RD-3500: Tensile Test Setup using HyperMesh

This tutorial demonstrates how to simulate a uniaxial tensile test using a quarter size mesh with symmetric boundary conditions.

The model is reduced to one-quarter of the total mesh with symmetric boundary conditions to simulate the presence of the rest of the part.

rd3500_01

Model Description

•	UNITS: Length (mm), Time (ms), Mass (kg), Force (kN) and Stress (GPa)

•	Simulation time Rootname_0000.rad [0 – 10.]

•	Boundary Conditions:

o	The 3 upper right nodes (TX, RY, and RZ)

o	The center node on left is totally fixed (TX, TY, Rx, RY, and RZ)

o	A symmetry boundary condition on all bottom nodes (TY, Rx, and RZ)

•	At the left side is applied a constant velocity = 1 mm/ms on -X direction.

•	Tensile test object dimensions = 11 x 100 with a uniform thickness = 1.7 mm

Johnson-Cook elastic plastic material /MAT/PLAS_JOHNS (Aluminum 6063 T7)

[Rho_I] Initial density = 2.7e-6 Kg/mm3

[E] Young’s modulus = 60.4 GPa

[nu] Poisson’s ratio = 0.33

[a] Yield Stress = 0.09026 GPa

[b] Hardening Parameter = 0.22313 GPa

[n] Hardening Exponent = 0.374618

[SIG_max] Maximum Stress = 0.175 GPa

[EPS_max] Failure Plastic Strain = 0.75

Input file for this tutorial: TENSILE_000.rad

Exercise

Step 1: Load the RADIOSS (Block) User Profile

1.	Launch HyperMesh Desktop.

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

3.	Select RADIOSS (Block140) and click OK.

Step 2: Load the solver deck

1.	Click File > Import > Solver Deck or click .

2.	Click the Select File icon to open the TENSILE_0000.rad file you saved to your working directory from the radioss.zip file. Refer to Accessing the Model Files.

3.	Click Open.

4.	Click Import.

5.	Click Close to close the window.

Step 3: Define material for the tensile test object

1.	In the Model browser, right-click and select Create > Material.

A Material with name material1 of card image M1_Elastic appears in the Entity Editor (EE) in the bottom pane of the Model browser.

2.	In the Entity Editor (EE), for Name, enter Mat_1 in the Value field.

3.	Set Card Image to M2_PLAS_JOHNS_ZERIL.

4.	Click Yes on the pop-up that warns of a card image change.

5.	Input the values, as shown in the following image in the EE.

rd3500_mat1_1

Step 4: Define property for the tensile test specimen

1.	In the Model browser, right-click and select Create > Property.

A Property with name property1 of card image P1_SHELL appears in the Entity Editor (EE) in the bottom pane of the Model browser.

2.	For Name, enter sheet_1.7.

3.	For Thick, enter 1.7. in the Value field corresponding to sheet thickness.

rd3500_02

Step 5: Assign material and property to the test specimen

1.	In the Model browser, select the SHELL_1 component. The Entity Editor opens for the component.

2.	For Name, enter Tensile_coupon.

3.	Click Prop_Id, to activate the option.

4.	Click Unspecified > Property.

5.	In the Select Property dialog, select sheet_1.7 from the list and click OK.

6.	Repeat steps 3 - 5 for Mat_Id and select Mat_1.

rd3500_04

Step 6: Create boundary conditions

1.	From the Utility browser, start the BCs Manager from the pull-down menu, select Tools > BCs Manager.

2.	For Name, enter constraint1, set Select type to Boundary Condition and set GRNOD to Nodes.

rd3500_constraint1

3.	Click on Nodes. A nodes selection appears. Select the three nodes, as shown in the figure below and click proceed.

rd3500_nodes4

4.	Fix degrees of freedom Tx, Ry and Rz.

5.	Click Create to create the constraint. The created constraint appears in the table, and handles appear in the graphics area.

6.	For Name, enter constraint2, set Select type to Boundary Condition and set GRNOD to Nodes.

7.	Select the node, as shown in the image below.

rd3500_node

8.	Fix degrees of freedom Tx, Ty, Rx, Ry and Rz.

rd3500_05

9.	Click Create to create the constraint. The created constraint appears in the table, and a handle appears in the graphics area.

10.	For Name, enter constraint3, set Select type to Boundary Condition and set GRNOD to Nodes.

11.	Select the nodes, as shown in the image below.

rd3500_nodes5

12.	Fix degrees of freedom Ty, Rx and Rz.

13.	Click Create to create the constraint. The created constraint appears in the table, also handles appear in graphics.

Step 7: Create Imposed Velocity

1.	For Name, enter velocity, set Select type as Imposed Velocity and set GRNOD to Nodes.

2.	Select the nodes, as shown in the image below.

rd3500_imp_vel

3.	Set the direction as X and Scale Y as -1.0.

4.	Click Create/Select curve ID for Curve ID. An XY curve editor appears.

5.	Click New to create a new curve.

6.	For Name, enter Load and click proceed.

7.	Enter the values, as shown in table below.

rd3500_xy

8.	Click Update to update the curve with the new values.

9.	Click Close to close the Curve editor, the created curve is assigned to this constraint.

10.	Click Create to create the velocity boundary condition.

11.	Click Close to close the BCs Manager.

Step 8: Create output requests and control cards

For this exercise the output request will be generated from the Engine file assistant which is located in the Utility browser.

1.	To start the Engine file assistant, select Tools > Engine File Assistant.

2.	Input the values, as shown below:

rd3500_engine_file_assistant

The tool generates typical output requests, such as stress, strain, velocity, etc.

rd3500_export

Step 9: Export the model as TENSILE_0000.rad

1.	From the File menu, click Export > Solver Deck or click the Export Solver Deck icon .

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

3.	Enter the name TENSILE_0000.rad and click Save.

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

5.	Select Merge starter and engine file to export the Engine and Starter file as one file.

6.	Click Export > Close.

Step 10: Open RADIOSS Manager from Start menu

Step 11: Run the model TENSILE_0000.rad using RADIOSS Manager

1.	Select the TENSILE_0000.rad for the Input file.

2.	Click Run.

rd3500_radioss_mgr

Step 12: Review the listing files for this run and verify the results

1.	See if there is any warning or errors on .out files.

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

Exercise Expected Results

rd3500_total_displace_14

Total Displacement Contour (mm)

rd3500_plastic_strain_14

Plastic Strain Contour