# RD-T: 3030 Buckling of a Tube Using Half Tube Mesh

This tutorial simulates buckling of a tube using half tube mesh with symmetric boundary conditions.

The figure illustrates the structural model used for this tutorial: a half tube with a rectangular section (38.1 x 25.4 mm) and length of 203 mm.

The model description is as follows:

• UNITS: Length (mm), Time (ms), Mass (kg), Force (kN) and Stress (GPa)
• Simulation time: Engine [0 - 10 ms]
• The tube thickness is 0.914 mm.
• An imposed velocity of 13.3 mm/ms (~30 MPH) is applied to the right end of the tube
• Elasto plastic material using Johnson-Cook law /MAT/PLAS_JOHNS (STEEL).

[Rho_Initial] Initial density = 7.85e-6 Kg/mm3

[E] Young's modulus = 210 GPa

[nu] Poisson coefficient = 0.3

[a] Yield Stress = 0.206 GPa

[b] Hardening Parameter = 0.450 GPa

[n] Hardening Exponent = 0.5

File needed to complete this exercise: BOXTUBE_0000.rad

## Start HyperCrash

1. Open HyperCrash.
2. Set the User profile to RadiossV2021 and the Unit system to kN mm ms.kg.
3. Set User Interface style as New.
4. Set the working directory to <install_directory>/tutorials/hwsolvers/radioss.
5. Click Run.
6. Click File > Import > Radioss.
7. In the input window, select BOXTUBE_0000.rad.
8. Click OK.

## Create and Assign a Material

1. Click Model > Material.
2. In the window, right-click and choose Create New > Elasto-plastic > Johnson-Cook (2).
3. For Title, enter Steel.
4. Enter all the material data, as shown.
5. Right-click in the Support entry box and click Select in graphics.
6. Select Include picked parts and select boxtube in the modeling window.
7. Press Enter, or click Yes in the lower right corner.
8. Click Save and then click Close.

## Create and Assign a Property

1. Click Model > Property.
2. In the window, right-click and select Create New > Surface > Shell (1).
3. For Title, enter Pshell.
4. For Shell thickness, enter 0.914.
5. Right-click in the Support entry box and click Select in graphics.
6. Select Include picked parts and select boxtube in the modeling window.
7. Press Enter, or click Yes in the lower right corner.
8. Click Save and then click Close.

## Define the Rigid Body

1. Click Mesh Editing > Rigid Body. Right-click in the display list area and select Create New.
2. Right-click in the modeling window and select Add nodes by box selection icon to select the nodes in the modeling window, as shown below:
3. Press Enter or click Save to validate.
Note: For the remainder of the tutorial, you need to have the ID of the main node of the rigid body.
4. Click Show Node Info icon in the toolbar, and select the rigid body main node in the modeling window.
The Node ID appears in the message window (node ID: 803).
5. Click Cancel in the lower right corner to exit the picking loop.
6. Click Close.

## Define Boundary Conditions

1. Click LoadCase > Boundary Condition.
2. Right-click in the display list area and select Create New.
3. In the Boundary condition field, enter the name Rigid_BC.
4. In the Node by Id field, enter 803, then click Ok.
5. To constrain the nodes, toggle Tx, Ty, Rx, Ry and Rz.
6. Click Save.

## Define Boundary Conditions Representing Symmetry

1. In the Boundary condition display list area, select Create New.
2. Name the new constraint set symmetry.
3. Right-click in the Support entry box and click Select in graphics.
4. Select Add nodes by box selection icon to select the nodes in the modeling window, as shown below:
5. Right-click to validate.
6. Toggle Tx, Ry and Rz.
7. Click Save, then click Close.

## Define the Imposed Velocity

1. Click LoadCase > Imposed Velocity. Right-click in the display list area and select Create New.
2. For Title, enter VELOCITY.
3. Right-click in the Time function parameter entry box and select Define New.
A Function Window opens.
4. For the function name, enter FUNC_VEL.
5. Enter the first point (0, 13.3) and click Validate.
6. Enter the second point (1e30, 13.3) and click Validate.
7. Click Save in the Function Window to accept the function.
8. Expand the Advanced selector at the bottom and in the Node by Id field, enter 803 and click Ok, (or toggle Add RB main nodes).
9. Go to the Properties tab and enter a Y-Scale factor = -1.
10. Set the direction of the imposed velocity to Z (translation).
11. Click Save and then click Close.

## Define a Rigid Wall

1. Click LoadCase > Rigid Wall > Create.
2. For Select RWALL, select Infinite Plane.
3. For Title, enter RIGID WALL.
4. Enter the following values:
M0:
X= 0
Y= 38.1
Z= -204
M1:
X= 0
Y= 38.1
Z= 1
5. In the Distance to search secondary nodes field, enter 20.
6. Toggle See.
7. Click See to visualize it in the modeling window.
8. Click Save, then click Close.

## Create a Self Contact for the Tube

1. Click LoadCase > Contact Interface.
2. Right-click in the Contact Interface list and select Create New > Multi usage (Type 7).
3. Toggle Self impact.
4. Right-click in the modeling window, and select Include picked parts icon and select the part in the modeling window.
5. Click Yes in the lower right corner of the main window to validate.
6. For Title, enter the name Contact.
7. Set Scale factor for stiffness as 1.
8. Set Min. gap for impact active to 0.900.
9. Set Coulomb friction to 0.200.
10. Click Save, then click Close.

## Export the Model

1. Under the Model menu, select Control Card.
2. Check Control Card to activate it.
Note: Make sure to save it before moving to the next Control Card.
3. Click File > Export > Radioss.
4. In the Write Block Format 140 Radioss File window that opens up, enter the name as BOXTUBE and click OK.
5. Leave the Header of Radioss File window empty and click Save Model.
The Starter file BOXTUBE_0000.rad is written. The model is now ready to run through the Starter and the Engine.

## Review the Results

Using HyperView, plot the displacement and strain contour at 10 ms.