Traversing in the machine coordinate system M-CS with M91

Application

You can use M91 to program machine-based positions, such as for moving to safe positions. The coordinates of positioning blocks with M91 are in effect in the machine coordinate system M-CS.

Machine coordinate system M-CS

Description of function

Effect

M91 is in effect blockwise and takes effect at the start of the block.

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 LBL "SAFE"

12 L Z+250 R0 FMAX M91

; Approach a safe position in the tool axis

13 L X-200 Y+200 R0 FMAX M91

; Approach a safe position in the plane

14 LBL 0

Here M91 is in a subprogram in which the control moves the tool to a safe position by first moving in the tool axis and then in the plane.

Since the coordinates refer to the machine datum, the tool always moves to the same position. That way, regardless of the workpiece preset, the subprogram can be repeatedly called in the NC program, for example, before tilting the rotary axes.

Without M91 the control references the programmed coordinates to the workpiece preset.

Presets in the machine

 
Machine

The coordinates for a safe position depend on the machine!

The machine manufacturer defines the position of the machine datum.

Notes

  • If you program incremental coordinates in an NC block with the miscellaneous function M91, then these coordinates are relative to the last position programmed with M91. For the first position programmed with M91, the incremental coordinates are relative to the current tool position.
  • The control considers any active tool radius compensation when positioning with M91.
  • Tool radius compensation

  • The control uses the tool carrier reference point when positioning in the tool axis.
  • Presets in the machine

  • The following position displays refer to the machine coordinate system M-CS and show the values defined with M91:
    • Nominal reference position (RFNOML)
    • Actual reference position (RFACTL)
  • Position displays

  • In the Editor operating mode, use the Workpiece position window to apply the current workpiece preset to the simulation. In this constellation you can simulate traverse movements with M91.
  • The Visualization options column

  • In the machine parameter refPosition (no. 400403) the machine manufacturer defines the position of the machine datum.