Remove the Build Tray and Supports

Remove the build tray and the support structures, leaving only the completed bridge part.

Removal of the build tray and printed supports completes the additive manufacturing part. This is comparable to removing extra material at the inlets and vents in a cast part or trimming excess material from a stamped part. You cannot use the part until these extra pieces are gone. Detaching the part from the tray also reveals any significant residual stresses since the part is free to deform.

Model change is the process you use to define portions of a model that are being added to or removed from some simulation steps. You can use model change to simulate additive or traditional manufacturing processes. For example, you could simulate the machining of a cast part.

Here, you will define a static step and use model change to remove the build tray and then to remove the 14 supports that were required to manufacture the bridge.

This task shows you how to:

Define the Static Step to Remove the Build Tray

  1. From the Procedures section of the action bar, click Static Step .
  2. Name the static step Static Step_Remove_BuildTray.
  3. Enter a step time, initial time increment, and maximum time increment of 1s.
  4. Click OK.
  5. From the Structural Restraints & Loads section of the Assistant, click Clamp .
  6. Select the two faces of the bridge parallel to the global xz plane.

    A clamp is added to these faces to prevent free body motion since the part was constrained by the build tray and supports that are being removed.

    The Support field indicates that two faces are selected.

  7. Click OK.
  8. From the Interactions section of the action bar, click Model Change Manager .
  9. Click Add .
    The Model Change dialog box opens.
  10. From the Support options, select Mesh part as the selection method.
  11. From the selection tree, select Sweep_3D_buildtray, and click OK.
  12. From the Model Change dialog box, click OK.

    The build tray is shown in the Model Change Manager as a component that you can change in the simulation model. It is active in all steps.

  13. Clear Sweep_3D_buildtray from the Static Step_Remove_Buildtray column.

    By clearing the check box, you are deactivating the build tray for the selected step and any subsequent steps.

  14. Click OK.
  15. From the tree, right-click Structural Analysis Case.1 > Static Step_Remove_Buildtray > Prescribed Temperature.2, and click Remove Prescribed Temperature.2 in Static Step_Remove_Buildtray.

Define the Static Step to Remove the Supports

  1. From the Procedure section of the action bar, click Static Step .
  2. Name the static step Static Step_Remove_Support.
  3. Enter a step time, initial time increment, and maximum time increment of 1s.
  4. Click OK.
  5. From the Interactions section of the action bar, click Model Change Manager .
  6. Click Add .
    The Model Change dialog box opens.
  7. From the tree, select FEM_AM > Nodes and Elements > Hex_Mesh_Bridge_Structure > Supports as Supports, and click OK.
  8. Clear Supports from the Static Step_Remove_Support column.
  9. Click OK.
  10. From the Structural Restraints & Loads section of the Assistant, click Clamp .
  11. Select the bottom surface of the center pillar of the bridge part.
    Tip: You can temporarily disable the view of surfaces or components to work with other objects that are behind them. Select any face or edge of the component you want to disable, and press F7 to disable the entire component. Select the 3D space, and press F8 to restore all disabled items.


  12. Click OK.

    A new clamp is created to replace the one previously defined to control the location of the bridge part. You will remove the previously defined clamp and other restraints in the next steps.

  13. From the tree, right-click Structural Analysis Case.1 > Static Step_Remove_Support > Clamp.2, and click Remove Clamp.2 in Static Step_Remove_Support.
    The clamp is removed from the Static Step_Remove_Support.
  14. From the tree, right-click Structural Analysis Case.1 > Static Step_Remove_Support > Fixed_Displacement_X, and click Remove Fixed_Displacement_X in Static Step_Remove_Support.
  15. Repeat Step 14 to remove Fixed_Displacement_Y and Fixed_Displacement_Z.
    The fixed displacements are removed from the Static Step_Remove_Support.
  16. From the Standard section of the action bar, click Feature Manager , and select Scenario .

    The scenario view of the Feature Manager is shown below.



    The Feature Manager displays the contributing parts, scenario features, and results plots. You can edit, delete, locate, and hide or show features and plots.

    Note: The row highlighted in yellow indicates an amplitude was applied on an entry using nonstandard units. You must take care with units when using amplitudes. The 3DEXPERIENCE platform converts units before performing other operations. This can result in unintended values when the amplitude is applied. In this case, we used Kelvin throughout the example and will use the same units to solve the simulation; therefore, there will be no issue and we can ignore this warning.