RD-T: 3540 Front Impact Bumper Model

This tutorial demonstrates how to find deformation, stress and energy absorbing capacity of various structural components of a vehicle hitting a stationary or moving object.

  • The component is crashworthy (safe) if it meets the plastic strain and energy targets.
  • A Bumper beam is one of the components that is used to protect passengers from front and rear collision.
  • Bumper beam crash tests are necessary, for instance, to calculate the energy absorption of this component during a crash.
  • UNITS: Length (mm), Time (ms), Mass (kg)
  • Simulation time: [0 – 100.0]
  • Boundary Conditions: Gravity load, initial velocity of -5.0 m/s of the bumper beam on the rigid wall
  • /MAT/LAW2 (PLAS_JOHNS): for Bumper parts and Crash box parts
  • /PROP/TYPE1 (SHELL): for Bumper beam parts and Crash box parts
  • /INTER/TYPE2: for tied interface that connects a set of slave nodes to a master surface. (connect coarse and fine meshes, model spotwelds, rivets, and so on)
  • /INTER/TYPE7: Penalty contact between all versus all
  • /FAIL/BIQUAD: to model failure
The model used consists of a simplified bumper model:

rd3540_bumper_model
Figure 1. Bumper Model

Load the Radioss User Profile

  1. Launch HyperMesh Desktop.
  2. From the Preferences menu, select User Profiles or click the userProfile-24 icon in toolbar.
  3. Select Radioss (Radioss2020) and click OK.

Import the Model

  1. Click File > Import > Solver Deck or click fileImportGeometry-24.
  2. Click the Select File icon files_panel to open the Bumper_start_0000.rad file you saved to your working directory from the radioss.zip file.
  3. Click Open.
  4. Click Import.
    Ignore the warning “No valid Engine File found…”
  5. Click Close to close the window.
  6. In the Model Browser, verify that the correct units are defined by expanding Cards, BEGIN_CARD.


    Figure 2.

Define Penetration/Intersection Check

  1. From the Tools menu, select Penetration Check.
  2. Change Entity type to Components.
  3. For Selection, click Components, then select the following components and click Close.


    Figure 3.
  4. For Thicknesss option, select Uniform Thickness and set the Value to 1.0.
  5. Select Consider edge penetration.


    Figure 4.
  6. Click Check and Close.
  7. In the Penetrations Browser, click the Review Failed Elements icon .
    Intersections and penetrations will be highlighted.
  8. Click Penetrations, as shown below:


    Figure 5.
  9. Click the Automatic Intersection/Penetration Fix icon to fix penetrations.

Create Materials

Two materials will be created.

  1. In the Model Browser, right-click and select Create > Material.
  2. In the Entity Editor, for Name, enter Mat_DP600.
  3. Set Card Image to M2_PLAS_JOHNS_ZERIL.
  4. Insert values, as shown below.


    Figure 6.
  5. In the Model Browser, right-click and select Duplicate to duplicate the material.
  6. In the Entity Editor, for Name, enter Mat_DP1000.
  7. Change values of SIGY, b and n to 0.5.


    Figure 7.

Create Failure to Material Card

  1. In the Model Browser, right-click and select Create > Failure.
  2. In the Entity Editor, for Name, enter FAIL_BIQUAD.
  3. Set Config to FAIL_BIQUAD.
  4. Set Mat_id, click Material, select Mat_DP1000 and click OK.
  5. For M-Flag, select 2: HSS steel.


    Figure 8.

Create the Properties

Two properties will be created.

  1. In the Model Browser, right-click and select Create > Property.
  2. In the Entity Editor, for Name, enter Prop_DP600.
  3. Set Card image to P1_SHELL.
  4. Insert values for the Crash_Box shell definition.


    Figure 9.
  5. In the Model Browser, right-click on the previously created property, Prop_DP600 and select Duplicate.
  6. In the Entity Editor, for Name, enter Prop_DP1000.
  7. Set Card Image to P1_SHELL.
  8. Change the Thick value to 1.8mm.


    Figure 10.

Assign Materials and Properties to Components

  1. In the Model Browser, expand the Components folder and left-click on the crash_box* components.
  2. In the Entity Editor, for Prop_Id, click the Value field <unspecified> to change to Property and select Prop_DP600 and click OK.
  3. For Mat_Id, click the Value field <unspecified> to change to Material and select Mat_DP600 and click OK.
  4. In the Model Browser, left-click on the BumperBeam* components.
  5. In the Entity Editor, for Prop_Id, click the Value field <unspecified> to change to Property and select Prop_DP1000 and click OK.
  6. For Mat_Id, click the Value field <unspecified> to change to Material and select Mat_DP1000 and click OK.

Create Spotwelds

The model has unrealized connectors which will be used to create spotwelds.

  1. From 1D page select connectors > spot and toggle the realize option to connect the bumper parts.
  2. Click connectors and select all.
  3. Set type= to type2(spring).
  4. For tolerance and diameter, insert a value of 8 and click realize.
  5. Click return.

Reflect the Model

  1. From the Tool page, select reflect.
  2. Change the entity selector to elems, then select elems, by collector and select the only the Bumper and Crash collectors, as shown. Click select.


    Figure 11.
  3. Select elems > duplicate > original comp.
    This will duplicate the element.
  4. Mirror/reflect the model at Y-axis. Select B as the basis point.


    Figure 12.


    Figure 13.
  5. Click reflect and return.
  6. From the Tool page, select reflect.
  7. Change the entity selector to connectors, click the connector entity selector and select all. Click again and select duplicate > original connector group.
  8. Reflect/mirror the model at Y-axis. Select B as the basis point.
  9. Click reflect and return to confirm.
  10. From the 1D page, select connectors and spot.
  11. Toggle the realize button and click connectors and select entities using the Shift+left-mouse in the window and draw a box.
  12. Click reflect and return.
    Note: Nodes at the midplane are not yet equivalenced.
  13. From the Tool page, select edges.
  14. Select all elements by a box, whose nodes are at free edges. Change the entity selector to elems amd select all.
  15. Set tolerance to 0.1mm.
  16. Click preview equiv, equivalence and return.

Create the Interface for Penalty Contact

Another useful way to view the model is using the Solver Browser which shows the model using the Solver entities.

  1. From the menu, click View > Solver Browser.
  2. In the Solver Browser, right-click Create > INTER > TYPE7.
  3. In the Entity Editor, for Name, enter all_contact.
  4. For Grnod_id(s) and Surf_id(M), change the entity selector to Components and select all parts containing shells (not the RW^^ components) and click OK.
  5. Insert values, as shown below.




    Figure 14.
  6. In the Solver Browser, right-click on the previously created /INTER/TYPE7 contact (all_contact) and click Review.
  7. Right-click on the previously created /INTER/TYPE7 contact (all_contact) and click Review to turn off the review.

Create the Rigid Body

  1. Click to change the view to XY-View.
  2. In the Model Browser, right-click Create > Component to create a new component.
  3. In the Entity Editor, for Name, enter RBODY.
  4. In the Entity Editor, select the Rbody option.
    Removes the Card Image, Prop_Id, and Mat_Id from the menu since they are not needed for rigid bodies.
  5. From the main menu, select Mesh > Create > 1D Elements > Rigids.
  6. For nodes 2-n, click the first down arrow and select Multiple nodes.
  7. For primary node, click the down arrow and select calculate node.
  8. Click the nodes entity selector. Use a window selection to select the last row of nodes of the Crash_Boxes by box. Click proceed and create.


    Figure 15.
  9. From the Solver Browser, select Rbody > MULTIPLE_NODES_RBODY > Elements.
  10. For MASS, enter 500 for the inertia.
  11. For J_XX, J_YY, and J_ZZ, enter 50.

Create the Boundary Condition

  1. Select View > Solver Browser, and right-click in the Solver tab area.
  2. Select Create > BOUNDARY CONDITIONS > BCS.
  3. For Title, enter Boundary_condition, right-click grnd_ID and click Create.
  4. Within the grnd_ID section, click on 0 Nodes beside Entity IDs, then Nodes.
    A nodes selection appears.
  5. Select the nodes, as shown below and click proceed.


    Figure 16.
  6. Activate all degrees of freedom; except of DOF1, translation in the X-direction.

Create the Gravity Load

  1. Select View > Solver Browser, and right-click in the Solver tab area.
  2. Select Create > BOUNDARY CONDITIONS > GRAV.
  3. For Title, enter Gravity_load.
  4. Right-click on grnd_ID and select Create.
  5. Within the grnd_ID section, for Name, enter all_nodes.
  6. Click on 0 Nodes beside Entity IDs, then Nodes.
    A node selection appears.
  7. Click on the nodes entity selector and select “all” to select all the nodes.
  8. Click proceed.
  9. For Dir, select Z as the gravity direction.
  10. Set Fscale(Y) to -1 to apply gravity in the negative direction.
  11. Right-click on fct_ID(T) and select Create.
  12. Right-click on fct_ID(T) and select Plot Curve.
    An XY curve editor appears.
  13. Enter the values, as shown below.


    Figure 17.

Create the Initial Velocity

  1. Select View > Solver Browser, and right-click in the Solver tab area.
  2. Select Create > BOUNDARY CONDITIONS > INIVEL.
  3. For Title, enter INIVEL.
  4. Click Set beside grnd_ID and pick the all_nodes set that was created in the gravity creation set.
  5. Click Velocity Components and enter, -5, 0, 0 for Vx, Vy and Vz fields, respectively.

Define the Rigid Wall

  1. Right-click in the Solver Browser and select Create > RWALL > CYL.
  2. For Name, enter RWALL.
  3. For XM, YM, ZM, enter -170, 0, -200, respectively.
  4. For Normal, enter 0, 0, -1, respectively.
  5. For Sliding, select 2: Sliding with friction.
  6. For FRIC, enter 0.2.
  7. For Dsearch, enter 200.0mm.
  8. For Diameter, enter 254.0mm.


    Figure 18.

Create Accelerometer for Post-Processing

  1. Right-click in the Solver Browser and select Create > ACCEL.
  2. For name, enterACCELER01.
  3. For Fcut, enter 1.650.
  4. For node_ID, click Node and select the node to the left in Figure 19 .


    Figure 19.
  5. In the Solver Browser, right-click on the previously created accelerometer, ACCELER01 and click Duplicate.
    A new Accelerometer is created.
  6. Click on the new accelerometer and rename to ACCELER02.
  7. For node_ID, click Node and select the node to the right in Figure 19.

Create a Cross Section

  1. Right-click in the Model Browser and select Create > Cross Section.
    A Cross Section Assistant opens.
  2. For Cross Section Name, enter section.
  3. For Entity Selection, click Components and change to Elements.


    Figure 20.
  4. Select elements in left crushbox using a window and click proceed.
  5. For Base Node, select the arrow to pick a node that defines the base node.
  6. Select the node on bumper side of the accelerometers and click proceed.
  7. For Normal Direction, click the Select direction arrow to pick a node.


    Figure 21.
  8. Click N1 to set N1 and N2, as shown, which defines the normal vector and click proceed.


    Figure 22.
  9. Click Create, then click Close.

Review the Cross Section

  1. In the Model Browser left-click on the cross section section and right-click and select review, or press the Q on the keyboard.
    If the nodes and element were not exactly on the plane, the automatic selection needs to be modified. See Edit the Cross Section Sets.


    Figure 23.
  2. If the nodes and elements are exactly are in one row, press Q to turn off the review.


    Figure 24.

Edit the Cross Section Sets

  1. With the section still selected, open the Entity Editor and right-click on grshel_id and select edit to edit the set of elements that defines the section.
  2. Click beside Entity IDs twice to edite the elements in the set.
  3. Left-click to select and right-click to deselect elements until all the elements selected are in a row.
  4. Click proceed and then click Close.
  5. In the Entity Editor, right-click grnod_id and select edit to edit the set of nodes that defines the section.
  6. Click beside Entity IDs twice to edit the nodes in the set.
  7. Left-click to select and right-click to deselect nodes until all the nodes selected are in a row, as shown.


    Figure 25.
  8. Click Proceed and close.
    To review the cross section, refer to Review the Cross Section.

Define 2nd Penetration Check

  1. From the Tools menu, select Penetration Check.
  2. Click Invoke Penetration check setup Widget icon .
  3. For Entity type, select Groups and select all_vers_all contact group.
  4. Click Check.
  5. In the Penetrations Browser, click the Review Failed Elements icon .
  6. Expand the Penetrations folder in the browser and select all_contact to see the elements with the penetrations.
  7. Click Automatic Penetration/Intersection Fix icon to remove penetrations.
  8. Click Recheck icon , if there are any penetrations or intersections.

Create Time History Outputs

Three separate time history outputs will be created in this step.

  1. Right-click in the Solver Browser and select Create > TH > RBODY.
  2. For Name, enter TH_RBODY.
  3. For Entity IDs, select Elements and select the one rigid body and click OK.
  4. For NUM_VARIABLES, select 1.


    Figure 26.
  5. In the Solver Browser and select Create > TH > RWALL.
  6. For Name, enter TH_RWALL.
  7. For Entity IDs, select Rigidwalls and select RWALL and click OK.
  8. For NUM_VARIABLES, select 1.


    Figure 27.
  9. In the Solver Browser and select Create > TH > ACCEL.
  10. For Name, enter TH_ACCELERO.
  11. For Entity IDs, select Accelerometers and select the two ACCELEROS and click OK.
  12. For NUM_VARIABLES, select 1.


    Figure 28.

Create Control Cards

  1. To start the Engine file assistant, select Tools > Engine File Assistant.
  2. Input the values, as shown below and click OK.


    Figure 29.
  3. Click Tools > Create Cards > ENGINE KEYWORDS > ANIM > ANIM/SHELL/DAMA to add additional engine control cards.
  4. For ALL, check the box.


    Figure 30.

Edit Control Cards

To edit an existing control card.

Click on the control card ENG_PRINT and change N_print to -100 to request output every 100 cycles.

Export the Model

  1. Click File > Export or click the Export icon .
  2. Click the folder icon and navigate to the destination directory where you want to export to.
  3. For Name, enter bumper_impact and click Save.
  4. Click the downward-pointing arrows next to Export options to expand the panel.
  5. Click Export to export the file.

Run the Model in the Solver

  1. Go to Start > Programs > HyperWorks 2020 > Radioss.
  2. For Input file, browse to the exercise folder and select the file bumper_impact_0000.rad.
  3. For Options, select -np 4 (Radioss Version, Starter and/or Engine, Number of CPUs).
  4. Click Run.

Post-process with HyperView and HyperGraph

When the simulation is done running, use the following steps.

  1. Open HyperView and click File > Load > Results.
  2. Under Load Model, select the bumper.h3d file.
  3. Global energies and forces can be plotted in HyperGraph by using the Build plots panel and loading the bumperT01 file.