# RD-T: 3550 Simplified Car Front Pole Impact

This tutorial demonstrates how to simulate frontal pole test with a simplified full car.

The model description is as follows:
• 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

1. Launch HyperMesh Desktop.
2. From the Preferences menu, select User Profiles or click the icon in toolbar.
3. Select Radioss (Radioss2021) and click OK.

## Open the Model File

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

## Create and Assign the Material for Windshield

1. In the Model Browser, right-click and select Create > Material.
The 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:
5. In the Model Browser, select components COMP-PSHELL_3 and COMP-PSHELL_16.
6. Click Mat_Id in the , select the material windshield and click OK to update the selected components with the created material.

## Create and Assign the Material for Rubber

1. In the Model Browser, right-click and select Create > Material.
The is displayed below the Model Browser.
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:
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.

## Create and Assign the STEEL Material

1. In the Model Browser, right-click and select Create > Material.
The is displayed below the Model Browser.
2. For Name, enter steel.
3. Set Card Image to M2_PLAS_JOHNS_ZERIL.
4. Input the values, as shown below:
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.

## Create an Infinite Plane Rigid Wall

1. In the Model Browser, right-click and select Create > Rigid Wall.
The 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.
7. Go to the Analysis > 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 and then click return.

## Create a Cylindrical Rigid Wall

1. In the Model Browser, right-click and select Create > Rigid Wall.
The is displayed.
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.
8. Go to Analysis > 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 and then click return.

## Define the Self Contact (TYPE7)

1. Hide all the 1D (TRUSSES) and 3D (SOLID) parts in the model by opening the Solver Browser and clicking PROP > SHELL, Isolate only.
2. Return to the Model Browser 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. For Surf_id (M) (master entity), set the option to Components, select displayed components, and click OK.
6. Input other parameters, as shown below.

## Define the Contact between the Engine and Radiator (TYPE7)

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, set the Card Image as TYPE7, and click Yes to confirm.
6. For Grnod_id (S) (slave entity), set the selector switch to Components, click Components, and select COMP-PSOLID_26.
7. For Surf_id (M) (master entity), set the selector switch to Set, click Set, and select engine.
8. Input the values, as shown below:

## Define the Initial Velocity

1. Click Tools > BCs Manager to start the BCS Manager.
2. For Name, enter 35MPH, set Select type as Initial Velocity and set GRNOD to Parts.
3. Click comps and select all of the parts in the model.
4. Set Vx as 15600.
5. Click Create to create the boundary condition.
The boundary condition appears in the table.
6. Click Close.

## Create Time History Nodes

1. In the Model Browser, isolate COMP-PSHELL_19.
2. Click Tools > Create > Cards > TH > NODE.
3. For Name, enter RAIL and select the nodes on the Rail, as shown below.
4. For NUM_VARIABLES, select 1 and for Data: Var, enter the following:

## Create Control Cards

1. To start the Engine file assistant, select Tools > Engine File Assistant.
2. Select Create engine file and enter,
1. Termination Time, enter 0.06.
2. Animation output frequency, enter 0.003.
3. Time history output request, enter 9e-5.
4. Nodal time step, enter 0.
5. Toggle Generate default output request.

## 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 FULLCAR 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 2021 > Radioss.
2. For Input file, browse to the exercise folder and select the file FULLCAR_0000.rad.
3. Click Run.

## Review the Results

The exercise is complete. Save your work to a HyperMesh file. You can view the results in HyperView.