Creating a Pocketing Operation for Open Pockets

You can create a Pocketing operation when the pocket to be machined comprises at least one soft boundary (that is, an open pocket).

Related Topics
Creating a Pocketing Operation for Closed Pockets
Pocketing
Selecting Guiding and Relimiting Elements
Defining a Virtual Bottom Plane

  1. Activate the Manufacturing Program and click Pocketing in the Prismatic Machining Operation 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 Open Pocket. If this is not the case, click Closed Pocket to switch to Open Pocket.
    2. Right-click the red Bottom in the icon and select Contour Detection from the contextual menu, then select the desired pocket bottom in the authoring window. .
    3. Optional: For edge selection only, change a boundary segment from Hard to Soft (or from Soft to Hard) by selecting the corresponding edge.
    4. Optional: Change all segments from Hard to Soft and from Soft to Hard using the Swap Hardness Mode contextual command.

    5. For parts containing islands, right-click the red bottom in the icon and select Island Detection. This allows island boundaries to be deduced automatically.



      The pocket boundary is automatically deduced due to the Contour Detection setting. This is indicated by the highlighted drive elements.

      Hard boundaries are shown by full lines and soft boundaries by dashed lines.



    6. Click the top plane in the icon then select the desired top element in the authoring window.
    7. Set the following offsets:


      • 1.5mm on hard boundary
      • 0.25mm on bottom

    8. Optional: If your part includes islands, 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. Go to the corresponding tabs to set parameters for:


      • Machining such as Machining Tolerance
      • Radial stepover conditions (overhang = 50, for example)
      • Axial stepover conditions (number of levels = 3, for example)
      • HSM
      • User Parameters

    3. For Back and forth tool path style, click the arrows next to the machining axis system to modify the proposed machining direction and progression direction.


      • Clicking the Machining direction arrow displays a dialog box for specifying the direction of paths.
      • Clicking the Progression direction arrow reverses the overall direction of progression of the paths.

  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 to specify the feedrates and spindle speeds for the operation.

  6. Select theMacros tab to specify the operation transition paths. 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 the Axial mode. An 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.