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.

Output formats of NC programs

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.

 
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.

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

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