Map Mastercam work offsets in CAMplete TruePath

Output multiple datums in your NC Program directly from Mastercam. The additional datums are output as datum shifts or auxiliary datums.

To set the work offset in Mastercam

You may use multiple datums in Mastercam as WCS for different operations. If so, you need to assign a work offset number specific to each datum. In this way, you correctly output the same datums in your G-code in TruePath.

To see the datum number for each toolpath, look at the Work Offset value on the Planes page of your toolpath parameters.

To edit the machining setup

1. Start TruePath.

2. In the ribbon, select Manage > Resources > Machines.

3. Select your machining setup.

4. Hold the Shift key and click Edit.

   For Fanuc machines:

   This example maps CAM indexes 1 through 5 to coordinate system G54.1 P1 through G54.1 P5, respectively.

   

   For Heidenhain machines:

   If you see a prompt, click No if you’re not using TNC Remo application.

   

5. Click OK after making the changes and close the Resource Manager.

To change preferences

Before you import the NCI data from Mastercam, enable the following preferences in CAMplete TruePath.

1. In the ribbon bar, select Manage > Tools > Options.

2. Click File Types.

3. From the drop-down menu, change the filter to Mastercam.

4. Enable these preference:

   • NCI - NCI 1053 Records Delimit Tool Paths

   • NCI - Use Cached Datums

     

5. Click Advanced Properties on the same page.

6. Click Datum Settings and enable Read Datum Index from NCI.

   

7. Click OK to save the changes and click Close.

8. Close TruePath to save the changes to the registry.

The next time you import the NCI in TruePath or create a project using the Mastercam plug-in, the datum changes appear in G-code and on the Coord Sys page of the CAM Wizard.