RD-3599: Gasket with HyperMesh

This tutorial demonstrates how to simulate a rubber gasket in sequential loading, given the following load sequence:

•	Translation Transverse (10 mm)

•	Translation Longitudinal (5 mm)

•	Torsion (20 Degrees)

rd3599_gasket_10SA1

Model Description

•	UNITS: Length (mm), Time (ms), Mass (kg), Force (kN) and Stress (GPa)

•	Simulation time:

o	Engine [0 – 1.501] in steps of 0.5 ms for each load case

•	The outer circumference area is fixed on all degrees of freedom (VX, VY, VZ) and the center node is fixed on X direction and the X and Y rotation (VX, WX, Wy)

•	The gasket dimensions are: Thickness = 100 mm, External Diameter = 200 mm and Internal Diameter = 50 mm.

•	Hyper-Elastic Material /MAT/LAW42 (Rubber)

[Rho_I] Initial density = 6.0-6 Kg/mm3

[nu] Poisson’s ratio = 0.495

[mue1] (1) = 0.6

[alfa1] (1) = 2

(alfa2] (2) = -2

Exercise

Step 1: Load the RADIOSS (Block) 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: Load the gasket.hm file

1.	From the toolbar, click the Open Model icon to open the gasket.hm file you saved to your working directory from the radioss.zip file. Refer to Accessing the Model Files.

2.	Click Open. The model loads into the graphics area.

Step 3: Define and assign material, property to Rubber

1.	In the Model browser, right-click and select Create > Material to create material.

2.	For Name, enter rubber.

3.	For Card Image, select M42_OGDEN and click Yes in the confirmation window.

4.	Input the values, as shown below:

rd3599_rubber_13

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

6.	For Name, enter gasket.

7.	For Card Image, select P14_SOLID and click Yes to confirm.

rd3599_gasket2_13

8.	In the Model browser, expand the Component folder and select GASKET. Right-click and Assign (or use the Entity Editor) the newly created property and material.

Step 4: Create a component for the rigid body at center of Gasket

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

2.	For Name, enter center and switch Card Image to None and click Yes to confirm.

3.	Select any color for easy visualization.

rd3599_center_13

Step 5: Create a rigid body at center of Gasket

1.	From the 1D page, select the rigids panel.

2.	For primary node, switch to calculate node.

3.	For nodes 2-n, switch to multiple nodes.

4.	Click the nodes and select a node in the inner face.

5.	Click nodes and select by face. HyperMesh will select all nodes on the inner face.

6.	Click create.

7.	Click return to exit the panel.

rd3599_gasket3_10SA1

Step 6: Create gasket inner fixed boundary conditions

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

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

3.	Select the master node of rigid body created in Step 5 and click proceed.

4.	Check the Tx translational and Rx, Ry rotational degrees of freedom.

5.	Click Create to create the inner fixed boundary condition.

rd3599_innerBC_13

Step 7: Create gasket inner Y displacement boundary conditions

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

2.	For Name, enter DISP_Y, set Select type to Imposed Displacement and set the GRNOD to Nodes.

3.	Select the master node of rigid body created in Step 5.

4.	Set Direction as Y.

5.	Click Create/Select curve to go to the XY curve editor.

6.	Click New and enter Name as DISP_Y. Click proceed.

7.	Enter the following values for X and Y:

X = {0, 0.5, 1.0}

Y = {0, 10, 10}

8.	Click Update and Close the XY curve editor GUI.

rd3599_dispY_13

9.	Click Create to create the boundary condition.

Step 8: Create gasket inner Z displacement boundary conditions

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

2.	For Name, enter DISP_Z, set Select type to Imposed Displacement and set the GRNOD to Nodes.

3.	Select the master node of rigid body created in Step 5.

4.	Set Direction as Z.

5.	Click Create/Select curve to go to the XY curve editor.

6.	Click New and enter Name as DISP_Z. Click proceed.

7.	Enter the following vales for X and Y:

X = {0, 0.5, 1, 1.5}

Y = {0, 0, 5, 5}

8.	Click Update and Close the XY curve editor GUI.

rd3599_dispZ_13

9.	Click Create to create the boundary condition.

Step 9: Create gasket inner Z rotation boundary conditions

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

2.	For Name, enter ROT20DEG_Z, set Select type to Imposed Displacement and set the GRNOD to Nodes.

3.	Select the master node of rigid body created in Step 5.

4.	Set Direction as ZZ.

5.	Click Create/Select curve to go to the XY curve editor.

6.	Click New and enter Name as ROT20DEG_Z. Click proceed.

7.	Enter the following vales for X and Y:

X = {0, 1, 1.5, 2}

Y = {0, 0, 0.349, 0.349}

8.	Click Update and Close the XY curve editor GUI.

rd3599_rot20degZ_10SA1

9.	Click Create to create the boundary condition.

Step 10: Create gasket outer boundary conditions

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

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

3.	Click Nodes and select a node on the outer surface.

4.	Click Nodes on the panel and then select by face to select all nodes on the outer surface.

5.	Check all the translational and rotational degrees of freedom.

6.	Click Create to create the outer fixed boundary condition.

rd3599_outerBC_10SA1

Step 11: Create output request and control cards

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	GASKET
CONTROL CARDS	MEMORY	Status	[Checked]
CONTROL CARDS	MEMORY	NMOTS	40000 Not needed
CONTROL CARDS	SPMD	Status	[Checked]
CONTROL CARDS	IOFLAG	Status	[Checked]
CONTROL CARDS	ANALY	Status	[Checked]
ALE-CFD-SPH	ALE_CFD_SPH_CARD	Status	[Checked]
ALE-CFD-SPH	ALE_CFD_SPH_CARD	ALE_Grid_Velocity	[Checked]
ALE-CFD-SPH	ALE_CFD_SPH_CARD	GridVel_Gamma	100.00
ENGINE KEYWORDS	RUN	Status	[Checked]
ENGINE KEYWORDS	RUN	RunName	GASKET
ENGINE KEYWORDS	RUN	Tstop	1.51
ENGINE KEYWORDS	PARITH	Status	[Checked]
ENGINE KEYWORDS	PARITH	Keyword2	ON
ENGINE KEYWORDS	PRINT	Status	[Checked]
ENGINE KEYWORDS	PRINT	N_Print	-1000
ENGINE KEYWORDS	ANIM/ELEM	Status	[Checked]
ENGINE KEYWORDS	ANIM/ELEM	VONM	[Checked]
ENGINE KEYWORDS	ANIM/ELEM	DENS	[Checked]
ENGINE KEYWORDS	ANIM/ELEM	PRES	[Checked]
ENGINE KEYWORDS	ANIM/VECT	Status	[Checked]
ENGINE KEYWORDS	ANIM/VECT	CONT	[Checked]
ENGINE KEYWORDS	ANIM/DT	Status	[Checked]
ENGINE KEYWORDS	ANIM/DT	Tstart	0
ENGINE KEYWORDS	ANIM/DT	Tfreq	0.05
ENGINE KEYWORDS	DT	Status	[Checked]
ENGINE KEYWORDS	DT	Tscale	0.0
ENGINE KEYWORDS	DT	Tmin	0.0
ENGINE KEYWORDS	TFILE	Time frequency	1.5e-3

Step 12: 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 GASKET 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 13: Open RADIOSS Manager from windows Start menu

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

2.	For Input file, browse to the exercise folder and select the file GASKET_0000.rad.

rd3599_radioss_mgr

Step 14: 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 and strain contour and vectors.

Exercise Expected Results

rd3599_results1_10SA1

Displacement Contour for the 3 load steps (mm)

rd3599_results2_10SA1

Von Mises Stress Contour at the end of the simulation