Apply a Machining Process

task target This task shows how to apply a machining process to selected geometry.
Open the desired CATPart document, then select a Machining workbench from the Start menu.

The machining process application uses a standard mechanism of instantiation of features from a feature reference. In this case, the feature reference is the machining process to be applied.

When you apply a machining process, the following steps are executed for each operation:

  • Default mapping execution in case of geometry selection
  • Checks execution
  • Tool query execution
  • Cutting conditions execution
  • Formula solving.
scenario 1. Select Open Catalog . Use the Catalog Browser to open the catalogAxialMP1.catalog you created in the previous task.
2. Double-click the AxialMachiningProcesses component family.
3. Double-click the machining process to be applied: AxialMachProcess1.

The Insert Object dialog box appears allowing you to apply the machining process.

Two input types can be defined:

  1. Geometry to machine.
    The default     Geometry to machine is the Manufacturing View.
    If this is not redefined by selecting     feature geometry, then only NC data of the machining process can be processed. In this case if geometry is referenced in checks, tool queries or formula, an error message is issued.

  2. Insertion level in a program.
    The program input only appears if     Insertion level in a program is activated. If no operation is yet inserted and only one Manufacturing Program is created, then that Manufacturing Program is the default program input.

Note that for drilling machining processes, if any selected design feature or geometry is linked to a design pattern, this pattern is taken as selected geometry.
4. Select the geometry to be machined. This may be either a design feature or a machining pattern.
   

Selecting a design feature
Note that the design feature can be a design hole or a hole pattern.

The design geometry is added on the machining pattern referenced by the machining operation.

Note that all the parameters (such as Jump Distance, Tool axis strategy, Projection mode, and Ordering mode) defined on the machining pattern at machining process creation time are kept.
   

Selecting a machining pattern

The selected machining pattern replaces the one defined on the operation at machining process creation time.

Note that the parameters of the selected machining pattern are taken into account. They replace the parameters (such as Jump Distance, Tool axis strategy, Projection mode, and Ordering mode) defined on the machining pattern referenced by the operation at machining process creation time.

The selected machining pattern is shared by all machining operations created in the program by the application of the machining process.
  5. Click OK in the Insert Object dialog box.
6. The program is updated with the operations contained in the machining process:
  • Spot Drilling
  • Drilling
  • Tapping.

These operations reference the selected geometry and make use of the formula and checks defined in the machining process.

In addition, the tool queries are resolved so that each operation references the desired tool.

end of task