HyperWorks Solvers

RD-3050: Simplified Car Pole Impact in HyperCrash

RD-3050: Simplified Car Pole Impact in HyperCrash

 Previous topic Next topic No expanding text in this topic  

RD-3050: Simplified Car Pole Impact in HyperCrash

 Previous topic Next topic JavaScript is required for expanding text JavaScript is required for the print function  

To simulate frontal pole test with a simplified full car.

rd3550_car

Model Description

•UNITS: Length (mm), Time (s), Mass (ton), Force (N) and Stress (MPa)
•Simulation time:  Engine file (_0001.rad)  [0 – 0.06 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/PLAS_JOHNS (WINDSHIELD)

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

[E] Young's Modulus = 76000 MPa

[nu] Poisson’s Ratio = 0.3

[symbol0] Yield Stress = 192 MPa

[K] Hardening Parameter = 220 MPa

[n] Hardening Exponent = 0.32

•Elasto-plastic Material /MAT/PLAS_JOHNS (STEEL)

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

[E] Young's Modulus = 210000 MPa

[nu] Poisson’s Ratio = 0.3

[symbol0] Yield Stress = 200 MPa

[K] Hardening Parameter = 450 MPa

[n] Hardening Exponent = 0.5

[SIG_max] Maximum Stress = 425 MPa

•Elasto-plastic Material /MAT/PLAS_JOHNS (RUBBER)

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

[E] Young's Modulus = 200 MPa

[nu] Poisson’s Ratio = 0.49

[symbol0] Yield Stress = 1e30 MPa

[n] Hardening Exponent = 1

 

Exercise

Step 1:  Retrieve the HyperMesh file

1.Open HyperCrash and set the User profile: to RADIOSS V14 and the Unit system: to kN mm ms. kg.
2.Set User Interface style as New.
3.Set the working directory to <install_directory>/tutorials/hwsolvers/radioss.
4.Click Run.
5.Click File > Import > Nastran.
6.In the input window, select full_car.nas.
7.Click OK.

Step 2:  Create WINDSHIELD material and assign to car windows

1.Click Model > Material.
2.In the Material list, right-click and select Create New > Elasto-Plastic > Johnson-Cook (2).
3.For Title, enter WINDSHIELD.
4.Enter all the material data, as shown in the image below.

rd3050_windshield_12

5.Click the Tree tab and select PSHELL3 and PSHELL16 in the tree.
6.Click 06_view to show only these parts.
7.Click the Material tab.
8.Right-click in the Support entry box and click Selected Parts of Tree selected_part_of_tree_button. This icon allows adding the part selected in the tree to the selection. The selected parts will be highlighted in the graphic area.
9.Click Save.

Step 3:  Create RUBBER material and assign to car tires

1.In the Material list, right-click and select Create New > Elasto-Plastic > Johnson-Cook (2).
2.For Title, enter RUBBER. Enter all the material data, as shown in the image below.

rd3050_rubber_13

3.Click the Tree tab and select PSHELL20 to PSHELL23 in the tree.
4.Click 06_view to show only these parts.
5.Click the Material tab.
6.Right-click in the Support entry box and click Selected Parts of Tree selected_part_of_tree_button. The selected parts will be highlighted in the graphic area.
7.Click Save.

Step 4:  Create STEEL material and assign to all other parts

1.In the Material list, right-click and select Create New > Elasto-Plastic > Johnson-Cook (2).
2.For Title, enter STEEL.
3.Enter all the material data, as shown in the image below.

rd3050_steel_13

4.Click the Tree tab and select PSHELL3, PSHELL16 and PSHELL20 to PSHELL23 in the tree.
5.Click 06_invert to invert the tree selection.
6.Click 06_view to show all the parts except the ones made with glass and rubber.

rd3050_car_13

7.Click the Material tab.
8.Right-click in the Support entry box and click Selected Parts of Tree selected_part_of_tree_button . The selected parts will be highlighted in the graphic area.
9.Click Save > Close.

Step 5:  Create a rigid wall to represent the ground

1.Click LoadCase > Rigid Wall > Create.
2.Under Rigid wall name > Select RWALL type, select Infinite Plane.
3.Enter the rigid wall name, Ground.
4.Enter the following values for M0 and M1:

rd3050_ground_13

5.In the Selection tab, set the Distance to search for slave nodes to 300.
6.Click See at the bottom of the panel to display the rigid wall.
7.Click Save.

Step 6:  Create Pole Rigid Walls

1.Under Rigid wall name > Select RWALL type, select Cylinder.
2.Enter the rigid wall name, Pole.
3.Enter the following values for M0 and M1:

rd3050_pole_13

4.Set the Diameter to 500.
5.Set the Distance to search for slave nodes to 1500.
6.Click See at the bottom of the panel to display the rigid cylinder.
7.Click Save.
8.Click Close to close the Rigid Walls panel.

Step 7:  Define interface with the whole car

1.Click LoadCase > Contact Interface.
2.In the window right-click and select Create New > Multi usage (Type 7).
3.Select the Self Impact box.
4.In the Title field, enter CAR_CAR.
5.Set [Istf] Stiffness definition to 2: (K=(Km+Ks)/2.
6.For [Gapmin] Min. gap for impact activ., enter 0.7.
7.For [Fric] Coulomb friction, enter 0.2.
8.Set [Iform] Friction penalty formulation to 2: (Stiffness).
9.In the Model Display toolbar, click Display All view_all_button to display the entire model.
10.Click in the [Mast_id] Master field. Move the cursor to the graphical window and right-click. The menu shown in the image below should appear. Choose the option Add selected parts by box 05_add_parts and use the mouse to drag a box to select the entire car in the graphic window.

rd3050_add_parts

11.Click Save.

Step 8:  Create an interface between engine and radiator

1.Right-click in the Contact list and select Create New > Multi usage (Type 7).
2.Check Create symmetric interface at saving box.
3.In the Title field, enter ENGINE_RADIATOR.
4.For [Istf] Stiffness definition, set to 2 (K=(Km+Ks)/2.
5.For [Gapmin] Min. gap for impact active, enter 0.7.
6.For [Fric] Coulomb friction, enter 0.2.
7.For [Iform] Friction penalty formulation, set to 2 [Stiffness].
8.In the Tree tab, highlight the part PSHELL28 (Radiator) and PSHELL30 (Engine) and Isolate them.
9.In the Contact Interface tab, click in the [Slav_id] Slave nodes field, move the cursor to the graphic window, right-click and select Include picked Part. Select the Radiator (PSHELL28).
10.In the Contact Interface tab, click in the [Mast_id] Master Surface field, move the cursor to the graphic window, right-click and select Include picked Part. Select the Engine (PSHELL30).
11.Click Save.
12.Click Close to close the Contact tab.

An additional symmetric interface is created.

Step 9:  Define Initial Velocities

1.Click LoadCase > Initial Velocity.
2.In the Velocity list, right-click and select Create New.
3.In the Title field, enter 35MPH.
4.In the Tree window, highlight FULL_CAR.
5.In the [Vx] field, enter 15600.
6.In the Initial Velocity tab and click in the [Gnod_id] Support field. Move the cursor to the graphic window, right-click and select Add selected parts of tree selected_part_of_tree_button.
7.Click Save > Close.

Step 10:  Define Time History Nodes

1.Click Data History > Time History.
2.In the Time History list, right-click and select Create New > TH of nodes.
3.For Title, enter RAIL.
4.In the Tree tab, select PSHELL19.
5.Click Isolate Tree Selections 06_view.
6.Go back to the Time History panel and click Add/Remove nodes by picking selection arrow_up in the second table.

rd3050_add-remove

7.Select six nodes on the rails, for example as shown in the following image:

rd3050_data_history

7.Click Yes in the lower right corner or right-click in the graphic window to exit the selection.
8.Click Save > Close.

Step 11:  Export the model

1.Create the Engine file:  From the menu bar, select Model > Control Card.
2.Check the Control Cards, as shown in the images below.
Note:Make sure to save all control card before editing the next.

rd3050_control_card

rd3050_control_card2

rd3050_control_card3

3.Under the Quality menu, click Model Checker to check the quality, then check All Solver Contact interfaces, remove all the initial penetrations in the model.
4.Under Mesh Editing menu, click Clean, then clean the model before exporting.
5.Click File > Export > RADIOSS, enter FULLCAR and click OK.
6.Leave the Header of RADIOSS File window empty and click Save Model. The Starter file FULLCAR_0000.rad is written.

Step 12:  Open RADIOSS from Windows Start menu

rd3050_solver_run

Step 13: Select the Starter file FULLCAR_0000.rad as Input file and Run the model

Exercise Expected Results

rd3050_results

Final deformation and energy balance plot

See Also:

RADIOSS Tutorials

HyperCrash User's Guide