# RD-T: 3060 Three Point Bending

This tutorial demonstrates how to set up 3-point bending model with symmetric boundary conditions in Y direction.

The model description is as follows:
• UNITS: Length (mm), Time (s), Mass (ton), Force (N) and Stress (MPa)
• Simulation time: in Engine file [0 - 6.601e-002 s]
• Only one half of the model is modeled because it is symmetric.
• The supports are totally fixed. An imposed velocity of 1000 mm/s is applied on the Impactor in the (-Z) direction
• Model size = 370mm x 46.5mm x 159mm
• Honeycomb Material /MAT/LAW28: HONEYCOMB

[Rho_I] Initial density = 3.0e-10ton/mm3

[E11], [E22] and [E33] Young's modulus (Eij) = 200 MPa

[G11], [G22] and [G33] Shear modulus (Gij) = 150 MPa

• Elasto-Plastic Material /MAT/LAW36: Inner, Outer and Flat

[Rho_I] Initial density = 7.85-9ton/mm3

[E] Young's modulus = 210000 MPa

[nu] Poisson's ratio = 0.29

• Strain Curve:
0 1 2 3 4 5 6 7 8 9
STRAIN 0 0.012002 0.014003 0.018003 0.022002 0.026003 0.030006 0.032 0.033005 0.033523
STRESS 325 335.968 343783 349.245 358.649 372.309 383.925 388.109 389.292 389.506
• Elastic Material /MAT/PLAS_JOHNS: Impactor

[Rho_I] Initial density = 8e-9ton/mm3

[E] Young's modulus = 208000 MPa

[nu] Poisson's ratio = 0.29

## Start HyperCrash

1. Open HyperCrash.
2. Set the User profile to RadiossV2022 and the Unit system to N_mm_s_T.
3. Set User Interface style as New.
5. Click Run.
6. Click File > Import > Radioss.
7. In the input window, select BENDING_0000.rad.
8. Click OK.

## Create and Assign Material

1. Click Model > Material.
2. In the window, right-click and select Create New > Elastic > Linear elastic (1) as shown below:
3. For Title, enter Rigid Material.
4. Enter all the material data, as shown in the following image.
5. Right-click in the entry box Support, and click Include picked parts to select the parts Impactor and Support in the モデリングウィンドウ.
6. Click Yes in the lower right corner.
7. Press Enter or click Save to validate.

## Create and Assign Material for Parts

1. In the window, right-click and select Create New > Elastic > Piecewise linear (36).
2. For Title, enter Shell Material.
3. Enter all the material data, as shown in the following image:
4. Open the Strain rate folder and click to add a row.
5. Right-click in Yield stress function field and click Select in Model to select an existing function in the model.
6. In the Function file window, select the function with an ID of 2, then click OK to import the curve. The function can be edited, as shown in the image below.
7. Click the Tree tab and select the parts Inner, Outer, and Flat on the tree.
8. Click to isolate this selection.
9. Click the Material tab.
10. Right-click in the entry box Support, and click Include picked parts to select the parts Inner, Outer and Flat in the モデリングウィンドウ as shown in the image.
11. Click Yes in the lower right corner.
12. Press Enter or click Save to validate.

## Create and Assign HCFoam Material

1. In the window, right-click and select Create New > Elastic > Honeycomb orthotropic (28).
2. For Title, enter Foam.
3. Enter all the material data, as shown in the image:
4. Right-click on the Yield stress function 11 field and click Select in Model to select a curve already present in the model.
5. In the Function file window, select the function with ID of 5, then select OK.
6. Repeat this process for the Yield functions, as shown in the following image.
7. Click the Tree tab and select the part HCFoam (7) on the tree.
8. Click to isolate this selection.
9. Click the Material tab.
10. Right-click in the entry box Support, and click Include picked parts to select HCFoam in the モデリングウィンドウ as shown in the image.
11. Click Yes in the lower right corner.
12. Click Save > Close.

## Create and Assign a Property

1. Click Model > Property.
2. In the window, right-click and select Create New > Surface > Surface > Shell (1).
3. For Title, enter Shell Property.
4. Enter Shell thickness and Shell element formulation values, as shown in the image.
5. Click the Tree tab and select the parts Inner, Outer and Flat on the tree.
6. Click to isolate this selection.
7. Click the Property tab.
8. Right-click in the entry box Support, and click Include picked parts to select the parts Inner, Outer and Flat in the モデリングウィンドウ to assign Shell property.
9. Click Yes in the lower right corner.
10. Click Save.

## Create and Assign an Impactor and Support Property

1. For Title, enter Rigid Property.
2. Enter the Shell thickness value as .9119, as shown in the image.
3. Click the Tree tab and select the parts Impactor and Support in the tree.
4. Click to show only these parts.
5. Click the Property tab.
6. Right-click in the entry box Support, and click Include picked parts to selects Impactor and Support in the モデリングウィンドウ to assign Rigid property.
7. Click Yes in the lower right corner.
8. Click Save.

## Create and Assign HCFoam Property

1. In the window, right-click and select Create New > Volume > General solid (14).
2. For Title, enter Foam.
3. Click the Tree tab and select HCfoam on the tree.
4. Click to isolate this selection.
5. Go back to the Property tab.
6. In the Flag for solid elements formulation field, select HEPH.
7. Right-click in the entry box Support, and click Include picked parts to select HCfoam in the モデリングウィンドウ to assign Foam property.
8. Click Yes in the lower right corner.
9. Click Save > Close.

## Create Impactor Rigid Body

1. From the menu bar, click Mesh Editing > Rigid Body.
2. In the window, right-click to select Create New, enter the name Impactor.
3. Click the Tree tab and select the Impactor assembly on the tree.
4. Click to show all parts.
5. Click the Mesh Editing tab.
6. Right-click in the entry box Support, and click Include picked parts to select Impactor in the モデリングウィンドウ.
7. Click Yes in the lower right corner.
8. Press Enter or click Save to validate.

## Create a Support Rigid Body

1. In the Title field, enter the name Support.
2. Right-click in the entry box Support, and click Include picked parts to select Support in the モデリングウィンドウ.
3. Click Yes to complete the selection.
4. Click Save.
The rigid body for Support should look like the following image.
5. Click Close.

## Define Boundary Conditions

1. Click LoadCase > Boundary Condition.
2. In the window, right-click to select Create New.
3. Press F6 to show the rigid bodies.
4. In the Title field, enter Boundary.
5. Right-click in the entry box Support and right-click in the モデリングウィンドウ. Click Add/Remove nodes by picking selection and select the main node of the rigid body.
6. Constrain all DOF except translation in Z as shown in the following image. To constrain the nodes, check the boxes for TX, TY, RX, RY and RZ.
7. Click Save.
8. Repeat the same process to create boundary conditions for the Support and Symmetry boundary condition for the inner/outer/flat.
9. Click the node selection icon to select the main node of Support, as shown in the following image.
10. Constrain all DOF by selecting TX, TY, TZ, RX, RY and RZ, as shown in the image.
11. Click Save.
12. In the Boundary condition creation field, enter Symmetry.
13. Click the Tree tab and select the parts Inner, Outer, HCfoam and Flat on the tree.
14. Click to isolate this selection.
15. Press the p key to change the perspective visualization.
16. Click the Boundary Condition tab.
17. From the Visualization toolbar, select the YZ View, as shown below.
18. Right-click in the entry box Support, right-click in the モデリングウィンドウ, and click Add nodes by box selection to select the nodes, as shown below.
19. To constrain the nodes, select TY, RX and RZ.
20. Click Save > Close.

## Define Imposed Velocity

1. Click LoadCase > Imposed > Imposed Velocity.
2. In the window, right-click to select Create New.
3. For Title, enter IMPOSED VELOCITY.
4. For Direction, select Z (translation) and -1000 for Y-Scale factor.
5. For Time function, use the predefined curve in the model Funct 1.
6. For Y Scale factor, enter -1000.
7. Press the F6 key to show the rigid bodies.
8. Click in the entry box Support and right-click in the モデリングウィンドウ. Click and select the main node of Impactor.
9. Click Yes in the lower-right corner.
10. Click Save > Close.

## Define Contacts

1. Click LoadCase > Contact Interface.
2. In the window, right-click and select Create New > Multi usage (Type 7).
3. Click on the check box next to Create symmetric interface at saving.
4. For Title, enter Support.
5. Click the Tree tab and select the parts Flat and Support on the tree.
6. Click to isolate this selection.
7. Click the Contact Interface tab.
8. Set Min gap for impact active to 0.2.
9. Set Coulomb friction to 0.1.
10. Set [Iform] Friction penalty formulation at 2[Stiffness].
11. Click in the Secondary nodes entry box and right-click in the モデリングウィンドウ.
12. Click Include Picked Parts and select FLAT.
13. Press Y or click Yes at the bottom right of the screen.
You are automatically moved to the selection of the Main surface.
14. Right-click and click Include Picked Parts and select Support.
15. Press Y or click Yes at the bottom right of the screen.
16. Click Save.
17. Repeat the same process to create contact between Outer and Impactor.
18. Click the Tree tab and select the parts Outer and Impactor on the tree.
19. Click to isolate this selection.
20. Right-click in the window and select Create New > Multi usage (Type 7).
21. Click the Contact Interface tab.
22. Click on the check box next to Create symmetric interface at saving.
23. In the Title, enter Imp_Outer.
24. Set Min gap for impact active to 0.2.
25. Set Coulomb friction to 0.1.
26. Set [Iform] Friction penalty formulation to 2[Stiffness].
27. Select Outer Part as Secondary and Impactor as Main, as shown in the image.
28. Click Save .
29. Repeat the same process for self impact for Outer, Inner and Flat, as self impact.
30. Click the Tree tab and select the parts Outer, Inner and Flat on the tree.
31. Click to isolate this selection.
32. Click the Contact Interface tab.
33. Select Self-Impact.
34. Set Title as Self.
35. Set the Min gap for impact active to 0.7.
36. Set the Coulomb friction to 0.1.
37. Set [Iform] Friction penalty formulation to 2[Stiffness].
38. Select components Outer, Inner and Flat, as shown in the image.
39. Click Save.

## Clean the Model

1. Click Mesh Editing > Clean.
2. Select All.
3. Click Clean > Close.

## Export the Model

1. Click Model > Control Card and select the control cards in the images below.
注: Make sure to save each control card before editing the next.
2. Click File > Export > Radioss.
3. In the Output window that opens, enter the name 3PBENDING and click OK.
4. Leave the Header of Radioss File window empty and click Save Model.
The Starter file 3PBENDING_0000.rad is written.
5. Open Altair Compute Console from the Start menu.
6. Run the model 3PBENDING_0000.rad using Altair Compute Console in the class_exercise folder.