Create a Circular Milling Operation

task target This task shows how to insert a Circular Milling operation in the program. To create the operation you must define:
  • the tool that will be used
pre-requisites Open the HoleMakingOperations.CATPart document, then select the desired Machining workbench from the Start menu.  

Make the Manufacturing Program current in the specification tree.
scenario 1. Select Circular Milling .

A Circular Milling entity along with a default tool is added to the program.

The Circular Milling dialog box appears directly at the Geometry tab page . 
2. If needed, enter Offset values for the Bottom and Contour.
3. Select the red hole depth representation then select hole geometry in the 3D window.
Just double click to end your selections.
4. If needed, you can invert the tool axis direction by selecting the axis representation in the sensitive icon.
5. Select the Strategy tab page and choose the machining mode:
  • Standard
  • Helical.
6. Specify the machining strategy parameters, which are common to the two machining modes:
  • Approach clearance
  • Plunge mode
  • Machining tolerance
  • Direction of cut
  • Percentage overlap
  • Compensation number depending on those available on the tool
  • Compensation application mode
  • Compensation output, which allows you to manage the generation of Cutter compensation (CUTCOM) instructions in the NC data output. 
Stepover parameters for Standard machining mode:
  • Breakthrough
  • Number of paths and Distance between paths
  • Axial mode: Maximum depth of cut or Number of levels (with or without top)
  • Sequencing mode: Axial first or Radial first
  • Automatic draft angle.
Stepover parameters for Helical machining mode:
  • Breakthrough
  • Helix mode: By angle or By pitch
  • Angle or Pitch value.
7. A tool is proposed by default when you want to create a machining operation. You can use an End Mill or a T-slotter in this type of operation.

If the proposed tool is not suitable, just select the Tool tab page to specify the tool you want to use. This is described in Edit the Tool of an Operation.
8. Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.

Note that in the toolpath represented in the strategy page, tool motion is at:

  • Motion at machining feedrate from 1 to 2
  • Motion at feedrates defined on macros from 2 to 3, 3 to 4, 4 to 2', 2' to 3' and 3' to 4'
  • Retract at retract feedrate from 4' to 5.
9. Select the Macros tab page to specify the operation's transition paths (approach and retract motion, for example). The general procedure for this is described in Define Macros of an Axial Machining Operation.
Before accepting the operation, you should check its validity by replaying the tool path.
10. Click OK to create the operation.
Example of output

If your PP table is customized with the following statement for Circular Milling operations:

CYCLE/CIRCULARMILLING, %MFG_TOTAL_DEPTH, %MFG_FEED_MACH_VALUE, &MFG_FEED_UNIT, %MFG_CLEAR_TIP

A typical NC data output is as follows:

CYCLE/CIRCULARMILLING, 38.500000, 500.000000, MMPM, 2.500000

You can use Edit Cycle to edit or choose output syntaxes. For more information please refer to Editing Cycle Syntaxes in Axial Machining Operations.

The parameters available for PP word syntaxes for this type of operation are described in the NC_CIRCULAR_MILLING section of the Manufacturing Infrastructure User's Guide.

end of task