cycles Notes on parameters/functions: Contour milling JK defines whether the milling cutter is to machine on the contour (center of milling cutter on the contour) or on the inside/outside of the contour. Open contours are machined in direction of contour definition. JK defines whether to move to the left or right of the contour. Pocket milling—roughing (O=0): Use JT to define whether a pocket is machined from the inside toward the outside, or vice versa.
4.8 Milling cycles Face milling Select milling Select the "Face milling" cycle Depending on the parameters, the cycle mills the following contours on the face.
Rounding radius (default: 0) A Polygon (Q>2): Rounding radius Circle (Q=0): Radius of circle Angle to X axis (default: 0) G14 T ID S F Polygon (Q>2): Position of figure Circle: No input Tool change point (see page 128) Turret pocket number Tool ID number Spindle speed/cutting speed Feed per revolution 4.
4.
4.8 Milling cycles Slot, radial Select milling Select "Slot, radial" This cycle mills a slot on the lateral surface. The slot width equals the diameter of the milling cutter.
4.
4.
4.
MFE 4.
4.
4.8 Milling cycles ICP contour, radial Select milling Select ICP contour, radial Depending on the parameters, the cycle mills a contour or roughs/ finishes a pocket on the lateral surface.
4.
4.8 Milling cycles Notes on parameters/functions: Contour milling JK defines whether the milling cutter is to machine on the contour (center of milling cutter on the contour) or on the inside/outside of the contour. Open contours are machined in direction of contour definition. JK defines whether to move to the left or right of the contour. Pocket milling—roughing (O=0): Use JT to define whether a pocket is machined from the inside toward the outside, or vice versa.
4.8 Milling cycles Helical-slot milling, radial Select milling Select helical-slot milling, radial The cycle mills a helical slot from the contour starting point to the thread end point. The starting angle defines the starting position for the slot. The slot width equals the diameter of the milling cutter.
WP 4.
4.
4.
4.8 Milling cycles Example of milling cycle Milling on the face In this example, a pocket is milled. The milling example in "9.8 ICP Example, Milling Cycle" illustrates the complete machining process on the face, including contour definition. The machining process is performed with the cycle ICP contour, axial. To describe a contour, define the basic contour first. Then superimpose the rounding arcs.
4.8 Milling cycles Engraving, axial The "Radial engraving" cycle engraves character strings in linear or polar layout on the face of the workpiece. For character table and more information, see page 335 You define the starting point of the character string in the cycle. If you do not define a starting point, the cycle starts at the current tool position. You can also engrave a logotype with several calls. For this purpose, specify the starting point with the first call.
4.8 Milling cycles Parameters: RB SCK MT MFS Retraction plane. Z position retracted to for positioning.
4.8 Milling cycles Engraving, radial The "Radial engraving" cycle engraves character strings in linear layout on the face of the workpiece. For character table and more information, see page 335 You define the starting point of the character string in the cycle. If you do not define a starting point, the cycle starts at the current tool position. You can also engrave a logotype with several calls. For this purpose, specify the starting point with the first call.
4.8 Milling cycles Parameters: SCK Safety clearance (see page 128) MT M after T: M function that is executed after the tool call T MFS M at beginning: M function that is executed at the beginning of the machining step MFE M at end: M function that is executed at the end of the machining step WP Displays which workpiece spindle is used to process the cycle (machine-dependent) Main drive Opposing spindle for rear-face machining The engraving cycles are not available in manual operation.
4.8 Milling cycles Engraving, axial/radial The MANUALplus can realize the characters listed in the following table. The text to be engraved is entered as a character string. Diacritics and special characters that you cannot enter in the editor can be defined, character by character, in NF. If text is defined in ID and a character is defined in NF, the text is engraved before the character. The engraving cycles are not available in manual operation.
4.9 Drilling and milling patterns 4.9 Drilling and milling patterns Note on using drilling/milling patterns: Drilling patterns: The MANUALplus generates the machine commands M12, M13 (apply/release block brake) under the following conditions: the drill/tap must be entered as driven tool (parameters driven tool AW and direction of rotation MD must be defined).
4.9 Drilling and milling patterns Linear drilling pattern, axial DRILLING PATTERN LINEAR, AXIAL Select drilling Select drilling, axial Select deep-hole drilling, axial Select tapping, axial Press the Pattern linear soft key Press Pattern linear to machine drilling patterns in which the individual features are arranged at a regular spacing in a straight line on the face.
4.
4.9 Drilling and milling patterns Milling pattern linear, axial LINEAR MILLING PATTERN, AXIAL Select milling Press the Pattern linear soft key Select slot, axial Select recessing, axial ICP Press Pattern linear to machine milling patterns in which the individual features are arranged at a regular spacing in a straight line on the face.
4.
4.9 Drilling and milling patterns Drilling pattern circular, axial CIRCULAR DRILLING PATTERN, AXIAL Select drilling Select drilling, axial Select deep-hole drilling, axial Select tapping, axial Press the Pattern circular soft key Press Pattern circular to machine drilling patterns in which the individual features are arranged at a regular spacing in a circle or circular arc on the face.
4.
4.9 Drilling and milling patterns Milling pattern circular, axial CIRCULAR MILLING PATTERN, AXIAL Call the milling menu Select slot, axial Select ICP contour, axial Press the Pattern circular soft key Press Pattern circular to machine milling patterns in which the individual features are arranged at a regular spacing in a circle or circular arc on the face.
4.
4.9 Drilling and milling patterns Drilling pattern linear, radial DRILLING PATTERN LINEAR, RADIAL Select drilling Select drilling, radial Select deep-hole drilling, radial Select tapping, radial Press the Pattern linear soft key Press Pattern linear during drilling cycles to machine drilling patterns in which the individual features are arranged at a regular spacing in a straight line on the lateral surface.
4.
4.9 Drilling and milling patterns Linear milling pattern, radial MILLING PATTERN LINEAR, RADIAL Select milling Press the Pattern linear soft key Select slot, radial Select ICP contour, radial Press Pattern linear during milling cycles to machine milling patterns in which the individual features are arranged at a regular spacing in a straight line on the lateral surface.
4.
4.9 Drilling and milling patterns Drilling pattern circular, radial CIRCULAR DRILLING PATTERN, RADIAL Select drilling Select drilling, radial Select deep-hole drilling, radial Select tapping, radial Press the Pattern circular soft key Press Pattern circular to machine drilling patterns in which the individual features are arranged at a regular spacing in a circle or circular arc on the lateral surface.
4.
4.9 Drilling and milling patterns Circular milling pattern, radial MILLING PATTERN CIRCULAR, RADIAL Select milling Select slot, radial Select ICP contour, radial Press the Pattern radial soft key Press Pattern circular to machine milling patterns in which the individual features are arranged at a regular spacing in a circle or circular arc on the lateral surface.
4.
4.9 Drilling and milling patterns Examples of pattern machining Linear hole pattern on face A linear hole pattern is to be machined on the face of the workpiece with the Drilling, axial cycle. This machining operation requires a traversable spindle and driven tools. The pattern is programmed by entering the coordinates of the first and last hole, and the number of holes. Only the depth is indicated for the drilling cycle.
4.9 Drilling and milling patterns Circular hole pattern on face A circular hole pattern is to be machined on the face of the workpiece with the Drilling, axial cycle. This machining operation requires a traversable spindle and driven tools. The center of the pattern is entered in Cartesian coordinates. Since this example is to illustrate how you drill a through hole, the hole end point Z2 is programmed such that the tool has to drill all the way through the workpiece before it reaches the end point.
4.9 Drilling and milling patterns Linear hole pattern on lateral surface A linear hole pattern is to be machined on the lateral surface of the workpiece with the Drilling, axial cycle. This machining operation requires a traversable spindle and driven tools. The drilling pattern is defined by the coordinates of the first hole, the number of holes, and the spacing between the holes. Only the depth is indicated for the drilling cycle.
4.10 DIN cycles 4.10 DIN cycles DIN cycle Select DIN cycle This function allows you to select a DIN cycle (DIN subprogram) and integrate it in a cycle program. The dialogs of the parameters defined in the subprogram are then shown in the form. The technology data that are programmed in the DIN cycle (in Manual mode, the currently active technology data) become effective as soon as you start the DIN subprogram. You can change the machine data (T, S, F) at any time by editing the DIN subprogram.
4.10 DIN cycles In the DIN subprogram you can assign texts and help graphics to the transfer values (see "Subprograms" Chapter in the "smart.Turn- and DIN Programming“ User's Manual). Danger of collision! Cycle programming: With DIN subprograms, the zero point shift is reset at the end of the cycle. Therefore, do not use any DIN subprograms with zero point shifts in cycle programming. In the DIN cycle, no starting point is defined.
4.
ICP programming HEIDENHAIN MANUALplus 620 359
5.1 ICP contours 5.1 ICP contours The Interactive Contour Programming (ICP) feature provides graphic support when you are defining the workpiece contours. (ICP is the abbreviation of "Interactive Contour Programming".) Contours created with ICP are used in the following: In ICP cycles (Teach-in, Manual Operation) In smart.Turn Each contour begins with a starting point.
5.1 ICP contours Form elements Chamfers and rounding arcs can be inserted at each corner of the contour. Undercuts according to DIN 76, DIN 509 E, and DIN 509 F can be inserted at paraxial, orthogonal contour corners. No deviations are tolerated in elements in the X direction. You can insert chamfers and rounding arcs at each corner of the contour. Undercuts according to DIN 76, DIN 509 E, DIN 509 F are only possible at paraxial, orthogonal contour corners.
5.1 ICP contours Calculation of contour geometry The MANUALplus automatically calculates all missing coordinates, points of intersection, center points, etc. that can be derived mathematically. If the entered data permit several mathematically possible solutions, you can inspect the individual solutions and select the proposal that matches the drawing. Each unresolved contour element is represented by a small symbol below the graphic window.
5.2 ICP editor in cycle mode 5.2 ICP editor in cycle mode In cycle mode you can create: Complex workpiece blank contours Contours for turning For ICP turning cycles For ICP recessing cycles For ICP recess-turning cycles Complex contours for milling with the C axis For the face For the lateral surface You activate the ICP editor with the Edit ICP soft key. This can only be selected when editing ICP turning cycles or milling cycles or the ICP workpiece blank contour cycle.
5.2 ICP editor in cycle mode Creating a new contour Define the contour name in the cycle dialog and press the Edit ICP soft key. The ICP editor switches to entering the contour. Press the Edit ICP soft key. The ICP editor opens the window "Selection of ICP contours." Define the contour name in the "file name" field press the Open soft key. The ICP editor switches to entering the contour. Press the Contour menu key. Press the Insert element soft key. The ICP waits for you to enter a contour name.
5.3 ICP editor in smart.Turn 5.3 ICP editor in smart.Turn In smart.Turn you can make: Blank contours and auxiliary blank contours Finished part contours and auxiliary contours Standard figures and complex contours for C-axis machining on the face on the lateral surface Standard figures and complex contours for Y-axis machining on the XY plane on the YZ plane Blank contours and auxiliary blank contours: You describe complex blanks element by element—like finished parts.
5.3 ICP editor in smart.Turn Editing a contour in smart.Turn Creating a blank contour Press the ICP menu key, then in the ICP submenu select Blank or Auxiliary blank. Press the Contour menu key. The ICP editor switches to entering the complex blank contour. Press the Bar menu key. Describe the standard workpiece blank "bar." Press the Tube menu key. Describe the standard workpiece blank "tube." Making a new contour for turning Press the ICP menu key, then in the ICP submenu, select the contour type.
5.3 ICP editor in smart.Turn Loading a contour from the cycle editing Press the ICP menu key, then in the ICP submenu, select the contour type. Press the Contour list soft key. The ICP editor shows the list of the contours created in cycle mode. Select and load the contour. Editing an existing contour Position the cursor in the corresponding program section. Press the ICP menu key, then: .. Select Contour editing in the ICP submenu. Press the Change ICP contour soft key.
5.4 Creating an ICP contour 5.4 Creating an ICP contour An ICP contour consists of individual contour elements. You program the contour by entering the individual contour elements one after the other in the correct sequence. The starting point is defined before you describe the first contour element. The end point is determined by the target point of the last contour element. The contour elements / subcontours are displayed as soon as they are programmed.
Press the Contour menu key. Press the Insert element soft key. 5.4 Creating an ICP contour ICP CONTOUR PROGRAMMING Soft keys for switching between lines menus and arcs menus Select the line menu. Select the arc menu. Specify the starting point. Select the line menu. Select the arc menu. Select the "Form elements" menu item. Select the element type and enter the known parameters of the contour element.
5.4 Creating an ICP contour Fits and inside threads With the Inside thread fit soft key, you can display an input form for calculating the machining diameter for fits and inside threads. After entering the required values (nominal diameter and tolerance class or thread type), you can apply the calculated value as the target point for the contour element. The machining diameter can only be calculated for suitable contour elements, e.g.
5.4 Creating an ICP contour Polar coordinates Entry of Cartesian coordinates is expected as standard. With the soft keys for polar coordinates you switch individual coordinates to polar coordinates. You can mix Cartesian coordinates and polar coordinates to define a point. Soft keys for polar coordinates Switches the field to entering the angle W. Switches the field to entering the radius P. Angular input Select the desired angle input by soft key.
5.4 Creating an ICP contour Contour graphics As soon as you have entered a contour element, the MANUALplus checks whether the element is resolved or unresolved. A resolved element is a contour element that is fully and unambiguously defined. It is drawn immediately. An unresolved element has not yet been fully defined by the entered data. Use of the ICP editor: It places a symbol below the graphics window. It reflects the element type and the line direction / direction of rotation.
5.4 Creating an ICP contour Selection of solutions If the data entered for unresolved contour elements permit several possible solutions, you can check all mathematically possible solutions with the Next solution / Previous solution soft keys. You then confirm the correct solution by soft key. If the contour still contains unsolved contour elements when you exit the editing mode, the MANUALplus will ask you whether to discard these elements.
5.4 Creating an ICP contour Selection functions In the ICP editor, the MANUALplus provides various functions for selecting contour elements, form elements, contour corners and contour areas. You can call these functions by soft key. Selected contour corners or contour elements are shown in red. Selecting a contour area Select the first element of the contour section. Selecting contour elements Next element (or the left arrow key) selects the next element in the direction of contour definition.
5.4 Creating an ICP contour Zero point shift With this function, you can move a complete turning contour. Activate zero point shift: Select "Zero point > Shift" in the finished part menu Enter the contour shift to move the defined contour Press the Save soft key Deactivate zero point shift: Select "Zero point > Reset" in the finished part menu to reset the zero point of the coordinate system to the original position The zero point shift cannot be reset after you exit the ICP editor.
5.4 Creating an ICP contour Copying a contour section in circular series With this function, you can define a contour section and append it to the existing contour in a circular series.
5.4 Creating an ICP contour Contour direction (cycle programming) The cutting direction during cycle programming depends on the direction of the contour. If the contour is described in the –Z direction, a tool with the orientation 1 must be used for longitudinal machining. (See "General tool parameters" on page 497.) The cycle used determines whether machining is transverse or longitudinal. If the contour is described in the –X direction, a tool with the orientation 3 must be used for transverse machining.
5.5 Editing ICP contours 5.5 Editing ICP contours The MANUALplus offers the following possibilities for extending or changing a programmed contour. Superimposing form elements Press the soft key. Select the desired form element. Select the corner to be changed. Confirm the corners for the form element and enter the data for the form element. Adding contour elements You can add to an ICP contour by entering additional contour elements that are "appended" to the existing contour.
5.5 Editing ICP contours Editing or deleting the last contour element To edit the last contour element: When the Change last soft key is pressed the data of the "last" contour element are presented for editing. Depending on the adjoining contour elements, corrections of linear or circular elements are either transferred immediately or the corrected contour is displayed for inspection. ICP highlights the affected contour elements in color.
5.5 Editing ICP contours Editing contour elements The MANUALplus provides various ways to change an existing contour. The procedure is illustrated in the following example of editing the length of an element. The other functions work similar to the procedure described here.
5.5 Editing ICP contours Changing the length of the contour element Press Manipulate. The menu displays functions for trimming, editing and deleting contours. Menu item Edit ... ... Select the contour element. Select the contour element to be edited. Present the selected contour element for editing. Make the changes. Load the changes. The contour or, if applicable, the possible solutions are displayed for inspection.
5.5 Editing ICP contours Shifting a contour Press Manipulate. The menu displays functions for trimming, editing and deleting contours. Menu item Edit ... ... Select the contour element. Select the contour element to be edited. Present the selected contour element for moving. Enter the new starting point of the reference element. Assume the new starting point (= new position). The MANUALplus shows the shifted contour. Confirm the new position for the contour.
5.5 Editing ICP contours Transformations – Rotating With this function you can rotate a contour about a center of rotation.
5.5 Editing ICP 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.
5.6 The zoom function in the ICP editor 5.6 The zoom function in the ICP editor The zoom functions make it possible to change the visible section by using soft keys, the arrow keys, and the PgUp and PgDn keys. The zoom function can be called in all ICP windows. The MANUALplus sizes the graphic section depending on the programmed contour. With the zoom function you can select another graphic section.
5.7 Defining the workpiece blank 5.7 Defining the workpiece blank In smart.Turn, the standard forms "bar" and "tube" are described with a G function. "Bar" blank The function describes a cylinder. Parameters X Cylinder diameter Z Length of the blank K Right edge (distance between workpiece zero point and right edge) ICP generates in smart.Turn a G20 in the BLANK section. "Tube" blank The function describes a hollow cylinder.
5.8 Contour elements of a turning contour 5.8 Contour elements of a turning contour With the "contour elements of a turning contour" you can create the following: In cycle mode Complex workpiece blank contours Contours for turning In smart.
5.8 Contour elements of a turning contour Vertical lines Select the line direction. Enter the line dimensions and define the transition to the next element. Parameters X Target point Xi Incremental target point (distance from starting point to target point) W Polar target point (angle) P Polar target point (radius) L Length of line U, F, D, FP, IC, KC, HC: See machining attributes on Page 361 In smart.Turn, ICP generates a G1. Horizontal lines Select the line direction.
5.8 Contour elements of a turning contour Line at angle Select the line direction. Enter the line dimensions and define the transition to the next element. Always enter the angle AN (<=90°) within the selected quadrant.
5.8 Contour elements of a turning contour Circular arc Select the arc’s direction of rotation. Enter the arc dimensions and define the transition to the next element.
5.8 Contour elements of a turning contour Contour form elements Chamfer/rounding arc Select the form elements. Select a chamfer. Select rounding arc. Enter the chamfer width BR or the rounding radius BR. Chamfer/rounding arc as first element: Enter element position AN. Parameters BR Chamfer width/rounding radius AN Element position U, F, D, FP: See machining attributes Page 361 Chamfers/rounding arcs are defined on contour corners.
5.8 Contour elements of a turning contour Thread undercut DIN 76 Select the form elements. Select Undercut DIN 76. Enter the undercut parameters. Parameters FP Thread pitch (default: value from standard table) I Undercut depth (radius) (default: value from standard table) K Undercut length (default: value from standard table) R Undercut radius (default: value from standard table) W Undercut angle (default: value from standard table) U, F, D, FP: See machining attributes Page 361 In smart.
5.8 Contour elements of a turning contour Undercut DIN 509 E Select the form elements. Select undercut DIN 509 E. Enter the undercut parameters. Parameters I Undercut depth (radius) (default: value from standard table) K Undercut length (default: value from standard table) R Undercut radius (default: value from standard table) W Undercut angle (default: value from standard table) U, F, D, FP: See machining attributes Page 361 In smart.Turn, ICP generates a G25.
5.8 Contour elements of a turning contour Undercut DIN 509 F Select the form elements. Select undercut DIN 509 F. Enter the undercut parameters.
5.8 Contour elements of a turning contour Undercut type U Select the form elements. Select the undercut type U. Enter the undercut parameters. Parameters I Undercut depth (radius) K Undercut length R Undercut radius P Chamfer/rounding U, F, D, FP: See machining attributes Page 361 In smart.Turn, ICP generates a G25. Undercuts can be programmed only between two linear elements. One of the two linear elements must be parallel to the X axis.
5.8 Contour elements of a turning contour Undercut type H Select the form elements. Select the undercut type H. Enter the undercut parameters. Parameters K Undercut length R Undercut radius W Plunging angle U, F, D, FP: See machining attributes Page 361 In smart.Turn, ICP generates a G25. Undercuts can be programmed only between two linear elements. One of the two linear elements must be parallel to the X axis.
5.8 Contour elements of a turning contour Undercut type K Select the form elements. Select the undercut type K. Enter the undercut parameters. Parameters I Undercut depth R Undercut radius W Angular length A Plunging angle U, F, D, FP: See machining attributes Page 361 In smart.Turn, ICP generates a G25. Undercuts can be programmed only between two linear elements. One of the two linear elements must be parallel to the X axis.
5.9 Contour elements on face 5.9 Contour elements on face With the "contour elements of a face" you can create complex milling contours. Cycle mode: Contour for axial ICP milling cycles smart.Turn: Contour for machining with the C axis Enter the dimensions of the front face contour elements in Cartesian or polar values. You can switch between them by pressing a soft key (see table). You can mix Cartesian coordinates and polar coordinates to define a point.
Direction: DF WF BR RB 0: Up-cut milling 1: Climb milling Cutter diameter Angle of the chamfer Chamfer width Return plane 5.9 Contour elements on face HF In smart.Turn, ICP generates a G100. Vertical lines on face Select the line direction. Enter the line dimensions and define the transition to the next contour element.
5.9 Contour elements on face Horizontal lines on face Select the line direction. Enter the line dimensions and define the transition to the next contour element. Parameters XK Cartesian target point XKi Incremental target point (distance from starting point to target point) C Polar target point (angle) P Polar target point L Length of line F: See machining attributes Page 361 In smart.Turn, ICP generates a G101.
5.9 Contour elements on face Line at angle on face Select the line direction. Enter the line dimensions and define the transition to the next contour element.
5.9 Contour elements on face Circular arc on face Select the arc’s direction of rotation. Enter the arc dimensions and define the transition to the next element.
5.9 Contour elements on face Chamfer/rounding arc on the face Select the form elements. Select a chamfer. Select rounding arc. Enter the chamfer width BR or the rounding radius BR. Chamfer/rounding arc as first element: Enter element position AN. Parameters BR Chamfer width/rounding radius AN Element position F: See machining attributes Page 361 Chamfers/rounding arcs are defined on contour corners. A "contour corner" is the point of intersection between the approaching and departing contour elements.
5.10 Contour elements on lateral surface 5.10 Contour elements on lateral surface With the "contour elements of a lateral surface" you can create complex milling contours. Cycle mode: Contour for radial ICP milling cycles smart.Turn: Contour for machining with the C axis Enter the dimensions of the lateral surface contour elements in Cartesian or polar values. You can use the linear dimension as an alternative to the angular dimension. You can switch between them by pressing a soft key (see table).
Milling/drilling attribute: QF 1: Contour milling 2: Pocket milling 3: Area milling 4: Deburring 5: Engraving 6: Contour milling and deburring 7: Pocket milling and deburring 14: Do not machine Milling location: HF 0: On the contour 1: Inside/left 2: Outside/right Direction: DF WF BR RB 0: Up-cut milling 1: Climb milling Cutter diameter Angle of the chamfer Chamfer width Return plane 5.10 Contour elements on lateral surface HC In smart.Turn, ICP generates a G110.
5.10 Contour elements on lateral surface Vertical lines on lateral surface Select the line direction. Enter the line dimensions and define the transition to the next contour element. Parameters CY Target point as linear dimension (reference: diameter XS) CYi Incremental target point as linear dimension (reference: diameter XS) P Target point as polar radius C Polar target point (angle) Ci Incremental polar target point – angle L Length of line F: See machining attributes Page 361 In smart.
5.10 Contour elements on lateral surface Line at angle on lateral surface Direction of the line Enter the line dimensions and define the transition to the next contour element.
5.10 Contour elements on lateral surface Circular arc on lateral surface Select the arc’s direction of rotation. Enter the arc dimensions and define the transition to the next element.
5.10 Contour elements on lateral surface Chamfers/rounding arcs on a lateral surface Select the form elements. Select a chamfer. Select rounding arc. Enter the chamfer width BR or the rounding radius BR. Chamfer/rounding arc as first element: Enter element position AN. Parameters BR Chamfer width/rounding radius AN Element position F: See machining attributes Page 361 Chamfers/rounding arcs are defined on contour corners.
5.11 C and Y axis machining in smart.Turn 5.11 C and Y axis machining in smart.Turn In smart.Turn, ICP supports the definition of milling contours and holes as well as the creation of milling and drilling patterns that are machined with the aid of the C or Y axis.
When describing a milling contour or hole you specify the reference plane. The reference plane is the position on which the milling contour or the hole is created. Face (C axis): The Z position (reference dimension) Lateral surface (C axis): The X position (reference diameter) XY plane (Y axis): The Z position (reference dimension) YZ plane (Y axis): The X position (reference diameter) It is also possible to nest milling contours and holes. Example: Defining a slot in a rectangular pocket.
5.11 C and Y axis machining in smart.Turn Representation of the ICP elements in the smart.Turn program Each ICP dialog in smart.Turn programs is followed by a section code of further G commands.
5.12 Face contours in smart.Turn 5.12 Face contours in smart.Turn In smart.Turn, ICP provides the following contours for machining with the C axis: Complex contours defined with individual contour elements Figures Holes Pattern of figures or holes Reference data for complex face contours The reference data is followed by the contour definition with individual contour elements: See "Contour elements on face" on page 398.
5.12 Face contours in smart.Turn TURN PLUS attributes In the TURN PLUS attributes you can define settings for the automatic program generation (AWG).
5.12 Face contours in smart.Turn Rectangle on face Reference data of face ID Contour name PT Milling depth ZR Reference dimension Parameters of figure XKM, YKM Center of figure (Cartesian coordinates) A Position angle (reference: XK axis) K Length B Width BR Rounding arc You can find the reference dimension ZR with the "select reference plane" function (see page 411). ICP generates: The FRONT section code with the reference dimension parameter. In nested contours, ICP generates only one section code.
5.12 Face contours in smart.Turn Polygon on face Reference data of face ID Contour name PT Milling depth ZR Reference dimension Parameters of figure XKM, YKM Center of figure (Cartesian coordinates) A Position angle (reference: XK axis) Q Number of corners K Length of edge Ki Width across flats (inscribed circle diameter) BR Rounding arc You can find the reference dimension ZR with the "select reference plane" function (see page 411).
5.12 Face contours in smart.Turn Linear slot on face Reference data of face ID Contour name PT Milling depth ZR Reference dimension Parameters of figure XKM, YKM Center of figure (Cartesian coordinates) A Position angle (reference: XK axis) K Length B Width You can find the reference dimension ZR with the "select reference plane" function (see page 411). ICP generates: The FRONT section code with the reference dimension parameter. In nested contours, ICP generates only one section code.
5.12 Face contours in smart.
5.12 Face contours in smart.
5.12 Face contours in smart.
5.13 Lateral surface contours in smart.Turn 5.13 Lateral surface contours in smart.Turn In smart.Turn, ICP provides the following contours for machining with the C axis: Complex contours defined with individual contour elements Figures Holes Pattern of figures or holes Reference data of lateral surface The reference data is followed by the contour definition with individual contour elements: See "Contour elements on lateral surface" on page 404.
5.13 Lateral surface contours in smart.Turn TURN PLUS attributes In the TURN PLUS attributes you can define settings for the automatic program generation (AWG).
5.13 Lateral surface contours in smart.Turn Circle on lateral surface Reference data of lateral surface ID Contour name PT Milling depth XR Reference diameter Parameters of figure Z Figure center CYM Center of figure as linear dimension (reference: diameter XR) CM Center of figure (angle) R Radius You can find the reference diameter XR with the "select reference plane" function (see page 411). ICP generates: The SURFACE section code with the reference dimension parameter.
5.13 Lateral surface contours in smart.Turn Rectangle on lateral surface Reference data of lateral surface ID Contour name PT Milling depth XR Reference diameter Parameters of figure Z Figure center CYM Center of figure as linear dimension (reference: diameter XR) CM Center of figure (angle) A Position angle K Length B Width BR Rounding arc You can find the reference diameter XR with the "select reference plane" function (see page 411).
5.13 Lateral surface contours in smart.Turn Polygon on lateral surface Reference data of lateral surface ID Contour name PT Milling depth XR Reference diameter Parameters of figure Z Figure center CYM Center of figure as linear dimension (reference: diameter XR) CM Center of figure (angle) A Position angle Q Number of corners K Length of edge Ki Width across flats (inscribed circle diameter) BR Rounding arc You can find the reference diameter XR with the "select reference plane" function (see page 411).
5.13 Lateral surface contours in smart.Turn Linear slot on lateral surface Reference data of lateral surface ID Contour name PT Milling depth XR Reference diameter Parameters of figure Z Figure center CYM Center of figure as linear dimension (reference: diameter XR) CM Center of figure (angle) A Position angle K Length B Width You can find the reference diameter XR with the "select reference plane" function (see page 411). ICP generates: The SURFACE section code with the reference dimension parameter.
5.13 Lateral surface contours in smart.Turn Circular slot on lateral surface Reference data of lateral surface ID Contour name PT Milling depth XR Reference diameter Parameters of figure Z Figure center CYM Center of figure as linear dimension (reference: diameter XR) CM Center of figure (angle) A Starting angle W End angle R Radius Q2 Direction of rotation B CW CCW Width You can find the reference diameter XR with the "select reference plane" function (see page 411).
5.13 Lateral surface contours in smart.
5.13 Lateral surface contours in smart.
5.13 Lateral surface contours in smart.
EPi H 5.13 Lateral surface contours in smart.Turn EP End angle (no entry: the pattern elements are equally divided into 360°) Angle between two figures Element position 0: Normal – the figures are rotated about the circle center (rotation) 1: Original position – the position of the figures relative to the coordinate system remains unchanged (translation) Parameters of the selected figure/hole You can find the reference diameter XR with the "select reference plane" function (see page 411).
5.14 Contours in the XY plane 5.14 Contours in the XY plane In smart.Turn, ICP provides the following contours for machining with the Y axis: Complex contours defined with individual contour elements Figures Holes Pattern of figures or holes Single surface Polygon Soft keys for polar coordinates Switches the field to entering the angle W. Switches the field to entering the radius P. Enter the dimensions of the XY plane contour elements in Cartesian or polar values.
5.14 Contours in the XY plane Starting point of contour in XY plane Enter the coordinates for the starting point and target point in the first contour element of the contour. Entering the starting point is only possible in the first contour element. In subsequent contour elements, the starting point results from the previous contour element in each case. Press the Contour menu key. Press the Insert element soft key. Specify the starting point.
5.14 Contours in the XY plane Horizontal lines in XY plane Select the line direction. Enter the line dimensions and define the transition to the next contour element. Parameters X Target point Xi Incremental target point (distance from starting point to target point) W Polar target point (angle) P Polar target point L Length of line F: See machining attributes Page 361 In smart.Turn, ICP generates a G171.
5.14 Contours in the XY plane Line at angle in XY plane Select the line direction. Enter the line dimensions and define the transition to the next contour element.
5.14 Contours in the XY plane Circular arc in XY plane Select the arc’s direction of rotation. Enter the arc dimensions and define the transition to the next contour element.
5.14 Contours in the XY plane Chamfer/rounding arc in XY plane Select the form elements. Select a chamfer. Select rounding arc. Enter the chamfer width BR or the rounding radius BR. Chamfer/rounding arc as first element: Enter element position AN. Parameters BR Chamfer width/rounding radius AN Element position F: See machining attributes Page 361 Chamfers/rounding arcs are defined on contour corners.
5.14 Contours in the XY plane Circle in XY plane Reference data in XY plane ID Contour name PT Milling depth C Spindle angle IR Limit diameter ZR Reference dimension Parameters of figure XM, YM Figure center R Radius You can find the reference dimension ZR and the limit diameter IR with the "select reference plane" function (see page 411). ICP generates: The section code FRONT_Y with the parameters limit diameter, reference dimension and spindle angle. The section code is omitted for nested contours.
5.14 Contours in the XY plane Rectangle in XY plane Reference data in XY plane ID Contour name PT Milling depth C Spindle angle IR Limit diameter ZR Reference dimension Parameters of figure XM, YM Figure center A Position angle (reference: X axis) K Length B Width BR Rounding arc You can find the reference dimension ZR and the limit diameter IR with the "select reference plane" function (see page 411).
5.14 Contours in the XY plane Polygon in XY plane Reference data in XY plane ID Contour name PT Milling depth C Spindle angle IR Limit diameter ZR Reference dimension Parameters of figure XM, YM Figure center A Position angle (reference: X axis) Q Number of corners K Length of edge Ki Width across flats (inscribed circle diameter) BR Rounding arc You can find the reference dimension ZR and the limit diameter IR with the "select reference plane" function (see page 411).
5.14 Contours in the XY plane Linear slot in XY plane Reference data in XY plane ID Contour name PT Milling depth C Spindle angle IR Limit diameter ZR Reference dimension Parameters of figure XM, YM Figure center A Position angle (reference: X axis) K Length B Width You can find the reference dimension ZR and the limit diameter IR with the "select reference plane" function (see page 411). ICP generates: The section code FRONT_Y with the parameters limit diameter, reference dimension and spindle angle.
5.
5.
5.
5.
5.14 Contours in the XY plane Single surface in XY plane This function defines a surface in the XY plane.
5.14 Contours in the XY plane Centric polygon in XY plane This function defines polygonal surfaces in the XY plane.
5.15 Contours in the YZ plane 5.15 Contours in the YZ plane In smart.Turn, ICP provides the following contours for machining with the Y axis: Complex contours defined with individual contour elements Figures Holes Pattern of figures or holes Single surface Polygon Soft keys for polar coordinates Switches the field to entering the angle W. Switches the field to entering the radius P. Enter the dimensions of the YZ plane contour elements in Cartesian or polar values.
5.15 Contours in the YZ plane TURN PLUS attributes In the TURN PLUS attributes you can define settings for the automatic program generation (AWG).
5.15 Contours in the YZ plane Starting point of contour in YZ plane Enter the coordinates for the starting point and target point in the first contour element of the contour. Entering the starting point is only possible in the first contour element. In subsequent contour elements, the starting point results from the previous contour element in each case. Press the Contour menu key. Press the Insert element soft key. Specify the starting point.
5.15 Contours in the YZ plane Horizontal lines in YZ plane Select the line direction. Enter the line dimensions and define the transition to the next contour element. Parameters Z Target point Zi Incremental target point (distance from starting point to target point) W Polar target point (angle) P Polar target point L Length of line F: See machining attributes Page 361 In smart.Turn, ICP generates a G181.
5.15 Contours in the YZ plane Line at angle in YZ plane Select the line direction. Enter the line dimensions and define the transition to the next contour element.
5.15 Contours in the YZ plane Circular arc in YZ plane Select the arc’s direction of rotation. Enter the arc dimensions and define the transition to the next contour element.
5.15 Contours in the YZ plane Chamfer/rounding arc in YZ plane Select the form elements. Select a chamfer. Select rounding arc. Enter the chamfer width BR or the rounding radius BR. Chamfer/rounding arc as first element: Enter element position AN. Parameters BR Chamfer width/rounding radius AN Element position F: See machining attributes Page 361 Chamfers/rounding arcs are defined on contour corners.
5.15 Contours in the YZ plane Circle in YZ plane Reference data in YZ plane ID Contour name PT Milling depth C Spindle angle XR Reference diameter Parameters of figure YM, ZM Figure center R Radius You can find the reference diameter XR with the "select reference plane" function (see page 411). ICP generates: The section code SURFACE_Y with the reference diameter and spindle angle. The section code is omitted for nested contours. A G308 with the parameters contour name and milling depth.
5.15 Contours in the YZ plane Rectangle in YZ plane Reference data in YZ plane ID Contour name PT Milling depth C Spindle angle XR Reference diameter Parameters of figure YM, ZM Figure center A Position angle (reference: X axis) K Length B Width BR Rounding arc You can find the reference diameter XR with the "select reference plane" function (see page 411). ICP generates: The section code SURFACE_Y with the reference diameter and spindle angle. The section code is omitted for nested contours.
5.15 Contours in the YZ plane Polygon in YZ plane Reference data in YZ plane ID Contour name PT Milling depth C Spindle angle XR Reference diameter Parameters of figure YM, ZM Figure center A Position angle (reference: X axis) Q Number of corners K Length of edge Ki Width across flats (inscribed circle diameter) BR Rounding arc You can find the reference diameter XR with the "select reference plane" function (see page 411).
5.15 Contours in the YZ plane Linear slot in YZ plane Reference data in YZ plane ID Contour name PT Milling depth C Spindle angle XR Reference diameter Parameters of figure YM, ZM Figure center A Position angle (reference: X axis) K Length B Width You can find the reference diameter XR with the "select reference plane" function (see page 411). ICP generates: The section code SURFACE_Y with the reference diameter and spindle angle. The section code is omitted for nested contours.
5.
5.
5.
5.15 Contours in the YZ plane Single surface in YZ plane This function defines a surface in the YZ plane.
5.15 Contours in the YZ plane Centric polygons in YZ plane This function defines centric polygons in the YZ plane.
5.16 Loading existing contours 5.16 Loading existing contours Integrating cycle contours in smart.Turn ICP contours that you have created for cycle programs can be loaded in smart.Turn. ICP converts the contours into G commands and integrates them in the smart.Turn program. The contour is now part of the smart.Turn program. The ICP editor considers the type of contour. For example, you can load a contour defined for the face only if you have selected the face (C axis) in smart.Turn. Extension Group *.
5.16 Loading existing contours DXF contours (option) Contours that exist in DXF format are imported with the ICP editor. You can use DXF contours both for cycle operation and for smart.Turn. Requirements of a DXF contour: Only two-dimensional elements The contour must be in a separate layer (without dimension lines, without wraparound edges, etc.). Depending on the setup of the lathe, contours for turning operations must be either in front of or behind the workpiece.
5.16 Loading existing contours Activate the ICP editor. Press the Contour list soft key. The ICP editor opens the window "Selection of ICP contours." Press the Next file type soft key until the DXF contours are displayed (see file extension "*.DXF"). Select the file. Open the selected file. Select the DXF layer. Load the selected contour. Blank or finished part contour: Supplement or adapt the contour, if necessary. C-axis or Y-axis contour: Complete the reference data.
Graphic simulation
6.1 Simulation mode of operation 6.1 Simulation mode of operation Press this soft key to start a graphic simulation from the following operating modes: smart.Turn Program Run Teach-in Manual Operation (cycles) When called from the smart.Turn mode, the graphic simulation opens the large simulation window and loads the selected program. When you call the simulation from the Machine modes of operation, either the small simulation window or the last window you used is opened.
The simulation is controlled by soft keys in all operating states. In addition, you can always use the menu keys (numeric keys) to control the simulation, even in the small simulation window, when the menu bar is not visible. Starting and stopping with soft keys Starts the simulation from the beginning. The soft key switches to the stop symbol; you can now use the soft key to stop and resume the simulation, depending on the simulation status. Resumes a stopped simulation (Single Block mode).
6.1 Simulation mode of operation The miscellaneous functions You use the miscellaneous functions to select the simulation window, to determine how the tool path is depicted, or to call the time calculation. The tables provide you with an overview of the menu and soft-key functions. Overview of the "miscellaneous functions" menu Selects the simulation window (see "Simulation window" on page 471). Activates a startup-block search (see "Simulation with mid-program startup" on page 478).
6.2 Simulation window 6.2 Simulation window Setting up the views With the simulation windows described in the following you check not only the turning work but also the drilling and milling operations. XZ view (turning view): The turning contour is depicted in the XZ coordinate system. The configured coordinate system is taken into account (tool carrier in front of/behind the turning center, vertical lathes).
6.2 Simulation window Single-window view Single-window view Only one view is shown in the small simulation window. You switch the view with the Main view soft key. You can also use this soft key when only one view is set in the large simulation window. With cycle programs, you can activate the face or lateral surface view only when the C axis is used in the program.
6.3 Views 6.3 Views Traverse path display Rapid traverse 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.
6.3 Views Tool depiction You adjust by soft key whether the tool cutting edge or the light dot is shown (see table at right). The tool cutting edge is shown with the correct angles and cutting radius, as defined in the tool database. Light-dot view: A white square (light dot) is shown at the currently programmed position. The light dot represents the position of the imaginary cutting edge. Soft keys for miscellaneous functions Switches between wire-frame graphics and cutting-path graphics.
6.3 Views 3-D view The "3-D View" menu item switches to a perspective view. With the 3-D view, you can display the workpiece, auxiliary contour and finished part in a solid-model view. If there are two or more auxiliary contours in the program, they are displayed by pressing the "auxiliary contour" soft key repeatedly. The "workpiece" display shows the defined workpiece blank or the workpiece after respective stages of machining.
6.4 The zoom function 6.4 The zoom function Adjusting the visible section Press this soft key to activate the zoom function. With the zoom menu, you can modify the section displayed in the simulation window. As an alternative to the soft keys, you can use the cursor keys and the PG DN and PG UP keys to change the visible section. For cycle programs, and when a program is simulated for the first time, MANUALplus automatically selects the displayed section. When you simulate the same smart.
6.4 The zoom function Modifying the section with the zoom menu When you activate the zoom menu, a red frame is shown in the simulation window. This red frame indicates the zoom area, which you can select using the Take over soft key or the Enter key. Use the following keys to change the frame size and position: Keys for modifying the red frame The arrow keys move the red frame in the indicated direction. Reduces the size of the red frame. Increases the size of the red frame.
6.5 Simulation with mid-program startup 6.5 Simulation with mid-program startup Startup block with smart.Turn programs smart.Turn programs are always simulated from the first block, regardless of which block the cursor is in. If you use the mid-program startup, the simulation suppresses the display up to the startup block. If there is a workpiece blank, the simulation scans the blocks up to this position, updates the blank and redraws it.
6.5 Simulation with mid-program startup Mid-program startup in cycle programs For cycle programs, you first place the cursor on a cycle and then call the simulation. The simulation begins with this cycle. All previous cycles are ignored. The Start block menu item is deactivated for cycle programs.
6.6 Time calculation 6.6 Time calculation Showing the machining times During simulation, the machining and idle-machine times are calculated. The machining times, idle times and total times are shown in the "Time calculation" table (green: machining times; yellow: idle times). If you are working with cycle programs, each cycle is shown in a separate line. In DIN programs, each line represents the use of a new tool (for each tool call with T).
6.7 Saving the contour 6.7 Saving the contour Saving the generated contour in the simulation You can save a contour generated in the simulation and read it into smart.Turn. In smart.Turn, you insert into the program the workpiece blank and finished part contour that you generated during simulation. Select the "Insert contour" function on the "ICP" menu. Example: You describe the blank form and finished part and simulate machining of the first setup.
Graphic simulation 6.
Tool and technology database HEIDENHAIN MANUALplus 620 483
7.1 Tool database 7.1 Tool database You usually program the coordinates for the contour by taking the dimensions from the drawing. To enable the MANUALplus to calculate the slide path, compensate the cutting radius and determine the number of cutting passes, you need to enter the tool length, cutting radius, tool angle, etc. The MANUALplus can save tool data for up to 250 tools (optionally 999), whereby each tool is identified with a number (ID code).
7.1 Tool database Tool types Tool types Taps (Page 508) Milling pins (Page 512) Touch probes (Page 513) Multipoint tools A multipoint tool is a tool with multiple cutting edges or multiple reference points. A data record is created for every cutting edge or every reference mark. Then all data records of the multipoint tool are linked together. For every data record of a multipoint tool, the position within the multipoint tool chain is shown in the tool list in the column "MU.
7.2 Tool editor 7.2 Tool editor Tool list In the tool list, the MANUALplus displays important parameters and the tool descriptions. You can recognize the tool type and the tool orientation from the provided sketch of the tool point. Sorting the tool list The tool list switches between sorting by ID number and by tool type (and orientation)“. The tool list switches between ascending and descending sorting. Displaying the entries of only one tool type.
Adding a new tool Press the soft key Select the tool type (see soft-key table at right). The MANUALplus opens the input window. First assign the ID number (1 to 16 places, alphanumeric) and specify the tool orientation. Enter further parameters. Assign a tool text (see Page 488). Soft keys for tool organization Opens the following type selection for adding a new tool.
7.2 Tool editor Tool texts Tool texts are assigned to the tools and displayed in the tool list. The MANUALplus manages the tool texts in a separate list. Connections: The descriptions are managed in the tool text list. Each entry is preceded by a "QT number." The parameter "Tool text QT" contains the reference number for the "tool text" list. The text indicated by QT is then displayed in the tool list. When the tool dialog box is open, MANUALplus lets you enter tool texts.
7.2 Tool editor Editing multipoint tools Creating multipoint tools For each cutting edge, or each reference point, make a separate data record with the tool description. Place the cursor on a first cutting edge. Press the soft key. Press the soft key. The tool editor considers this cutting edge to be the main cutting edge (MU=0). Place the cursor on a next cutting edge. Press the soft key. The tool editor adds this cutting edge to the multipoint tool chain.
7.2 Tool editor Removing complete multipoint tools Place the cursor on a cutting edge of the multipoint tool. Press the soft key. Press the soft key. The tool editor lists all cutting edges of the multipoint tool. Place the cursor on a cutting edge no. 0 of the multipoint tool. The multipoint tool chain is removed.
7.2 Tool editor Editing tool-life data The MANUALplus counts the tool age in RT and the quantity of finished parts in RZ. When the predefined tool age or the part quantity limit has been reached, the tool is considered to be worn out. Setting a limit to tool life Set the soft key to "Tool life." The tool editor opens the Tool life MT input field for editing. Enter the tool life in the "h:mm:ss" format (h=hours; m=minutes; s=seconds).
7.2 Tool editor Manual change systems Your machine must be configured by the machine manufacturer if you want to use manual change systems. Refer to your machine manual. A tool holder is designated as a manual change system if it can accommodate various tool inserts via an integral clamping device. Most clamping devices designed as polygon coupling enable rapid, position-precise replacement of tool inserts.
7.2 Tool editor Holder table In the "to_hold.hld" holder table, define the holder type and the tool setting dimensions of the holder. Because the geometric information is currently only evaluated with holders of the "manual change system" type, the management of standard tool holders in the holder table is not required.
7.
7.2 Tool editor You can create a new holder with the "New line" soft key. The new line is always added at the end of the table. You may only use ASCII characters in the holder table for holder names. Diacritics or Asian characters are not permitted. You can also view and edit the holder table in opened tool forms. Use the 'Holder Editor" soft key for this purpose on the third form page (MTS entry).
7.2 Tool editor Setting up the holder for manual change systems Set up the manual change system holder in the turret assignment: Select turret assignment: Press the "Turret list" soft key Select an unassigned turret pocket and press the "Special functions" soft key Open the holder table: Press the "Set up holder" soft key Select the holder and press the "Adopt ID no.
7.3 Tool data 7.3 Tool data General tool parameters The parameters listed in the following table are available for all tool types. Parameters for specific tool types are described in the later chapters.
7.3 Tool data Parameters for drilling tools DV Drill diameter BW Drill angle: Point angle of the drill AW Driven tool : This parameter specifies for drilling and tapping tools during cycle programming whether switching commands are generated for the spindle or the driven tool.
7.3 Tool data Tool text (QT): You can assign a tool text to each tool. The text is shown in the tool list. Because the tool texts are shown in a separate list, the reference to the text is entered in QT (see "Tool texts" on page 488). Cutting material (SS): This parameter is required if you want to use the cutting data from the technology database (see "Technology database" on page 514). Compensation factors (CK, FK, DK): These parameters serve for the tool-specific adjustment of the cutting values.
7.3 Tool data Standard turning tools Select "New tool." Select lathe tools. For tools with round cutting edge, switch to dialog for button tools. For tool orientations TO=1, 3, 5 and 7, you can enter the tool angle EW. The tool orientation values TO=2, 4, 6, 8 are used for neutral tools. "Neutral" tools are tools that are centered precisely in the tool tip. One of the setting dimensions for neutral tools refers to the center of the tool-tip radius.
7.3 Tool data Recessing tools Select "New tool." Select recessing tools. Recessing tools are used for recessing, parting, recess turning and finishing (only smart.Turn).
7.3 Tool data Thread-cutting tools Select "New tool." Select thread-cutting tools. The help graphics illustrate the dimensions of the tools. Special parameters for thread cutting tools RS Cutting radius SB Cutting width EW Tool angle (range: 0° <= EW <= 180°) SW Point angle (range: 0° <= SW <= 180°) DN Tool width SD Shank diameter ET Maximum plunging depth NL Usable length For further tool parameters, see Page 497.
7.3 Tool data Twist drills and indexable-insert drills Select "New tool." Select drilling tools. For indexable-insert drills, switch to dialog for indexable-insert drills. The help graphics illustrate the dimensions of the tools. Special parameters for twist drills DV Drill diameter BW Drill angle: Point angle of the drill AW Driven tool : This parameter specifies for drilling and tapping tools during cycle programming whether switching commands are generated for the spindle or the driven tool.
7.3 Tool data NC center drill Select "New tool." Select special tools. Select special drilling tools. Select NC center drill. The help graphics illustrate the dimensions of the tools. Special parameters for NC center drills DV Hole diameter BW Point angle For further tool parameters, see Page 497. For drilling operations with constant cutting speed, the drilling diameter (DV) is used to calculate the spindle speed.
7.3 Tool data Centering tool Select "New tool." Select special tools. Select special drilling tools. Select centering tools. The help graphics illustrate the dimensions of the tools. Special parameters for centering tools DV Hole diameter DH Stud diameter BW Drill angle SW Point angle ZA Stud length For further tool parameters, see Page 497. For drilling operations with constant cutting speed, the drilling diameter (DV) is used to calculate the spindle speed.
7.3 Tool data Counterbore Select "New tool." Select special tools. Select special drilling tools. Select counterbore. The help graphics illustrate the dimensions of the tools. Special parameters for counterbores DV Hole diameter DH Stud diameter ZA Stud length For further tool parameters, see Page 497. For drilling operations with constant cutting speed, the drilling diameter (DV) is used to calculate the spindle speed.
7.3 Tool data Countersink Select "New tool." Select special tools. Select special drilling tools. Select counterbore. The help graphics illustrate the dimensions of the tools. Special parameters for countersinks DV Hole diameter DH Stud diameter BW Drill angle For further tool parameters, see Page 497. For drilling operations with constant cutting speed, the drilling diameter (DV) is used to calculate the spindle speed.
7.3 Tool data Tap Select "New tool." Select taps. The help graphics illustrate the dimensions of the tools. Special parameters for taps DV Thread diameter HG Thread pitch AL Length of first cut For further tool parameters, see Page 497. The thread pitch (HG) is evaluated if the corresponding parameter is not defined in the tapping cycle.
7.3 Tool data Standard milling tools Select "New tool." Select milling tools. The help graphics illustrate the dimensions of the tools. Special parameters for standard milling tools DV Cutter diameter AZ Number of teeth DD Cutter diameter compensation SL Cutting length For further tool parameters, see Page 497. For milling operations with constant cutting speed, the milling cutter diameter (DV) is used to calculate the spindle speed.
7.3 Tool data Thread milling tools Select "New tool." Select special tools. Select special milling tools. Select the thread milling tool. The help graphics illustrate the dimensions of the tools. Special parameters for thread milling tools DV Cutter diameter AZ Number of teeth FB Cutter width HG Pitch DD Cutter diameter compensation For further tool parameters, see Page 497. For milling operations with constant cutting speed, the milling cutter diameter (DV) is used to calculate the spindle speed.
7.3 Tool data Angle cutters Select "New tool." Select special tools. Select special milling tools. Select angle cutters. The help graphics illustrate the dimensions of the tools. Special parameters for angle cutters DV (Large) milling diameter AZ Number of teeth FB Cutter width FB<0: Large cutter diameter on front FB>0: Large cutter diameter on back FW Cutter angle DD Cutter diameter compensation For further tool parameters, see Page 497.
7.3 Tool data Milling pins Select "New tool." Select special tools. Select special milling tools. Select milling pins. The help graphics illustrate the dimensions of the tools. Special parameters for milling pins DV Cutter diameter AZ Number of teeth SL Cutting length FW Cutter angle DD Cutter diameter compensation For further tool parameters, see Page 497. For milling operations with constant cutting speed, the milling cutter diameter (DV) is used to calculate the spindle speed.
7.3 Tool data Touch probes Select "New tool." Select special tools. Select handling systems and touch probes. Select touch probes. The help graphics illustrate the dimensions of the tools. Special parameters for touch probes SL Cutting length TP Selection of touch probes For further tool parameters, see Page 497. The MANUALplus must be specially prepared by the machine tool builder for the use of a 3-D touch probe.
7.4 Technology database 7.4 Technology database The technology database manages the cutting data according to the machining mode, the workpiece material and the cutting material. The graphic on this page shows the composition of the database. Each cube represents a data record with cutting data. In its standard version, the technology database is designed for 9 workpiece-material/tool-material combinations. You can optionally expand the database to 62 workpiece material-cutting material combinations.
The technology editor can be called from the Tool Editor and smart.Turn operating modes. Database access of the following combinations are supported: Work material/operating mode combinations (blue) Cutting material/operating-mode combinations (red) Work-material/tool-material combinations (green) Editing workpiece and cutting material designations: The technology editor keeps one list each with workpiece designations and cutting material designations.
7.4 Technology database Editing a workpiece material or cutting material list Work material list Select the "Work materials" menu item. The editor opens the list with the workpiece material designations. Adding a workpiece material: Press the soft key. Enter the workpiece designation (maximum 16 characters). The sorting number is assigned sequentially. Deleting a workpiece material: Press the soft key.
7.4 Technology database Displaying/editing cutting data Displaying cutting data of the machining modes: Select the "Cutting data" menu item. The editor opens the dialog for selecting a workpiece material/cutting material combination. Select the desired combination and press OK. The technology editor displays the cutting data. Displaying cutting data of the workpiece materials: "Extras/.." menu item “... Select "Work material table...
7.4 Technology database Editing cutting data: Call the table with cutting data. With the arrow keys, select the cutting data field you want to edit. Press the soft key Enter the value and confirm with the Enter key. Adding new cutting data: Set any workpiece-material/cutting material combinations. Press the soft key. The editor opens the "New cutting data" dialog box. Set the new material/cutting material combinations.
Organization mode of operation
8.1 Organization mode of operation 8.1 Organization mode of operation This mode of operation offers various functions for communication with other systems, data backup, setting of parameters, and diagnosis. Login code Code number Possibilities The following functions are available: Editing user parameters Login code Some parameter settings and functions may only be accessed by qualified personnel. Users need to enter a code number to log in to this mode.
8.2 Parameters 8.2 Parameters Parameter editor The parameter values are entered in the configuration editor. Each parameter object has a name (e.g. CfgDisplayLanguage) that gives information about the parameters it contains. Each object has a key for unique identification. The MANUALplus displays an icon at the beginning of each line in the parameter tree showing additional information about this line.
8.2 Parameters Displaying help texts Position the cursor on the parameter. Press the info key. The parameter editor opens the window with information on these parameters. Press the info key again to close the information window. Searching for parameters Press the Find soft key Enter the search criteria. Press the Find soft key again. Exiting the parameter editor Press the End soft key.
8.2 Parameters List of user parameters Language setting: Parameter: NC and PLC conversational language settings / ... ... / NC conversational language (101301) ENGLISH GERMAN CZECH FRENCH ITALIAN SPANISH PORTUGUESE SWEDISH DANISH FINNISH DUTCH POLISH HUNGARIAN RUSSIAN CHINESE CHINESE_TRAD SLOVENIAN ESTONIAN KOREAN LATVIAN NORWEGIAN ROMANIAN SLOVAK TURKISH LITHUANIAN ... / PLC conversational language (101302) See NC conversational language ...
8.2 Parameters General settings: Parameter: System / ... Meaning ... / Definition of the units of measure valid for the display (101100) / ... ... / Unit of measure for display and user interface (101101) metric Use the metric system inch Use the inch system ... / General settings for automatic operation (601800) / ... .../ Service life management (601801) ON Tool life monitoring is active OFF Tool life monitoring is inactive ...
8.2 Parameters Settings for the simulation: Parameter: Simulation / ... Meaning ... / General settings (114800) / ... ... / Restart with M99 (114801) ON Simulation begins again at beginning of program OFF Simulation stops ... / Traverse delay [s] (114802) ... / Machining times for the NC functions in general (115000) / ... Delay time after each path has been graphically simulated. The simulation speed can thus be influenced.
8.2 Parameters Settings for fixed cycles and units: Parameters: processing / ... Meaning ... / General settings (602000) / ... ... / External safety clearance (SAR) [mm] (602005) External safety clearance on workpiece blank ... / Internal safety clearance (SIR) [mm] (602006) Internal safety clearance on workpiece blank ... / External on machined part (SAT) [mm] (602007) External safety clearance on machined part ...
8.2 Parameters Machining parameters (processing) Machining parameters are used by the work plan generation (TURN PLUS) and various machining cycles. General settings Global technology parameters – Safety clearances Global safety clearance Speed limiting [SMAX] Global speed limiting. You can define a small speed limit in the program head of the TURN PLUS program.
8.
8.2 Parameters Global parameters for finished parts Global parameters for finished parts Max. inward copying angle [EKW] Tolerance angle for recess areas, used for distinguishing turning from recessing (mtw = contour angle).
8.2 Parameters BBG (drilling limitation elements): Contour elements intersected by UBD1/UBD2 UBD1/UBD2 have no effect when "Centric predrilling" has been defined as main machining operation followed by "Finish-drilling" as submachining operation in the machining sequence (see smart.Turn and DIN Programming User's Manual). Prerequisite: UBD1 > UBD2 UBD2 must permit subsequent inside machining with boring bars.
8.
8.2 Parameters Centric predrilling – Machining Machining Drilling depth ratio [BTV] TURN PLUS checks the 1st and 2nd drilling steps.
8.2 Parameters Roughing – Machining standards Machining standards Standard/Full-surface – external/longitudinal [RAL] Standard/Full-surface – internal/longitudinal [RIL] Standard/Full-surface – external/transverse [RAP] Standard/Full-surface – internal/transverse [RIP] Input for RAL, RIL, RAP, RIP: 0: Full-surface roughing cycle, including plunge-cutting. TURN PLUS looks for a tool for full-surface machining.
8.
8.2 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.
8.2 Parameters Roughing – Machining cycles Fixed cycles Overhang length outside [ULA] Relative length for external rough-machining enabling roughing beyond the target position in longitudinal direction. ULA is not considered when the cutting limitation is in front of or within the overhang. Overhang length inside [ULI] Relative length for internal rough-machining enabling roughing beyond the target position in longitudinal direction.
8.2 Parameters Finishing – Machining standards Machining standards Tool angle – external/longitudinal [FALEW] Point angle – internal/longitudinal [FILEW] Tool angle – external/transverse [FAPEW] Point angle – internal/transverse [FIPEW] Tool selection Finishing cycles are primarily executed with standard finishing tools. If form elements such as recesses (type FD) and undercuts (type E, F, G) cannot be machined with a standard finishing tool, one form element after the other is skipped.
8.
8.2 Parameters Finishing – Machining analysis Machining analysis Minimum finishing transverse length [FMPL] TURN PLUS checks the frontmost element of the outside contour to be finish-machined.
8.
8.2 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.
8.2 Parameters Thread cutting Thread cutting – Approach and departure Approach and departure are at rapid traverse (G0).
8.2 Parameters Measuring The measuring parameters are assigned to the fit elements as an attribute. Measurement procedure Measuring loop counter [MC] Defines the measurement/loop intervals Measuring path length in Z [MLZ] Distance in Z for departure movement Measuring path length in X [MLX] Distance in X for departure movement Measuring oversize [MA] Oversize still applied to the element to be measured.
8.2 Parameters Drilling – Safety clearances Safety clearances Internal safety clearance [SIBC] Retraction distance for deep-hole drilling ("B" for G74) Driven drills [SBC] Safety clearance for driven tools on face and lateral surface. Stationary drills [SBCF] Safety clearance on face and lateral surface for tools that are not driven. Driven taps [SGC] Safety clearance for driven tools on face and lateral surface.
8.2 Parameters Milling Milling – Approach and departure Approach and departure are at rapid traverse (G0).
8.3 Transfer 8.3 Transfer The Transfer mode is used for data backup and data exchange via networks or USB devices. When we speak of "files" in the following, we mean programs, parameters and tool data. The following file types can be transferred: Programs (cycle programs, smart.Turn programs, DIN main and subprograms, ICP contour descriptions) Parameters Tool data Data backup HEIDENHAIN recommends backing up the tool data and programs created on MANUALplus on an external device at regular intervals.
8.3 Transfer Connections You can establish connections over the network (Ethernet) or with a USB storage device. Data is transferred over the Ethernet or USB interface. Network (via Ethernet): The MANUALplus supports SMB networks (Server Message Block, WINDOWS) and NFS networks (Network File Service). USB storage devices can be connected directly to the control. The MANUALplus uses only the first partition of a USB storage device.
8.3 Transfer Ethernet interface (with software 548328-xx) Network configuration settings Control name - Computer name of the control DHCP (Dynamic Host Configuration Protocol) OFF: The other network settings have to be configured manually. Static IP address. ON: The network settings are automatically configured by a DHCP server.
8.3 Transfer Ethernet interface (with software 54843x-xx) Introduction The control is shipped with a standard Ethernet card to connect the control as a client in your network. The control transmits data via the Ethernet card with the smb protocol (Server Message Block) for Windows operating systems, or the TCP/IP protocol family (Transmission Control Protocol/Internet Protocol) and with support from the NFS (Network File System).
8.3 Transfer Control configuration General network settings Press the DEFINE NET soft key to enter the general network settings. The Computer name tab is active: Setting Meaning Primary interface Name of the Ethernet interface to be integrated in your company network.
8.3 Transfer Press the Configuration button to open the Configuration menu: Setting Meaning Status Interface active: Connection status of the selected Ethernet interface Name: Name of the interface you are currently configuring Plug connection: Number of the plug connection of this interface on the logic unit of the control Profile Here you can create or select a profile in which all settings shown in this window are stored.
8.
8.3 Transfer Select the Ping/Routing tab to enter the ping and routing settings: Setting Meaning Ping In the Address: field, enter the IP number for which you want to check the network connection. Input: Four numerical values separated by periods, e.g. 160.1.180.20. As an alternative, you can enter the name of the computer whose connection you want to check Press the Start button to begin the test.
8.3 Transfer Setting Meaning DHCP server active on: IP addresses as of: Define the IP address as of which the control is to derive the pool of dynamic IP addresses. The control transfers the values that appear dimmed from the static IP address of the defined Ethernet interface; these values cannot be edited. IP addresses up to: Define the IP address up to which the control is to derive the pool of dynamic IP addresses.
8.3 Transfer Network settings specific to the device Press the Network soft key to enter the network settings for a specific device. You can define any number of network settings, but you can manage only seven at one time Setting Meaning Network drive List of all connected network drives.
8.3 Transfer USB connection Select the Organization mode and plug the USB storage device in at the USB port on the MANUALplus. Press the Transfer soft key (login required). Press the Connections soft key. Press the USB soft key. The MANUALplus opens the USB dialog box. This dialog box is for the settings for the connection target. Soft keys for USB connection Use the soft keys to disconnect and reconnect USB storage devices. Creates a folder of the specified name on the USB storage device.
The MANUALplus manages DIN programs, DIN subprograms, cycle programs and ICP contours in different directories. When you select "Program group," the control automatically switches to the applicable directory. Parameters and tool data are stored under the file name entered for Backup name and saved to a ZIP file located in the "para" or "tool" folder on the control. You can then send this backup file to a project folder in the remote station.
8.3 Transfer Transferring programs (files) Selecting the program group Press the Transfer soft key (login required). Press the Connections soft key. Press the USB soft key. Press the Network soft key. Select a project folder and press the Selection soft key (USB), or the Connect (network) soft key. Return to data selection. Switch to program transfer. Open a selection of program types. Activate DIN programs (or other program types) for transfer. Soft keys for program group selection *.
8.3 Transfer Selecting the program In the window on the left, the MANUALplus shows a file list of the control. The files of the remote station are displayed in the window on the right when a connection is established. With the cursor keys you can switch back and forth between the two windows. When selecting a program, place the cursor on the desired program and press the Mark soft key. You can also select all programs with Mark everything. Marked programs are highlighted in color.
8.3 Transfer Transferring parameters Parameters are backed up in two steps: Creating a parameter backup: The parameters are archived in ZIP files and stored in the control. Transmitting/Receiving the parameter backup files. Restoring parameters: Restores the backup files into the active data on the MANUALplus (login required). Parameter selection You can also create a parameter backup without connecting to an external storage device. Press the Transfer soft key (login required).
8.3 Transfer Transferring tool data Tools are backed up in two steps: Creating a tool backup: The parameters are archived in ZIP files and stored in the control. Transmitting/Receiving the tool backup files. Restoring tools: Restores the backup files into the active data on the MANUALplus (login required). Tool selection You can also create a tool backup without connecting to an external storage device. Press the Transfer soft key (login required). Open the tool transfer.
8.3 Transfer Service files Service files contain various log files used by the service department for troubleshooting. All important information is summarized in a services file record as a zip file. Path and file names of the backup files: \data\SERVICEx.zip ("x" stands for a consecutive number) The MANUALplus always generates the service file with the number "1". Already existing files are renamed to the numbers 2 to 5. An existing file with the number 5 is deleted.
8.3 Transfer Creating a data backup file A data backup performs the following steps: Copies the program files to the transfer folder. NC main programs NC subprograms (with graphics) Cycle programs ICP contours Soft keys for data backup Starts backing up the data to a complete transfer folder. Creates a parameter backup and copies all backup files from "\para" and "\table" to the project folder. (PA_Backup.zip, TA_Backup.
8.3 Transfer Importing NC programs from predecessor controls The program formats of the predecessor controls MANUALplus 4110 and CNC PILOT 4290 differ from the format of the MANUALplus 620. However, you can use the program converter to adapt programs of the predecessor control to the new control. This converter is a component of the MANUALplus. The converter completes the required adaptations as automatically as possible.
8.3 Transfer Use the cursor keys to select the folder, then press the Enter key to switch to the right window. With the cursor keys, select the NC program to be converted. Mark all NC programs. Start the import filter for converting the program(s) to the MANUALplus format. The names of imported cycle programs, ICP contour descriptions, DIN programs and DIN subprograms are given the prefix "CONV_..." In addition, the MANUALplus adapts the extension and imports the NC programs to the correct folders.
8.3 Transfer M functions are left unchanged. Calling ICP contours: When an ICP contour is called, the converter prefixes "CONV_..." to the name. Calling DIN cycles: When a DIN cycle is called, the converter prefixes "CONV_..." to the name. HEIDENHAIN recommends adapting converted NC programs to the circumstances of the MANUALplus and then testing them before using them for production. Converting DIN programs DIN/ISO programs not only have new solutions for tool management, technology data, etc.
8.3 Transfer Remember the following when converting DIN programs of the CNC PILOT 4290: Tool call (T commands of the TURRET section): T commands containing a reference to the tool database are left unchanged (example: T1 ID“342-300.1“). T commands containing tool data cannot be converted. Variable programming: Variable accesses to tool data, machine dimensions, D compensation values, parameter data and events cannot be converted. These program sequences have to be adapted.
8.4 Service pack 8.4 Service pack If changes or additional features are required in the control software, your machine tool builder will provide you with a service pack. The service pack is usually installed with the aid of a USB memory stick (1 GB or larger). The software required for the service pack is compressed in the setup.zip file. This file is saved on the USB stick. Installing a service pack The control has to be shut-down during the installation of the service pack.
8.4 Service pack The MANUALplus checks whether the service pack can be used for the current software version of the control. Answer the confirmation prompt "Do you really want to switch off?" Then the actual update program starts. Set the desired language (e.g. English) and do the update. After the software update the MANUALplus automatically restarts. Keep the USB stick so that you can undo the installation of the service pack if necessary.
8.
Tables and overviews HEIDENHAIN MANUALplus 620 571
9.1 Thread pitch 9.1 Thread pitch Thread parameters To determine the thread parameters, the MANUALplus 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 573.) . P: Thread depth R: Thread width A: Thread angle, left W: Thread angle, right Calculation formula: Kb = 0.26384*F – 0.
F P R A W Q=12 Nonstandard thread – – – – – External * 0.61343*F F 30° 30° Internal * 0.54127*F F 30° 30° External * 0.61343*F F 30° 30° Internal * 0.54127*F F 30° 30° External * 0.61343*F F 30° 30° Internal * 0.54127*F F 30° 30° External * 0.8*F F 30° 30° Internal * 0.8*F F 30° 30° External * 0.8*F F 30° 30° Internal * 0.8*F F 30° 30° Q=18 NPSC U.S. cylindrical pipe thread with lubricant External * 0.8*F F 30° 30° Internal * 0.
9.
9.
9.
9.
9.1 Thread pitch Q = 19 NPFS U.S.
9.2 Undercut parameters 9.2 Undercut parameters DIN 76—undercut parameters The MANUALplus 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.
9.
9.2 Undercut parameters DIN 509 E – undercut 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.
9.3 Technical information 9.3 Technical information Specifications Components MC 7410T main computer with CC 61xx controller unit 12.1-inch TFT color flat-panel display Operating system HEROS real-time operating system for machine control Memory 1.8 GB (on CFR compact flash memory card) for NC programs Input resolution and display step X axis: 0.5 µm, diameter: 1 µm Z and Y axes: 1 µm U, V and W axes: 1 µm C and B axes: 0.
9.
9.
B-axis machining (optional) Machining with the B axis Tilting the working plane Rotating the machining position of the tool DXF import Importing contours for turning Importing contours for milling smart.
9.3 Technical information User functions DINplus programming Programming in DIN 66025 format Extended command format (IF... THEN ... ELSE...
Tool database For 250 tools For 999 tools (optional) Tool description can be entered for every tool Automatic inspection of tool-tip position with respect to the contour Compensation of tool-tip position in the X/Y/Z plane High-precision correction via handwheel, capturing compensation values in the tool table Automatic tool-tip and cutter radius compensation Tool monitoring for lifetime of the insert (tool tip) or the number of workpieces produced Tool monitoring with automatic tool chan
9.
Option ID Description 0 to 6 Additional axis 354540-01 Additional control loops 9.3 Technical information Option number 353904-01 353905-01 367867-01 367868-01 370291-01 307292-01 8 Software option 1 632226-01 Cycle programming Contour description with ICP Cycle programming Technology database with 9 workpiece-material/toolmaterial combinations 9 Software option 2 632227-01 smart.Turn Contour description with ICP Programming with smart.
9.3 Technical information Option number Option ID Description 42 Software option DXF import 632231-01 DXF import Loading of DXF contours 54 B-axis machining 825742-01 Machining with the B axis Tilting the working plane Rotating the machining position of the tool 55 Software option C-axis machining 633944-01 C-axis machining 63 TURN PLUS 825743-01 Automatic generation of smart.
9.4 Compatibility in DIN programs 9.4 Compatibility in DIN programs The format of DIN programs of the CNC PILOT 4290 predecessor control differs from the format of the MANUALplus 620. However, you can use the program converter to adapt programs of the predecessor control to the new control. When opening an NC program, the MANUALplus 620 recognizes the programs of the predecessor control. The program concerned will be converted after a confirmation prompt. "CONV_..." will be prefixed to the program name.
9.4 Compatibility in DIN programs A warning will be issued if the following G functions are used in a contour description: G10, G38, G39, G52, G95, G149. These functions are now modal. Warnings may occur for the thread functions G31, G32, G33; it is recommended to test these functions. The "Contour mirroring/shifting G121" function is converted to G99, but the principle of function is compatible. A warning will be issued for G916, G917 and G930 because the principle of function has changed.
9.
9.
9.
9.
9.
9.
9.
9.
9.4 Compatibility in DIN programs Synchronization commands Spindle synchronization, workpiece transfer G30 Converting and mirroring þ G121 Contour mirroring/shifting þ G720 Spindle synchronization þ G905 Measuring C-angle offset þ G906 Measuring angular offset during spindle synchronization – G916 Traversing to a fixed stop þ G917 Controlled parting using lag error monitoring þ G991 Controlled parting using spindle monitoring – G992 Values for controlled parting – G119 No.
9.4 Compatibility in DIN programs Variable programming, program branches # variables Evaluation during program conversion þ V variables Evaluation during program run þ IF..THEN.. Program branching þ WHILE.. Program repeat þ SWITCH..
9.
9.
Overview of cycles
10.1 Workpiece blank cycles, single cut cycles 10.
10.2 Turning cycles 10.
10.3 Recessing and recess-turning cycles 10.
10.4 Thread cycles 10.
10.5 Drilling cycles 10.
10.6 Milling cycles 10.
10.
C D Absolute coordinates ... 44 Additive compensation ... 112 Additive compensation for cycle programming ... 128 Alphanumeric keyboard ... 55 API thread ... 267 API thread, recutting ... 275 Axis designations ... 43 Axis values, setting ... 91, 92 Copy Circular ... 376 Linear ... 375 Mirror ... 376 Cut, ICP contour-parallel, longitudinal ... 178 Cut, ICP contour-parallel, longitudinal finishing ... 182 Cut, ICP contour-parallel, transverse ... 180 Cut, ICP contour-parallel, transverse finishing ...
Index F I I Feed angle ... 258 Feed rate ... 82 Feed rate reduction for drilling Cycle programming Deep-hole drilling ... 291, 294 Drilling cycle ... 287, 289 File organization ... 116 Fit calculation ... 370 Fits ... 370 Form elements (ICP) Fundamentals ... 361 Form elements, ICP ... 361 Full-surface machining Fundamentals ... 37 ICP circular pattern on face ... 420 ICP circular pattern on lateral surface ... 430 ICP circular slot in XY plane ... 442 ICP circular slot in YZ plane ...
M O ICP starting point of contour in XY plane ... 433 ICP starting point of contour in YZ plane ... 450 ICP starting point of face contour ... 398 ICP starting point of lateral surface contour ... 404 ICP starting point of turning contour ... 387 ICP transitions between contour elements ... 369 ICP undercut DIN 509 E ... 393 ICP undercut DIN 509 F ... 394 ICP undercut DIN 76 ... 392 ICP undercut type H ... 396 ICP undercut type K ... 397 ICP undercut type U ... 395 ICP vertical lines in XY plane ...
Index R S T Rapid positioning milling ... 304 Rapid traverse positioning ... 133 Recess turning with ICP, axial ... 242 Recess turning with ICP, radial ... 240 Recess turning with ICP, radial finishing ... 244 Recess turning, axial ... 226 Recess turning, axial finishing ... 234 Recess turning, axial finishing— expanded ... 238 Recess turning, ICP axial, finishing ... 246 Recess turning, radial ... 225 Recess turning, radial finishing ... 232 Recess turning, radial finishing— expanded ...
W Tool measurement with a touch probe ... 101 Tool position in turning cycles ... 147 Tool touch probe, calibrating ... 96 Tool types ... 484 Tool-life data, editing ... 491 Tools Driven tools ... 87 Tool administration (tool management) ... 484 Tool compensation, entering ... 103 Tool list ... 486 Tools in different quadrants ... 84 Tools in different quadrants ... 84 Tools measurement with an optical gauge ... 102 Tool-tip radius compensation (TRC) ... 48 Touch probe ... 101 Touch-off ... 100 Transfer ..
Index
1079948-21 · Ver01 · SW02 · H · 1/2014
