Create a Boring and Chamfering Operation

task target This task shows how to insert a Boring and Chamfering 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 Boring and Chamfering .

A Boring and Chamfering entity along with a default tool is added to the program.

The Boring and Chamfering dialog box appears directly at the Geometry tab page . 
2. Select the red hole depth representation then select hole geometry in the 3D window.
Just double click to end your selections.

The sensitive icon is updated with the following information:

  • depth, diameter, counterbore depth and angle of the first selected feature
  • number of points to machine.
3. If needed, specify the tool axis orientation.
4. Select the Strategy tab page to specify the following parameters:
  • approach clearances A and A2
  • depth mode: by shoulder
    The depth value used is the one specified in the Geometry tab page
  • breakthrough distance B
  • first compensation number depending on those available on the tool for boring
  • second compensation number depending on those available on the tool for chamfering
  • Compensation application mode.

For more information, refer to Axial Machining Strategy Parameters.
Note that in the tool path represented in the strategy page, tool motion is as follows:
Boring
  • Motion at machining feedrate from 1 up to the position where hole is to be bored
  • Possibly, activation of second tool compensation number
  • Rapid feedrate up to a clearance position before start of chamfering.
Chamfering
  • Motion at chamfering feedrate from clearance position to 2
  • Dwell for specified duration
  • Possibly, activation of first tool compensation number
  • Retract at retract feedrate from 2 to 3.
    If a Plunge mode is selected (By Tip or By Diameter), you can deactivate the plunge motion for the Chamfering phase of the operation by deselecting the Plunge for chamfering checkbox. In this case, the plunge motion will be done for the boring phase only.
  5. A tool is proposed by default when you want to create a machining 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.
6. Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.
You can specify a machining feedrate for the boring phase of the operation and a chamfering feedrate for the chamfering phase.
Similarly, you can specify a  machining spindle speed for the boring phase and a smaller spindle speed for the chamfering phase.
7. If you want to specify approach and retract motion for the operation, select the Macros tab page to specify the desired transition paths. 

The general procedure for this is described in Define Macros of an Axial Machining Operation.

  8. Before accepting the operation, you should check its validity by replaying the tool path.
9. Click OK to create the operation.
Example of output

If your PP table is customized with the following statement for Boring and Chamfering operations:

CYCLE/BORE, %MFG_TOTAL_DEPTH, %MFG_FEED_MACH_VALUE,
    %MFG_CHAMFERFEED_VALUE, &MFG_FEED_UNIT, %MFG_SPINDLE_MACH_VALUE,
    %MFG_SPINDLE_LOW_VALUE, &MFG_SPNDL_UNIT, %MFG_CLEAR_TIP, DWELL,
    %MFG_DWELL_REVOL

A typical NC data output is as follows:

CYCLE/BORE, 25.000000, 500.000000, 150.000000, MMPM, 
70.000000, 40.000000, RPM, 5.000000, DWELL, 3

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_BORING_AND_CHAMFERING section of the Manufacturing Infrastructure User's Guide.

end of task