Example: Simultaneous turning
The following NC program uses Cycle 882 SIMULTANEOUS ROUGHING FOR TURNING and Cycle 883 TURNING SIMULTANEOUS FINISHING.
Program sequence
- Call the tool (e.g., TURN_ROUGH)
- Activate turning mode
- Pre-position
- Select the contours by using SEL CONTOUR
- Cycle 882 SIMULTANEOUS ROUGHING FOR TURNING
- Call the cycle
- Call the tool (e.g., TURN_FINISH)
- Activate turning mode
- Cycle 883 TURNING SIMULTANEOUS FINISHING
- Call the cycle
- End of program
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.
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 1341941_1 MM | |||
1 BLK FORM ROTATION Z DIM_D FILE "1341941_blank.H" | |||
2 FUNCTION MODE TURN | ; Activate turning mode | ||
3 TOOL CALL "TURN_ROUGH" | ; Tool call | ||
4 CYCL DEF 800 ADJUST XZ SYSTEM ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
5 FUNCTION TURNDATA SPIN VCONST: ON VC:400 SMAX800 | ; Constant surface speed | ||
6 M145 | ; Reset the tool offset | ||
7 FUNCTION TCPM F TCP AXIS POS PATHCTRL AXIS REFPNT TIP-CENTER | ; Activate TCPM | ||
8 L X+120 Y+0 R0 FMAX | ; Pre-position | ||
9 L Z+20 R0 FMAX M303 | |||
10 FUNCTION TURNDATA BLANK "1341941_blank.H" | ; Workpiece blank update | ||
11 SEL CONTOUR "1341941_finish.h" | ; Define the contour | ||
12 CYCL DEF 882 SIMULTANEOUS ROUGHING FOR TURNING ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
13 CYCL CALL | ; Cycle call | ||
14 M305 | |||
15 TOOL CALL "TURN_FINISH" | ; Tool call | ||
16 CYCL DEF 800 ADJUST XZ SYSTEM ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
17 FUNCTION TURNDATA SPIN VCONST: ON VC:400 SMAX800 | ; Constant surface speed | ||
18 M145 | ; Reset the tool offset | ||
19 FUNCTION TCPM F TCP AXIS POS PATHCTRL AXIS REFPNT TIP-CENTER | ; Activate TCPM | ||
20 L X+120 Y+0 R0 FMAX | |||
21 L Z+20 R0 FMAX M303 | |||
22 CYCL DEF 883 TURNING SIMULTANEOUS FINISHING ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
23 CYCL CALL | ; Cycle call | ||
24 M305 | |||
25 FUNCTION TURNDATA BLANK OFF | ; Deactivate workpiece blank update | ||
26 CYCL DEF 801 RESET ROTARY COORDINATE SYSTEM | |||
27 FUNCTION MODE MILL | ; Activate milling mode | ||
28 TOOL CALL 0 Z | |||
29 PLANE RESET TURN FMAX | |||
30 M30 | ; End of program run | ||
31 END PGM 1341941_1 MM |
NC program 1341941_blank.h
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.
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 1341941_BLANK MM |
1 L X+0 Z+0.4 |
2 L X+80 |
3 L Z-139.6 |
4 L X+0 |
5 L Z+0.4 |
6 END PGM 1341941_BLANK MM |
NC program 1341941_finish.h
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.
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 1341941_FINISH MM |
1 L X+0 Z+0 RR |
2 CR Z-65.136 X+15 R+33 DR+ |
3 RND R2 |
4 L Z-86 |
5 RND R10 |
6 L X+78 Z-95 |
7 RND R5 |
8 L Z-100 |
9 END PGM 1341941_FINISH MM |