# Exercise 2: Define Boundary Conditions and Loads for the Head and A-Pillar Impact Analysis

In this exercise, you will define LS-DYNA boundary conditions, loads, and contacts in Engineering Solutions. Also, you will set up the boundary conditions and load data for a LS-DYNA analysis of a hybrid III dummy head impacting an A-pillar.

The head and A-pillar are 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 Engineering Solutions model file.

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 head_2.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 a Node Set

In this step, you will create a node set, *SET_NODE_LIST, which will contain all of the nodes in the head component of the model.

1. In the Solver Browser, right-click and select Create > *SET > *SET_NODE > *SET_NODE_LIST from the context menu.
Engineering Solutions creates and opens a new set in the Entity Editor.
2. For Name, enter Vel_Nodes.
3. For Entity IDs, click 0 Nodes > Nodes.
4. In the panel area, click nodes > by collector.
5. Select the head component checkbox as seen in Figure 4.
6. Click select.
7. Click proceed.

## Define the Velocity

In this step, you will define the velocity for the model.

1. In the Solver Browser, right-click and select Create > *INITIAL > *INITIAL_VELOCITY from the context menu.
Engineering Solutions creates and opens a new load collector in the Entity Editor.
2. Click NSID (Node Set ID), and then select Set.
3. In the Select Set dialog, select Vel_Nodes and then click OK.
4. For VX (x-component of mass center of velocity), enter 5.

In this step, you will create a load collector for the constraints to be created.

1. In the Model Browser, right-click and select Create > Load Collector from the context menu.
Engineering Solutions creates and opens a new load collector in the Entity Editor.
2. For Name, enter SPC.
3. Optional: Click the Color icon, and select a color to display the load collector.
4. Set card image to <None>.

## Create Constraints on the Pillar's End Nodes

In this step, you will create constraints on the ends of the pillar component of the model.

1. In the Solver Browser, right-click and select Create > *BOUNDARY > *BOUNDARY_SPC_NODE from the context menu.
A new constraint load is created and opened in the Entity Editor.
2. Click NSID (Node Set ID) and then select nodes for SPC.
3. Verify all six DOF (degree of freedom) checkboxes are selected.
4. Verify the load type is set to *BOUNDARY_SPC.
5. Review the Constraints created on the pillar's end nodes by right-clicking and selecting Plot Loads and Vector in the context menu.

## Define a *SET_SEGMENT for the Secondary Entities

In this step, you will create a new contactsurf on the pillar element of the model.

1. In the Solver Browser, right-click and select Create > *SET > *SET_SEGMENT > *SET_SEGMENT from the context menu.
Engineering Solutions creates and opens a new contactsurf in the Entity Editor.
2. For Name, enter pillar_secondary.
3. Optional: Click the Color icon, and select a color to display the contactsurf.
4. For Elements, click 0 Elements > Elements.
5. In the panel area, set the second switch to elems as seen in the following image.
6. Click elems > by collector.
7. Select the pillar checkbox as seen in the following image.
8. Click select.
10. Review the contactsurf to make sure that the pyramids are pointing out of the pillar as seen in Figure 11.

## Define a *SET_SEGMENT for the Main Entities

In this step, you will create a contactsurf on the head component of the model.

1. In the Solver Browser, right-click and select Create > *SET > *SET_SEGMENT > *SET_SEGMENT from the context menu.
Engineering Solutions creates and opens a new contactsurf in the Entity Editor.
3. Optional: Click the Color icon, and select a color to display the contactsurf.
4. For Elements, click 0 Elements > Elements.
5. In the panel area, set the first switch to add solid faces.
6. Set the second switch to elems.
7. Click elems > by collector.
8. Select the head checkbox as seen in the following image.
9. Click select.
10. Use the nodes selector to select three nodes that belong to the same face of a solid element.
11. In the face angle field, enter 30.
13. Review the contactsurf to make sure that its pyramids are pointing out of the head as seen in Figure 13.

## Create a Engineering Solutions Group

In this step, you will create a Engineering Solutions group with the SurfaceToSurface card image.

1. In the Solver Browser, right-click and select Create > *CONTACT > *CONTACT_SURFACE_TO_SURFACE > *CONTACT_SURFACE_TO_SURFACE from the context menu.
Engineering Solutions creates and opens a new group in the Entity Editor.
2. For Name, enter contact.

## Add the Slave and Master Contactsurfs to the Engineering Solutions Group

In this step, you will add the slave and master contactsurfs to the Engineering Solutions group.

In this step, the Entity Editor should be open for the contact group.
1. In the Entity Editor, click MSID and set the entity selector to Contactsurfs.
2. Click Contactsurfs.
3. In the Select Contactsurfs dialog, select head_master and then click OK.
4. Click SSID, and set the entity selector to Contactsurfs.
5. Click Contactsurfs.
6. In the Select Contactsurfs dialog, select pillar_slave and then click OK.

## Edit the Group card image

In this step, you will define the automatic option for the group in Engineering Solutions.

In this step, the Entity Editor should still be open for the contact group.
In the Entity Editor, for the first Options parameter, select Automatic.

## Review the Group Main and Secondary Surfaces

In this step, you will review the main and secondary surfaces for the group.

1. Click interfaces from the Analysis page as seen in the following image.
The Interfaces panel opens.