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

In this step you will open the LS-DYNA user profile.

1. Start HyperMesh Desktop.
2. In the User Profile dialog, set the user profile to LS-DYNA, Keyword971_R8.0.

In this step you will open the model file, seat_deformer.hm.

1. From the menu bar, click File > Open > Model.
2. In the Open Model dialog, navigate to your working directory and open the file, seat_deformer.hm

In this step you will position the dummy to its H-Point location.

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 to activate the global positioning parameters in the Entity Editor.

   
   
   Figure 2.

3. In the Entity Editor, for the Global rotation attribute Rx, type 180.
   The dummy rotates.
4. Under H-Point location, click on the coordinates area and then click .

   
   
   Figure 3.

5. In the graphics area, select the node tagged as H-Point Location on the seat.

   
   
   Figure 4.

6. In the panel area, click proceed.
   The dummy automatically moves to the selected H-Point location.

   
   
   Figure 5.

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.

Figure 6.

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 7.

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 the following image and click OK.

      
      
      Figure 8.

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 9.

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 following components as displayed in the image below.

      
      
      Figure 10.

   4. Click proceed when finished.
6. In the Dummy dislacement Direction field, type -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, type 1.0 mm/ms.
9. In the Dummy Displacement Step field, type 20.0 mm.
10. In the Imposed Contact Thickness field, type 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 and ready to be solved by the solver.

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

When the seat deformer model has been solved by the solver, you should find the d3plot files to visualize the animations in HyperView. The displacement fields on the seat should look similar to the images below.

Figure 11.

Check also that LS-DYNA has written out the dynain file, which 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).

To update the initial model with the simulation results, proceed as follows:

1. If you have closed the Pre-Simulation (Seat Deformer) tool, re-open it.
2. Verify that the Import *INITIAL_STRESS_SOLID checkbox is enabled. By default, this checkbox is enabled in order to update the solid elements with the initial stress values coming from the simulation results.
3. Click Import dynain File, then select the resulting 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 will look similar to the image below.

   
   
   Figure 12.