Machining small contour steps with M97

Application

With M97 you can produce contour steps that are smaller than the tool radius. The control does not damage the contour and does not issue an error message.

 
Tip

HEIDENHAIN recommends using the more powerful function M120 (#21 / #4-02-1) instead of M97.

After activating M120 you can produce complete contours without error messages. M120 also considers circular paths.

Description of function

Effect

M97 is in effect blockwise and takes effect at the end of the block.

Application example

Contour step without M97

Contour step with M97

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 8 Z S5000

; Insert the tool with diameter 16

* - ...

21 L X+0 Y+30 RL

22 L X+10 M97

; Machine the contour step using the path intersection

23 L Y+25

24 L X+50 M97

; Machine the contour step using the path intersection

25 L Y+23

26 L X+100

For radius-compensated contour steps, the control uses M97 to determine a path intersection that is in the extension of the tool path. The control extends the tool path each time by the tool radius. This means that the smaller the counter step is and the larger the tool radius, the greater the contour extension is. The control moves the tool beyond the path intersection and thus avoids damage to the contour.

Without M97 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.

Notes

  • Program M97 only for outside corners.
  • For further machining operations, please note that shifting the contour corner results in more residual material. You may then need to rework the contour step with a smaller tool.