Create a User Feature for Machining

task target This task shows how to:
  • define a User Feature for Machining
  • create a machining process that makes use of the User Feature. 

Please refer to the Product Knowledge Template User's Guide for more information about creating user features, storing them in catalogs, and reusing them in documents.
task target

Mapping Rule File

A default mapping dedicated to the User Features and their use in Axial Operations can be defined through a mapping rule file.

This file is located in \resources\msgcatalog\CATMfgUdfForMappingToMfg.CATNls. It contains:

  • Drilling Point (MfgHolePoint) which has to be an input or output point of the User Feature
  • Drilling Axis (MfgHoleAxis) which has to be an input or output planar face of the User Feature
  • Drilling Diameter (MfgHoleDiameter) which has to be a published parameter of the User Feature
  • Drilling Depth (MfgHoleDepth) which has to be a published parameter of the User Feature.

It enables you to use a User Feature when defining a machining pattern or an axial operation without any other mapping consideration.

For more complex mapping rules, the Machining Process functionality is more suitable.
scenario 1. In the Part Design workbench, select Insert > Knowledge Templates > User Feature.

The User Feature Definition dialog box appears.

The left part of the graph displays the features that are required to build the selected object.
To rename these features, just select a feature in the graph and enter a new name in the Name field. When the Inputs tab is selected, the user feature inputs are indicated by red arrows in the geometry area.
2. In the Parameters tab, all available parameters are displayed along with their values. By default, the instantiation process of a user feature forbids the modification of a parameter value. If you want to get round this, you can publish a parameter. That means you must declare that the value of this parameter can be modified in a user feature instance.
To do so, select the parameter to be modified in a forthcoming instantiation and check the Published option.

You can rename a parameter.  Just select it and enter its new name in the Name field. For the purpose of this scenario, declare the Depth for NC and Diameter for NC parameters as published. Note that a published parameter is identified by a Yes in the Published column.

The Type tab manages the User Feature type that will be accessible in the formula definition. In this example, it is UserFeature1. Managing type is required in order to access all user feature attributes in the Machining Process definition.

Click OK to define the user feature.
3. Select a Machining workbench from the Start menu and select Machining Process View .

The Machining Process View dialog box appears.

4. Select Machining Process . 

The dialog box is updated with a new machining process as shown. 
5. Select Drilling .

The Operation Definition dialog box appears, if the Start Edit mode is selected in the Tools > Options > Machining > Operation settings.
6. Just click OK to add a reference Drilling operation to the machining process.
The reference operation has an associated Tool Query.

You can associate Formulas or Checks to the operation and specify a Tool Query.
7. Right-click the Drilling operation in the Machining Process View and select Edit Formula.

The Formula Editor dialog box appears at the Numerical Expressions tab page.

A formula is an expression associated to an operation or a machining feature attribute, which will be converted to a F(x) formula when the machining process is applied.

Define the Diameter and Depth attributes of the formula as shown: 

8.

In the Geometrical Expressions tab page, define the Drilling Point and Axis as shown below. 

Fill in the two fields with:

  • anchor point of the Drilling operation as "Entry Point for NC" user feature input parameter

  • axis of the Drilling operation as "Entry Face for NC" user feature input parameter.

Click OK to assign the formula to the Drilling operation.
9. Double-click the Tool Query associated to the Drilling operation.

The Tool Query Definition dialog box appears.

Define a simple tool query as shown below.
10.

In the Look in list, select the ToolsSampleMP tool repository.

Click OK to assign the tool query to the Drilling operation.
11. Select File > Save As to save the machining process in a CATProcess document called
UserFeatureMachProcess01.CATProcess, for example.

You can then apply this machining process following the general procedure described in Apply a Machining Process.

end of task