HM-4620: Create Rigid Walls, Model Data, Constraints, Cross Sections, and Output with LS-DYNA

In this tutorial you will: create *PART_INERTIA for the vehicle mass component, velocity on all nodes except barrier nodes with *DEFINE_BOX and *INITIAL_VELOCITY, a contact between the crash boxes, the bumper, and the barrier with *CONTACT_AUTOMATIC_GENERAL, and a stationary rigid wall; use *DATABASE_HISTORY_NODE to specify nodes to be output; use *DATABASE_CROSS_SECTION_PLANE to specify the output of resultant forces; and make nodes a part of the mass rigid body with *CONSTRAINED_EXTRA_NODES.

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

Overview of *PART_INERTIA, *CONSTRAINED_EXTRA_NODES, *DATABASE_CROSS_SECTION_(Option), and *RIGIDWALL

In this section, you will learn about *PART_INERTIA, *CONSTRAINED_EXTRA_NODES, *DATABASE_CROSS_SECTION_(Option), and *RIGIDWALL.

*PART_INERTIA

The INERTIA option enables inertial properties and initial conditions to be defined rather than calculated from the finite element mesh. This applies to rigid bodies only. When importing a LS-DYNA model into Engineering Solutions, the *PART_INERTIA IRCS parameter value is changed from 0 to 1. The inertia components are changed from global to local axis.

This allows inertia components to be automatically updated when *PART_INERTIA elements are translated or rotated. When selecting *PART_INERTIA elements to translate or rotate, select elements by comp. This selection method ensures the inertia properties are automatically updated.

*CONSTRAINED_EXTRA_NODES

This card defines extra nodes to be part of a rigid body. In Engineering Solutions, it is created from the Solver Browser or Model Browser, Create Cards menu (access from the Tools pull-down menu), or the Quick Access tool (Ctrl + F) when a keyword is entered.

*DATABASE_CROSS_SECTION_(Option)

*DATABASE_CROSS_SECTION_(Option) defines a cross section for resultant forces written to the ASCII SECFORC file. The options are PLANE and SET.

For the PLANE option, a cutting plane must be defined. For best results, the plane should cleanly pass through the middle of the elements, distributing them equally on either side.

The SET option requires the equivalent of the automatically generated input via the cutting plane to be identified manually and defined in sets. All nodes in the cross-section and their related elements contributing to the cross-sectional force resultants should be defined in sets.

*DATABASE_CROSS_SECTION_SET and *DATABASE_CROSS_SECTION_PLANE are created from the Solver Browser or Model Browser, Create Cards menu (access from the Tools pulldown menu), or the Quick Access tool (Ctrl + F) when a keyword is entered.

*RIGIDWALL

A *RIGIDWALL provides a method for treating contact between a rigid surface and nodal points of a deformable body.

In Engineering Solutions, *RIGIDWALL keyword cards are created from the Solver Browser or Model Browser, Create Cards menu (access from the Tools pull-down menu), or the Quick Access tool (Ctrl + F) when a keyword is entered.

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.

Import the LS-DYNA Model

In this step, you will import the LS-DYNA model file into Engineering Solutions.

  1. From the menu bar, click File > Import > Solver Deck.
    The Import - Solver Deck tab opens.
  2. In the File field, navigate to bumper_start.key.
  3. Click Import.

Define *PART_INERTIA

In this step, you will define *PART_INERTIA for the vehicle mass component to partially take into account the inertia properties and mass of the missing parts.

  1. In the Model Browser, Components folder, click vehicle mass.


    Figure 1.
    The Entity Editor opens, and displays the component's card data.
  2. In the Entity Editor, Edit the component's card data.
    1. Set Options to Inertia.
    2. For XC (X coordinate of center of mass), enter 700.
    3. For YC (Y coordinate of center of mass), enter 0.0.
    4. For ZC (Y coordinate of center of mass), enter 170.
    5. For TM (translational mass), enter 800.
    6. For IXX (XX component of target inertia), enter 1.5E+07.
    7. For IXY (XY component of target inertia), enter -5.0E+03.
    8. For IXZ (XZ component of target inertia), enter -8.0E+06.
    9. For IYY (YY component of target inertia), enter 5.0E+07.
    10. For IYZ (YZ component of target inertia), enter -900.
    11. For IZZ (ZZ component of target inertia), enter 6.0E+07.
    12. For VTX (Initial translational velocity of rigid body in x direction), enter -10.

Create a *DEFINE_BOX that Contains Non-Barrier Nodes

In this step, you will create a *DEFINE_BOX in Engineering Solutions that contains all nodes except barrier nodes.

  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 > *DEFINE > *DEFINE_BOX from the context menu.


    Figure 2.
    A new block opens in the Entity Editor.
  3. In the Entity Editor, define the block.
    1. For Name, enter box velocity.
    2. Optional: Click the Color icon, and select a color for the block.
    3. For Xmin Ymin Zmin, enter -530, -800, 0 as seen in Figure 3.


      Figure 3.
    4. For Xmax Ymax Zmax, enter 200, 800, 300 as seen in Figure 4.


      Figure 4.

Create Initial Velocity

In this tutorial, you will create initial velocity on all nodes except barrier nodes.

A velocity boundary condition can also be created on a set of nodes from the Solver Browser or Model Browser, Create Cards menu (access from the Tools pull-down menu), or the Quick Access tool (Ctrl + F) when a keyword is entered.
  1. In the Solver Browser, right-click and select Create > *INITIAL > *INITIAL_VELOCITY from the context menu.


    Figure 5.
    A new load opens in the Entity Editor.
  2. In the Entity Editor, define the load.
    1. For VX (Initial velocity in the global X direction), enter –10.
    2. Click BOXID, and then click Block.


      Figure 6.
    3. In the Select Block dialog, select box velocity and then click OK.


      Figure 7.

View the Nodes in the Node Entity Set

In this step, you will view the closest nodes which are in the pre-defined node entity set (*SET_NODES_LIST) named Constrain Vehicle using two methods.

  1. Method 1
    1. In the Solver Browser, SET folder, SET_NODE_LIST folder, right-click on Constrain Vehicle and select Review from the context menu.
      The set's nodes highlight as seen in Figure 8.


      Figure 8.
    2. Right-click on Constrain Vehicle and select Review from the context menu.
      The entities return to their original display color as seen in Figure 9.


      Figure 9.
  2. Method 2
    1. From the menu bar, click Tools > Edit > Sets.
    2. In the Entity Sets panel, click review.
    3. Set the display RLs/hide RLs toggle to hide RLs as seen in Figure 10.
      Note: This option filters all nodal rigid body sets from the list.


      Figure 10.
    4. Select the Constrain Vehicle set.
      The set's nodes highlight as seen in Figure 11.


      Figure 11.
    5. Close the panel by clicking return.

Create *CONSTRAINED_EXTRA_NODES_SET

In this step, you will create a *CONSTRAINED_EXTRA_NODES_SET.

  1. In the Solver Browser, right-click and select Create > *CONSTRAINED > *CONSTRAINED_EXTRA_NODES_SET from the context menu.


    Figure 12.
    A new constrained extra node opens in the Entity Editor.
  2. In the Entity Editor, define the constrained extra node.
    1. For Name, enter ExtraNodes.
    2. For PID, click Unspecified > Component.


      Figure 13.
    3. In the Select Component dialog, select vehicle mass and then click OK.


      Figure 14.

Define Nodes in the Constrain Vehicle

In this step, you will define the nodes in the Constrain Vehicle set to be a part of the vehicle mass rigid body.

In this step, the Entity Editor should be open for the ExtraNodes constrained extra node.
  1. For NSID, click Unspecified > Set.
  2. In the Select Set dialog, select Constrain Vehicle and then click OK.

View Extra Nodes of the Vehicle Mass Rigid Body

In this step, you will view the extra nodes that are a part of the vehicle mass rigid body.

  1. Review ExtraNodes by completing one of the following options:
    • In the Solver Browser right-click on ExtraNodes and select Review (press Q) from the context menu.
    • In the Model Browser right-click on ExtraNodes and select Review (press Q) from the context menu.
    The extra nodes temporarily display red, the PID (vehicle mass) displays blue, and all of the other entities temporarily display grey as seen in Figure 15.


    Figure 15.
  2. Return all of the entities to their original display color by right-clicking on ExtraNodes and selecting Review from the context menu.

Create an Entity Set

In this step, you will create an entity set, *SET_PART_LIST, for the vehicle mass component.

All other components not in this set will be included in the contact.
  1. In the Solver Browser, right-click and select Create > *SET > *SET_PART > *SET_PART_LIST from the context menu.
    Tip: You can also create a *SET_PART_LIST from the Model Browser, Create Cards menu (access from the Tools pull-down menu), or the Quick Access tool (Ctrl + F) when a keyword is entered.


    Figure 16.
    A new set opens in the Entity Editor.
  2. In the Entity Editor, define the set.
    1. For name, enter Exempt Parts.
    2. For Entity IDs, click 0 Components > Components.
    3. In the Select Components dialog, select vehicle mass and then click OK.

Create a *CONTACT_AUTOMATIC_GENERAL Contact

In this step, you will create a *CONTACT_AUTOMATIC_GENERAL contact.

  1. In the Solver Browser, right-click and select Create > *CONTACT > *CONTACT_AUTOMATIC_GENERAL from the context menu.


    Figure 17.
    A new group opens in the Entity Editor.
  2. For name, enter impact.

Define Secondary Surface

In this step, you will define the secondary surface with secondary set type 6, part set ID for exempted parts.

In this step the Entity Editor should be open for the impact group.
  1. Click SSID.
  2. Set the entity selector to Set.
  3. Click Set.
  4. In the Select Set dialog, select Exempt Parts and then click OK.
  5. Select the ExemptSlvPartSet checkbox.
    The SSTYPE (secondary surface type) value changes from 2 (part set ID) to 6 (part set ID for exempted parts) as seen in Figure 18.


    Figure 18.

Create an Entity Set

In this step, you will create an entity set, *SET_PART_LIST, to specify the elements that will contribute to the cross-sectional force results.

  1. In the Solver Browser, right-click and select Create > *SET > *SET_PART > *SET_PART_LIST from the context menu.


    Figure 19.
    A new group opens in the Entity Editor.
  2. In the Entity Editor, define the set.
    1. For Name, enter CrossSectionPlane-Parts.
    2. For Entity IDs, click 0 Components > Components.
    3. In the Select Components dialog, select interior crashbox and exterior crashbox.
    4. Click OK.

Define a Section

In this step, you will define a section by creating a *DATABASE_CROSS_SECTION_PLANE.

  1. In the Solver Browser, right-click and select Create > *DATABASE > *DATABASE_CROSS_SECTION_PLANE from the context menu.


    Figure 20.
    A new group opens in the Entity Editor.
  2. For Name, enter CrossSection_Plane.

Define the Location and Size of the Section Plane

In this step, you will define the location and size of the section plane.

In this step the planes origin (the tail of the normal vector) is defined by a base node. The Entity Editor should be open for the CrossSection_Plane cross section.
  1. Create a base node.
    1. Open the Create Nodes panel by clicking Geometry > Create > Nodes > XYZ from the menu bar.
      Tip: You can also open the Create Nodes panel by pressing F8.
    2. In the x field, enter -320.
    3. In the y field, enter -500.
    4. In the z field, enter 100.


      Figure 21.
    5. Click create.
      A new node displays as seen in Figure 22.


      Figure 22.
    6. Click return.
  2. In the Entity Editor, define the XTAIL, YTAIL, ZTAIL (base node) for the section.
    1. Click XTAIL, YTAIL, ZTAIL (base node), and then click .
    2. In the graphics area, select the base node you created in step 1 as seen in Figure 23.
      Note: If the base node is not visible, click on the Visualization toolbar to display elements as a wireframe (skin only).


      Figure 23.
    3. Click proceed.
      The Entity Editor displays the coordinates of the base node in the XTAIL, YTAIL, ZTAIL field as seen in Figure 24.


      Figure 24.
  3. Set Geometry type to Finite plane.
  4. Define the normal vector.
    1. Click Normal, and then click .
    2. In the panel area, set the orientation selector to x-axis.
    3. Click proceed.
  5. Define the edge vector.
    1. Click Edge, and then click .
    2. In the panel area, set the orientation selector to y-axis.
    3. Click proceed.
      The Entity Editor displays the coordinates of the edge vector L in the Normal field.
  6. For LENL (length of edge a, in the L direction), enter 100.
  7. For LENM (length of edge b, in the M direction), enter 200.
    Tip: If you know the coordinates of the base node, edge, and normal, you can manually enter them in the Entity Editor.


    Figure 25.

Specify the Parts Secondary to the Cross Section

In this step, you will specify the parts secondary to the cross section.

In this step the Entity Editor should be open for the CrossSection_Plane cross section.
  1. For PSID, click Unspecified > Set.
  2. In the Select Set dialog, select CrossSectionPlane-Parts and then click OK.

View the Entities Secondary to the Rigid Wall

In this step, you will view the entities secondary to the rigid wall.

  1. In the Solver Browser, right-click on CrossSection_Plane and select Review from the context menu.
    The secondary entities and rigid wall highlight and all of the other entities temporarily display grey as seen in Figure 26.


    Figure 26.
  2. Return the entities to their original display color by right-clicking on CrossSection_Plane and selecting Review from the context menu.

Create a *DEFINE_BOX that Contains Barrier and Bumper Nodes

In this step, you will create a *DEFINE_BOX containing the nodes making up the barrier and the left side of the bumper.

These nodes will be secondary to the rigid wall.
  1. In the Solver Browser, right-click and select Create > *DEFINE > *DEFINE_BOX from the context menu.


    Figure 27.
    A new block opens in the Entity Editor.
  2. In the Entity Editor, define the block.
    1. For Name, enter half model.
    2. Optional: Click the Color icon and select a color to display the block.
    3. For Xmin Ymin Zmin, enter -600, -800, 0.
    4. For Xmax Ymax Zmax, enter -460, 0, 400.


      Figure 28.

Create a *RIGIDWALL_PLANAR_FINITE

In this step, you will define a Engineering Solutions group by creating *RIGIDWALL_PLANAR_FINITE.

*RIGIDWALL are created from the Solver Browser or Model Browser, Create Cards menu (access from the Tools pull-down menu), or the Quick Access tool (Ctrl + F) when a keyword is entered.
  1. In the Solver Browser, right-click and select Create > *RIGIDWALL > *RIGIDWALL_PLANAR_FINITE from the context menu.


    Figure 29.
    A new rigid wall opens in the Entity Editor.
  2. For Name, enter wall.

Define the Location and Size of the Rigid Wall

In this step, you will create a node from the create nodes panel and then select it for the base node.

In the Create Nodes panel, XYZ sub-panel, the rigid wall’s origin (the tail of the normal vector) is defined by a base node. In this step the Entity Editor should be open for the rigid wall
  1. Create a base node.
    1. Open the Create Nodes panel by clicking Geometry > Create > Nodes > XYZ from the menu bar.
      Tip: You can also open the Create Nodes panel by pressing F8.
    2. Click to open the XYZ subpanel.
    3. In the x field, enter -600.
    4. In the y field, enter -750.
    5. In the z field, enter 90.
    6. Click create.
      Tip: If the base node is not visible, click on the Visualization toolbar to display elements as a wireframe (skin only).
    7. Click return.
  2. For XT, YT, and ZT enter -600, -750, and 90 as seen in Figure 30.
    Note: You can also select the node created in step 1 for the rigid wall base.


    Figure 30.
  3. Set Geometry type to Finite plane.
  4. Define the normal vector.
    1. Click Normal, and then click .
    2. In the panel area, set the orientation selector to x-axis.
    3. Click proceed.
  5. Define the edge vector.
    1. Click Edge, and then click .
    2. In the panel area, set the orientation selector to y-axis.
    3. Click proceed.
  6. For Length LENL, enter 165.
  7. For Length LENM, enter 250.
    Note: The input values for LENL and LENM are the length of the edges a and b in the L and M directions, respectively. These values define the extent of the rigid wall.


    Figure 31.

Specify Nodes as Secondary to the Rigid Wall

In this step, you will use the Entity Editor for the rigid wall to specify the nodes in the *DEFINE_BOX half model as secondary to the rigid wall.

In this step the Entity Editor should be open for the rigid wall
  1. Click BOXID > Block.
  2. In the Select Block dialog, select half model and then click OK.
  3. For FRIC (Interface friction), enter 1.0.

Specify Nodes to be Output

In this step, you will specify some nodes to be output to the ASCII NODOUT file with *DATABASE_HISTORY_NODE.

  1. In the Solver Browser, right-click and select Create > *DATABASE > *DATABASE_HISTORY_NODE from the context menu.


    Figure 32.
    A new output block opens in the Entity Editor.
  2. In the Entity Editor, define the output block.
    1. For Name, enter nodeth.
    2. For Entity IDs, click 0 Nodes > Nodes.
    3. In the graphics area, select a few nodes of interest as seen in Figure 33.


      Figure 33.
    4. Cick proceed.

Export the Model

In this step, you will export the model to an LS-DYNA 971_R# formatted input file.

  1. From the menu bar, click File > Export > Solver Deck.
    The Export - Solver Deck tab opens.
  2. Set File type to LsDyna.
  3. In the File field, navigate to your working directory and save the file as Bumper_complete.key.
  4. Click Export.

Submit the Input File

In this step, you will submit the LS-DYNA input file to the LS-DYNA 970 solver.

  1. From the Start Menu, open the LS-DYNA Manager program.
  2. From the solvers menu, select Start LS-DYNA analysis.
  3. Load the bumper_complete.key file.
  4. Start the analysis by clicking OK.

View the results in HyperView

In this step, you will view the results in HyperView.

This exercise is complete.
Save your work to a Engineering Solutions file.