CRASH-2100: Simplified Car Front Pole Impact

The goal of this tutorial is to simulate a frontal pole test with a simplified full car.

crash_2100_01

The model file used in this exercise can be found in the es.zip file. Copy the file(s) from this directory to your working directory.

•	UNITS: Length (mm), Time (s), Mass (ton), Force (N) and Stress (MPa)

•	Simulation time: Engine file (_0001.rad) [0 – 0.0601 ms]

•	An initial velocity of 15600 mm/s is applied on the car model to impact a rigid pole of radius 250 mm.

•	Elasto-plastic Material /MAT/LAW2 (Windshield)

[Rho_I] Initial Density = 2.5x10-9 ton/mm3

[E] Young's Modulus = 76000 MPa

[nu] Poisson’s Ratio = 0.3

[a] Yield Stress = 192 MPa

[b] Hardening Parameter = 200 MPa

[n] Hardening Exponent = 0.32

•	Elasto-plastic Material /MAT/LAW2 (Rubber)

[Rho_I] Initial Density = 2x10-9 ton/mm3

[E] Young's Modulus = 200 MPa

[nu] Poisson’s Ratio = 0.49

[a] Yield Stress = 1e30 MPa

[n] Hardening Exponent = 1

•	Elasto-plastic Material /MAT/LAW2 (Steel)

[Rho_I] Initial Density = 7.9x10-9 ton/mm3

[E] Young's Modulus = 210000 MPa

[nu] Poisson’s Ratio = 0.3

[a] Yield Stress = 200 MPa

[b] Hardening Parameter = 450 MPa

[n] Hardening Exponent = 0.5

[SIG_max] Maximum Stress = 425 MPa

Step 1: Load the Engineering Solutions RADIOSS user profile

1.	From the Start menu, select Engineering Solutions > Crash (HyperMesh) or click on the Standard toolbar.

2.	Select Crash > RADIOSS.

Click OK.

Step 2: Load the model file

1.	Click the Open Model icon on the Standard toolbar.

2.	In the Open Model dialog, navigate to the fullcar.hm file.

3.	Click Open. The model loads into the graphics area.

Step 3: Create and assign the material for the windshield components

1.	In the Model browser, right-click and select Create > Material. The Entity Editor is displayed below the Model browser.

2.	For Name, enter windshield.

3.	Set Card Image as M2_PLAS_JOHNS_ZERIL and click Yes to confirm.

4.	Input the values, as shown below:

rd3550_windshield_14

5.	In the Model browser, select components COMP-PSHELL_3 and COMP-PSHELL_16.

6.	Click Mat_Id in the EE, select the material windshield and click OK to update the selected components with the created material.

Step 4: Create and assign the material for the rubber components

1.	In the Model browser, right-click and select Create > Material. The Entity Editor is displayed.

2.	For Name, enter rubber.

3.	Set Card Image to M2_PLAS_JOHNS_ZERIL and click Yes to confirm.

4.	Input the values, as shown below:

rd3550_rubber_14

5.	In the Model browser, select components COMP-PSHELL_20 through COMP-PSHELL_23.

6.	For Mat_Id, select the material rubber and click OK to update the selected components with the created material.

Step 5: Create Steel material and assign to all other parts

1.	In the Model browser, right-click and select Create > Material. The Entity Editor is displayed.

2.	For Name, enter steel.

3.	Set Card Image to M2_PLAS_JOHNS_ZERIL.

4.	Input the values, as shown below:

rd3550_steel_14

5.	In the Model browser select all components labeled with COMP-PSHELL and COMP-PROD, except COMP-PSHELL_3, COMP-PSHELL_16 and COMP-PSHELL_20 to COMP-PSHELL_23.

6.	For Mat_Id, select the material steel and click OK to assign the material to the selected components.

Step 6: Create a Rigid Wall

1.	In the Model browser, right-click and select Create > Rigid Wall. The Entity Editor is displayed.

2.	For Name, enter ground.

3.	Set Geometry type as Infinite plane.

4.	Click Base node and select 'any node' from the model.

5.	Define the normal vector Z = -1.

6.	Set distance d = 300.

rd3550_rwall_14

7.	Go to the Setup > Rigid Walls panel.

8.	Move to the geom page.

9.	Click name and select Ground from the list.

10.	Click the edit tab besides base node and change values of the coordinates as indicated below.

X = -2300, Y = 1200, and Z = -1.

11.	Click update > return.

Step 7: Create a Cylindrical Rigid Wall to represent Pole

1.	In the Model browser, right-click and select Create > Rigid Wall. The Entity Editor will display.

2.	For Name, enter pole.

3.	Set the Geometry type as Cylinder.

4.	Click Base node and select ‘any node’ from the model.

5.	Define the normal vector Z= 1.

6.	For Radius node, do not select anything. Leave it as <Unspecified>.

7.	Set distance d= 1500.

rd3550_pole_14

8.	Go to Setup > Rigid Walls panel.

9.	Move to the geom page.

10.	Click name and select Pole from the list.

11.	Click the edit tab besides base node and change values of the coordinates as indicated below.

X = -320, Y = 1250, and Z = 0.

12.	Set Radius = 250.

13.	Click update > return.

Step 8: Defining Contact using TYPE 7 interface (Self Contact)

1.	Hide all the 1D (TRUSSES) and 3D (SOLID) parts in the model by going to the Solver browser PROP > SHELL, Isolate only. Return to the Model browser.

2.	From the Model browser, right-click and select Create > Contact. The Entity Editor will display.

3.	For Name, enter CAR_CAR.

4.	Set Card Image to TYPE7 and click Yes to confirm.

5.	Set the option to Components for Surf_id (M) (master entity), and select displayed components and click OK.

6.	Input other parameters as shown below.

rd3550_car_car_14

Step 9: Defining Contact using TYPE 7 interface between Engine and Radiator

1.	In the Solver browser, right-click and select Create > SURF_EXT > PART.

2.	For Name, enter engine.

3.	Click on Components and select COMP-PSOLID_24.

4.	In the Model browser, right-click and select Create > Contact.

5.	For Name, enter ENGINE_RADIATOR and set the Card Image as TYPE7 and click Yes to confirm.

6.	For Grnod_id (S) (slave entity), set the selector switch to Components and click Components, select COMP-PSOLID_26.

7.	For Surf_id (M) (master entity), set the selector switch to Set and click Set, select engine.

8.	Input the values, as shown below:

rd3550_engine_radiator_14

Step 10: Defining initial velocity

1.	From the Utility menu, click the BC's Manager or click the BCs Manager icon in the Crash toolbar.

2.	For Name, enter 35MPH, set the Select type field to Initial Velocity and set GRNOD to Parts.

3.	Click comps and select all of the parts in the model.

4.	Set Vx as 15600.

rd3550_35mph

5.	Click Create to create the boundary condition and boundary condition appears in the table.

6.	Click Close.

Step 11: Create Time History Nodes

1.	In the Model browser, isolate COMP-PSHELL_19.

2.	Click Tools > Create Solver Cards > TH > NODE.

3.	For Name, enter RAIL and select nodes on the Rail, as shown below.

rd3550_19

4.	For NUM_VARIABLES, select 1 and for Data: Var, enter the following:

rd3550_rail_14

Step 12: Create output requests and control cards

1.	Launch the Solver browser by selecting View > Solver Browser.

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	Car_Analysis
ENGINE KEYWORDS	RUN	Status	[Checked]
ENGINE KEYWORDS	RUN	Run Number	1
ENGINE KEYWORDS	RUN	Tstop	0.0601
ENGINE KEYWORDS	PRINT	Status	[Checked]
ENGINE KEYWORDS	PRINT	N_Print	-1000
ENGINE KEYWORDS	TFILE	Status	[Checked]
ENGINE KEYWORDS	TFILE	Time Frequency	9e-5
ENGINE KEYWORDS	ANIM/ELEM	Status	[Checked]
ENGINE KEYWORDS	ANIM/ELEM	EPSP	[Checked]
ENGINE KEYWORDS	ANIM/ELEM	VONM	[Checked]
ENGINE KEYWORDS	ANIM/ELEM	HOURG	[Checked]
ENGINE KEYWORDS	ANIM/VECT	Status	[Checked]
ENGINE KEYWORDS	ANIM/VECT	VEL	[Checked]
ENGINE KEYWORDS	ANIM/VECT	CONT	[Checked]
ENGINE KEYWORDS	ANIM/VECT	FOPT	[Checked]
ENGINE KEYWORDS	ANIM/DT	Status	[Checked]
ENGINE KEYWORDS	ANIM/DT	TStart	0
ENGINE KEYWORDS	ANIM/DT	Tfreq	0.003

Step 13: Export the model

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

2.	Enter a filename in the destination directory where you want to run.

3.	Enter the name FULLCAR and click Save.

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

5.	Click Merge starter and engine file to export the engine file with the model in one file.

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

Step 14: Run the solver using RADIOSS Manager

1.	Go to Start > Programs > Altair HyperWorks <version> RADIOSS.

2.	For Input file, browse to the exercise folder and select the file FULLCAR_0000.rad.

rd3550_radioss_mgr

Step 15 (Optional): View the Results in HyperView

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