Exercise 1: Define Model Data for the Seat Impact Analysis

In this exercise, you will define and review model data for a LS-DYNA analysis of a vehicle seat impacting a rigid block. The seat and block model is shown in Figure 1.

This exercise will help you become familiar with defining an LS-DYNA model data in Engineering Solutions. The model used in this exercise is depicted in Figure 1.

Load the LS-DYNA User Profile

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.

Retrieve the Engineering Solutions File

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.

Create an XY Plot

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.
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.

Create Two Stress-Strain Curves

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.
6. Click return.

Create a Dummy XY Curve

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

Create a *DEFINE_TABLE

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.
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.
6. In the CurveId(1) field, click Unspecified > Curve.
7. In the Select Curve dialog, select curve1 and then click OK.
8. In the CurveId(2) field, click Unspecified > Curve.
9. In the Select Curve dialog, select curve2 and then click OK.
10. Click Close.

Create a Non-Linear Material

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

Update the Components with the New Material

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

Create a Beam Element

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.
4. Using the node B selector, select the center node of the right nodal rigid body as seen in 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.
6. Click return.

Display Node IDs

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.
8. Click return.

Set the Current Component to Welding

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

In the Model Browser, Components folder, right-click on welding and select Make Current from the context menu.
Engineering Solutions sets the welding component as the current collector.

Select the RgdBody Type for the Rigid Configuration

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.

Create the Nodal Rigid Body

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.
4. Click nodes 2-n: nodes > by id.
5. In the id= field, enter 425, 426, 427 and 431.
6. Press Enter.
7. Unselect the attach nodes as set checkbox.
8. Click create.
Engineering Solutions creates the nodal rigid body as seen in Figure 22.
9. Click return.
Engineering Solutions does not create *CONSTRAINED_JOINT_STIFFNESS; it is not needed for this joint to work.

Display Node IDs

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.
9. Click return.

Activate Coincident Picking

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.

Set the Current Component to Joint

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

In the Model Browser, Components folder, right-click on joint and select Make Current from the context menu.
Engineering Solutions sets the joint component as the current collector.

Create a Revolute Joint

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

Rigid bodies must share a common edge along which to define a joint. This edge, however, must not have nodes merged together. Two rigid bodies will rotate relative to each other along the axis defined by the common edge.
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.
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.
12. Click return.

Define *DEFORMABLE_TO_RIGID

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

Review Component Data

In this section, you will review the model’s component data using the Model Browser, Solver Browser, or Component Table tool.

Method 1: Use the Model Browser

In this section, you will review the model's component data using the Model Browser.

1. Display only parts of the model with a particular material and section.
1. In the Model Browser, click .
2. Right-click on steel and select Isolate from the context menu.
Engineering Solutions only displays the components that have the selected material assigned.
3. Click , select a material, and scroll through the material using the up and down arrow keys in the Model Browser to review the materials.
The corresponding parts are automatically isolated in the view.
4. In the Model Browser click .
5. Right-click on shell section and select isolate from the context menu.
Engineering Solutions only displays the components that have the selected section assigned.
2. Display all components.
1. In the Model Browser, click .
3. Rename a part.
1. Right-click on the part you would like to rename, and then select rename from the context menu.
2. In the editable field, enter a new name for the entity.
The part's new name changes in the Solver Browser and the Model Browser.
4. Renumber a part ID.
1. In the Model Browser, click on a part's ID field.
The ID field becomes editable.
2. Enter a number that does not conflict with the existing part IDs, and then press Enter.

Method 2: Use the Solver Browser

In this section, you will review the model's component data using the Solver Browser.

1. Display only parts with a particular material.
1. In the Model Browser, Materials folder, right-click on Steel and select Isolate from the context menu.
2. In the Solver Browser, *SECTION folder, select components based on properties.
2. Display all components.
1. In the Solver Browser, click the *MAT folder.
3. Rename a part.
1. In the Solver Browser, select the part you would like to rename.
The Entity Editor opens, and displays the part's corresponding data.
2. Select Name, and enter a new name for the part.
The part's new name changes in the Solver Browser and the Model Browser.
4. Renumber a part ID.
1. In the Solver Browser, select the part you would like to change the ID of.
The Entity Editor opens, and displays the part's corresponding data.
2. For ID, enter a new ID for the part.
The part's new ID changes in the Solver Browser and Model Browser.

Method 3: Use the Component Table

In this section, you will review the model's component data using the component table.

1. Display only parts with a particular material.
1. Enable the Quick Access Tool by clicking Ctrl > F.
2. In the Quick Access Tool, enter Utility Component Table and press Enter.
The Components and Properties dialog opens.
3. In the Components and Properties dialog, click Display > By Material from the menu bar.
4. In the panel area, click mats.
5. Select the steel checkbox.
6. Click Select.
7. Click proceed.
The Component Table only displays the components with the material steel assigned. All other components are turned off.
2. Display all components.
1. From the menu bar, click Display > All.
The table displays all of the components in the model.
3. Rename a part.
1. From the menu bar, click Table > Editable.
Note: You can edit any of the columns that have a white background. For example, you can edit Part name, Part id and Thickness.
The table becomes editable.
2. Click any Part name field.
The field becomes editable.
3. In the Confirm dialog, click Yes.
The part's new name changes in the Solver Browser and the Model Browser.
4. Renumber a part ID.
1. From the menu bar, click Table > Editable.
The table becomes editable.
2. Click any Part Id field.
The field becomes editable.
3. Enter a new ID that does not conflict with any existing part IDs.
4. In the Confirm dialog, click Yes.
The part's new ID changes in the Solver Browser and the Model Browser.