Create a Drilling Operation

task target This task shows how to insert a Drilling 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 Drilling I_MfgDril.gif (895 bytes). A Drilling entity along with a default tool is added to the program. The Drilling dialog box appears directly at the Geometry tab page . This tab page includes a sensitive icon to help you specify the geometry of the hole or hole pattern to be machined. 
2. Select the red hole depth representation then select the pattern of 10 holes as shown below. Just double click to end your selections.

The sensitive icon is updated with the following information:
  • depth and diameter of the first selected feature
  • hole extension type: through hole
  • number of points to machine.
3. If needed, you can invert the tool axis direction by selecting the axis representation in the sensitive icon.
4. If needed, you can define a clearance by first double clicking the Jump Distance parameter in the sensitive icon then specifying a value in the Edit Parameter dialog box that appears.
5. Select the Strategy tab page to specify the following machining parameters:
  • Approach clearance
  • Depth mode: by tip
    The depth value used is the one specified in the Geometry tab page.
  • Breakthrough distance
  • Compensation number depending on those available on the tool
  • Compensation application mode.

The other parameters are optional in this case.
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.

Remember that you can make use of the hole diameter found on the selected hole feature to select an appropriate tool. 
6. Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.

Note that in the Drilling tool path represented in the strategy page, tool motion is as follows:

  • machining feedrate from 1 to 2
  • retract or rapid feedrate from 2 to 3.
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.
Before accepting the operation, you should check its validity by replaying the tool path.
8. Click OK to create the operation.
Example of output

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

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

A typical NC data output is as follows:

CYCLE/DRILL, 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_DRILLING section of the Manufacturing Infrastructure User's Guide.

end of task