Part Operation

task target This task shows you how to create a part operation in the manufacturing process.
When you open a Machining workbench on a CATPart or CATProduct document, the manufacturing document is initialized with a part operation.
scenario 1. Select Part Operation .

A new part operation is initialized in the manufacturing process and a Part Operation entity is added to the tree.

To access the parameters of the part operation, double-click the Part Operation entity in the tree or use the contextual menu. The Part Operation dialog box appears.

 

Name and Comment
2. If needed, enter a new part operation name and assign comments to the part operation.
 

Machine
3. Click Machine to assign a machine tool to the part operation.
Please refer to Machine Editor for more information.
 

Reference Machining Axis System
4. Click Reference Machining Axis System to assign a reference machining axis system to the part operation. The Machining Axis System dialog box appears.

This is similar to the procedure described in Insert a Machining Axis Change.

Output coordinates will be expressed in the reference machining axis system. If a local machining axis system is inserted in the program, coordinates will be expressed in the local axis system.

 

Product or Part
5. Click Product or Part to associate an existing product (CATProduct) or part (CATPart) to the part operation. This procedure is described in Set Up and Part Positioning.

Note: In a Manufacturing Hub context, Product Instance Selection replaces Product or Part in the Part Operation editor.
 

Geometry tab
  6. Select the Geometry tab to associate the following geometry to the part operation:
  • Design part: Just click Design Part then select the desired geometry. This is useful if you want to do material removal simulations later.
  • Stock: Just click Stock then select the desired geometry. This is useful for certain surface machining operations and also for material removal simulations.
  • Fixtures: Just click Fixtures then select the desired geometry. This is useful if you want to do material removal simulations later.
  • Safety plane: Just click Safety Plane then select the desired plane that will be used as a global safety plane for the part operation.
  • Traverse box planes: Just click Traverse Box Planes then select 5 planes that define a global traverse box for the part operation.
  • Transition planes: Just click Transition Planes then select the desired planes that will be used as a global transition planes for the part operation.
  • Rotary planes: Just click Rotary Planes then select the desired planes that will be used as a global rotary planes for the part operation.
  The generation of transition paths in the program takes into account:
  • Traverse box planes and Transition planes to create linear tool path motions
  • Rotary planes to create machine rotations:
    • between machining operations
    • between tool change and machining operation.

The Safety plane is not taken into account for the generation of transition paths.
    When the geometry is selected, the identifiers are displayed in the corresponding fields and tool tips (see example below).
 

Position tab
7. Select the Position tab to specify the following reference positions on the part operation:

   
  • Tool change point
    For machines created using the NC Machine Tool Builder product, the tool change point is read from the machine and cannot be modified in the Part Operation.
    For Multi-slide lathe machines, the tool change point is read from the machine and cannot be modified in the Part Operation.
   
  • Table center setup
  • Home point
    You can select the check box to use the Home point defined on the machine.
 

Simulation tab
  8. Select the Simulation tab to specify the stock tessellation tolerance. In previous releases, this tolerance was fixed at 0.2mm.

 

Option tab
9. Select the Option tab to specify the following options:

  • Intermediate stock for milling and turning operations.
    If this check box is selected, automatic computation of the intermediate stock is enabled. The computed stock is taken into account for tool path computation. 
    A clearance can be assigned to the stock.
  • Automatic stock selection for turning operations.
    This option enables automatically updating the input stock for operations in a manufacturing program for turning (that is, turning operations and axial operations along the spindle axis).
    A lathe machine must be selected in this case.
  • Use Spindle Axis System according to the spindle involved in the machining operation.
    A Multi-slide lathe machine or a Mill-Turn machine must be selected.
    If this check box is selected, tool tip points are computed based on the spindle that is set on the machining operation.
    If this check box is not selected, the main spindle axis is used. This is determined by the default reference machining axis system set on the Part Operation.

Collision Checking tab
  10. Select the Collision Checking  tab to specify whether or not you want to have quick feedback about collisions during the tool path replay.

The options on this tab are available for Milling operations only.

  1. Select the Activate Collision Checking check box if you want to have quick feedback about collisions during the tool path replay.
    In this case the other options become available for selection.
  2. Select the On design part check box to detect collisions between the tool/tool holder and the design part specified on the Part Operation's Geometry tab.
  3. Select the On fixtures check box to detect collisions between the tool/tool holder and the fixtures specified on the Part Operation's Geometry tab.
  4. If needed, you can set offsets on the tool or tool assembly, which are used as "safety" distances.

For more information, see:

Note that barrel tools, boring bars, and user-representation tools are not supported.
11. Click OK to create the part operation. The tree is updated with the new entity.

end of task