Creating a Pocketing Operation for Closed Pockets

You can create a Pocketing operation in the manufacturing program when the pocket to be machined comprises hard boundaries only (that is, a closed pocket).

Related Topics
Creating a Pocketing Operation for Open Pockets
Pocketing

  1. Activate the Manufacturing Program and click Pocketing in the Prismatic Machining Operations toolbar.

    A Pocketing entity is added to the Manufacturing Program.

    The Pocketing dialog box appears directly at the Geometry tab .

    The bottom and flanks of the icon are colored red indicating that this geometry is required for defining the pocket. All other pocket geometry is optional.



  2. Still in the Geometry tab:

    See Selecting Geometry

    1. Make sure that the Pocketing style is set to Closed Pocket. If it is not, click Open Pocket to switch to Closed Pocket.
    2. Right-click the red bottom in the icon and select Contour Detection from the contextual menu.
    3. Click red bottom then select the desired pocket bottom in the authoring window.

      The Contour Detection option automatically deduces the part boundary. This is indicated by the highlighted drive elements.



      Note: The bottom and flanks of the icon are now colored green indicating that this geometry is now defined.

    4. Optional: An alternative to Contour Detection is to select By Belt of Faces or By Boundary of Faces in the contextual menu.

      In this case the Selecting Edges and Faces to Define Geometry appears to help you specify the pocket boundary.

    5. Click the top plane in the icon then select the desired top element in the authoring window.
    6. Set the following offsets:1.5mm on hard boundary and 0.25mm on bottom
    7. Right-click the red bottom in the icon and select Island Detection. This allows island boundaries to be deduced automatically.
    8. Optional: Right-click the Island label in the authoring window and specify different offsets on individual islands using Offset on Island.

  3. Select the Strategy tab .

    1. Choose the desired Tool path style: Inward helical, Outward helical, or Back and forth.
    2. Set the parameters for machining (such as machining tolerance), radial and axial strategy, finishing, HSM, and User Parameters.



  4. Go to the Tool tab to select a tool.

    See Specifying a Tool Element in a Machining Operation

  5. Select the Feeds and Speeds tab and specify the feedrates and spindle speeds for the operation.

  6. Select the Macro tab and add approach and retract motions to the operation. To specify approach motion:

    See Defining Macros on Milling Operations

    1. In the Macro Management frame, right-click the Approach line and select the Activate contextual command.
    2. In the Current Macro Toolbox frame, select Axial mode. A sensitive icon representing this approach motion is displayed.
    3. Double-click the distance parameter in the sensitive icon and enter the desired value in the pop-up dialog box.
    4. Repeat this procedure to specify retract motion.



  7. Click Tool Path Replay to check the validity of the operation.

    See Replaying the Tool Path


    • The tool path is computed.
    • A progress indicator is displayed.
    • You can cancel the tool path computation at any moment before 100% completion.


  8. Click OK to create the operation.