Exercise 1: Define Model Data for the Seat Impact Analysis

In this step, you will load the LS-DYNA user profile in Engineering Solutions.

1. Start Engineering Solutions Desktop.
2. In the User Profile dialog, set the user profile to LsDyna.

In this step, you will open the model file in Engineering Solutions.

1. Open the 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 seat_start.hm file.
   The model appears in the graphics area.
3. Observe the model using various visual options available in HyperMesh, such as rotation and zooming.

In this step, you will create an XY plot.

1. Open the Plots panel by clicking XYPlots > Create > Plots from the menu bar.
2. In the plot= field, enter seat_mat.
3. Set plot type to standard as seen in Figure 2.

   
   
   Figure 2.

4. Leave the like = field empty.
   When an existing plot is selected, the new plot adopts its attributes.
5. Click create plot.
6. Click return.

In this step, you will input data from a file to create two stress-strain curves.

1. Open the Read Curves panel by clicking XYPlots > Create > Curves > Read Curves from the menu bar.
2. Leave the plot = field set to seat_mat.
3. Click browse.
4. In the Open dialog, open the seat_mat_data.txt file.
5. Click input.
   Engineering Solutions creates two curves, and names them 0.001 and 0.004 as seen in Figure 3.

   
   
   Figure 3.

6. Click return.

In this step, you will create a dummy XY curve to be used to create a *DEFINE_TABLE.

1. Open the Edit Curves panel by clicking XYPlots > Edit > Curves from the menu bar.
2. Open the create subpanel.
3. Click plot =, and select seat_mat.
4. Select math.
5. In the x = field, enter {0.0, 0.2}.
6. In the y = field, enter {0.4, 0.4}.

   
   
   Figure 4.

7. Click create.
   Engineering Solutions creates a curve in the seat_mat plot, and names it curve3 as seen in Figure 5.

   
   
   Figure 5.

8. Click return.

In this step, you will create a *DEFINE_TABLE from the dummy curve created in Create a Dummy XY Curve.

1. In the Model Browser, Curve folder, click curve3.

   
   
   Figure 6.

   The Entity Editor opens, and displays the curve's corresponding data.
2. Select the DEFINE_TABLE checkbox.
3. For ArrayCount, enter 2.
   Note: This is the number of strain rate values to be specified.
4. In the Data: VALUE row, click .
5. In the ArrayCount dialog, enter 0.001 in the strain rate VALUE(1) field and 0.004 in the strain rate VALUE(2) field.

   
   
   Figure 7.

6. In the CurveId(1) field, click Unspecified > Curve.

   
   
   Figure 8.

7. In the Select Curve dialog, select curve1 and then click OK.

   
   
   Figure 9.

8. In the CurveId(2) field, click Unspecified > Curve.
9. In the Select Curve dialog, select curve2 and then click OK.
10. Click Close.

    
    
    Figure 10.

In this step, you will create a non-linear material (*MAT_PIECEWISE_LINEAR_PLASTICITY).

1. Open the Solver Browser by clicking View > Browsers > Engineering Solutions > Solver from the menu bar.
2. In the Solver Browser, right-click and select Create > *MAT > MAT (1-50) > 24-*MAT_PIECEWISE_LINEAR_PLASTICITY from the context menu.

   
   
   Figure 11.

   Engineering Solutions creates and opens a new material in the Entity Editor.
3. For Name, enter steel.
4. For Rho (Mass density), enter 7.8 E-6.
5. For E (Young modulus), enter 200.
6. For PR (Poisson ratio), enter 0.3.
7. For SIGY (Yield stress), enter 0.25.
8. Click LCSS and then click curve.

   
   
   Figure 12.

9. In the Select Curve dialog, select curve3 and then click OK.

   
   
   Figure 13.

In this step, you will update the base_frame and back_frame components with the non-linear material created in Create a Non-Linear Material.

1. Enable the Quick Access Tool by pressing Ctrl > F.
2. In the Quck Access Tool, enter Utility Component Table and press Enter.
   The Components and Properties dialog opens.
3. In the Components and Properties dialog, click Table > Editable from the menu bar as seen in Figure 14.

   
   
   Figure 14.

4. Assign the material steel to the base_frame and back_frame components.
   1. Select the base_frame component.
   2. Set Assign Values to Material name.
   3. Set HM-Mats to steel.
   4. Click Set.
   5. In the Confirm dialog, click Yes.
   6. Repeat steps 4.a through 4.e for the back_frame component.
   The Material name for base_frame and back_frame is set to steel as seen in Figure 15.

   
   
   Figure 15.

5. From the menu bar, click Table > Quit.

In this step, you will create a beam element, *ELEMENT_BEAM, to complete the seat's back_frame connection to the side_frame on the left side.

1. Restore a pre-defined view.
   1. In the Model Browser, Views folder, right-click on Beam_view and select Show from the context menu.
2. Set the current component to beams.
   1. In the Model Browser, Component folder, right-click on beams and select Make Current from the context menu.
      Engineering Solutions sets the beam component as the current collector.
3. Create the beam element.
   1. Open the Bars panel by clicking Mesh > Create > 1D Elements > Bars from the menu bar.
   2. Under orientation, select node.
      Note: You will select a direction node later to define the beam’s section orientation.
   3. Using the node A selector, select the center node of the left nodal rigid body as seen in Figure 16.

      
      
      Figure 16.

   4. Using the node B selector, select the center node of the right nodal rigid body as seen in Figure 17.

      
      
      Figure 17.

   5. Using the direction node selector, select any non-center node on one of the nodal rigid bodies.
      Engineering Solutions creates the beam as seen in Figure 18.

      
      
      Figure 18.

   6. Click return.

In this step, you will display node IDs.

1. Click on the Display toolbar.
   The Numbers panel opens.
2. Set the entity selector to nodes.
3. Click nodes > by id.
4. In the id= field, enter 425-427, 431.
5. Press Enter.
6. Select the display checkbox.
7. Click on.
   Engineering Solutions displays the IDs as seen in Figure 19.

   
   
   Figure 19.

8. Click return.

In this step, you will set the current component to welding.

In this step, you will select the rgdbody type for theEngineering Solutions rigid configuration.

1. Click Mesh > Assign > Element Type from the menu bar.
   The Element Type panel opens.
2. Select the elements to update.
   1. Click rigid =, and then select RgdBody.
3. Click update.
4. Click return.

In this step, you will create the nodal rigid body (*CONSTRAINED_NODAL_RIGID_BODY).

1. In the Solver Browser, right-click and select Create > *CONSTRAINED > *CONSTRAINED_NODAL_RIGID_BODY > *CONSTRAINED_NODAL_RIGID_BODY from the context menu.
2. In the Rigids panel, set the nodes 2-n selector to multiple nodes.
3. Using the node1 selector, select the beam’s free end as seen in Figure 20.

   
   
   Figure 20.

4. Click nodes 2-n: nodes > by id.
5. In the id= field, enter 425, 426, 427 and 431.
6. Press Enter.

   
   
   Figure 21.

7. Unselect the attach nodes as set checkbox.
8. Click create.
   Engineering Solutions creates the nodal rigid body as seen in Figure 22.

   
   
   Figure 22.

9. Click return.
   Engineering Solutions does not create *CONSTRAINED_JOINT_STIFFNESS; it is not needed for this joint to work.

In this step, you will display node IDs.

1. On the Visualization toolbar, click to display the model's elements as wireframe elements skin only.
2. Open the Numbers panel.
3. Set the entity selector to nodes.
4. Click nodes > by id.
5. In the id= field, enter 1635, 1636.
6. Press Enter.
7. Select the display checkbox.
8. Click on.
   Engineering Solutions displays the IDs as seen in Figure 23.

   
   
   Figure 23.

9. Click return.

In this step, you will activate coincident picking from the graphics panel.

1. Click Preferences > Graphics from the menu bar.
   The Graphics panel opens.
2. Select the coincident picking checkbox.
3. Click return.

In this step, you will set the joint component as the current collector.

In this step, you will create a joint between two nodal rigid bodies (*CONSTRAINED_JOINT_REVOLUTE).

1. In the Solver Browser, right-click and select Create > *CONSTRAINED > *CONSTRAINED_JOINT_REVOLUTE > *CONSTRAINED_JOINT_REVOLUTE from the context menu.
2. In the Joints panel, set joint type to revolute.
3. Using the node 1 selector, click node 1635.
   The coincident picking mechanism displays the nodes 1635 and 1633 as seen in Figure 24.

   
   
   Figure 24.

4. From the coincident picking mechanism, click node 1635.
   Engineering Solutions selects node 1635 for node 1 in rigid body A.
5. Using the node 2 selector, select the node created in step 4.
   The coincident picking mechanism displays two nodes: 1635 and 1633.
6. From the coincident picking mechanism, click node 1633.
   Engineering Solutions selects node 1633 for node 2 in rigid body B.
7. Using the node 3 selector, click node 1636.
   The coincident picking mechanism displays two nodes: 1636 and 1634.
8. From the coincident picking mechanism, click node 1636.
   Engineering Solutions selects node 1636 for node 3 in rigid body A.
9. Using the node 4 selector, select the node created in step 8.
   The coincident picking mechanism displays two nodes: 1636 and 1634.
10. From the coincident picking mechanism, click node 1634.
    Engineering Solutions selects node 1634 for node 4 in rigid body B.
11. Click create.
    Engineering Solutions creates the joint as seen in Figure 25.

    
    
    Figure 25.

12. Click return.

In this step, you will define *DEFORMABLE_TO_RIGID to set up the moving seat as rigid until the time of impact with the block, to reduce computation time.

1. Create an entity set that contains the base_frame, back_frame, and cover components.
   1. In the Solver Browser, right-click and select Create > *SET > *SET_PART > *SET_PART_LIST from the context menu.

      
      
      Figure 26.

      Engineering Solutions creates and opens a new set in the Entity Editor.
   2. For Name, enter set_part_seat.
   3. For Entity IDs, click 0 Components > Components.

      
      
      Figure 27.

      The Select Components dialog opens.
   4. In the Select Components dialog, select base_frame, back_frame, and cover and then click OK.

      
      
      Figure 28.

2. Define *DEFORMABLE_TO_RIGID to switch the deformable seat to rigid at the beginning of the analysis.
   1. In the Solver Browser, right-click and select Create > *DEFORMABLE_TO_RIGID > *DEFORMABLE_TO_RIGID from the context menu.

      
      
      Figure 29.

      Engineering Solutions creates and opens a new load collector in the Entity Editor.
   2. For Name, enter dtor.
   3. For ArrayCount, select 1.
   4. For PSID, click Unspecified > Set.

      
      
      Figure 30.

      The Select Set dialog opens.
   5. In the Select Set dialog, select set_part_seat and then click OK.
   6. For MRB, click Unspecified > Component.
   7. In the Select Component dialog, select rigid block and then click OK.
3. Define *DEFORMABLE_TO_RIGID_AUTOMATIC to switch the rigid seat to deformable when contact between the seat and block is detected.
   1. In the Solver Browser, right-click and select Create > *DEFORMABLE_TO_RIGID > *DEFORMABLE_TO_RIGID_AUTOMATIC from the context menu.

      
      
      Figure 31.

      Engineering Solutions creates and opens a new load collector in the Entity Editor.
   2. For Name, enter dtor_automatic.
   3. For SWSET (set number of this automatic switch set), enter 1.
   4. Set CODE (activation switch code) to 0: Switch takes place at time 1.
   5. For TIME1, enter 175.
      Note: The switch will not take place before this time.
   6. For R2D, select 1.
      Note: On export, the number of rigid parts to be switched to deformable is written to the R2D field (card 2, field 6). This number is based on the number of parts in the entity set you select next.
   7. Click PSID > Set.
      Note: PSIDR2D is the part ID of the part which is switched to a rigid material.

      
      
      Figure 32.

      The Select Set dialog opens.
   8. In the Select Set dialog, select set_part_seat and then click OK.