RD-T: 3500 Tensile Test Setup

This tutorial demonstrates how to simulate a uniaxial tensile test using a standardized specimen with a defined cross-sectional area which is stretched until fracture.

The tensile test is a standardized method of material testing to determine the yield strength, tensile strength, elongation at break and other material parameters. It is one of the quasi-static, destructive test methods.

rd3500_01
Figure 1.
The model description is as follows:
  • UNITS: Length (mm), Time (ms), Mass (kg), Force (kN) and Stress (GPa)
  • Simulation time D01 [0 – 40.]
  • At the right side, a constant velocity is applied = 1 mm/ms on -X direction.
  • Tensile test object dimensions = 12 x 200 with a uniform thickness = 1.7 mm

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

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

[E] Young's modulus = 60.4 GPa

[nu] Poisson's ratio = 0.33

[SIGMA_Y] Yield Stress = 0.09026 GPa

[UTS] Ultimate Tensile Stress = 0.175 GPa

[E_UTS] Engineering strain at UTS = 0.24

[SIG_max] Maximum Stress = 0 GPa

[EPS_max] Failure Plastic Strain = 0.75

Input file for this tutorial: tensile_start_0000.rad

Load the Radioss User Profile

  1. Launch HyperMesh Desktop.
  2. From the Preferences menu, select User Profiles or click the userProfile-24 icon in toolbar.
  3. Select Radioss (Radioss2021) and click OK.

Import the Model

  1. Click File > Import > Solver Deck or click fileImportGeometry-24.
  2. Click the Select File icon files_panel to open the tensile_start_0000.rad file you saved to your working directory from the radioss.zip file.
  3. Click Open.
  4. Click Import.
    Ignore the warning “No valid Engine File found…”
  5. Click Close to close the window.
  6. In the Model Browser, verify that the correct units are defined by expanding Cards, BEGIN_CARD.


    Figure 2.

Create the Material

  1. In the Model Browser, right-click and select Create > Material.
  2. In the Entity Editor, for Name, enter Aluminum 6063T7.
  3. Set Card Image to M2_PLAS_JOHNS_ZERIL.
  4. Click Yes on the pop-up that warns of a card image change.
  5. In the Entity Editor, input the values, as shown in the following image.
  6. Click on the component, Tensile_coupon.
  7. In the Entity Editor, for Mat_Id, click twice on Unspecified and select the newly created material.
  8. Click OK.


    Figure 3. Material card of component Tensile_coupon

Create the Property

  1. In the Model Browser, right-click and select Create > Property.
  2. For Name, enter sheet_1.7.
  3. For Thick, enter 1.7. in the Value field corresponding to sheet thickness.
  4. In the Entity Editor, input the values, as shown in the following image.
  5. Click on the component, Tensile_coupon.
  6. In the Entity Editor, for Prop_Id, click twice on Unspecified and select the newly created property.
  7. Click OK.

    rd3500_02
    Figure 4. Property Card of Component Tensile_coupon

Create the Rigid Body

  1. In the Model Browser, right-click and select Create > Component.
  2. In the Entity Editor, for Name, enter Rigid Body.
  3. Set Card Image to None.
  4. From the Mesh pull-down menu, select Create > 1D Elements > Rigids.
  5. Set Secondary node(s) (nodes2-n) to Multiple Nodes.
  6. Set primary node to Calculate Node.
  7. Click Nodes and select the nodes as shown in Figure 5.
  8. Click create and return.


    Figure 5. Selection of the secondary nodes of the rigid body

Create the Boundary Conditions

  1. Select View > Solver Browser, and right-click in the Solver tab area.
  2. Select Create > BOUNDARY CONDITIONS > BCS.
  3. For Title, enter constraint1 and right-click grnd_ID and click Create.
  4. Within the grnd_ID section, click on 0 Nodes beside Entity IDs, then Nodes.
    A nodes selection appears.
  5. Select the nodes, as shown below and click proceed.

    rd3500_nodes4
    Figure 6.
  6. Check the box beside DOF1, DOF2, DOF3, DOF4, DOF5, and DOF6 to fix all the degrees of freedom.
  7. Right-click BCS > Create to create a second constraint for the Rigid Body.
  8. For Title, enter constraint2.
  9. Right-click grnd_ID and select Create.
  10. Type “o” for options and select graphics > coincident picking to select the main node of the Rigid Body.
  11. Within the grnd_ID section, click 0 Nodes beside Entity IDs, then Nodes.
    A node selection appears.
  12. Select the node 990, as shown below and click proceed.


    Figure 7.
  13. Activate all degrees of freedom, except of DOF1, translation in the X-direction.

Create the Imposed Velocity

  1. Select View > Solver Browser, and right-click in the Solver tab area.
  2. Select Create > BOUNDARY CONDITIONS > IMPVEL.
  3. For Title, enter imposed_velocity and right-click grnd_ID and click Create.
  4. Within the grnd_ID section, click on 0 Nodes beside Entity IDs, then Nodes.
    A nodes selection appears.
  5. Click node 990 to select the main node of the rigid body and click proceed.
  6. Right-click on fct_ID(T) and select Create.
  7. Right-click on fct_ID(T) and select Plot Curve.
    An XY curve editor appears.
  8. Enter the values, as shown in the table below.

    rd3500_xy
    Figure 8.
  9. Click Update to update the curve with the new values.
  10. Click Close to close the Curve editor.
    The created curve is assigned to this constraint.

Create Time History Output

  1. In the Solver Browser, right-click Create > TH > RBODY
  2. In the Entity Editor, for Name enter TH_RBODY.
  3. For Entity ID’s select Elements, select the Rigid Body and click proceed.
  4. Set NUM_VARIABLES to 1 for DEF (default).
  5. From the Geom page, select temp nodes. Pick two nodes (yellow) with a distance of 80 mm .


    Figure 9. Temporary nodes with a distance of 80mm
  6. In the Solver Browser, right-click Create > TH > NODE.
  7. In the Entity Editor, for Name enter TH_Measuring_Nodes.
  8. For Entity ID’s select Nodes and select the nodes with the numbers 102 and 616 and click proceed.
  9. For Nodes identification, select the Tool page > find > nodes > set the tick for numbers > find.
  10. Set NUM_VARIABLES to 1 for DEF (default).

Create Output Requests

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
    Figure 10. Settings and Output Variables for the Engine File

Export the Model

  1. From the File menu, click Export > Solver Deck or click the Export Solver Deck icon fileExportSolver-24.
  2. For File, click the folder icon files_panel 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 and make sure “Auto export engine file” is checked.
  5. Click Export and then click Close.
  6. Open Altair Compute Console from Start menu.
  7. Select the TENSILE_0000.rad for the Input file.
  8. Click Run.
  9. Review the output files for this run and verify the results. See if there is any warning or errors on the .out files.
  10. Using HyperGraph, plot the displacement and stress curve (lower left and right) and the X-Force from the Rigid Body (upper right).


    Figure 11. Simulation Results of the Tensile Test