Pre-calculating a radius-compensated contour with M120 (#21 / #4-02-1)
Application
With M120 the control pre-calculates a radius-compensated contour. This way the control can produce contours that are smaller than the tool radius without damaging the contour or issuing an error message.
Requirement
- Software option Adv. Function Set 3 (#21 / #4-02-1)
Description of function
Effect
M120 takes effect at the start of the block and remains active beyond the milling cycles.
M120 can be reset by the following NC functions:
- M120 LA0
- M120 without LA
- Radius compensation R0
- Departure functions (e.g., DEP LT)
Application example
Contour step with M97 | Contour step with M120 |
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.
11 TOOL CALL 8 Z S5000 | ; Insert the tool with diameter 16 |
* - ... | |
21 L X+0 Y+30 RL M120 LA2 | ; Activate contour pre-calculation and move in the working plane |
22 L X+10 | |
23 L Y+25 | |
24 L X+50 | |
25 L Y+23 | |
26 L X+100 |
With M120 LA2 in NC block 21, the control checks the radius-compensated contour for undercuts. In this example the control calculates the tool path starting from the current NC block for two NC blocks at a time. Then the control uses radius compensation while positioning the tool to the first contour point.
When machining the contour, the control extends the tool path in each case so that the tool does not damage the contour.
Without M120 the tool would move on a transitional arc around the outside corners and damage the contour. At such locations the control interrupts machining with the Tool radius too large error message.
Input
If you define M120, the control continues the dialog and prompts you for the number of LA NC blocks to be calculated in advance (up to 99).
Notes
- Use the Simulation mode to test the NC program before execution
- Slowly prove-out the NC program
- For further machining operations, please note that residual material remains in the contour corners. You may then need to rework the contour step with a smaller tool.
- If you always program M120 in the same NC block as the radius compensation you can achieve consistent and clearly structured programs.
- If radius compensation is active and you execute the following functions, the control aborts program run and displays an error message:
- PLANE functions (#8 / #1-01-1)
- M128 (#9 / #4-01-1)
- FUNCTION TCPM (#9 / #4-01-1)
- CALL PGM
- Cycle 12 PGM CALL
- Cycle 32 TOLERANCE
- Cycle 19 WORKING PLANE
- Tip
You can still execute NC programs from earlier controls that contain Cycle 19 WORKING PLANE.
Example
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 "M120" MM | |
1 BLK FORM 0.1 Z X+0 Y+0 Z-10 | |
2 BLK FORM 0.2 X+110 Y+80 Z+0 | ; Workpiece blank definition |
3 TOOL CALL 6 Z S1000 F1000 | ; Insert the tool with diameter 12 |
4 L X-5 Y+26 R0 FMAX M3 | ; Move in the working plane |
5 L Z-5 R0 FMAX | ; Infeed in the tool axis |
6 L X+0 Y+20 RL F AUTO M120 LA5 | ; Activate contour pre-calculation and move to the first contour point |
7 L X+40 Y+30 | |
8 CR X+47 Y+31 R-5 DR+ | |
9 L X+80 Y+50 | |
10 L X+80 Y+45 | |
11 L X+110 Y+45 | ; Move to the last contour point |
12 L Z+100 R0 FMAX M120 | ; Retract the tool and reset M120 |
13 M30 | ; End of program run |
14 END PGM "M120" MM |
Definition
Abbreviation | Definition |
---|---|
LA (look ahead) | Number of look-ahead blocks |