RD-3060: Three Point Bending with HyperCrash

This tutorial demonstrates how to set up a 3-point bending model with symmetric boundary conditions in Y direction (across the XZ plane).

rd3060_3-point_bending

Model Description

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

•	Simulation time: in Rootname_0001.rad [0 – 7.0E-2s]

•	Only one half of the model is modeled because it is symmetric.

•	The supports are totally fixed. An imposed velocity of 1000 mm/s is applied on the Impactor in the (–Z) direction

•	Model size = 370mm x 46.5mm x 159mm

•	Honeycomb Material /MAT/LAW28: HONEYCOMB

[Rho_I] Initial density = 3.0e-10 ton/mm3

[E11], [E22] and [E33] Young’s modulus (Eij) = 200 MPa

[G11], [G22] and [G33] Shear modulus (Gij) = 150 MPa

•	Elasto-Plastic Material /MAT/LAW36: Inner, Outer and Flat

[Rho_I] Initial density = 7.85-9 ton/mm3

[E] Young’s modulus = 210000 MPa

[nu] Poisson's ratio = 0.29

•	Strain Curve:

	0	1	2	3	4	5	6	7	8	9
STRAIN	0	0.010	0.013	0.015	0.020	0.025	0.030	0.035	0.040	0.045
STRESS8E-	300	310	320	330	340	350	360	370	380	400

•	Elastic Material /MAT/PLAS_JOHNS: Impactor

[Rho_I] Initial density = 8e-9 ton/mm3

[E] Young’s modulus = 208000 MPa

[nu] Poisson's ratio = 0.29

Step 1: Import the RADIOSS mesh model

1.	Open HyperCrash 2017.

2.	For User profile:, select RADIOSS V14.

3.	For Unit system:, select N mm s T.

4.	Select User interface style as New.

5.	Click Run.

6.	Click File > Import > RADIOSS.

7.	In the input window, navigate to the correct directory and select BENDING_0000.rad.

Click OK.

Step 2: Create and assign a material

1.	Click Model > Material.

2.	In the Window, right-click and select Create New > Elastic > Linear elastic (1) as shown below:

rd3060_linear_elastic_12

3.	For Title, enter Rigid Material.

4.	Enter all the material data, as shown in the following image.

rd3060_rigid_mat_14

5.	Right-click in the entry box Support and click Include picked parts and select the parts Impactor and Support in the graphics area.

6.	Click Yes in the lower right corner to validate.

7.	Press ENTER or click Save to validate.

Step 3: Create and assign a material for Inner, Outer, and Flat parts

1.	In the Window, right-click and select Create New > Elasto-plastic > Piecewise linear (36).

2.	For Title, enter Shell Material.

3.	Enter all the material data, as shown in the following image:

rd3060_plas_tab

4.	Open the Strain rate folder and click to add a row.

5.	Right-click in Yield stress function field and click Select in Model to select an existing function in the model.

rd3060_select_model

6.	In the Function file window, select the function with an ID of 2, then click OK to import the curve. The function can be edited, as shown in the image below.

rd3060_function_14

7.	Click the Tree tab and select the parts Inner, Outer, and Flat on the tree.

8.	Click to isolate this part.

9.	Click the Material tab.

10.	Right-click the entry box Support, and click Include picked parts in the graphic area, and select the parts Inner, Outer and Flat in the graphics area as shown in the following image.

rd3060_parts

11.	Click Yes in the lower right corner to validate.

12.	Press ENTER or click Save to validate.

Step 4: Create and assign a new material for HCFoam

1.	In the Window, right-click and select Create New > Honeycomb > Honeycomb orthotropic (28).

2.	For Title, enter Foam.

3.	Enter all the material data, as shown in the following image:

rd3060_honeycomb_13

4.	Right-click on the Yield stress function 11 field and click Select in Model to select a curve already present in the model.

5.	In the Function file window, select the function with ID of 5, then select OK.

6.	Repeat this process for the Yield functions, as shown in the following image.

rd3060_yield_functions_13

7.	Click the Tree tab and select the part HCFoam (7) on the tree.

8.	Click to show only this part.

9.	Click the Material tab.

10.	Right-click in the entry box Support, and click Include picked parts to select the part HCFoam in the graphics area as shown in the following image.

rd3060_hcfoam

11.	Click Yes in the lower right corner.

12.	Click Save > Close.

Step 5: Create and assign a property

1.	Click Model > Property.

2.	In the Window, right-click and select Create New > Surface > Shell (1), as shown below.

rd3060_shell_12

3.	For Title, enter Shell Property.

4.	Enter Shell thickness and Shell element formulation values, as shown in the following image.

rd3060_shell_prop_14

5.	Click the Tree tab and select the parts Inner, Outer and Flat on the tree.

6.	Click to show only these parts.

7.	Click the Property tab.

8.	Right-click in the entry box Support, and click Include picked parts to select the parts Inner, Outer and Flat in the graphics area to assign Shell property.

9.	Click Yes in the lower right corner.

10.	Click Save.

Step 6: Create and assign a property for Impactor and Support

1.	For Title, enter Rigid Property.

2.	Enter the Shell thickness value as .9119, as shown in the following image.

rd3060_rigid_prop_14

3.	Click the Tree tab and select the parts Impactor and Support in the tree.

4.	Click to show only these parts.

5.	Click the Property tab.

6.	Right-click in the entry box Support and click Include picked parts to select the parts Impactor and Support in the graphics area to assign Rigid property.

7.	Click Yes in the lower right corner.

8.	Click Save.

Step 7: Create and assign a property for HCFoam

1.	In the Window, right-click and select Create New > Volume > General solid (14).

2.	For Title, enter Foam.

3.	Click the Tree tab and select the part HCfoam on the tree.

4.	Click to show only this part.

5.	Go back to the Property tab.

6.	In the Flag for solid elements formulation, select HEPH.

rd3060_solid_14

7.	Right-click in the entry box Support and click Include picked parts to select HCfoam in the graphics area to assign Foam property.

8.	Click Yes in the lower right corner.

9.	Click Save > Close.

Step 8: Create rigid body for Impactor

1.	From the menu bar, click Mesh Editing > Rigid Body.

2.	In the window, right-click to select Create New, enter the name Impactor.

3.	Click the Tree tab and select the Impactor assembly on the tree.

4.	Click to show all parts.

5.	Click the Mesh Editing tab.

6.	Right-click in the entry box Support and right-click in the graphic area (as shown below). Select Include picked parts option to select Impactor in graphic area.

rd3060_impactor

7.	Click Yes > Save.

Step 9: Create rigid body for Support

1.	In the Title field, enter the name Support.

2.	Click in the entry box Support and right-click in the graphic area. Click Include picked parts option to select Support in the graphic area.

3.	Click Yes to complete the selection.

4.	Click Save. The rigid body for Support should look like the following image.

rd3060_support

5.	Click Close.

Step 10: Define boundary conditions for the model

1.	Click LoadCase > Boundary Condition.

2.	In the window, right-click to select Create New.

3.	Press F6 to show the rigid bodies.

4.	In the Title field, enter Boundary.

5.	Right-click in the entry box Support and right-click in the graphic area. Click Add/Remove nodes by picking selection and select the master node of the rigid body.

rd3060_impactor_master

6.	Constrain all DOF except translation in Z as shown in the following image. To constrain the nodes, check the boxes for TX, TY, RX, RY and RZ.

rd3060_bc_comp_14

7.	Click Save.

8.	Repeat the same process to create boundary conditions for the Support and Symmetry boundary condition for the inner/outer/flat.

9.	Click node selection icon to select master node of Support, as shown in the following image.

rd3060_support2

10.	Constrain all DOF by selecting TX, TY, TZ, RX, RY and RZ, as shown in the following image.

rd3060_bc_comp2_14

11.	Click Save.

12.	In the Boundary condition creation field, enter Symmetry.

13.	Click the Tree tab and select the parts Inner, Outer, HCfoam and Flat on the tree.

14.	Click to show only these parts.

15.	Press the p key to change the perspective visualization.

16.	Click the Boundary Condition tab.

17.	From the Visualization toolbar, select the YZ View, as shown below.

rd3060_YZ_view

18.	Right-click in the entry box Support, right-click in the graphic window, and click Add nodes by box selection to select the nodes, as shown in the image below

rd3060_nodes

19.	To constrain the nodes, select TY, RX and RZ.

rd3060_bc_comp3_14

20.	Click Save > Close.

Step 11: Define Impactor Velocity

1.	Click LoadCase > Imposed > Imposed Velocity.

2.	In the window, right-click to select Create New.

3.	For Title, enter IMPOSED VELOCITY.

4.	For Direction, select Z (translation) and -1000 for Y-Scale factor.

5.	For Time function, use the predefined curve in the model Funct 1.

6.	For Y Scale factor, enter -1000.

7.	Press the F6 key to show the rigid bodies.

8.	Click in the entry box Support and right-click in the graphic area. Click and select the master node of Impactor.

9.	Click Yes in the lower-right corner.

rd3060_rigid_body

10.	Click Save > Close.

Step 12: Define contacts for the model

1.	Click LoadCase > Contact Interface.

2.	In the window, right-click and select Create New > Multi usage (Type 7).

3.	Click on the check box next to Create symmetric interface at saving.

4.	For Title, enter Support.

5.	Click the Tree tab and select the parts Flat and Support on the tree.

6.	Click to show only these parts.

7.	Click the Contact Interface tab.

8.	Set Min gap for impact active to 0.2.

9.	Set Coulomb friction to 0.1.

10.	Set [Iform] Friction penalty formulation at 2 [Stiffness].

11.	Click in the Slave nodes entry box and right-click in the graphic window. A menu appears, click Include Picked Parts and select the FLAT.

12.	Press Y or click Yes at the bottom right of the screen. HyperCrash will automatically move to the selection of the Master surface.

13.	Right-click and click Include Picked Parts and select the Support.

14.	Press Y or click Yes at the bottom right of the screen.

rd3060_flat_comp

15.	Click Save.

16.	Repeat the same process to create contact between Outer and Impactor.

17.	Click the Tree tab and select the parts Outer and Impactor on the tree.

18.	Click to show only these parts.

19.	Right-click in the window and select Create New > Multi usage (Type 7).

20.	Click the Contact Interface tab.

21.	Click on the check box next to Create symmetric interface at saving.

22.	In the Title, enter Imp_Outer.

23.	Set Min gap for impact active to 0.2.

24.	Set Coulomb friction to 0.1.

25.	Set [Iform] Friction penalty formulation to 2 [Stiffness].

26.	Select Outer Part as Slave and Impactor as Master, as shown in the following image.

rd3060_slave_outer

27.	Click Save.

28.	Repeat the same process for self impact for Outer, Inner and Flat, as self impact.

29.	Click the Tree tab and select the parts Outer, Inner and Flat on the tree.

30.	Click to show only these parts.

31.	Click the Contact Interface tab.

32.	Select Self-Impact.

33.	Set Title as Self.

34.	Set the Min gap for impact active to 0.7.

35.	Set the Coulomb friction to 0.1.

36.	Set [Iform] Friction penalty formulation to 2 [Stiffness].

37.	Select components Outer, Inner and Flat, as shown in the following image.

rd3060_component

38.	Click Save.

Step 13: Clean the model

1.	Click Mesh Editing > Clean.

rd3060_clean_menu

2.	Select All.

3.	Click Clean > Close.

Step 14: Export the model

1.	Click Model > Control Card and select the control cards in the images below.

Note:

Make sure to save each control card before editing the next.

rd3060_control_card

rd3060_control_card2

rd3060_control_card2A

rd3060_control_card3

2.	Click File > Export > RADIOSS.

3.	In the Output window that opens, enter the name 3PBENDING and click OK.

4.	Leave the Header of RADIOSS File window empty and click Save Model.

The Starter file 3PBENDING_0000.rad is written.

Step 15: Open RADIOSS Manager from windows Start menu

rd3060_solver_run_13

Step 16: Run the model 3PBENDING_0000.rad using RADIOSS Manager in the class_exercise folder

Step 17: Review the listing files for this run and verify on the results

1.	Using HyperView, plot the displacement and strain contour.

rd3060_results14

Plastic Strain Simple Average and Rigid Body Force (Impactor)