HM-4650: Seat Deformer with LS-DYNA Pre-Simulation

In this tutorial, you will learn how to setup a LS-DYNA model to simulate the seat deformation under the dummy.

Before you begin, copy from <>/interfaces/lsdyna/ to your working directory.

The driver seat and environment used in this tutorial are based on the LS-DYNA Toyota Yaris model, provided on the National Crash Analysis Center (NCAC) website.

The LS-DYNA dummy model used in this tutorial is a release version of the THOR-Mod Kit/Metric crash test dummy with SD3 shoulder posted on the NHTSA website.

Load the LS-DYNA Profile

In this step, you will load the LS-DYNA profile in HyperMesh.

  1. Start HyperMesh Desktop.
  2. In the User Profiles dialog, set the user profile to LsDyna.
  3. Set the template drop-down to Keyword971_R8.0.

Retrieve and View the Model File

In this step, you will open the model file and view it in HyperMesh.

  1. Open a model file by completing one of the following options:
    • Click File > Open > Model from the menu bar.
    • Click on the Standard toolbar.
  2. In the Open Model dialog, open the file.
The model appears in the graphics area.

Figure 1.

Position the Dummy to its H-Point Location

In this step, you will move the dummy to its H-Point Location on the seat.

  1. From the menu bar, click Tools > Dummy to open the Dummy Browser.
  2. In the Dummy Browser, click on the THOR_FE dummy entity.

    Figure 2.
    The global positioning parameters are activated in the Entity Editor.
  3. For Rx, under Global rotation, enter 180.
    The dummy rotates.
  4. Under H-Point location, click on the coordinates area and then click .
  5. In the graphics area, select the node tagged as H-Point Location on the seat as seen in Figure 3.

    Figure 3.
  6. In the panel area, click proceed.
    The dummy automatically moves to the selected HPoint location as seen in Figure 4.

    Figure 4.

Generate the Seat Deformer Model

In this step, you will generate the Seat Deformer model for the LS-DYNA simulation.

After positioning the dummy to its H-Point location on the seat, intersections between the dummy and seat foam parts occur as seen in Figure 5.

Figure 5.
The Seat Deformer tool enables you to export an input deck, for the appropriate solver, in order to simulate the deformation of the seat under the dummy. The simulation result files are then imported to update the initial FE model, and thus remove the intersections and penetrations between the dummy and the seat.

Figure 6.
  1. Open the Seat Deformer tool from the menu bar by clicking Tools > Pre- Simulation(Seat Deformer).
  2. In the PreSimulation dialog, under PreSimulation Set-Up, set Unit System to mm,ms,kg.
  3. Select the dummy components penetrating the seat foam.
    1. In the Dummy field, click 0 Components > Components.
    2. In the Select Components dialog, select the components shown in Figure 7 and click OK.

      Figure 7.
  4. Select the seat mechanism.
    1. In the Seat field, switch the selector to Mechanisms.
    2. Click 0 Mechanisms > Mechanisms.
    3. In the Select Mechanisms dialog, select Driver_Seat and click OK.
      Note: By selecting a mechanism, only the components defined in the bodies will be taken into account. The nodes will not be taken into account. In this example, the Seat_Cushion body is composed of a set of components and a set of nodes. The nodes will not be taken into account in the process.

      Figure 8.
  5. Select the fixed nodes of the seat.
    1. In the Fixed Nodes Of Seat field, click 0 Nodes > Nodes.
    2. In the panel area, click nodes > by collector.
    3. Select the components depicted in Figure 9.

      Figure 9.
    4. Click proceed.
  6. In the Dummy Displacement Direction field, enter -0.3, 0, -0.7.
  7. In the Export File field, specify the file path and name of your working directory.
  8. In the Dummy Velocity field, enter 1.0 mm/ms.
  9. In the Dummy Displacement Step field, enter 20.0 mm.
  10. In the Imposed Contact Thickness field, enter 1.0 mm.
  11. Click Export to start the export process of the LS-DYNA seat deformer pre-simulation input deck.
The LS-DYNA model is exported to the given location. The LS-DYNA model is ready to be solved by the solver.

Review Simulation Results and Update the Model

In this step, you will review the seat deformer simulation results and update the initial model in HyperMesh.

  1. Review the simulation results.
    1. Find the d3plot files in HyperMesh to visualize the animations.
      The displacement fields on the seat should look similar to Figure 10.

      Figure 10.
    2. Ensure LS-DYNA has written out the dynain file.
      The dynain file contains the new coordinates of the seat nodes at the end of the simulation as well as the *INITIAL_STRESS cards for the different type of elements present in the seat model (beam/shell/solid).
  2. Update the initial model.
    1. Optional: Open the Pre-Simulation(Seat Deformer) tool if it is closed.
    2. Verify the Import *INITIAL_STRESS_SOLID checkbox is enabled.
      The Import *INITIAL_STRESS_SOLID checkbox updates the solid elements with the initial stress values coming from the simulation results.
    3. Click Import dynain File.
    4. Select the dynain file of the seat deformer simulation.
      Default updates the node coordinates of the seat and the solid elements with their corresponding initial stress card. The resulting updated model should look similar to Figure 11.

      Figure 11.