Permitting positive tool oversizes with M107 (#9 / #4-01-1)
Application
With M107 (#9 / #4-01-1), the control does not interrupt machining in case a positive delta value is measured. The function is in effect with active 3D tool compensation and for LN straight lines.
3D tool compensation (#9 / #4-01-1)
With M107 you can, for example, use the same tool in a CAM program for pre-finishing with oversize and then later for final finishing without oversize.
Requirement
- Software option Adv. Function Set 2 (#9 / #4-01-1)
Description of function
Effect
M107 takes effect at the start of the block.
In order to reset M107, program M108.
Application 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.
11 TOOL CALL 1 Z S5000 DR2:+0.3 | ; Insert a tool with a positive delta value |
12 M107 | ; Permit positive delta values |
The control exchanges the tools and activates M107 in the next NC block. That way the control permits positive delta values and does not issue an error message, such as during pre-finishing.
Without M107 the control issues an error message upon positive delta values.
Notes
- Before actual machining, check in the NC program to make sure that the positive delta values of the tool will not result in contour damages or collisions.
- With peripheral milling the control issues an error message in the following case:
3D tool compensation during peripheral milling (#9 / #4-01-1)
- With face milling the control issues an error message in the following cases:
Definition
Abbreviation | Definition |
---|---|
R | Tool radius |
R2 | Corner radius |
DR | Delta value of the tool radius |
DR2 | Delta value of the corner radius |
TAB | Value refers to the tool management |
PROG | Value refers to the NC program, meaning from the tool call or from compensation tables |