HyperWorks Solvers

RD-3000: Tensile Test Setup using HyperCrash

»Click here to display Table of Contents« RADIOSS > Tutorials and Examples > Tutorials > Large Displacement Finite Element Analysis > HyperCrash:

RD-3000: Tensile Test Setup using HyperCrash
RD-3000: Tensile Test Setup using HyperCrash

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

rd3500_tensile

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_0001.rad [0 – 10.]

•	Boundary Conditions:

o	The 3 upper right nodes (TX, 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

[EPS_max] Failure plastic strain = 0.75

[SIG_max] Maximum stress = 0.175 GPa

Input file for this tutorial: TENSILE_0000.rad

Exercise

Step 1: Import the mesh

1.	Open HyperCrash and set the User profile: to RADIOSS V14 and the Unit system: to kN mm ms kg.

1.	Click Run.

2.	From the menu bar, select File > Import > RADIOSS.

3.	In the Select RADIOSS File(s) dialog, select TENSILE_0000.rad.

4.

Click OK.

Setting up the Problem in HyperCrash

Step 2: Create and assign a material

1.	From the menu bar, select Model > Material.

2.	Right-click in the material list and select Create New > Elasto-plastic > Johnson-Cook (2).

3.	For Title, enter Aluminum. Enter all the material data listed above.

4.	In the bottom of the material window, right-click in the Support entry box and select Include picked parts icon .

rd3000_include_pick_part_14

5.	Select the part in the graphics area (left-click).

6.	Right-click to validate the selection.

7.	Press ENTER or click Save > Close.

Step 3: Create and assign a property

1.	From the menu bar, select Model > Property.

2.	Right-click in the property list and select Create New > Surface > Shell (1).

3.	For Title, enter Pshell.

4.	For Shell Thickness, enter 1.7.

5.	In the bottom of the property window, right-click in the Support entry box and select Include picked parts icon .

6.	Select the part in the graphics area.

7.	Right-click to validate the selection.

8.	Click Save > Close.

Step 4: Define boundary conditions representing symmetry

1.	From the menu bar, select LoadCase > Boundary Condition.

2.	Right-click in the display list area and select Create New.

3.	For Name, enter constraint1 and click Save. Expand the folders Translation and Rotation.

4.	Right-click in the Support entry box, click Select in graphics and select Add/Remove nodes by picking selection icon to select the nodes in the Graphic Window, as shown in the figure below:

rd3000_bc2

5.	Click Yes in the Dialog menu bar to validate your selection.

6.	To constrain the nodes, toggle Tx, Ry and Rz and click Save.

7.	Repeat the same operations to create constraint2, as shown in the figure below:

rd3000_node

8.	Toggle Tx, Ty, Tz, Rx, Ry and Rz, and click Save.

9.	Repeat the same operations to create constraint3, as shown in the figure below. Press SHIFT, left-click and hold the mouse to draw a box to select the nodes.

rd3000_constraint3

10.	Toggle Ty, Rx, and Rz.

11.	Click Save > Close.

Step 5: Define the imposed velocity

1.	From the menu bar, select LoadCase > Imposed > Imposed Velocity.

2.	Right-click in the display list area and select Create New.

3.	Set the Title to imposed_velocity.

4.	Right-click in the entry box for Time function and select Define Function. A Function Window opens up.

5.	For Function name, enter FUNC_VEL.

6.	Enter the first point (0,1) and click Validate.

7.	Enter the second point (1e30,1) and click Validate.

8.	Click Save in the dialog.

9.	Right-click in the Support entry box, click Select in graphics and select the Add nodes by box selection icon , to select the nodes in the graphic window, as shown in the figure below:

rd3000_Yscale

10.	Go to the Properties tab and enter a Y-Scale factor = -1.

11.	Ensure Direction of the imposed velocity is set to X (translation).

12.	Click Save > Close.

Step 6: Select a node for time history output

1.	From the menu bar, select Data History > Time History.

2.	In the list display area, right-click and select Create New > TH of nodes.

3.	Enter the title Node_79.

4.	Click Add Row to add a new row. With that row selected, scroll down to the input section and enter NODid as 79 and press ENTER.

As an alternative, use the Pick button to select a node in the graphic window.

5.	Click Save > Close.

Step 7: Create Control Cards, Export the Starter and Engine files

1.	From the menu bar, select Model > Control Card:

control_card_menu

2.	Enter the values for the Control Cards, as shown in the images below, saving after every step:

rd3000_control_card2

rd3000_control_card4

rd3000_control_card_tfile

rd3000_anim_dt

rd3000_anim_eltype_restype

rd3000_anim_vect

3.	Click File > Export > RADIOSS to export the solver file.

4.	In the Write Block Format 140 RADIOSS File window that opens, navigate to your desired run directory and create a new folder named TENSILE_TEST.

5.	For filename, enter TENSILE and click OK.

6.	Leave the Header window empty and click on Save Model. The file TENSILE_0000.rad is written.

The model is now ready to run through the Starter and the Engine. It will produce the result files TENSILEA* for animation in HyperView and TENSILE01 for time history plotting in HyperGraph.

RADIOSS Computing

Step 8: Run RADIOSS Starter and RADIOSS Engine

1.	Launch RADIOSS from the Start menu. A HyperWorks Solver Run Manager window appears.

rd3000_run_mgr_14

2.	In the Input file field, select TENSILE_0000.rad. from the folder you created.

3.	Click Run.

The HyperWorks Solver View window is opened. The RADIOSS Starter will run and on completion the RADIOSS Engine will automatically run.

Step 9: Review the listing files for this run and verify the results

1.	See if there are any warnings or errors in the .out files.

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

Exercise Expected Results

rd3000_contour_total_disp

Total Displacement Contour (mm)

rd3000_contour_plastic_strain

Plastic Strain Contour

See Also:

RADIOSS Tutorials

HyperCrash User's Guide