Create a Machining Process

This task shows how to create a machining process containing a sequence of axial machining operations: Spot Drilling, Drilling, and Tapping.

For each operation you can associate Knowledgeware expressions such as formula and checks and specify a tooling query.

This enables to establish relations on data such as features, machines, and tools that are not yet known at machining process build time. For example, you can use this capability to determine the depth of cut from the hole depth.

In addition, you can use f(x) capability to link the various parameters of machining operations. For example, for an machining process where a rework phase follows a roughing phase, the offsets of the rework can be determined from the offsets used in the roughing step.

For more information about these capabilities, refer to Knowledgeware and Machining Processes.
Select a Machining workbench from the Start menu. No CATPart or CATProcess is needed at this stage.

If the Machining Process toolbar is not already displayed, select it using View > Toolbars.

Make sure that Start Edit mode is set in Tools > Options > Machining > Operations.

Initialize the Machining Process with Machining Operations
1. Select Machining Process View . The Machining Process View dialog box appears.
2. Select Machining Process . The dialog box is updated with a new machining process as shown. 
3.  Select the Spot Drilling icon. The Spot Drilling dialog box appears.
At this stage you can set certain parameters such as feeds and speeds and machining strategy. However, there is only limited access to geometry parameters and it is not possible to specify a tool.
4. Just click OK to add a reference Spot Drilling operation to the machining process.

The reference operation has an associated Tooling Query.
5. In the same way add Drilling and Tapping operations to the machining process by selecting first the Drilling icon then the Tapping icon. The Machining Process View dialog box is updated as shown.
  Note that any machining activity named according to the structure String.number will be managed at instantiation time by checking the unique name in a given program. This is an extension of the standard mechanism for default names:
Drilling.1 will give Drilling.1, then Drilling.2, and so on.
So:
MyOwnName.1 will give MyOwnName.1 then MyOwnName.2 and so on.
However:
MyOwnName will give MyownName then MyOwnName, and so on.

Associate Formula to the Machining Operations
6. Right-click the Spot Drilling operation in the Machining Process View and select Edit Formula. The Formula Editor dialog box appears.

Define a formula as shown below. It corresponds to the following criteria: 
the tool tip approach clearance is half the depth of the Spot Drill machining feature.

7.

Click OK to assign the formula to the Spot Drilling operation.

You can assign formula to the Drilling and Tapping operations in the same way.

Associate Checks to the Machining Operations
8.

Right-click the Spot Drilling operation in the Machining Process View and select Edit Checks. The Checks Editor dialog box appears.

Define a check as shown below. It corresponds to the criteria: 
the Spot Drilling operation is only available for design holes with a diameter greater than 2mm.

You can assign checks to the Drilling and Tapping operations in the same way.

Define Tool Queries for the Machining Operations
9. Double-click the Tooling Query associated to the Spot Drilling operation. The Tool Query Definition dialog box appears.

Define a simple tooling query as shown below. It corresponds to the criteria:
find a spot drill in the ToolsSampleMP tool repository whose name is Spot Drill D10.

10.

Click OK to assign the tooling query to the Spot Drilling operation.

You can assign tool queries to the Drilling and Tapping operations in the same way (to find tools Drill D10.5 and Tap D12, for example).
  Through the Copy/Paste mechanism, you can manage more than one Tooling Query on an operation. When you instantiate the Machining Process, the first query is executed. If there is no tool found, the next query is executed and so on until a result is obtained or the last query is reached. This enables you to query several tool catalogs, different tool types, and have less constrained queries.

Save the Machining Process
11. Select File > Save As to save the machining process in a CATProcess document (called AxialMachiningProcess1.CATProcess, for example).
  12. Right-click the Machining Process in the Machining Process View and select Save in Catalog.
    The Save in Catalog dialog box appears. Click the [...] button and specify a new catalog name (catalogAxialMP1.catalog, for example).

Click OK to save the machining process as a component in the specified catalog.

The following are initialized automatically:

  • family name: Machining Process
  • component name: name given to the machining process using File > Save As.

However, you can change family or component in the Catalog Editor workbench. Click here to see how you can organize machining processes in a catalog using that workbench.
    See Apply a Machining Process for information about applying machining processes to geometry such as design features and machining patterns.
 

More About Creating Machining Processes

  • For Hole features, when you use string parameters in Checks, Formulas and Tool Queries you must put the value in double quotes ("). For example:
    Hole.Hole type = "Tapered"
 
  • The Formula Editor, Checks Editor and Tool Query dialog boxes have several common areas:
  1. All expressions of the current entity (tool query or machining operation and for a machining operation, either formulas or checks).
  2. The commands list.
  3. Area for editing the current expression with restrictions and help for using Operator, Function and Unit lists. To validate an edited expression, you must select the Add button.
  4. All the possible attributes that you can use in an expression, according to the Knowledgeware description:
    • the different Knowledgeware packages which group a set of object types: the Machining Resources, Machining Features and Machining Activities packages are always available
    • the object types list for the selected package
    • the attributes list for a selected type: select an attribute to insert it in the expression.
  5. For the Tool Query dialog box, a fifth area allows you to define the tool type and tool repository.
  • In the same way as for a machining operation, you can associate a check on a machining process. Just right-click the machining process in the Machining Process View and select Edit Checks. You can then constrain the domain of application of the machining process in the Checks Editor dialog box. Note that checks created on Machining Processes can only be executed through the Machining Processes Instantiation Manager functionality (see Apply Machining Processes Automatically for more information).
  • In the same way as for machining operations, machining axis systems can be used in machining processes.
 
  • Parameters can be added on machining operations and features in the Knowledge Advisor workbench.
    Please refer to Knowledgeware and Machining Processes.
    In this case the Machining Process View displays a generic node named Parameters under the machining object node. Under this generic node appears the parameter node with its name, its value and/or its formula (depending on the Knowledge parameter display setting).