Workpiece datum in the CAD file
Application
The workpiece preset is not always located in a manner that lets you machine the entire part. Therefore, the control has a function with which you can define a new datum and a working plane.
Related topics
- Presets in the machine
Description of function
When you select the Datum icon, the control displays the following information in the list view area:
- Distance between the datum that has been set and the workpiece preset
- Orientation of the working plane
You can apply a workpiece datum set in CAD Viewer and shift it, if required, by entering values directly in the List View area.
The control displays values not equal to 0 in orange.
- Workpiece datum for tilted machining
The datum with the orientation of the working plane can be set at the same positions as a preset.
Workpiece preset in the CAD file
If you have set a workpiece datum, the control displays the Datum icon in the menu bar with a yellow area.
Setting the workpiece preset or workpiece datum and orienting the coordinate system
The datum and its optional orientation can be inserted as NC block or comments in the NC program by using the TRANS DATUM AXIS function for the datum and the PLANE SPATIAL function for the orientation.
If you define only one datum and its orientation, then the control inserts the functions in the NC program as an NC block.
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.
4 TRANS DATUM AXIS X... Y... Z... |
5 PLANE SPATIAL SPA... SPB... SPC... TURN MB MAX FMAX |
If you additionally select contours or points, then the control inserts the functions in the NC program as comments.
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.
4 ;TRANS DATUM AXIS X... Y... Z... |
5 ;PLANE SPATIAL SPA... SPB... SPC... TURN MB MAX FMAX |
You can save the workpiece preset and workpiece datum information to a file or the clipboard even without the CAD Import software option (#42 / #1-03-1).
The control retains the content of the clipboard only as long as CAD Viewer is open.