RD-3540: Front Impact Bumper Model using HyperMesh

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

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. The modeling steps that are covered are:

•	Associating /PART, with /MAT and /PROP.

•	Converting node-to-node connections (/RBODY) into a mesh-less welding formulation (/INTER/TYPE2 with /SPRING) using HyperMesh connectors.

•	Defining the contact for the elements in the bumper with an /INTER/TYPE7 card.

•	Defining the interaction between bumper and barrier with an /INTER/TYPE7 card.

•	Defining the interaction between barrier and rigid wall with the /RWALL/PLANE and /BOX/RECTA cards.

•	Specify the output of resultant forces for a plane on the left interior and exterior crash boxes with /SECT.

•	Creating a /TH/NODE card to output time history for nodes.

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

Exercise

The model used consists of a simplified bumper model (see image below):

rd3540_bumper_model

Bumper model

Step 1: Load the RADIOSS (Block) User Profile

1.	Launch HyperMesh Desktop.

2.	From the Preferences menu, select the User Profiles or click the icon in toolbar.

3.	Select RADIOSS (Block140) and click OK.

Step 2: Load the bumper.hm file

1.	Click the Open Model icon to open the bumper.hm file you saved to your working directory from the radioss.zip file. Refer to Accessing the Model Files.

2.	Click Open.

The model loads into the graphics area.

Step 3: Define vehicle mass component to partially take into account the inertia properties and mass of the missing parts of the vehicle

1.	In the Model browser, right-click and select Create > Component. The Entity Editor (EE) will open.

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 DOF’s checked, click create to create the rigid body.

Note:

A spider will be drawn connecting the created node to the edge nodes of the structure modeled.

14.	Click Card Edit 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 exit the panel.

Step 4: Create a GRNOD/BOX/RECTA that contains all nodes except barrier nodes

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.	Optionally, select a Color.

5.	Enter Corner1 and Corner2 X, Y, and Z coordinates, as shown below.

rd3540_box_velocity

Step 5: Create initial velocity on bumper except barrier

1.	Click Tools > BCs Manager.

2.	In the BCs Manager, enter Name as trans_vel.

3.	Select 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

7.	After the above step, a set named InitialVelocity_grnodbox is created automatically or you can create this set before the above step and then refer to this set in the above step, instead of BOX.

8.	Click the Create > Close.

Step 6: Define master surface for contact

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

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

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

Step 7: Create 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

Step 8: Create a system that specifies the location and the cross section plane normal

1.	Click the numbering icon 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.

Click on.

Note:

Node numbers will 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 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.

Step 9: Create a set of elements that will contribute to the cross-sectional force results

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 to Elements selector active, select two rows of element on either side of the system, as shown in figure below.

rd3540_XsectionPlane

Step 10: 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 which is defined in previous step, as shown below.

rd3540_crosssection-plane

Step 11: Select the section for 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

Step 12: Create a BOX/RECTA and GRNOD/BOX containing the nodes making up the barrier and bumper’s left side

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.	Optionally, select a Color.

4.	Enter Corner1 and Corner2 X, Y and Z coordinates, as shown below:

rd3540_half_model

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

Step 13: Define a rigid wall

1.	Press the F8 key to enter the create nodes panel.

2.	Select the XYZ () 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

Step 14: Create output requests 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

Step 15: Export the model

1.	Click File > Export or click the Export icon .

2.	For File:, click the folder icon and navigate to the destination directory where you want to export to.

3.	Enter the name bumper_impact and click Save.

4.	Click the downward-pointing arrows next to Export options to expand the panel.

5.	Toggle Merge starter and engine file to export the engine file with the model file (or export separately).

6.	Click Export to export both model and engine file.

Step 16: Run the solver using RADIOSS Manager

1.	Go to Start > Programs > Altair HyperWorks 14.0 > RADIOSS.

2.	For Input file, browse to the exercise folder and select the file bumper_impact_0000.rad.

rd3540_run_mgr_14

Step 17 (Optional): View the results in HyperView

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

RD-3540: Front Impact Bumper Model using HyperMesh

RD-3540: Front Impact Bumper Model using HyperMesh

RD-3540: Front Impact Bumper Model using HyperMesh

Exercise

See Also: