RD-T: 3000 Tensile Test Setup

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


rd3500_tensile
Figure 1.
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
Figure 2.
The model description is as follows:
  • UNITS: Length (mm), Time (ms), Mass (kg), Force (kN) and Stress (GPa)
  • Simulation time Rootname_0001.rad [0 - 10.]
  • Boundary Conditions:
    • The 3 upper right nodes (TX, RY, and RZ)
    • 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] Plasticity yield stress = 0.09026 GPa

[b] Plasticity hardening parameter = 0.22313 GPa

[n] Plasticity hardening exponent = 0.374618

[EPS_p_max] Failure plastic strain = 0.75

[SIG_max0] Plasticity maximum stress = 0.175 GPa

Model Files

Before you begin, copy the file(s) used in this tutorial to your working directory.

Start HyperCrash

  1. Open HyperCrash.
  2. Set the User profile to RadiossV2022 and the Unit system to kN mm ms.kg.
  3. Set User Interface style as New.
  4. Set your working directory to where the downloaded file is located.
  5. Click Run.
  6. Click File > Import > Radioss.
  7. In the input window, select TENSILE.rad.
  8. Click OK.

Create and Assign a Material

  1. From the menu bar, select Model > Material.
  2. In the Material tab, right-click 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 selectpartgeneral-24.

    rd3000_include_pick_part_14
    Figure 3.
  5. Select the part in the modeling window (left-click).
  6. Right-click to validate the selection.
  7. Press Enter or click Save > Close.

Create and Assign a Property

  1. From the menu bar, select Model > Property.
  2. In the Property tab, right-click 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 the Include picked parts icon selectpartgeneral-24.
  6. Select the part in the modeling window.
  7. Right-click to validate the selection.
  8. Click Save > Close.

Define Boundary Conditions Representing Symmetry

  1. From the menu bar, select LoadCase > Boundary Condition.
  2. Right-click in the Boundary Condition tab and select Create New.
  3. For Title, enter constraint1 and click Save.
  4. Expand the Translation and Rotation folders.
  5. Right-click in the Support entry box, click Select in graphics and select the Add/Remove nodes by picking selection icon arrow_up to select the nodes in the modeling window, as shown in the figure below:

    rd3000_bc2
    Figure 4.
  6. Click Yes in the Dialog menu bar to validate your selection.
  7. To constrain the nodes, toggle Tx, Ry and Rz and click Save.
  8. Repeat the same operations to create constraint2, as shown in below:

    rd3000_node
    Figure 5.
  9. Toggle Tx, Ty, Tz, Rx, Ry and Rz, and click Save.
  10. Repeat the same operations to create constraint3, as shown in below.
  11. Press Shift, left-click and hold the mouse to draw a box to select the nodes.

    rd3000_constraint3
    Figure 6.
  12. Toggle Ty, Rx, and Rz.
  13. Click Save > Close.

Define Imposed Velocity

  1. From the menu bar, select LoadCase > Imposed > Imposed Velocity.
  2. Right-click in the Imposed Velocity tab and select Create New > Imposed Velocities.
  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 selectbyboxadd-24, to select the nodes in the modeling window, as shown in below:

    rd3000_Yscale
    Figure 7.
  10. Go to the Properties tab and enter a Y-Scale factor = -1.
  11. Ensure Direction is set to X (translation).
  12. Click Save > Close.

Define a Time History Node

  1. From the menu bar, select Data History > Time History.
  2. In the Time History tab, right-click and select Create New > TH of nodes.
  3. In the Title field, enter Node_79.
  4. Click Add Row addrow to add a new row.
  5. With that row selected, for NODid, enter 79 and press Enter.
    As an alternative, use the Pick button to select a node in the modeling window.
  6. Click Save > Close.

Export the Model

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

    control_card_menu
    Figure 8.
  2. Enter the values for the Control Cards, as shown in the images below, saving after every step:

    rd3000_control_card2
    Figure 9.

    rd3000_control_card4
    Figure 10.

    rd3000_control_card_tfile
    Figure 11.

    rd3000_anim_dt
    Figure 12.

    rd3000_anim_eltype_restype
    Figure 13.

    rd3000_anim_vect
    Figure 14.
  3. Click File > Export > Radioss to export the solver file.
  4. In the Write Block Format 2022 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 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.

Open Compute Console from the Windows Start Menu

  1. From the Start menu, select Compute Console.
    The Altair Compute Console opens.
  2. In the Input file field, select TENSILE_0000.rad from the folder you created.


    Figure 15.
  3. Click Run.
    The Radioss Starter will run and on completion the Radioss Engine will automatically run.

Expected Results


rd3000_contour_total_disp
Figure 16. Total Displacement Contour (mm)

rd3000_contour_plastic_strain
Figure 17. Plastic Strain Contour