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%). Feed symbols (F display) Status "Cycle ON" Cycle or program execution is active. Status "Cycle OFF" Cycle or program execution is not active. Symbol

Spindle

"S" is the identification letter for spindle data. Depending on which mode of the Constant speed soft key is active, data is entered in: Revolutions per minute (constant speed) Meters per minute (constant cutting speed). The input range is limited by the maximum spindle speed. You define the speed limitation in "Set T, S, F", in machine parameters 805/855, or in DIN programming with the G26 command. The speed limit remains in effect until a new speed limit value is programmed. The speed compensation controller (speed override) allows you to change the spindle speed (range: 50% to 150%). The subscript number after the identification letter "S" indicates the gear range. If you are machining with a constant cutting speed, MANUALplus calculates the spindle speed from the position of the tool tip. The smaller the diameter of the tip, the higher the spindle speed. The maximum spindle speed, however, is never exceeded. The spindle symbols indicate the direction of spindle rotation as seen from the point of view of the machinist. Spindle symbols (S display) Direction of spindle rotation M3 Symbol
Direction of spindle rotation M4

Spindle stopped

Spindle position-controlled (M19)

3.4 Machine Setup

The machine always requires a few preparations, regardless of whether you are machining a workpiece manually or automatically. In Manual mode the following functions are subitems of the "Setup" menu item: Setting the axis values (defining workpiece zero point) Setting the protection zone Defining the tool change position Setting C-axis values

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 (without run-in) X2, Z2 end point of thread (without run-out) F1 thread pitch (= feed rate) U thread depth No input: Depth is calculated External thread: U=0.6134*F1 Internal thread: U=0.5413*F1 I 1st cutting depth I<U: First cut with cutting depth Ifurther cuts: Reduction of cutting depth down to J. I=U: One cut No input: Calculation from U and F1 A feed angle (default: 30): Range: 60 < A < 60 A<0: Infeed on left thread flank A>0: Infeed on right thread flank W J T S D E taper angle: Range: 60 < A < 60 remaining cutting depthdefault: 1/100 mm tool number spindle speed / cutting speed number of thread startsdefault: 1 single-start thread incremental gradientdefault: 0 E=0: Constant pitch E>0: Increase the pitch per revolution by E E<0: Decrease the pitch per revolution by E
Parameter combinations for taper angle: X1/Z1, X2/Z2 X1/Z1, Z2, W Z1, X2/Z2, W Cycle run 7 Calculate the proportioning of cuts. Move to starting point X1, Z1. Move to end point Z2 at programmed feed rate. Return on paraxial path and approach for next thread groove. Repeat 3 and 4 for all thread grooves. Approach for next pass, taking the reduced cutting depth and the "feed angle A" into account. Repeat 3 to 6 until "no. threads D" and "depth U" are reached.

API thread

Select "API 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. Cycle parameters
X, Z starting point X1, Z1 starting point of thread (without run-in) X2, Z2 end point of thread (without run-out) F1 thread pitch (= feed rate) U thread depth No input: Depth is calculated External thread: U=0.6134*F1 Internal thread: U=0.5413*F1 I 1st cutting depth I<U: First cut with cutting depth Ifurther cuts: Reduction of cutting depth down to J. I=U: One cut No input: Calculation from U and F1 A feed angle (default: 30): Range: 60 < A < 60 A<0: Infeed on left thread flank A>0: Infeed on right thread flank W taper angle: Range: 45 < W < 45 WE run-out angle: Range: 0 < WE < 90 J remaining cutting depthdefault: 1/100 mm T tool number S spindle speed / cutting speed D number of thread startsdefault: 1 single-start thread
Parameter combinations for taper angle: X1/Z1, X2/Z2 X1/Z1, Z2, W Z1, X2/Z2, W Cycle Programming
Cycle run 7 Calculate the proportioning of cuts. Move to thread starting point X1, Z1. Move to end point Z2 at programmed feed rate, taking the "run-out angle WE" into account. Return on paraxial path and approach for next thread groove. Repeat 3 and 4 for all thread grooves. Approach for next pass, taking the reduced cutting depth and the "feed angle A" into account. Repeat 3 to 6 until "no. threads D" and "depth U" are reached.

Contour milling: 7 Depending on "R," approach the workpiece and plunge to the first milling plane. Mill the first plane. Plunge to the next milling plane. Repeat 5 to 6 until the milling depth is reached. Position to starting point Z and deactivate C axis.
Pocket millingRoughing: 7 Move to the safety clearance and plunge to the first milling plane. Depending on "J," machine the milling plane either from the inside towards the outside, or vice versa. Plunge to the next milling plane. Repeat 4 to 5 until the milling depth is reached. Position to starting point Z and deactivate C axis.
Pocket millingFinishing: 7 Depending on "R," approach the workpiece and plunge to the first milling plane. Finish-machine the edge of the pocketone working plane after the other. Depending on "J," finish-machine the milling floor either from the inside towards the outside, or vice versa. Finish-machine the pocket at the programmed feed rate. Position to starting point Z and deactivate C axis.

ICP contour, axial

Select "ICP contour, axial."
Depending on the parameters, the cycle mills a contour or roughs/ finishes a pocket on the face. Notes on parameters/functions: Machining of contour or pocket: defined in "U." Milling direction: depends on definition in "H" and the direction of tool rotation (see Cutting direction for contour milling and pocket milling on page 224). Milling cutter compensation: effective (except for contour milling with J=0). Approach and departure: For closed contours, the point of the surface normal from the tool position to the first contour element is the point of approach and departure. If no surface normal intersects the tool position, the starting point of the first element (for rectangles, the longer element) is the point of approach and departure. The tool approaches directly or on an arc according to "approaching radius R." Contour milling: "J" 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. Pocket millingroughing (O=0): "Contour milling J" defines whether a pocket is machined from the inside towards the outside, or vice versa. Pocket millingfinishing (O=1): First, the edge of the pocket is machined; then the pocket floor is machined. "J" defines whether a pocket floor is finished from the inside towards the outside, or vice versa.

P infeed depthdefault: Total depth in one infeed U overlap factor No input: Contour milling U>0: Pocket milling(minimum) overlap of milling paths = U*milling diameter I contour-parallel oversize K oversize in infeed direction FZ infeed ratedefault: Active feed rate E reduced feed rate for circular elementsdefault: Active feed rate H cutting directiondefault: 0 H=0: Up-cut milling H=1: Climb milling J milling direction: For surfaces or polygons (with "RE = 0"), "J" defines whether a unidirectional or bidirectional milling operation is to be executed. J=0: Unidirectional J=1: Bidirectional O roughing/finishing: Milling sequence (only for pocket milling) default: 0 O=0: Roughing O=1: Finishing
Cycle run 3 Activate the C axis and position to spindle angle C at rapid traverse (only in Teach-in mode). Calculate the proportioning of cuts (infeeds to the milling planes, infeeds in the milling planes). Move to the safety clearance and plunge to the first milling plane.
Roughing Machine the milling plane, taking "J" (unidirectional or bidirectional) into account. Plunge to the next milling plane. Repeat 4 to 5 until the milling depth is reached. Position to starting point Z and deactivate C axis.
Finishing: 6 Finish-machine the edge of the islandone working plane after the other. Finish-machine the floor from the outside towards the inside. Position to starting point Z and deactivate C axis.

Slot, radial

Select the "Slot, radial" cycle.
This cycle mills a slot on the lateral surface. The slot width equals the diameter of the milling cutter. Cycle parameters
X, Z starting point C spindle angle (C-axis position)default: Current spindle angle C1 angle of slot target pointdefault: Spindle angle C X1 milling top edge (diameter)default: Starting point X Z1 target point of slot X2 milling floor L slot length A angle to Z axisdefault: 0 P infeed depthdefault: Total depth in one infeed FZ infeed ratedefault: Active feed rate T tool number S spindle speed / cutting speed F feed per revolution
Parameter combinations for the position and orientation of the slot: See graphic support window Cycle run 5 Activate the C axis and position to spindle angle C at rapid traverse (only in Teach-in mode). Move at rapid traverse to slot starting point X, Z if defined. Approach at infeed rate FZ. Mill to slot end point at programmed feed rate. Retract to starting point X.

If you enter a comment in an empty block, the block number is deleted and only the comment is stored in this block. (An "empty block" is a block that consists of the block number only.) If the NC block already contains NC commands, the comment is appended to the end of the block. To change comments, place the cursor at the beginning of the comment and press Change word. MANUALplus then displays the "alphanumeric keyboard" and the current text of the comment. You can now edit the comment as desired by changing, adding to, etc. If you wish to delete comments, place the cursor at the beginning of the comment and press Delete block or Delete word, as applicable. The comment is deleted.
Mark several successive NC blocks (block sequence) to be able to cut, copy or delete them. If you cut or copy the block sequence, it is taken into the clipboard. You can then insert this block sequence at a different position in the program, or call a different DIN program and insert the block sequence there. The block sequence remains stored in the clipboard until it is overwritten or MANUALplus is switched off. Copying and pasting blocks Position the cursor on the beginning of a block.
Call the block functions.
Mark the beginning of the block.
Position the cursor on the end of a block.
Mark the end of the block.
Copy the block and transfer it to the clipboard.
Cut the block out and transfer it to the clipboard.
Load a new DIN program (if required).
Place the cursor on the position where the block is to be inserted.
Transfer the block sequence from the clipboard (the NC blocks are inserted below the cursor).

Menu structure

Select the function group by menu key. G and M functions: The function number and further parameters that vary depending on the function are entered subsequently. Comment, subprogram and T, S, F: The required parameters are entered subsequently. Variable functions: MANUALplus switches to other menus for entering further data.
DIN functions G function Traversing commands, cycles, and other G commands. M function Switching functions for machine components and program control functions (see M Functions on page 408). Machine data Entry of F, S, T (see Set T, S, F on page 392). Comment Entry of comments (see Editing DIN Programs on page 281). Program variable functions Switch to the "Program variable menu" (see Programming Variables on page 396). Machine variable functions Switch to the "Machine variable menu" (intended for special cases and of no importance to the DIN programmer). Subprogram call Program a subprogram call (see Subprograms on page 406).

Contour-parallel oversize (equidistant) G58
G58 defines a contour-parallel oversize. G58 is programmed before recessing or roughing cycles. Parameters

P oversize

A negative oversize is permitted with the cycle G89. The following cycles take the oversizes into account: Roughing cycles: G817, G818, G819, G827, G828, G829, G83 Recessing cycles: G86x Recess turning cycles: G81x, G82x The cycle G83 does not cancel the oversizes after execution of the cycle. If an oversize is programmed with G58 and in the cycle, the oversize from the cycle is used. Example: G58 %58.nc [G58] N1 T3 G95 F0.25 G96 S200 M3 N2 G0 X120 Z2 N3 G58 P2 N4 G819 P5 N5 G0 X80 Z2 N6 G1 Z-15 B-1 N7 G1 X102 B2 N8 G1 Z-22 N9 G1 X90 Zi-12 B1 N10 G1 Zi-6 N11 G1 X100 A80 B-1 N12 G1 Z-47 N13 G1 X120 N14 G80 END
6.11 Contour-Based Turning Cycles

Contour definition

For contour-based cycles (turning / recessing / recess turning cycles), the cycle call is followed by the contour definition: G0 defines the starting point of the contour section. The contour section is described with G1, G2, G3, G12 and G13 commands. G80 concludes the contour definition.

End of cycle G80

G80 concludes the contour definition after roughing, recessing and undercut cycles. A block with G80 must not contain any other commands.
Longitudinal contour roughing G817/G818
The cycles machine the contour area described by the current tool position and the data defined in the subsequent blocks in longitudinal direction without recessing (see Contour definition on page 310). Parameters G817, G818
X cutting limit (diameter value): The control machines up to the cutting limit. P maximum infeed: The proportioning of cuts is calculated so that an "abrasive cut" is avoided and the infeed distance is <= P. H type of departure (default: 1): 0: Machine contour outline after each pass 1: Retract at 45; machine contour outline after last pass 2: Retract at 45; do not machine contour outline I oversize X (diameter value)(default: 0) K oversize Z (default: 0)
Note on the execution of the cycle: MANUALplus automatically determines the cutting and infeed directions from the current tool position relative to the starting point / end point of the contour area. Tool position at the end of the cycle: G817: Cycle starting point Z; last retraction diameter X G818: Cycle starting point Descending contour elements are not machined. The tool must be located outside the defined contour area. Cutting radius compensation: Active. G57/G58 oversizes are taken into account if I/K is not programmed. After the cycle has been executed, the oversizes are canceled. Safety clearance after each step: Parameter "Current parametersMachiningSafety distances."

The control determines the undercut parameters from the cylinder diameter (see tables).
Undercut parameters DIN 509 E (dimensions in mm) Undercut Undercut Undercut Diameter depth I length K radius R < 18 > 18 - 80 > 80 0,25 0,35 0,2,0,6 0,6 1
Undercut parameters DIN 509 F (dimensions in mm) Undercut Undercut Undercut Transverse Diameter depth I length K radius R depth P < 18 > 18 - 80 > 80 0,25 0,35 0,2,0,6 0,0,1 0,2 0,3
Undercut angle (for undercuts according to DIN 509 E and F): 15 Transverse angle (for undercuts according to DIN 509 F): 8
Undercut according to DIN 509 E with cylinder machining G851
The cycle machines the adjoining cylinder, the undercut, and finishes with the plane surface. It also machines a cylinder start chamfer when you enter at least one of the parameters "B" or "RB." Parameters
I undercut depth (default: Value from standard table) K undercut length (default: Value from standard table) W undercut angle (default: Value from standard table) B cylinder 1st cut lengthno input: No chamfer machined at start of cylinder RB 1st cut radiusno input: No chamfer radius is machined WB 1st cut angle (default: 45) E reduced feed rate (default: Active feed rate): For the plunge cut and the cylinder start chamfer H type of departure (default: 0): H=0: Tool returns to the starting point H=1: Tool remains at the end of the plane surface U finishing oversize for the area of the cylinder (default: 0)
Example: G851 %851.nc [G851] N1 T21 G95 F0.23 G96 S248 M3 N2 G0 X60 Z2 N3 G851 I3 K15 W30 R2 B5 RB2 WB30 E0.2 H1 N4 G0 X50 Z0 N5 G1 Z-30 N6 G1 X60 N7 G80 END
Note: Parameters that are not programmed are automatically calculated from the diameter of the cylinder in the standard table (see DIN 509 E, DIN 509 Fundercut parameters on page 527). Blocks following the cycle call N. G851 I. K. W. /Cycle call N. G0 X. Z. /Corner point of cylinder start chamfer N. G1 Z. /Undercut corner N. G1 X. /End point of plane surface N. G80 /End of contour definition
Undercuts can only be executed in orthogonal, paraxial contour corners along the longitudinal axis. Cutting radius compensation: Active. Oversizes: are not taken into account.
Undercut according to DIN 509 F with cylinder machining G852
I undercut depth (default: Value from standard table) K undercut length (default: Value from standard table) W undercut angle (default: Value from standard table) R undercut radius (default: Value from standard table) P transverse depth (default: Value from standard table) A transverse angle (default: Value from standard table) B cylinder 1st cut lengthno input: No chamfer machined at start of cylinder RB 1st cut radiusno input: No chamfer radius is machined WB 1st cut angle (default: 45) E reduced feed rate (default: Active feed rate): For the plunge cut and the thread chamfer H type of departure (default: 0): H=0: Tool returns to the starting point H=1: Tool remains at the end of the plane surface U finishing oversize for the area of the cylinder (default: 0)

You can add up to 20 "transfer values" to a subprogram. These are: LA to LF, LH, I, J, K, O, P, R, S, U, W, X, Y, Z. The transfer values are available as variables within the subprogram. The identification code is: "#__.", followed by the parameter designation in lowercase letters (for example: #__la). You can use these transfer values when programming with variables within the subprogram (see figure to the bottom right). The transfer parameter LN is reserved for transferring integer values from 0 to 9999. The variables #256 #285 are available in any subprogram for internal calculations (local variables). If a subprogram is to be executed repeatedly, enter the number of times the subprogram is to be repeated in the parameter "number repeats Q." Dialog texts You can define the parameter descriptions that precede/follow the input fields in an external subprogram. MANUALplus automatically sets the unit of measure for parameter values to the metric system or inches. A maximum of 19 descriptions can be entered. The parameter descriptions can be positioned within the subprogram as desired.
Example:. [//] [la=1; s=bar diameter] [lb=1; s=starting point in Z] [lc=1; s=chamfer/rounding (-/+)]. [//].
Parameter descriptions: [//]beginning [pn=n; s=parameter text (up to 16 characters) ] [//]end pn: n: Parameter designations (la, lb,.) Conversion number for units of measurement 0: Non-dimensional 1: "mm" or "inches" 2: "mm/rev" or "inch/rev" 3: "mm/min" or "inch/min" 4: "m/min" or "feet/min" 5: Rev/min 6: Degrees () 7: "m" or "inch"

6.30 M Functions

With M functions, you can control the program run and program switching functions for the machine (machine commands). Entering M functions Select "M function."
Enter the number of the M function. Define the parameters, if applicable.
M commands for program-run control M00 Program stop interrupts execution of a DIN program. Program run is continued after Cycle START has been pressed. M01 Optional stop: In "Program run" mode, you can use Continuous run to determine whether cycle programs or DIN programs are to be interrupted at an M01 command. If this function is disabled, MANUALplus interrupts execution of the program when M01 is reached and continues program run after Cycle START has been pressed. M30 End of program indicates the end of a program or subprogram. (M30 does not need to be programmed.) If you press "Cycle START" after M30, program execution is repeated from the start of the program. M99 End of program with return jump to start of program or to the defined block number and restart. MANUALplus restarts program execution from: The start of program if no "next block NS" is defined, or From the block number NS if a "next block NS" is defined. M417 deactivates protection zone monitoring. M418 activates protection zone monitoring. Note on using M99: All modal functions (feed rate, spindle speed, tool number, etc.) which are effective at the end of program remain in effect when the program is restarted. You should therefore reprogram the modal functions at the start of program or at the startup block.

8.2 Parameters

Current parameters
Current parameters "Setup (menu) [1]" menu item Workpiece zero point [1]Main spindle [1] Distance between "Machine zero point and workpiece zero point" (usually determined with "Set axis values"). Zero point coordinate X [mm] Zero point coordinate Z [mm] Tool change point [2] Distance between "Machine zero point and tool change point" (usually determined with "Set tool change point"). Tool change point X coordinate [mm] Tool change point Z coordinate [mm] Zero point shift, C axis [3] Tool monitoring [4] Zero point shift, C axis [] Activate/deactivate tool life monitoring Tool life switch 0: Off 1: On Additive compensation [5] 16 compensation value setsyou can also define this parameter with "Set additive compensation." Compensation 901 in X Compensation 901 in Z Compensation 902 in X Compensation 902 in Z. "Machine parameters [2]" menu item Feed rates [1]Manual control [1] Rapid traverse contouring speed for manual control Feed rate contouring speed for manual control (usually set with "Set T, S, F") Feed per revolution for manual control Feed rate for rapid traverse in X Feed-rate for rapid traverse in Z
Feed rates [1]Automatic mode [2]
Current parameters Speeds [2] For spindle 1 (main spindle) and spindle 2 (driven tool): Zero point shift (M19) [] The parameter determines the offset in position between the spindle reference point and the reference point of the angle encoder (rotary encoder). After receiving the reference pulse from the rotary encoder, the current actual position is overwritten by the parameter value. Number of revolutions for chip breaking Number of additional spindle revolutions for disengaging the tool during spindle stop. M5/M19 Angle (usually set with "Set T, S, F"). Speed value VConstant (G96) (usually set with "Set T, S, F"). Speed value NConstant (G97) (usually set with "Set T, S, F"). Speed limit (G26) (usually set with "Set T, S, F"). "NC switches [3]" menu item Display type [1] The data is displayed in the "Actual value display" fields (machine window). Actual display typethe numbers have the following meaning: 0: Actual value 1: Following error 2: Distance of traverse 3: Tool tipreferenced to machine zero point 4: Slide position 5: Distance between reference cams / reference pulse 6: Nominal position 7: Difference between tool tip / slide position 8: Nominal IPO position Tool measurement type [2] This parameter defines how to determine the tool set-up dimensions in setup mode. Type (of tool measurement): 0: Touch-off 1: Touch probe 2: Optical gauge Measuring feed: Feed rate for approaching the touch probe Measuring range: Measuring range: The tool stops when it has traversed to the maximum measuring range without reaching the touch probe.
Current parameters Settings [3] Set the system to "metric mode" or "inch mode" and define the behavior for searching the start block. Changes do not take effect until the control is restarted. Output to printernon-functional Metric/Inch 0: Metric 1: Inch Start block search 0: Off 1: On (Note: The system must be prepared for the start block function.) "PLC parameters [4]" menu item "Graphics parameters [5]" menu item Standard window size [1] These parameters define the display area for the graphic simulation of DIN programs. MANUALplus accounts for the height and width of the screen and may even enlarge the window size in the vertical or horizontal direction. Minimum X coordinatesmallest X coordinate displayed Minimum Z coordinatesmallest Z coordinate displayed Delta Xvertical expansion Delta Zhorizontal expansion Standard workpiece blank [2] These parameters define the standard workpiece blank and are used for calculating the "unrolled lateral surface." Outside diameter: The "unrolled lateral surface" is calculated from the diameter. Length of blank: Horizontal dimension of "unrolled lateral surface." Right edge of blank part: Position of the unrolled lateral surface relative to the coordinate origin. If you enter a positive value, the "right blank edge" is located to the right of the coordinate origin. Inside diameternon-functional "Machining [6]" menu item Safety clearances [1] The following safety clearances are used in several cycles and during execution of specific DIN cycles (see cycle definitions): External safety clearance [SAR] Internal safety clearance [SIR] External on machined part [SAT] Internal on machined part [SIT] The PLC parameters are described in your machine manual.

Defining a rounding To define the rounding, enter "Rounding radius B." MANUALplus inserts the rounding in the existing ICP contour and draws the "perfected" contour. If the contour contains further corners, MANUALplus offers the next contour corner for selection (see figure to the bottom right).
The ICP contour has been completely defined. Back concludes ICP programming and Input finished concludes the ICP cycle.
Checking the ICP cutting cycle After the cutting operation has been completed, it is checked with the Simulation function. The simulation function is called with the Graphics soft key. You can then transfer the cycle to the cycle program with the Save or Overwrite.
ICP finishing The ICP contour "777" ("Matrix") is also used for the finishing cycle.
Checking the ICP finishing cycle With the graphic simulation function, you can check the execution of the ICP finishing cycle (Graphics soft key). You can then transfer the cycle to the cycle program with the Save or Overwrite. MANUALplus finishes the contour in the defined "contour direction" (see figure to the bottom right).
Cycle program "ICP example Matrix" Besides the ICP cycles, the created cycle program also includes the positioning cycles for tool change (see figure to the right). Functions of the cycles: N1: Remove the material (roughing) N2: Position the tool for tool change N3: Finish-machine the workpiece N4: Position the tool for removing the workpiece
This example illustrates the use of an ICP recessing cycle. The individual working steps for machining the ICP contour and integrating the contour into ICP cycles are based on the workpiece drawing. In the process described below, you create an ICP contour description and a cycle program for parts production. The machining operation is performed with the "ICP recessing radial" cycle. Required tool Recessing tool: Position T4 WO = 1 Tool orientation R = 0.2 Tool radius K = 5 Cutting width Sequence of working steps
Clamp a workpiece blank (diameter 60 mm, length 65 mm). Machine setup Define the workpiece zero point Measure the tool dimensions Switch to "Teach-in" mode. Enter the positioning cycles for tool change. Call the "ICP cut radial" cycle. ICP contour programming. Integrate the ICP contour in the recessing, finishing cycle.
9.4 ICP Example "Recessing Cycle"
ICP recessing radial The procedure presupposes that the machine has been set up and the control is in "Teach-in" mode. The allowances for pre-cutting are programmed in the ICP recessing cycle. The cutting width is not entered. MANUALplus automatically calculates the proportioning of cuts such that the infeed per pass is < 80% of the cutting width defined in the tool data (see figure to the top right). After defining the cycle parameters, press Edit ICP to call the ICP programming function. You can now switch to the input mode by pressing Add element. First you enter the "rough contour." Then you use the "superimposition" function to define the roundings.

Diagnosis. 455 Dialog texts for subprograms. 407 DIN commandsoverview. 280 DIN cycle (cycle programming). 239 DIN example Milling. 519 Threaded stud. 516 DIN macros. 83, 278 DIN programs. 278 Direction of rotation (tool parameters). 426 Display type (actual-position display). 433 Displaying and editing parameters. 431 Distance-to-go display. 46 Drilling Cycle programming Deep-hole drilling. 193 Drilling. 191 Tapping. 195 DIN programming Deep-hole drilling cycle G74. 355 Simple drilling cycle G71. 354 Tapping G36. 357 Drilling cycles Cycle programming. 190 DIN programming. 354 Drilling pattern Cycle programming Pattern circular, face. 230 Pattern circular, lateral surface. 234 Pattern linear, face. 228 Pattern linear, lateral surface. 232 DIN programming Circular pattern, face G745. 385 Circular pattern, lateral surface G746. 389 Linear pattern, face G743. 383 Linear pattern, lateral surface G744. 387 Drilling tools. 423 Driven tool. 426
Editing. 39 Editing address parameters. 283 Element position of undercuts (ICP). 263 End milling cutter. 413 End of cycle G80. 310 End point of ICP contour. 243 Equidistant line (MCRC). 29 Equidistant line (TRC). 28 Error display. 36 Error messages. 36 Index
Ethernet. 442 Examples Cycle program, creating . 461 DIN example Milling. 519 Threaded stud. 516 ICP example Matrix. 483 Milling. 507 Recessing cycle. 495 Threaded stud. 470 Machine, setting up.. 459 Selecting a cycle program. 460 Extension. 39
F display. 47 Face (ICP contour elements). 268 Face milling (cycle programming). 211 Face view (simulation). 70 Facing. 419 Facing tools. 419 Feed per minute Cycle mode. 48 DIN cycle G94. 298 Feed per revolution for manual control (parameter). 432 Feed per revolution, driven tools. 47 Feed rate Cycle mode. 48 DIN programming Constant feed rate G94. 298 Feed per revolution G95/G195. 298 Feed per tooth G193. 298 Feed rate, programming. 392 Feed rate contouring speed for manual control (parameter). 432 Feed rate reduction for drilling Cycle programming Deep-hole drilling. 194 Drilling cycle. 191 DIN programming Deep-hole drilling cycle G74. 355 Simple drilling cycle G71. 354
Figure definition Face Full circle G304. 368 Polygon G307. 370 Rectangle G305. 369 Lateral surface Full circle G314. 380 Polygon G317. 382 Rectangle G315. 381 Figure milling cycle, face G793. 364 Figure milling cycle, lateral surface G794. 377 Figure milling, axial (cycle programming). 204 Figure milling, radial (cycle programming). 216 Files, transferring. 446 Fine-finishing tools. 412 Finishing DIN cycle, contour finishing G89. 318 Finishing cycle, longitudinal/transverse. 105 Finishing tools. 412 Form elements (ICP) Form elements, entering. 263 Fundamentals. 242 Superimposing form elements. 259 Function selection. 33

G793 Contour and figure milling cycle, face. 364 G794 Contour and figure milling cycle, lateral surface. 377 G797 Area milling, face. 366 G798 Helical-slot milling. 379 G799 Thread milling, axial. 358 G80 End of cycle. 310 G81 Longitudinal roughing. 319 G811 Simple recess-turning cycle, longitudinal. 332 G815 Recess-turning cycle, longitudinal. 333 G817 Longitudinal contour roughing. 311 G818 Longitudinal contour roughing. 311 G819 Longitudinal contour roughing with recessing. 313 G82 Transverse roughing. 320 G821 Simple recess-turning cycle, transverse. 332 G825 Recess-turning cycle, transverse. 333 G827 Transverse contour roughing. 314 G828 Transverse contour roughing. 314 G829 Transverse contour roughing with recessing. 316 G83 Simple contour repeat cycle. 321 G836 Contour-parallel roughing. 317 G85 undercut cycle. 345 G851 Undercut DIN 509 E. 347 G852 Undercut DIN 509 F. 348 G853 Undercut DIN 76. 349 G856 Undercut type U. 350 G857 Undercut type H. 351 G858 Undercut type K. 352 G859 Parting cycle. 353 G86 Simple recessing cycle. 330 G861 Contour recessing axial. 324 G862 Contour recessing radial. 324 G863 Axial contour recessing cycle, finishing. 326 G864 Radial contour recessing cycle, finishing. 326 G865 Simple axial recessing cycle. 328 G866 Simple radial recessing cycle. 328 G867 Axial recessing, finishing. 329 G868 Radial recessing, finishing. 329 G87 Line with radius. 322 G88 Line with chamfer. 323 G89 Contour finishing. 318 G9 Precision stop. 391 G94 Constant feed rate. 298 G95 Feed per revolution. 298 G96 Constant cutting speed. 299 G97 Spindle speed. 299 List operations. 34 Local variables (DIN programming). 397 Log file. 455 Logoff. 454 Logon. 454
M functions DIN programming. 408 Fundamentals of cycle programming. 82 M cycle, entering (cycle programming). 97 M19 (spindle positioning, cycle programming). 97 M00 Program STOP. 408 Machine commands. 409 Machine data Cycle programming. 83 DIN programming. 286 Display configuration. 439 Input and display. 46 Machine dimensions. 435 Machine operating panel. 24 Machine reference points. 27 Machine setup. 50 Machine variables. 286 Machine zero point. 27 Machine, setting up (example). 459 Machining times. 74 Magnify / Reduce ICP contour graphics. 247 Simulation. 73 Marking (program transfer). 446 Marking for block functions (DIN programming). 285 Mathematical functions. 396 Maximum speed. 47 Cycle mode. 46 Display. 46 Speed limitation G26/G126. 297 Menu. 39 Menu key. 39 Menu selection. 33 Menu structure (DIN programming). 286 Metric. 434 Milling cutter radius compensation DIN programming. 300 Fundamentals. 29 Milling cycles. 201

Switch-on. 43 System error. 37 System service. 455 System start. 43
T display. 47 Tangential transition. 245 Tapered thread Cycle programming. 168 DIN cycle G353. 343 Tapping tools. 424 Teach-in. 62 Terms used. 39 Thread Cycle programming API thread. 170 API thread, recutting. 178 Tapered thread. 168 Tapered thread, recutting. 176 Tapping, axial/radial. 195 Thread and undercut cycles. 162 Thread chamfer. 180 Thread cycle. 165 Thread cycle, expanded. 166 Thread depth. 163 Thread milling, axial. 197 Thread position. 162 Thread recutting. 172 Thread recutting, expanded. 174 Thread run-in / thread run-out. 163 DIN programming API thread G352. 342 Extended longitudinal multi-start thread G351. 341 Metric ISO thread G35. 339 Simple longitudinal single-start thread G350. 340 Single path G33. 338 Tapered thread G353. 343 Tapping G36. 357 Thread cycle, simple G32. 337 Thread milling, axial G799. 358 Universal thread cycle G31. 335 Thread angle (thread cycle). 163 Thread cutter. 413
Thread undercut DIN 76 Cycle programming Thread undercut DIN 76. 180 DIN programming Undercut contour G25. 344 Undercut cycle G85. 345 With cylinder machining G853. 349 ICP programming Thread undercut DIN 76. 265 Thread-cutting tools. 422 Time calculation (simulation). 74 Time calculationparameter. 438 Tool change point Approach the tool change position (cycle programming). 90 Defining the tool change position. 52 Tool change point G14. 291 Tool edge compensation G148. 302 Tool life monitoring Fundamentals. 59 Tool data. 427 Tools Power-driven tools. 47 Reference point. 418 Supplementary parameters. 426 T display. 47 T number, entering in cycle mode. 46 Tool administration (tool management). 412 Tool call. 47 Tool compensation, entering. 58 Tool data. 418 Tool dimensions fundamentals. 28 Tool input menu. 418 Tool life management. 427 Tool life monitoring, working with.. 59 Tool list. 414 Tool organizationFundamentals. 414 Tool orientation. 418 Tool texts. 416 Tool types. 412 Tool, programming (DIN programming). 392 Tools in different quadrants. 48 Tool-tip and cutter radius compensation DIN programming. 300 Fundamentals. 28 Touch probe. 56 Touch-off. 54 Transfer. 441
Transfer values for subprograms. 407 Transferring parameters. 451 Transferring tool data. 452 Twist drill cutter. 413 Twist drills. 413
Wait for moment G204. 391 Warnings during simulation. 38 Wear compensation. 412 WHILE command (DIN programming). 402 WINDOW command (DIN programming). 394 WINDOWS networks. 442 Wire frame graphics (simulation). 68 Word functions (DIN programming). 283 Word length (serial data transfer). 445 Working with cycles. 80 Workpiece zero point. 27, 50 Workpiece-blank definition Cycle programming. 85 DIN programming. 288

Operating Instructions

MANUALplus 4110

Engraving Inscriptions

English (en) 8/2005
MANUALplus_4110_Gravieren_en.indd 1

12.08.2005 12:05:06

1 Engraving.... 1 1.1 Engraving Inscriptions.. 1 1.2 Parameters of the Subprogram Call... 3 1.3 Example: Engraving the Front Face.. 4 1.4 Example: Engraving the Lateral Surface.. 9 1.5 Character Set... 11

Engraving

HEIDENHAIN includes a set of NC subprograms with DataPilot for engraving inscriptions (large and small letters, numbers, and various special characters). The installation program transfers these NC subprograms together with the NC sample programs Grav_Sti and Grav_Man into the machine BEISPIEL. The names of the NC subprograms are listed in the Engraving Inscriptions operating instructions. The subprograms and sample programs for engraving are also saved in compressed format in the file Grav_4110.zip in the machine BEISPIEL in the NCPS directory. Copy this ZIP file to the NCPS directory of other DataPilot machines and unzip it if you want to engrave with other DataPilot machines as well. The compressed file with subprograms and sample programs for engraving is also on the DataPilot CDROM (path: JH\DP4110\ZIP\Grav_4110.zip).
1.1 Engraving Inscriptions
The C axis is used for engraving. You can adjust the size, orientation and position of the characters. As a default, the subprograms engrave the character strings on the front face: linear or polar on the lateral surface: linear

August 2005

Engraving characters strings
Program a character string according to the following scheme: Insert a milling tool Pre-position the milling tool to the beginning of the character string Call in sequence the subprograms with the characters to be engraved Retract the tool The characters are engraved starting at the current tool position. The reference point depends on whether the characters are in linear or polar alignment: Linear: The reference point is the bottom left corner of the character Polar: The reference point is the center of the bottom edge of the character
HEIDENHAIN MANUALplus 4110
1.2 Parameters of the Subprogram Call
Specify in the call parameters of the subprogram the details of the characters appearance. L: Name of the subprogram (See Character Set on page 11.) LA: Letter height in [mm] LB: Rotated angle of the letter in [] Linear front face: 0 = Vertical characters: the characters are aligned in sequence in positive XK direction Polar front face: LB has no function Lateral surface 0: Characters are engraved from CY to +CY Lateral surface 90: Characters are engraved from Z to +Z LC: Milling plane Front face: Z position, infeed depth during milling Lateral surface: X diameter, infeed depth during milling LD: Retraction plane Front face: Z position retracted to for positioning Lateral surface: X diameter retracted to for positioning LE: Engraving on the front face or lateral surface 0: Front face 1: Lateral surface LF: Linear or polar alignment (only relevant for the front face) 0: Characters are aligned linearly 1: Characters are bent upwards over the center of the coordinate cross 2: Characters are bent downwards under the center of the coordinate cross LH: Reference diameter Front face: Diameter over which the character string is engraved with polar alignment Lateral surface: Diameter for calculation of the unrolled lateral surface (G120) I: Separation factor the separation between the characters is calculated according to the following formula: LA / 6 * I If I is not entered, I=1 is used for calculation Q: Number of repetitions (can be used if the same character is to be engraved immediately following)
1.3 Example: Engraving the Front Face
The following sample program engraves character strings in various orientations and positions onto the front face.
Character string HEIDENHAIN
The character string is engraved in polar alignment, bent upwards, at Z = 10. Programming the character string: Position the tool to C=35 Parameters for subprogram call: Letter height: LA=15 mm Milling plane at Z=10 (LC=10) Retraction plane at Z=7 (LD=7) Engraving on the front face (LE=0) Polar character string bent upwards (LF=1) Diameter over which the character string is engraved (LH): Bottom edge of character=85 Separation factor (I) is not programmed; the default separation is valid
Example: Program and block structure. N5 N6 N7 N8 N9 G0 X60 Z5 G0 Z-5 G110 C-35 L"H" LA15 LC-10 LD-7 LE0 LF1 LH85 L"E" LA15 LC-10 LD-7 LE0 LF1 LH85
N10 L"I" LA15 LC-10 LD-7 LE0 LF1 LH85 N11 L"D" LA15 LC-10 LD-7 LE0 LF1 LH85 N12 L"E" LA15 LC-10 LD-7 LE0 LF1 LH85 N13 L"N" LA15 LC-10 LD-7 LE0 LF1 LH85 N14 L"H" LA15 LC-10 LD-7 LE0 LF1 LH85 N15 L"A" LA15 LC-10 LD-7 LE0 LF1 LH85 N16 L"I" LA15 LC-10 LD-7 LE0 LF1 LH85 N17 L"N" LA15 LC-10 LD-7 LE0 LF1 LH85 N.

Character string MANUALplus 4110 The character string is engraved in polar alignment, bent downwards, at Z = 10. Programming the character string: Position the tool to C=4 Parameters for subprogram call: Letter height: LA=15 mm Milling plane at Z=10 (LC=10) Retraction plane at Z=7 (LD=7) Engraving on the front face (LE=0) Polar character string bent downwards (LF=2) Diameter over which the character string is engraved (LH): Bottom edge of character=115 Separation factor: 1.3 * default separation (I=1.3)
Example: Program and block structure. N19 G110 C4 N20 L"M" LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N21 L"A" LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N22 L"N" LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N23 L"U" LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N24 L"A" LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N25 L"L" LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N26 L"KP" LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N27 L"KL" LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N28 L"KU" LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N29 L"KS" V1 LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N30 L"BLANK" V1 LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N31 L"4" V1 LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N32 L"1" V1 LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N33 L"1" V1 LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N34 L"0" V1 LA15 LC-10 LD-7 LE0 LF2 LH115 I1.3 N.
Character string Traunreut The character string is engraved linearly. Programming the character string: Position the tool to XK = 25, YK = 15 Parameters for subprogram call: Letter height: LA=10 mm Angle: LB=180 Milling depth to Z=0 (LC=0) Retraction plane to Z=3 (LD=3) Engraving on the front face (LE=0) Linear character string (LF=0) Separation factor: 1.4 * default separation (I=1.4)
Example: Program and block structure. N36 G0 Z5 N37 G100 XK25 YK15 N38 L"T" LA10 LB180 LC0 LD3 LE0 LF0 I1.4 N39 L"KR" LA10 LB180 LC0 LD3 LE0 LF0 I1.4 N40 L"KA" LA10 LB180 LC0 LD3 LE0 LF0 I1.4 N41 L"KU" LA10 LB180 LC0 LD3 LE0 LF0 I1.4 N42 L"KN" LA10 LB180 LC0 LD3 LE0 LF0 I1.4 N43 L"KR" LA10 LB180 LC0 LD3 LE0 LF0 I1.4 N44 L"KE" LA10 LB180 LC0 LD3 LE0 LF0 I1.4 N45 L"KU" LA10 LB180 LC0 LD3 LE0 LF0 I1.4 N46 L"KT" LA10 LB180 LC0 LD3 LE0 LF0 I1.4 N.

Character string Zyklen- und (Cycles and) The character string is engraved linearly at an angle. Programming the character string: Position the tool to XK = 39, YK = 4 Parameters for subprogram call: Letter height: LA=6 mm Angle: LB=215 Milling depth to Z=0 (LC=0) Retraction plane to Z=3 (LD=3) Engraving on the front face (LE=0) Linear character string (LF=0) Separation factor: 1.6 * default separation (I=1.6)
Example: Program and block structure. N48 G100 XK39 YK-4 N49 L"Z" LA6 LB215 LC0 LD3 LE0 LF0 I1.6 N50 L"KY" LA6 LB215 LC0 LD3 LE0 LF0 I1.6 N51 L"KK" LA6 LB215 LC0 LD3 LE0 LF0 I1.6 N52 L"KL" LA6 LB215 LC0 LD3 LE0 LF0 I1.6 N53 L"KE" LA6 LB215 LC0 LD3 LE0 LF0 I1.6 N54 L"KN" LA6 LB215 LC0 LD3 LE0 LF0 I1.6 N55 L"MINUS" LA6 LB215 LC0 LD3 LE0 LF0 I1.6 N56 L"BLANK" LA6 LB215 LC0 LD3 LE0 LF0 I1.6 N57 L"KU" LA6 LB215 LC0 LD3 LE0 LF0 I1.6 N58 L"KN" LA6 LB215 LC0 LD3 LE0 LF0 I1.6 N59 L"KD" LA6 LB215 LC0 LD3 LE0 LF0 I1.6 N.
Character string DIN-Programme (DIN programs) The character string is engraved linearly at an angle. Programming the character string: Position the tool to XK = 0, YK = 30 Parameters for subprogram call: Letter height: LA=5 mm Angle: LB=145 Milling depth to Z=0 (LC=0) Retraction plane to Z=3 (LD=3) Engraving on the front face (LE=0) Linear character string (LF=0) Separation factor: 1.6 * default separation (I=1.6)
Example: Program and block structure. N61 G100 XK0 YK-30 N62 L"D" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N63 L"I" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N64 L"N" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N65 L"MINUS" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N66 L"P" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N67 L"KR" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N68 L"KO" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N69 L"KG" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N70 L"KR" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N71 L"KA" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N72 L"KM" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N73 L"KM" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N74 L"KE" LA5 LB145 LC0 LD3 LE0 LF0 I1.6 N.
1.4 Example: Engraving the Lateral Surface Character string Steuerungen

The character string Steuerungen (Controls) is engraved from CY to +CY. Programming the character string: Position the tool to Z=110 and C=45 Parameters for subprogram call: Letter height: LA=12 mm Angle: LB=0 (from CY to +CY) Milling depth to diameter 120 (LC=120) Retraction depth to diameter 126 (LC=126) Engraving on the lateral surface (LE=1) Linear character string (LF=0) Diameter (for G120): LH=120 Separation factor: 1.3 * default separation (I=1.3)
Example: Program and block structure. N5 N6 N7 N8 N9 G110 C-45 G0 X126 G0 Z-110 L"S" LA12 LB0 LC120 LD126 LE1 LF0 LH120 I1.3 L"KT" LA12 LB0 LC120 LD126 LE1 LF0 LH120 I1.3
N10 L"KE" LA12 LB0 LC120 LD126 LE1 LF0 LH120 I1.3 N11 L"KU" LA12 LB0 LC120 LD126 LE1 LF0 LH120 I1.3 N12 L"KE" LA12 LB0 LC120 LD126 LE1 LF0 LH120 I1.3 N13 L"KR" LA12 LB0 LC120 LD126 LE1 LF0 LH120 I1.3 N14 L"KU" LA12 LB0 LC120 LD126 LE1 LF0 LH120 I1.3 N15 L"KN" LA12 LB0 LC120 LD126 LE1 LF0 LH120 I1.3 N16 L"KG" LA12 LB0 LC120 LD126 LE1 LF0 LH120 I1.3 N17 L"KE" LA12 LB0 LC120 LD126 LE1 LF0 LH120 I1.3 N18 L"KN" LA12 LB0 LC120 LD126 LE1 LF0 LH120 I1.3 N19 L"BLANK" LA12 LB0 LC120 LD126 LE1 LF0 LH120 I1.3 N.
Character string der Extra-Klasse The character string der Extra-Klasse (in a class of their own) is engraved from Z to +Z. Programming the character string: Position the tool to Z=110 and C=45 Parameters for subprogram call: Letter height: LA=12 mm Angle: LB=90 (from Z to +Z) Milling depth to diameter 120 (LC=120) Retraction depth to diameter 126 (LC=126) Engraving on the lateral surface (LE=1) Linear character string (LF=0) Diameter (for G120): LH=120 Separation factor (I) is not programmed; the default separation is valid
Example: Program and block structure. N21 G110 C45 N22 G0 Z-110 N23 L"KD" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N24 L"KE" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N25 L"KR" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N26 L"BLANK" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N27 L"E" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N28 L"KX" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N29 L"KT" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N30 L"KR" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N31 L"KA" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N32 L"MINUS" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N33 L"K" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N34 L"KL" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N35 L"KA" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N36 L"KS" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N37 L"KS" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N38 L"KE" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N39 L"BLANK" LA12 LB90 LC120 LD126 LE1 LF0 LH120 N.