Understanding milling formats

This tutorial gives you a basic understanding of the correspondence between toolpath moves and program formats. You create a milling post, but the concepts are applicable to all types of post processors. This tutorial is in metric units.

1. Open 001.fm in FeatureCAM from the Examples\Tutorials\XBUILD folder.
2. Generate toolpaths, and single step through the program. This simple program performs the following moves:
   • Rapids from the Tool Change Location to the Z rapid plane above the slot.
   • Rapids in Z to the Plunge clearance.
   • Feeds down in Z into the slot.
   • Feeds across in X.
   • Rapids to the Z rapid plane.
   • Rapids to the tool change position.
3. Select the text.CNC post processor from the Examples\Tutorials\Xbuild folder. This is a post processor that simply outputs the name of each program format that is called. This shows you the order in which the program formats are called for this program.
4. Click the NC Code tab. The following code is displayed:

   Program_Start - begins the program, grabs the first tool and rapids above the part.

   Z_Rapid - rapids to plunge clearance plane.

   Linear_Move - feeds down into the slot.

   Linear_Move - feeds across in X.

   Z_Rapid - rapids to the Z Rapid Plane.

   Program_End - ends program, turns off coolant, rewinds program.

   File_End - ends file, usually just a % to end the transmission.

   Note: The tool is never explicitly positioned to the Tool Change Location as the simulation might lead you to believe.
5. Select slot2 in the tree view, and generate the NC code. The following code is created.

   Program_Start
   Z_Rapid
   Linear_Move
   Linear_Move
   Z_Rapid
   Rapid_Move
   Z_Rapid
   Linear_Move
   Linear_Move
   Z_Rapid
   Program_End
   File_End

   Because both features use a 5 mm tool, all that is needed between the features is to move to the new location and cut another slot. The program accomplishes this with the new Rapid_Move format. This format performs a rapid move in X and Y.

6. Edit slot2 to have a width of 10 mm, and regenerate the code. This forces a tool change from a 5 mm tool to a 10 mm tool. The following code is created:

   Program_Start
   Z_Rapid
   Linear_Move
   Linear_Move
   Z_Rapid
   TOOL_CHANGE
   Z_Rapid
   Linear_Move
   Linear_Move
   Z_Rapid
   Program_End
   File_End

7. TOOL_CHANGE is the new program format. This format changes the tool and rapids to the next location in X and Y.
8. Edit slot2 and change Width to 5 mm, and its speed to 1000 rpm. Regenerate the NC code. The TOOL_CHANGE segment has been replaced by the Segment_Start format. If there is a change in fixture IDs or a change in speed this format is called instead of the TOOL_CHANGE format.

Summary of new formats in this tutorial