Multiple Faces Programming (MFP) (PartMaker)

You can program machining operations in different faces (planes) and specify up to 50 different faces for a part. A separate Face window is associated with each face of a part. PartMaker determines the order of machining based on the order of the faces. You can choose to finish all machining operations on one face before proceeding to the next or perform all operations with a tool on all faces, then change tools.

Example 1:

Your Job file contains 3 faces named Face1, Face2, Face3. You may be planning to machine multiple parts using different work offsets for each face or be planning to use an indexer to rotate a part.

As a final result you want a single program file, named Job123.txt, however, such a file cannot be verified by N-SEE verification (no longer available in Version 5 and higher), you have to verify each face individually.

Do the following:

1. Ensure Face1, Face2, Face3. can be used as valid file names; that is, they should not contain spaces, periods, or commas. Another restriction is that they cannot contain a dash (-) character.
2. Select Job Optimizer > Post Options to display the Post Options dialog.
3. In the Post Options dialog:
   1. Select the Separate Faces option.
   2. Click OK to close the dialog.
4. Select Job Optimizer > Generate NC Program.

   PartMaker creates three separate NC program files (Face1.txt, Face2.txt, and Face3.txt) on your computer. PartMaker also creates a file called NC Programs.txt, which is displayed in the NC Program window so you can view the content of the separate NC program files in sequential order.

   PartMaker also generates separate setup files for N-SEE (no longer available in Version 5 and higher), so you can go to N- SEE and verify each file (Face1, Face2, Face3) individually.

5. When you are satisfied with verification of individual faces, select Job Optimizer > Post Options and deselect the Separate Faces option.
6. Select Job Optimizer > Generate NC Program. When PartMaker prompts you to enter a filename, type Job123. PartMaker then creates and displays this file.

Example 2:

You have a job file with three faces and you want to create two program files: PROG1.txt and PROG2.txt, where the first two faces will be written to PROG1.txt and the third face to PROG2.txt. You also want the corresponding program numbers to be: 1001, 1002.

To do this:

1. Select View > Setup. Ensure your faces are named as following:

   ***-PROG1-1001

   ***-PROG1-1001

   ***-PROG2-1002

   *** above can be replaced by any text of your choice. This text does not have to be of any specific length. The only restriction is that it cannot contain a dash (-) character.

   If your CNC does not require program numbers, you can use shorter names:

   ***-prog1

   ***-prog1

   ***-prog2

2. Select Job Optimizer > Post Options to display the Post Options dialog.
3. In the Post Options dialog:
   1. Select the Separate Faces option.
   2. Click OK to close the dialog.
4. Select Job Optimizer > Generate NC Program.

   PartMaker creates two separate NC Program files on your computer. PartMaker also creates a file called NC Programs.txt, which is displayed in the NC Program window so you can view the content of the separate NC program files in sequential order.