Machining Processes

Machining process capabilities can be useful when your work habits include:


The proposed solution uses two major steps:

Feeding the System with Your Know-How

This is the Build Time step that includes creating machining processes and storing them in V5 Catalogs. It is usually performed by the Administrator or Support Group.

Create Machining Processes

  1. You need to create different Machining Operations without geometry: just start from an empty session. 
  2. Activate the Machining Process toolbar in the View>Toolbars menu to display the Machining Process commands:
    • Machining Process View : to display the Machining Process window
    • Machining Process : to create a new Machining Process.
  3. Create your Machining Process operation by operation: all axial operations are available. 
    Define parameters for operations just like in a Manufacturing Program (Offset, Feeds & Speeds, and so on).
  4. Thanks to Knowledgeware integration, you can define formula and checks for each operation.
  5. Define tool query for each operation.

A user task for creating a machining process is described in this guide.

Store Machining Processes in Catalogs

You can either:

See Save the Machining Process for more information.

  1. Save the CATProcess containing the machining processes (do not close this document).
  2. Create a new Catalog with Catalog Editor.
  3. Save the machining process in this catalog.
  4. Save the catalog.

See Organizing machining processes in catalogs for more information.

Using the Machining Process

This is the Run Time step, usually performed by the NC Programmer.

  1. Retrieve the machining process from the catalog using Open Catalog .
  2. Apply the machining process in your NC program.
  3. Edit the created machining operations to complete geometry selection and possibly the tool definition. This is the case if no Tool Query was defined or the Tool Query did not find a suitable tool.

See Applying a machining process for more information.

Step by Step Example

When working with Pocketing operations, you usually use a different set of options depending on the geometric shape to machine or the part material type.

You can define and put in the system a machining process to be used for:

Steps for Creating the Machining Process

Click Machining Process .

  1. Define one or more machining operations.
  2. For the machining operations, define your preferred Options, Strategies, Parameters, Macros, and possibly tool queries.
  3. Save the CATProcess document using File > Save. 
  4. Store the Machining Process in a V5 Catalog.
  5. Select (or create) the Component Family in which you want to store the machining process.
  6. Click Add Component .
  7. Select Select External Feature in the dialog box that appears.
  8. Select the CATProcess document, then the Machining Process.

Some Hints 

In order to facilitate the NC Programmer job at selection time:

Steps for Using the Machining Process

Click Open Catalog .

  1. Navigate in your catalog, and select the required Machining Process.
  2. Select the operation after which you want the Pocketing operation to be created, and click OK.
  3. Edit the Machining Operations to specify the Tool to be used if no Tool Query was defined in the machining process and complete geometry selection.

Some Hints 

Catalog organization (structure, comments) is key for a quick and efficient selection of machining processes by the end-user.

For more information, refer to the following: