RD-T: 3540 Front Impact Bumper Model

In this tutorial you will learn how to use HyperMesh to set up a Radioss input deck for analysis of the impact of a bumper against a barrier behind rigid wall.

For this tutorial it is recommended to complete the introductory tutorial HM-1000: Getting Started with HyperMesh, as well as RD-T: 3520: Pre-processing for Pipes Impact for the basic concepts on the HyperMesh Radioss interface.

The units used in the model are millisecond, millimeter and kilogram (ms, mm, kg), and the tutorial is based on Radioss Block 14.0.

The model used consists of a simplified bumper model:

rd3540_bumper_model
Figure 1. Bumper Model

Load the Radioss User Profile

  1. Launch HyperWorks Desktop.
  2. From the Preferences menu, select User Profiles or click the userProfile-24 icon in toolbar.
  3. Select Radioss (Block140) and click OK.

Open the Model File

  1. Click the Open Model icon fileOpenModel-24 to open the bumper.hm file you saved to your working directory from the radioss.zip file.
  2. Click Open.
    The model loads into the modeling window.

Define the Vehicle Mass Component

  1. In the Model Browser, right-click and select Create > Component.
    The Entity Editor opens.
  2. For Name, enter Vehicle mass.
  3. Set Card Image to None and click Yes to confirm.
  4. Click Geometry > Create > Nodes > XYZ to open the Nodes panel.
  5. In the X field, enter 700.
  6. In the Y field, enter 0.
  7. In the Z field, enter 170.
  8. Click create to create the node.
  9. Go to the 1D page, and click rigids.
  10. Click the selector arrow nodes 2-n and select sets.
  11. For primary node, select the node created in the steps above.
  12. Click sets and select the Constrain Vehicle set.
  13. With all the DOFs checked, click create to create the rigid body.
    A spider will be drawn connecting the created node to the edge nodes of the structure modeled.
  14. Click Card Edit entityCards-24 in the toolbar, set the selector to elements and select the rigid body created.
  15. Click edit.
  16. Fill the mass and inertia information in the card image, as shown in the table below:
    Mass JXX JXY JXZ JYY JYZ JZZ
    800 1.5E+07 -5.0E+03 -8.0E+06 5.0E+07 -900 6.0E+07
  17. Set ICOG as 4 and set Ispher as 0.
  18. Click return to go back to the main menu.

Create a Rectangular Node Group Box

  1. Click View > Browsers > HyperMesh > Solver to activate the Solver Browser, if it is not active on your screen.
  2. Right-click in the Solver Browser and select Create > BOX > BOX/RECTA.
    The Entity Editor opens.
  3. For Name, enter box velocity.
  4. Click Color and select a color from the color palette.
  5. Enter Corner1 and Corner2 X, Y, and Z coordinates, as shown below.

    rd3540_box_velocity
    Figure 2.

Create the Initial Velocity on Bumper

  1. Click Tools > BCs Manager.
  2. In the BCs Manager, enter Name as trans_vel.
  3. Set the Select type as Initial Velocity under the Create header.
  4. Set the entity selector to BOX under GRNOD.
  5. Click on it and select box velocity.
  6. Enter -10, 0, 0 for Vx, Vy and Vz fields, respectively.

    rd3540_trans_vel
    Figure 3.
    A set named InitialVelocity_grnodbox is created. You can also create this set before the above step and then refer to this set in the above step, instead of BOX.
  7. Click Create and then click Close.

Define the Master Contact Surface

  1. Right-click in the Solver Browser and select Create > SURF_EXT > PART.
    The Entity Editor opens.
  2. For Name, enter barrier_surface.
  3. For Entity IDs, click on Components.
  4. In the Select Components dialog, select barrier and click OK.

    rd3540_barrier_surface
    Figure 4.
  5. Right-click in the Solver Browser and select Create > SURF > PART.
    The Entity Editor opens.
  6. For Name, enter bumper_surface.
  7. For Entity IDs, click on Components.
  8. In the Select Components dialog, select bumper, exterior crashbox left, exterior crashbox right, interior crashbox left, and interior crashbox right and click OK.

    rd3540_bumper_surface
    Figure 5.
  9. Right-click in the Solver Browser and select Create > SURF > SURF.
    The Entity Editor opens.
  10. For Name, enter barrier_bumper_surface.
  11. For Entity IDs, select Sets.
  12. Click on Sets and select barrier_surface and bumper_surface and click OK.

    rd3540_barrier_bumper_surface
    Figure 6.

Create the Self-Impact Contact between Parts of the Bumper

  1. Right-click in the Solver Browser and select Create > INTER > TYPE7.
    The Entity Editor opens.
  2. For Name, enter impact.
  3. For Grnod_id (S) (slave entity), set the selector to Components.
  4. Click Components, select bumper, interior crashbox (left and right) and exterior crashbox (left and right) and click OK.
  5. For Surf_id (M) (master entity), set the selector to Set.
  6. Click Set, select barrier_bumper_surface and click OK.
  7. Set Igap to 2.
  8. For the static coefficient Fric, enter 0.15.

    rd3540_impact_14
    Figure 7.

Create a System Specifying the Location and Cross-Section Plane Normal

  1. Click the numbering icon infoNumbers-24 on the toolbar.
  2. Click the nodes selector and select by id.
  3. For the IDs, enter 6224, 6227, and 5993.
  4. Check the display check box on.
  5. Click on.
    Node numbers appear next to the node for selection in further steps.
  6. From the Analysis page, click systems.
  7. Go to the create by node reference page.
  8. Select Node ID 6224 for origin node.
  9. Select Node ID 6227 for z- axis.
  10. Select Node ID 5993 for yz plane.
  11. Click create to create a system.
  12. Click the Card Edit icon entityCards-24 on the toolbar.
  13. Set the entity selector to systs.
  14. Select the system and click edit.
  15. Change the option from Skew to Frame.
  16. Click return.

Create a Set of Elements

  1. Right-click in the Solver Browser and select Create > GRSHEL > SHEL.
    The Entity Editor opens.
  2. For Name, enter CrosssectionPlane-elements.
  3. For Entity IDs, toggle the Elements selector active, and select two rows of element on either side of the system, as shown in the figure below.

    rd3540_XsectionPlane
    Figure 8.

Define a Section

  1. Right-click in the Solver Browser and select Create > SECT > SECT.
  2. For Name, enter Crosssection_Plane.
  3. For Frame_ID, select the system defined in the previous step by clicking on the screen.
  4. For grshel_ID, select the set CrosssectionPlane-elements defined in the previous step, as shown below.


    Figure 9.

Define Time History Output

  1. Right-click in the Solver Browser and select Create > TH > SECTIO.
  2. For Name, enter Section_force.
  3. For Entity IDs, toggle Crosssections and select Crosssection_Plane.
  4. For NUM_VARIABLES, select 1 and for Data: Var, enter DEF.
    This selects the default output for Radioss.

    rd3540_section_force
    Figure 10.

Create Slave Nodes to the Rigid Wall

These nodes will be slave to the rigid wall.
  1. Right-click in the Solver Browser and select Create > BOX > BOXRECTA.
  2. For Name, enter half model.
  3. Click Color and select a color from the color palette.
  4. Enter the Corner1 and Corner2 X, Y and Z coordinates, as shown below:

    rd3540_half_model
    Figure 11.
  5. Right-click in the Solver Browser and select Create > GRNOD > BOX.
  6. For Name, enter RigidwallSlave_grnodbox.
  7. For Entity IDs, set the selector to Box and select the above created half model (BOX/RECTA).

    rd3540_rigidwallslave_grnodbox
    Figure 12.

Define the Rigid Wall

  1. Press the F8 key to enter the Create Nodes panel.
  2. Select the XYZ (nodeXYZ-24) subpanel.
  3. For x=, y= and z=, enter the values -600, 750 and 90, respectively.
  4. Click create.
  5. Right-click in the Solver Browser and select Create > RWALL > PLANE.
  6. For Name, enter wall.
  7. Set Geometry type as Infinite Plane.
  8. With the Base node selector active, select the node that was created in step 4.
  9. Set Normal to 1,0,0.
  10. For grnod_id1 (S), toggle Set and select RigidWallSlave_grnodbox (GRNOD/BOX).
  11. For fric, specify 1.0 for the friction coefficient.

    rd3540_wall_14
    Figure 13.

Create Output Request and Control Cards

  1. Launch the HyperMesh Solver Browser from View > Browsers > HyperMesh > Solver.
  2. Right-click in the Solver Browser general area to create the cards, shown below with the given values for each parameter:
    Keyword Type Keyword Parameter Parameter Value
    CONTROL CARDS TITLE Status [Checked]
    CONTROL CARDS TITLE TITLE Bumper_Impact
    ENGINE KEYWORDS RUN Status [Checked]
    ENGINE KEYWORDS RUN Tstop 20
    ENGINE KEYWORDS PARITH Status [Checked]
    ENGINE KEYWORDS PARITH Keyword2 ON
    ENGINE KEYWORDS PRINT Status [Checked]
    ENGINE KEYWORDS PRINT N_Print -1000
    ENGINE KEYWORDS TFILE Status [Checked]
    ENGINE KEYWORDS TFILE Time Frequency 0.1
    ENGINE KEYWORDS ANIM/ELEM Status [Checked]
    ENGINE KEYWORDS ANIM/ELEM EPSP [Checked]
    ENGINE KEYWORDS ANIM/ELEM VONM [Checked]
    ENGINE KEYWORDS ANIM/BRICK/TENS Status [Checked]
    ENGINE KEYWORDS ANIM/BRICK/TENS STRESS [Checked]
    ENGINE KEYWORDS ANIM/BRICK/TENS STRAIN [Checked]
    ENGINE KEYWORDS ANIM/SHELL/TENS/STRESS Status [Checked]
    ENGINE KEYWORDS ANIM/SHELL/TENS/STRESS MEMB [Checked]
    ENGINE KEYWORDS ANIM/SHELL/TENS/STRAIN Status [Checked]
    ENGINE KEYWORDS ANIM/SHELL/TENS/STRAIN MEMB [Checked]
    ENGINE KEYWORDS ANIM/VECT Status [Checked]
    ENGINE KEYWORDS ANIM/VECT DISP [Checked]
    ENGINE KEYWORDS ANIM/VECT VEL [Checked]
    ENGINE KEYWORDS ANIM/DT Status [Checked]
    ENGINE KEYWORDS ANIM/DT Tstart 0
    ENGINE KEYWORDS ANIM/DT Tfreq 1
    ENGINE KEYWORDS DT/NODA Status [Checked]
    ENGINE KEYWORDS DT/NODA CST 0 - Tmin 3.6e-4

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. Select Merge starter and engine file to export both the Starter and Engine file in one file.
  6. Click Export to export the file.

Run the Model in the Solver

  1. Go to Start > Programs > HyperWorks 2019 > Radioss.
  2. For Input file, browse to the exercise folder and select the file bumper_impact_0000.rad.
  3. Click Run.

Review the Results

The exercise is complete. Save your work to a HyperMesh file.