RD-3595: Three Point Bending with HyperMesh

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

rd3595_3point_bending

Model Description

•	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-10 ton/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 = 7.85-9 ton/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-9 ton/mm3

[E] Young’s modulus = 208000 MPa

[nu] Poisson's ratio = 0.29

Exercise

Step 1: Load the RADIOSS User Profile

1.	Launch HyperMesh Desktop.

2.	From the Preferences menu, select the User Profiles or click the icon in toolbar.

3.	Select RADIOSS (Block140) and click OK.

Step 2: Retrieve the RADIOSS file

1.	Click File > Import > Solver Deck or click .

2.	Click the Select File icon to open the BENDING_0000.rad file you saved to your working directory from the radioss.zip file. Refer to Accessing the Model Files.

3.	Click Import.

4.	Click Close to close the window.

Step 3: Create and Assign material and property for HCFOAM

1.	In the Model browser, right-click and select Create > Material. The new material appears in the Entity Editor.

2.	For Name, enter Foam.

3.	For Card Image, select M28_HONEYCOMB and click Yes to confirm.

4.	Input values, as shown below:

rd3595_foam_13

5.	In the Model browser, right-click and select Create > Property to create a new property.

6.	For Name, enter Foam and set the new property Card Image as P14_SOLID. Leave all the settings as default, except for ISOLID which should be set to 24.

7.	In the Model browser, right-click on the component HCFoam and select Assign. Assign Foam as the Prop_Id and Foam as the Mat_Id.

8.	Click Apply.

Step 4: Create and Assign material and property for the component Inner

1.	In the Model browser, right-click and select Create > Material. The new material appears in the Entity Editor.

2.	For Name, enter Inner.

3.	For Card Image, select M36_PLAS_TAB and click Yes to confirm.

4.	Input the values, as shown below:

rd3595_inner_14

5.	In the Model browser, right-click and select Create > Property to create a new property.

6.	For Name, enter Inner and set Card Image as P1_SHELL. Leave all the settings as default, except for Ishell which should be set to 4 and Thick which should be set to 9.119e-01.

7.	In the Model browser, right-click on the component Inner and select Assign. Assign Inner as the Prop_Id and Inner as the Mat_Id.

Step 5: Create and Assign material and property for the component Outer

1.	In the Model browser, right-click on the material Inner and select Duplicate. Name the new material Outer. This creates a new material that is identical to the source material.

2.	In the Model browser, right-click on the property Inner and select Duplicate. Name the new property Outer. This creates a new property that is identical to the source property.

3.	In the Model browser, right-click on the component Outer and select Assign. Assign Outer as the Prop_Id and Outer as the Mat_Id.

Step 6: Create and Assign material and property for the component Flat

Follow the procedure described in Step 5 with Outer replaced by Flat.

Step 7: Create and assign material and property for Impactor

1.	In the Model browser, right-click and select Create > Material. The new material shows up in the Entity Editor.

2.	For Name, enter Impactor.

3.	For Card Image, select M1_ELAST.

4.	Input the values, as shown below:

rd3595_impactor_13

5.	In the Model browser, right-click on the property Inner and select Duplicate. Name the new property Impactor. This creates a new property that is identical to the source property.

6.	In the Model browser, right-click on the component Impactor and select Assign. Assign Impactor as the Prop_Id and Impactor as the Mat_Id.

Step 8: Create and assign material and property for Support

Follow the same procedures as in Step 5. Create a copy of Impactor property and material with name support and assign it to component support.

Step 9: Create a rigid body to make Impactor and Support Rigid

1.	In the Model browser, right-click and select Create > Component.

2.	For Name, enter Impact rigid.

3.	Select any color for easy visualization.

4.	Set Card Image to None.

5.	Go to the 1D page, select the rigids panel.

6.	Verify that you are in the create subpanel.

7.	For dependent switch to comps.

8.	For primary node switch to calculate node.

9.	Click comps.

10.	Select Impactor, then click select.

11.	Click create.

12.	Click return to exit the panel.

13.	Similarly, create rigid body for Support component in a collector with the name “Support rigid” using Steps 9.1 to 9.12.

rd3595_impact_rigid

Step 10: Define imposed velocity and boundary condition for the impactor

1.	From the Utility page, start the BCs Manager.

2.	For Name, enter IMPOSED_VELOCITY, set Select type to Imposed Velocity and set the GRNOD to Nodes.

3.	Click nodes and select the master node of the rigid body of the Impactor, as shown in the following image.

rd3595_impvel

4.	Set the Direction as Z.

5.	Set Scale Y to -1000.0 as the direction of velocity is opposite to the global Z-axis.

6.	Set the Curve ID to Select curve.

7.	Select the predefined curve to Func1.

8.	Click create to create the imposed velocity.

rd3595_imposedvel_10SA1

9.	For Name, enter Impactor_constraints, set Select type to Boundary Condition and set the GRNOD to Nodes.

10.	Click nodes and select the master node of the rigid body.

11.	Check all the degrees of freedom to constrain, except Tz.

12.	Click create to create the boundary condition.

Step 11: Define fixed boundary condition for the support

1.	From the Utility page, start the BCs Manager.

2.	For Name, enter Support_fixed, set Select type to Boundary Condition and set the GRNOD to Nodes.

3.	Select the master node of the rigid body created on Supporter, as shown in the following image.

4.	Check all the degrees of freedom.

5.	Click create to create the boundary condition.

rd3595_impvel

rd3595_supportfix_13

Step 12: Define symmetry boundary condition for the foam, inner, outer and flat

1.	From the Utility page, start the BCs Manager.

2.	For Name, enter SYMMETRY_XZ, set Select type to Boundary Condition and set the GRNOD to Nodes.

3.	Select the nodes of the foam, inner, outer and flat, as shown in the following image.

4.	Check the degrees of translational degrees of freedom Y and rotational degrees of freedom X and Z to constraint.

5.	Click create to create the boundary condition.

rd3595_symmetry_xz

rd3595_symmetry_13

6.	Click close to exit the BC Manager.

Step 13: Define contacts between the beam and the support

1.	Launch the HyperMesh Solver browser from View > Browsers > HyperMesh > Solver.

2.	In the Solver browser, right-click and select Create > INTER > TYPE7.

3.	Enter the values, as shown below:

rd3595_support_13

4.	Set the Surf_id (M) for the master selection to Components and select the Support component.

5.	Set the Grnod_id (S) for the slave selection to Components and select the Flat component.

6.	Similarly create the contact for Impactor with Outer, as shown below.

rd3595_impactor2_13

Step 14: Define the self contact between the beam components

Using the directions in Step 13, create a new Type 7 interface named Self with the components Outer, Inner, and Flat as Master and the same components Outer, Inner, and Flat as Slave. This will make the components self-contact instead of self-penetrate. Verify that the interface has a Fric of 0.1 and Gapmin of 0.2.

rd3595_self_13

Step 15: Create Interface time history

1.	Right-click in the Solver browser and select Create > TH > INTER.

2.	For Name, enter IMPACTOR.

3.	Switch the entity selector to groups.

4.	Click groups and select the interfaces Impactor and Support from the list.

Click OK.

6.	Set NUM_VARIABLES to 1 and Data: Var to DEF.

rd3595_impactor_14

Step 16: Creating control cards and output requests

1.	Launch the HyperMesh Solver browser from View > Browsers > HyperMesh > Solver.

2.	Right-click in the Solver browser general area to create the cards shown below with the given values for each parameter:

Keyword Type	Keyword	Parameter	Parameter Value
CONTROL CARDS	TITLE	Status	[Checked]
CONTROL CARDS	TITLE	TITLE	3PBENDING
ENGINE KEYWORDS	RUN	Status	[Checked]
ENGINE KEYWORDS	RUN	RunName	3PBENDING
ENGINE KEYWORDS	RUN	RunNumber	1
ENGINE KEYWORDS	RUN	Tstop	7.01e-2
ENGINE KEYWORDS	TFILE	Status	[Checked]
ENGINE KEYWORDS	TFILE	Time_frequency	0.0001
ENGINE KEYWORDS	PRINT	Status	[Checked]
ENGINE KEYWORDS	PRINT	N_Print	-100
ENGINE KEYWORDS	ANIM/ELEM	Status	[Checked]
ENGINE KEYWORDS	ANIM/ELEM	VONM	[Checked]
ENGINE KEYWORDS	ANIM/ELEM	EPSP	[Checked]
ENGINE KEYWORDS	ANIM/VECT	Status	[Checked]
ENGINE KEYWORDS	ANIM/VECT	VEL	[Checked]
ENGINE KEYWORDS	ANIM/VECT	CONT	[Checked]
ENGINE KEYWORDS	ANIM/DT	Status	[Checked]
ENGINE KEYWORDS	ANIM/DT	Tstart	0
ENGINE KEYWORDS	ANIM/DT	Tfreq	2.5e-3
ENGINE KEYWORDS	DT	Status	[Checked]
ENGINE KEYWORDS	DT	Tscale	0.0
ENGINE KEYWORDS	DT	Tmin	0.0
ENGINE KEYWORDS	DT/NODA	Status	[Checked]
ENGINE KEYWORDS	DT/NODA	CST_0	[Checked]
ENGINE KEYWORDS	DT/NODA/CST_0	Tscale	0.9
ENGINE KEYWORDS	DT/NODA/CST_0	Tmin	7e-7
ENGINE KEYWORDS	DT/NODA	DEL	[Checked]
ENGINE KEYWORDS	DT/NODA/DEL	Tscale	0.9
ENGINE KEYWORDS	DT/NODA/DEL	Tmin	3.5e-8
ENGINE KEYWORDS	RBODY_ENGINE RBODY/ON	Status	[Checked]
ENGINE KEYWORDS	RBODY_ENGINE	NUM_rbnodes	2
ENGINE KEYWORDS	RBODY_ENGINE	Data: Nodes	29664 29665

Step 17: Export the model

1.	Click File > Export or click the Export icon .

2.	For File:, navigate to the destination directory where you want to export to.

3.	For name, enter 3BENDING and click Save.

4.	Click the downward-pointing arrows next to Export options to expand the panel.

5.	Click Merge starter and engine file to export solver deck as one file (or export separately).

6.	Click on Export to export solver deck.

Step 18: Open RADIOSS Manager

1.	Go to Start > Programs > Altair HyperWorks 14.0 > RADIOSS.

2.	For Input file, browse to the exercise folder and select the file 3PBENDING_0000.rad.

rd3595_radioss_mgr

Step 19: Review the listing files for this run and verify on the results

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

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

Exercise Expected Results

rd3595_results_stress_14

von Mises Stress Contour (MPa)

rd3595_results_strain_14

Plastic Strain Contour

rd3595_results_14

Contact Force for Impactor Interface