HM-4700: Using the PAM-CRASH 2G Interface in HyperMesh

In this tutorial, you will: create Control Cards, boundary conditions, time histories, functions, and sensor cards; define materials, HyperMesh groups, and rigid walls; assign element types; and export a PAM-CRASH 2G data deck.

Before you begin, copy the rail-dyna.hm file from <hm.zip>/interfaces/pamcrash/ to your working directory.

Also, it is recommended that you complete the introductory tutorial, HM-1000: Getting Started with HyperMesh.

Load the PAM-CRASH User Profile

In this step, you will load the PAM-CRASH profile in HyperMesh.

  1. Start HyperMesh Desktop.
  2. In the User Profile dialog, set the user profile to Pamcrash.
  3. Set the subprofile to Pamcrash2G2012.
    Selecting the PAM-CRASH user profile and the Pamcrash2G2012 subprofile sets the FE input reader to PAM-CRASH 2G and loads the PAM-CRASH 2G 2012 FE output template. It also loads the PAM-CRASH 2G Utility menu, which contains numerous tools specific to this interface. The graphical user interface is tailored to PAM-CRASH 2G users.


    Figure 1.

Retrieve and View the Model File

In this step, you will open the model file and view it in HyperMesh.

The leg_geom.hm file contains IGES lines representing the layout of the leg and coordinate systems for bodies and joints.
  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 rail-dyna.hm file.
The model appears in the graphics area.


Figure 2.

Create Control Cards

In this step, you will create Control Cards for PAM-CRASH 2G.

The settings of the Control Cards influence the default values for defining materials. PAM-CRASH 2G decks cannot be executed without error if Control Cards are undefined.
  1. Define the title card.
    1. In the Solver Browser, right-click and select Create > CONTROL CARDS > TITLE from the context menu.
      A new Control Card opens in the Entity Editor.
    2. In the TITLE field, enter This is my first PAM-CRASH example.


      Figure 3.
  2. Create and define the output Control Cards.
    1. In the Solver Browser, right-click and select Create > CONTROL CARDS > OCTRL from the context menu.
      The OCTRL Control Card defines output control parameters.
      A new Control Card opens in the Entity Editor.
    2. For VALUE, under THPOUTPUT_OPT, enter 0.005.


      Figure 4.
    3. For VALUE, under DSYOUTPUT_OPT, enter 0.005.
    4. In the Solver Browser, right-click and select Create > CONTROL CARDS > RUNEND from the context menu.
      The RUNEND Control Card defines end of run parameters.
      A new Control Card opens in the Entity Editor.
    5. For TIO2, enter 0.06.


      Figure 5.
  3. Define the file optional keyword.
    1. In the Solver Browser, right-click and select Create > CONTROL CARDS > FILE from the context menu.
      A new Control Card opens in the Entity Editor.
    2. For NAME, enter rail-dyna.hm.


      Figure 6.
  4. Define the time step optional keyword.
    1. In the Solver Browser, right-click and select Create > CONTROL CARDS > TCTRL from the context menu.
      A new Control Card opens in the Entity Editor.
    2. Select the SHELL_TIMESTEP_OPT checkbox.
    3. Set TIMESTEP_OPT_LS to LARGE.
    4. Set TIMESTEP_OPT_BN to BEND.


      Figure 7.

Assign Element Types

In this step, you will assign element types for PAM-CRASH 2G.

Depending on the analysis requirement, the HyperMesh basic element type can be changed.

For example, a quad4 can be a SHELL or a MEMBR element. The tria3 element can be a TRIA_C, SHELL, or MEMBR element. The tetra4, the penta6, and the hexa8 elements define the SOLID elements of PAM-CRASH. Properties can be added for the selected element type using Control Cards.

  1. Open the Element Type panel by clicking Mesh > Assign > Element Type from the menu bar.
  2. Open the 2D & 3D subpanel.
  3. Click quad4 = and select SHELL.
  4. Click elems > all.
  5. Click update.
  6. Click return to exit the panel.

Define a Material and /PART Cards

In this step, you will define a material and /PART cards for PAM-CRASH 2G.

  1. Rename the tmp component.
    1. In the Model Browser, Component folder, select the tmp component.


      Figure 8.
      The Entity Editor opens, and displays the component's card data.
    2. For Name, enter topbottom.
  2. Create and define a type 102 material .
    1. In the Model Browser, right-click and select Create > Material from the context menu.
      A new material opens in the Entity Editor.
    2. For Name, enter new mat.
    3. Set card image to MAT_2D.
      Note: The template provides MAT_1D, MAT_2D, and MAT_3D dictionaries. Material types from 200 to 230 are defined with MAT_1D. Materials types from 100 to 151 are defined with MAT_2D. Material types from 1 to 41 are defined with MAT_3D. Use the card previewer to switch the material type.
    4. Set Material Type to Type 102.
    5. For RHO, enter 7.85e-9.
    6. For E, enter 20000.
    7. For SIGMay, enter 250.
    8. For NU, enter 0.3.
  3. Assign a material and thickness to the side and topbottom collectors.
    1. In the Model Browser, Component folder, select side and topbottom.
      The Entity Editor opens and displays the selected component's common card data.
      Figure 9.
    2. Set card image to Part_2D.
    3. For Material, click Unspecified > Material.
    4. In the Select Material dialog, select new mat and then click OK.
      HyperMesh assigns the new mat material to the selected components.
    5. For h (thickness), enter 2.5.

Define HyperMesh Groups

In this step, you will define HyperMesh groups: sliding interface for PAM-CRASH 2G.

This step describes how to define a type 36 self contacting sliding interface. A second interface is defined only for tutorial purposes.

  1. Define the group.
    1. In the Solver Browser, right-click and select Create > CONTACT > CNTAC36 from the context menu.
      A new group opens in the Entity Editor.


      Figure 10.
    2. For Name, enter self_impact.
    3. Select a new color for the group.
    4. For SLFACM, enter 1.0.
  2. Add the slave components.
    In this step, the Entity Editor should be open for the self_impact group.
    1. Click Slave entity IDs.
    2. Set the entity selector to Components.


      Figure 11.
    3. Click Components.
    4. In the Select Components dialog, select side and topbottom and then click OK.


      Figure 12.
  3. Define an additional contact.
    This procedure explains how to define a type 34 master slave (element - node) contact.
    1. In the Solver Browser, right-click and select Create > CONTACT > CNTAC34 from the context menu.


      Figure 13.
      A new group opens in the Entity Editor.
    2. For Name, enter masterslave.
    3. Select a new color for the group.
    4. For SLFACM, enter 1.0.
  4. Add the master elements and slave nodes.
    In this step, the Entity Editor should be open for the masterslave group.
    1. For Master entity IDs, click 0 Elements > Elements.
    2. In the panel area, set the switch to elems.


      Figure 14.
    3. Using the elems selector, select two elements as seen in Figure 15.


      Figure 15.
    4. Click add.
    5. Click return.
    6. For Slave entity IDs, click 0 Nodes > Nodes.
    7. In the panel area, set the switch to nodes.
    8. Using the nodes selector, select two nodes as seen in Figure 16.


      Figure 16.
    9. Click add.
    10. Click return.
The master elements are marked with square indents, and the slave nodes displays as seen in Figure 17.


Figure 17.

Define a Rigid Wall

In this step, you will define a rigid wall for PAM-CRASH 2G.

This step explains how to define a type 4 infinite rigid wall with a base node at -1.00, 0.0, 0.0.
  1. Create a base node for the rigid wall.
    1. From the menu bar, click Geometry > Create > Nodes > XYZ.
    2. For x, enter –1.0.
    3. For y, enter 0.0.
    4. For z, enter 0.0.
    5. Click create.
      HyperMesh generates the base node as seen in Figure 18


      Figure 18.
    6. Click return to exit the panel.
  2. Create and define the rigid wall card.
    1. From the menu bar, click BCs > Create > Rigid Walls.
    2. In the Rigid Walls panel, Name field, enter rwall1.
    3. Click type = and select RWALL.
    4. Select a color.
    5. In the size =, enter 100.
      The display size of the rigid wall is specified.


      Figure 19.
    6. Click create.
  3. Define rigid wall geometry.
    1. Open the geom subpanel.
    2. Double-click name=, and select rwall1.
    3. Set the switch after shape to plane.
    4. Set the toggle after shape to infinite.
    5. Under normal vector, set the switch to vectors.
    6. Click the second switch and select x-axis.


      Figure 20.
    7. Using the base node selector, select the node you created in step 1.
    8. Click update.
      The rigid wall displays as seen in Figure 21.


      Figure 21.
  4. Add secondary nodes for the rigid wall.
    1. Go to the add subpanel.
    2. Set slaves to nodes.
    3. Click nodes > by id.
    4. In the id field, enter 1-21 and then press ENTER.
      21 nodes at the interface of the rail and the rigid wall highlight. One of the nodes is not selected.


      Figure 22.
    5. Click the unhighlighted node.
      Note: You can also click nodes > id and enter 1012 in the id field.
    6. Click add.
      The selected nodes are now set as secondarys.


      Figure 23.
  5. Add motion to the rigid wall.
    1. Open the motion subpanel.
    2. Set the switch below name to components.
    3. In the x comp field, enter 1.0.
    4. Set type of motion to velocity.


      Figure 24.
    5. Click update.
    6. Click return to exit the panel.

Define Attributes in the Card Previewer

In this step, you will define attributes in the card previewer.

  1. In the Model Browser, Group folder, click rwall1.
    The Entity Editor opens and displays the group's card data.
  2. Set Friction type flag to No Sliding.
  3. Set Rigid Wall Descriptor – Plane Type to Type 4.
    Tip: The parameters in the Entity Editor are according to the definitions made. It is now possible to define the mass and the initial velocity for moving rigid wall with finite mass.
  4. For mRW, enter 1.
  5. For VINIT, enter 2000.

Create Boundary Conditions

In this step, you will create model boundary conditions for PAM-CRASH 2G.

  1. Create a load collector.
    1. In the Model Browser, right-click and select Create > Load Collector from the context menu.
      The new load collector becomes the current collector. Any new loads created will be placed in this collector.
      A new load collector opens in the Entity Editor.
    2. For Name, enter boundary conditions.
    3. Select a card image.
    4. Select a color.
  2. Specify the constraints.
    1. Open the Constraints panel by clicking BCs > Create > Constraints from the menu bar.
    2. Click load types, and select BOUNC.
      All constraints that are now created will be displacement boundary conditions.
    3. Click nodes > by id.
    4. In the id field, enter 990-1011.
    5. Press ENTER.
      22 nodes highlight.


      Figure 25.
    6. In the relative size= field, enter 10.
    7. Click create.
      Constraints are now added to the selected nodes.


      Figure 26.
    8. Click return to exit the panel.

Create Time Histories

In this step, you will create time histories for PAM-CRASH 2G.

For PAM-CRASH 2G, time histories may be defined for nodes, elements, and local coordinate systems. For this step, you will only create time histories for nodes and elements. The operation is the same for any type of time history that is created.
  1. Create a node time history card.
    1. In the Model Browser, Load Collector folder, right-click on Boundary Conditions and select Hide from the context menu.
      The display of loads turns off.
    2. From the menu bar, click Setup > Create > Output Blocks.
    3. In the name field, enter node_thp.
    4. Using the nodes select, select a few nodes.
    5. Click create.
      The time history for nodes is created.
  2. Create an element time history card.
    1. In the name field, enter elem_thp.
    2. Set the entity selector to elems.
    3. Select a few elements.
    4. Click create.
  3. Review time histories entities.
    1. Click review.
    2. Select elem_thp.
      The entities associated with this time history highlight.
    3. Click return to exit the panel.
  4. View the time history card image.
    1. In the Model Browser, Output Blocks folder, right-click on elem_thp and click Card Edit.
      The time history card is displayed as it will look in the output.
    2. Click return twice to exit the panel.

Create a Function

In this step, you will generate a curve and a function.

This step describes how to generate curves, which corresponds to the function cards /FUNCT in PAM-CRASH 2G. This curve should serve as a function for a logical sensor switching on and off. At time=0, the sensor is on. At time=0.01, the sensor is switched off.
  1. From the menu bar, click XY Plots > Create > Curves > Single Curve.
  2. Select math.
  3. In the x = field, enter {0, 0.01, 0.1}.
    Tip: Include the brackets in the x = field.
  4. In the y = field, enter {1, 0, 0}.
    Tip: Include the brackets in the x = field.


    Figure 27.
  5. Click create.
    HyperMesh generates a curve.


    Figure 28.
  6. Click return.

Create a Sensor Card

In this step, you will create a sensor card.

Sensors are implemented as properties in HyperMesh. In this example we refer to the curve defined in Create a Function.
  1. From the Analysis page, click safety > sensors.
  2. In the name = field, enter sensor.
  3. Click card image =, and select SENSOR.
  4. Click create/edit.
    The Card Image dialog opens.
  5. Set Sensor type to Type 5 (logical function switch Sensor).
  6. Click LCS > curve1.
  7. Click return twice to exit the panels.

Export a Data Deck

In this step, you will export a PAM-CRASH 2G data deck from HyperMesh.

  1. From the menu bar, click File > Export > Solver Deck.
    The Export - Solver Deck tab opens.
  2. In the File field, enter rail.pc.
    rail.pc is the PAM-CRASH 2G file you will create.
  3. Set Template to Pamcrash2G2012.
  4. Click Export.
    HyperMesh writes the deck. A message in the Status bar indicates the process is completed.