Creating a Part Operation

You can create and edit a Part Operation in the Activities Process Tree. Now all the options related to the machine assignment are removed from the Part Operation and are placed in the Resource Configuration View. The Position, Simulation, and Collision Checking tabs are merged in the Option tab and hence number of tabs are reduced in the Part Operation. The 2D view is used to select geometries in the Setup tab.

This task shows you how to:

Create and Edit a Part Operation

You can access and create a Part Operation in the Activities Process Tree.

  1. From any product or 3D part:
    1. Select a machining app then the Programming section.
      A PPR Context with an empty Manufacturing Cell is created with a Activities Process Tree.
    2. Create a generic machine or assign a machine from the database.
      As soon as a machine is assigned to the Manufacturing Cell, a Part Operation and a Manufacturing Program are created in the Activities Process Tree.
    3. Alternatively, open an existing Machining Process or PPR Context.

      By default, the Activities Process Tree is available.

    1. Select a machining app then the Programming section.
      An empty Manufacturing Cell is created with an Activities Process Tree.
    2. Create a generic machine or assign a machine from the database.
      As soon as a machine is assigned to the Manufacturing Cell, a Part Operation and a Manufacturing Program are created in the Activities Process Tree.
    3. Alternatively, open an existing Machining Process or PPR Context.

      By default, the Activities Process Tree is available.



  2. If you need to add a Part Operation, click Part Operation .
  3. Double-click the Part Operation in the Activities Process Tree.

    The dialog box to edit a Part Operation varies depending on the type of the machine.

    • When the assigned machine is a milling machine, the Part Operation is:

    • When the assigned machine is a mill turn machine, the Part Operation is:

    • When the assigned machine is a wire EDM machine, the Part Operation is:

  4. Optional: Click Comment to edit the Part Operation Name and assign Comments to the Part Operation.
  5. Optional: Edit the Setup Options, and Transition Path tabs.
  6. Optional: Edit the Air Cut Optimization parameter.

    • If activated: Removes cutting motion when the tool does not remove any material, reducing machining time.
    • If deactivated: Keeps cutting motion when the tool does not remove any material, reducing computation time.

  7. Click Analyze to open the Geometry Analyzer dialog box containing the selected geometry points.
  8. Click Reset all selections to reset all geometry selections in the 3DEXPERIENCE platform.
  9. Click Define Feature to Recognize to select the faces of the feature to recognize for geometric form reuse.

    Note: If the part contains several geometric forms, you must define a setup and a new NC assembly for each form on the part.

  10. Click Show/Hide the offset to show/hide the offsets in 3DEXPERIENCE platform.

Assign a Reference Machining Axis System

You can assign a reference machining axis system to the Part Operation.

  1. Click Reference Machining Axis System .
    The Machining Axis System dialog box is displayed.
  2. See Inserting Machining Axis Changes.

    Notes:
    • Output coordinates are expressed in the reference machining axis system.
    • If a local machining axis system is inserted in the Manufacturing Program, coordinates are expressed in the local axis system.

Define the Setup of the Part Operation

You can define the geometry of the Setup Assembly, the Design, the Stock, Check elements and Safety planes from the Setup tab.

Note: Sketches are not supported to define design parts, stocks, or fixtures.

  1. Go to the Setup tab .
  2. Assign an existing setup assembly to the Part Operation.
    1. Click Setup Assembly to associate an existing setup assembly to the Part Operation.

      Note: The setup assembly can be linked to only one setup position. To select the same setup assembly, create a new instance under the manufacturing cell using the Insert Setup Assembly command or copying/pasting an existing instance.

      The icon turns to .
    2. If required, click to remove the currently associated setup assembly.
      The icon turns back to .
    Note: When replacing the Product or the Part, a warning message is displayed if points have been created in the machining program . For example: When defining the order of the pocket in a roughing operation, delimiting the curve guide in tube machining, or defining the point to probe in a multi-point probing operation. You can:

    • Delete these points: The operations associated to these points are incomplete and select new points again
    • Keep these points: The new product/part of the part operation is identical.

  3. Click Design Part then select the required geometry.

    Recommendation: You should define a solid as a part, and not only surfaces.

    The geometry of the design part is associated to the Part Operation. This is useful for material removal simulations.
  4. Click stock then select the required geometry.
    A rough stock is associated to the Part Operation. This is useful for some Surface Machining Operations and also for material removal simulations.
  5. Click Fixtures then select the required geometry.
    Fixtures are associated to the Part Operation. This is useful when you want to do material removal simulations.
  6. Click Safety Plane then select the required plane.
    This plane is associated to the Part Operation, as its global safety plane.
    Note: For wire EDM operations, this parameter is replaced by the Output Plane. This plane defines the height of the tool path on the Z-axis.
  7. Optional: Specify a feeds and speeds configuration to filter the search results of cutting resources when launched from Search from Session, Search from Catalog, or Search from Database in the operation panel.

    Note: The lists displays what is defined under Me > Preferences > App Preferences > Simulation > Machining > NC Machining Apps Common Services > Resources.

    The values are undefined by default, that is, no filter is applied to the search results based on the feeds and speeds configuration.

    If at least one value is defined, resources that have a feeds and speeds configuration that matches the value specified on setup are included in the search results. Conversely, resources without a feeds and speeds configuration are excluded from the search results.

  8. Click + to add a Setup.
    A Setup tab is added.

  9. Click the left or right arrow to modify the order of the existing setups.
  10. Click the red cross to delete an existing setup.
  11. Right-click then Reference Machining Axis System on Part Operation Setup tab:
  12. Click Table Center Setup and modify the reference positions.
    Setup delta X 4.00 mm, SetUp delta Y 0.00mm, SetUp delta 0.00mm.
  13. Click OK.

Edit the Options of the Part Operation

You can edit several options of the Part Operation from the Option tab.

  1. Go to the Option tab .

    Only the relevant options are selectable:

    Tool Path points based on the turret axis system, and Collision Checking, On geometries, Collisions check in on design part.
  2. In General:
    1. Define the value of the Stocks Accuracy.

      The Stock Accuracy is the tolerance used to compute tessellations for material removal simulations.

      By default, The Stock Accuracy is set to 0.2 mm.

    2. For wire EDM operations, define the value of the Machine Upper Head Height.

      The Machine Upper Head Height defines the output of the upper guide height, which is used by the post-processor to compute U and V machine values.

    3. Click Undo to revert to the default value.
    4. Select the required check boxes:
      • Use Spindle Axis System defined in the Machining Operation: When selected, computes the tooltip points 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.
        Note: Select a multi-slide lathe machine or a mill-turn machine.
      • Toolpath points based on the turret axis system: When selected, computes the tool path points and APT output based on the turret axis system for turning operations.

        By default, this check box is cleared and the tool path points and APT output are computed with respect to Part Operation axis system, in the spindle plane.

  3. In Intermediate Stock:
    1. Select Activate the Intermediate Stock check box to enable the automatic computation of the intermediate stock.

      When the tool path is computed, dynamic residual stock is computed at the same time, therefore a tool path without collisions with stock, with minimum NC macro modifications. In this example:

      • In the first level, the linking motions are created above the stock.



      • In the last level, the linking motions are created in the first level and the stock clearance defined in the Intermediate Stock of the Part Operation.



    2. Define the value of the Stock Clearance.

      By default, the Stock Clearance is set to 5.00 mm.

  4. In Collision Checking:
    1. Select the Activate collisions checking check box to get quick feedback about collisions during the tool path computation.

      Note: Barrel tools and boring bars are not supported.

      The collisions checking parameters become available. For more information, see Collision Checking: Stock, Design, and Fixtures for Material Removal Simulation.
    2. Select the On design part check box to detect collisions between the tool/tool holder and the design part specified in the Part Operation Geometry tab.
    3. Select the On fixtures check box to detect collisions between the tool/tool holder and the fixtures specified in the Part Operation Geometry tab.
    4. Select the Collisions Checking with Machine Head. If the machine head is complex and the tool path size is large, collision checking may be long, especially with tight machining tolerance.

      • The machine head collision checking requires the machine kinematic so only the machine head mounted on MTB milling machine is supported. This includes machine heads on milling machines.
      • Generic and Mill turn machines are not supported.
      • Interchangeable head is not supported.
      • The system does not know what happened before the first point of the current operation and the machine configuration for the first point corresponds to the one resulting of a motion from the Home position to this first point. Therefore, the machine configuration for the first point may differ from the actual one resulting from previous operations and machine instructions.
      • If some tool path positions are not reachable, a warning is displayed Collision checking is not complete due to some unreachable positions.

      See Tool Collision Checking.
    5. Optional: Set offsets on the tool or tool assembly, which are used as safety distances.
    6. Set the Minimum depth collision detection value.
      Applying negative offsets on part surfaces, drive curves, or surfaces leads to the detection of too many collisions, with the display of unwanted warnings. Setting the Minimum depth collision detection enables you to set a threshold under which collisions are not detected nor displayed. While Minimum depth collision detection has no maximum value, it cannot be greater than the tool corner radius defined in the Machining Operation.

      By default, these values are set to 0mm.

  5. In Kinematics Checking:
    1. Select the Activate Kinematics Checking to consider Machine kinematics constraints at tool path computation time.
    2. Define the value of the Max Variation on Rotary DOF.

      By default, the Max Variation on Rotary DOF is set to 45.00 deg.

  6. Define the value of the Stocks Accuracy.

    The Stock Accuracy is the tolerance used to compute tessellations for material removal simulations.

    By default, the Stock Accuracy is set to 0.2 mm.

  7. Click to revert to the default value.

Activate the Generation of Transition Paths

Except for a mill-turn or a lathe machine, you can activate the generation of transition paths from the Transition Path tab.

  1. Select Transition Path .
  2. Select the Activate the generation Transition Paths check box.
    The icons used to specify the required geometry become available.

    Note: When the check box Generate Transition Path is:
    • Selected: The Manufacturing Program context menu items Generate Machine Rotations and Delete Generated Machine Rotations are not available. All the generated machine rotations are removed from the Activities Process Tree.
    • Cleared: The Manufacturing Program context menu items Generate Machine Rotations and Delete Generated Machine Rotations are available.
    • See Inserting Machine Rotations.
  3. Click Traverse Box Plane, then select five planes that define a global traverse box for the Part Operation.
  4. Click Transition Plane, then select the planes that are used as a global transition planes for the Part Operation.
  5. Click Rotary Plane, then select the planes that is used as a global rotary plane for the Part Operation.

Select the Milling Head Mount Point from a List

When you select a head, the available mount points are listed, then you can select one of those mounting points for the Part Operation.

  1. In the Activities Process Tree, right-click a Head Change operation.
  2. Select the required head from the list of available mount points, such as Mount_Point_1.
    Note: The machine simulation uses the selected head mount point and also checks reachability.

    See also Inserting Head Changes.