Example: polar straight lines

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

0 BEGIN PGM LINEARPO MM

1 BLK FORM 0.1 Z X+0 Y+0 Z-20

2 BLK FORM 0.2 X+100 Y+100 Z+0

; Workpiece blank definition

3 TOOL CALL 1 Z S4000

; Tool call

4 CC X+50 Y+50

; Define the datum for polar coordinates

5 L Z+250 R0 FMAX

; Retract the tool

6 LP PR+60 PA+180 R0 FMAX

; Pre-position the tool

7 L Z-5 R0 F1000 M3

; Move to working depth

8 APPR PLCT PR+45 PA+180 R5 RL F250

; Approach the contour at point 1 on a circular path with tangential connection

9 LP PA+120

; Move to point 2

10 LP PA+60

; Move to point 3

11 LP PA+0

; Move to point 4

12 LP PA-60

; Move to point 5

13 LP PA-120

; Move to point 6

14 LP PA+180

; Move to point 1

15 DEP PLCT PR+60 PA+180 R5 F1000

; Depart contour on a circular path with tangential connection

16 L Z+250 R0 FMAX M2

; Retract the tool, end of program run

17 END PGM LINEARPO MM