Create a Machining Process 
for Machinable Features

task target This task shows how to create a machining process that will be used to apply a sequence of axial machining operations to machinable features.

More information about creating machining processes with formula, checks and tool queries is available in Create a Machining Process in the NC Manufacturing Infrastructure User's Guide. 
scenario 1. Select the Machining Process View icon . The Machining Process View dialog box appears.
2. Select the Machining Process icon . The dialog box is updated with a new machining process as shown. 

3. Select the Drilling icon. The Operation Definition dialog box appears, if the Start Edit mode is selected in the Tools > Options > Machining > Operation settings.
4. Just click OK to add a reference Drilling operation to the machining process.

5. In the same way, add reference Counterboring and Reaming operations to the machining process by selecting first the Counterboring icon then the Reaming icon. The Machining Process View dialog box is updated as shown.
6. Double click the Tool Query associated to the reference Drilling operation. The Tool Query Definition dialog box appears.
7.

Select the tool repository Tool AssembliesSample01 using the Look in combo. Define a query as shown below:

This query will search Tool AssembliesSample01 for a drill whose nominal diameter is between 0.85 and 0.95 times the machining axial feature's diameter.
Click OK to assign the tool query to the reference Drilling operation.

Assign a simple tool query to the reference Counterboring operation:

This query will search Tool AssembliesSample01 for an end-mill whose nominal diameter is the same as the machining axial feature's counterbore diameter.

Assign a simple tool query to the reference Reaming operation:

This query will search Tool AssembliesSample01 for a reamer whose nominal diameter is the same as the machining axial feature's diameter.
You can associate Formulas and/or Checks to the reference operations. For example:

Formula for the reference Counterboring operation:

This formula will ensure that:

  • the depth machined will equal the counterbore depth
  • the diameter machined will equal the counterbore diameter.

A Check for the Counterboring operation:

This check ensures that only counterbore holes (type 2) will be machined.

Formula for the reference Reaming operation:

This formula will ensure that:

  • the depth machined will equal the feature depth less the counterbore depth
  • the origin offset will be set to minus the counterbore depth.
8. Select File > Save As to save the machining process in a CATProcess document called
Drill_CBore_Ream_01.CATProcess, for example.
  9. Right click the Machining Process in the Machining Process View and select the Save in Catalog contextual command.
  10. The Save in Catalog dialog box appears. Click the [...] button and specify a new catalog name (AxialMP01.catalog, for example).

Click OK to save the machining process as a component in the specified catalog.
    For the next step in the procedure, please refer to Apply Machining Process on Machinable Features.

end of task