Mirroring with TRANS MIRROR
Application
Use the TRANS MIRROR function to mirror contours or positions about one or more axes.
The TRANS MIRROR RESET function allows you to reset mirroring.
Related topics
- Cycle 8 MIRRORING
Description of function
Mirroring is a modal function that is effective as soon as it has been defined in the NC program.
The control mirrors contours or positions about the active workpiece datum. If the datum is outside the contour, the control will also mirror the distance to the datum.
If you mirror only one axis, the machining direction of the tool is reversed. The rotational direction defined in a cycle will remain unchanged (e.g., if defined within one of the OCM cycles (#167 / #1-02-1)).
Depending on the selected AXIS axis values, the control will mirror the following working planes:
- X: The control mirrors the YZ working plane
- Y: The control mirrors the ZX working plane
- Z: The control mirrors the XY working plane
Designation of the axes of milling machines
You can select up to three axis values.
If mirroring is active, the control displays it on the TRANS tab of the Status workspace.
Input
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 TRANS MIRROR AXIS X | ; Mirror X coordinates about the Y axis |
To navigate to this function:
Insert NC function All functions Special functions Functions Coordinate transformations TRANS TRANS MIRROR
The NC function includes the following syntax elements:
Syntax element | Meaning |
---|---|
TRANS MIRROR | Syntax initiator for mirroring |
AXIS or RESET | Enter mirroring of axis values or reset mirroring |
X, Y or Z | Axis values to be mirrored Only if AXIS has been selected |
Notes
- This function can be used only in the FUNCTION MODE MILL machining mode.
- If you execute mirroring with TRANS MIRROR or Cycle 8 MIRRORING, then the control overwrites the current mirroring.
Notes on using these functions in conjunction with tilting functions
- Program only the recommended transformations in the respective reference system
- Use tilting functions with spatial angles instead of with axis angles
- Use the Simulation mode to test the NC program
The type of tilting function has the following effects on the result:
- If you tilt using spatial angles (PLANE functions except for PLANE AXIAL or Cycle 19), previously programmed transformations will change the position of the workpiece datum and the orientation of the rotary axes:
- Shifting with the TRANS DATUM function will change the position of the workpiece datum.
- Mirroring changes the orientation of the rotary axes. The entire NC program, including the spatial angles, will be mirrored.
- If you tilt using axis angles (PLANE AXIAL or Cycle 19), a previously programmed mirroring has no effect on the orientation of the rotary axes. You use these functions for direct positioning of the machine axes.