Problem: Modeled a rubber material using hyperelastic material properties.
Horizontal spacer
Download required files here

1) Click on File, then click on Save As....

2) Type the name of the new database as rubber.mud and click Save.

3) Click on File then choose Import pick IGES.... Find the directory where you have saved rubber.igs then choose Open. The link to the file should be attached on the top of the page.





1) Under the Geometry & Mesh tab, click on Convert. Enter 8 and 20 for the Divisions of U and V. Then click on Surface to Elements

2) Screen pick the Surface list and to End list Right-Click on your mouse.

3) Enter 20 and 8 for the Divisions of U and V. Then click on Surface to Elements

4) Screen pick the Surface list and to End list Right-Click on your mouse.

5) Enter 8 and 120 for the Divisions of U and V. Then click on Surface to Elements

6) Screen pick the Surface list and to End list Right-Click on your mouse.

7) Under the Geometry & Mesh tab, click on Curve Divisions. Enter 130 for the #Divisions. Then click on Apply Curve Divisions.

8) Screen pick the Surface and to End list Right-Click on your mouse.

9) Enter 10 for the #Divisions. Then click on Apply Curve Divisions Screen pick the Surfaces shown on the image below. and to End list Right-Click on your mouse.

10) Enter 50 for the #Divisions. Then click on Apply Curve Divisions Screen pick the Surfaces shown on the image below. and to End list Right-Click on your mouse.

11) Enter 60 for the #Divisions. Then click on Apply Curve Divisions Screen pick the Surfaces shown on the image below. and to End list Right-Click on your mouse.

12) Enter 8 for the #Divisions. Then click on Apply Curve Divisions Screen pick the Surfaces shown on the image below. and to End list Right-Click on your mouse.

13) Under the Geometry & Mesh tab, click on Planer. Select Quad Mesh!. Screen pick the Surfaces shown on the image below. and to End list Right-Click on your mouse.



















1) Under the Operations group, click on Sweep.

2) Click All.



1) Under the Boundry Conditions tab, click on New(Structural) then click on Fixed Displacement.

2) Enter base-fix for the Name.

3) Click on Properties for the Name.

4) Choose Displacement X and Displacement Y to be fixed. Then click OK.

5) Click on Add. Screen pick the Surfaces shown on the image below. and to End list Right-Click on your mouse.







1) Under the Material Properties tab, click on New. Choose Standard

2) Enter rubber for the Name.

3) Click on Structural .

4) Under the Strutural Properties choose Mooney for the Type. Enter 80 and 20 for C10 and C01 respectively. Then click OK.

5) Click on Add. Screen pick the Elements shown on the image below and to End list Right-Click on your mouse.







1) Click on the Geometric Properties tab.

2) Click on New(Structural). Choose Planer and then click on Plane Strain.

3) Enter seal for the Name.

4) Click on Properties Change the Thickness to 1. Then click OK.

5) Click on Add. Screen pick the Elements shown on the image below. and to End list Right-Click on your mouse.







1) Undrer the Contact tab. Click on Rigid.

2) Enter door for the Name. Choose Properties and then click on Parameters.

3) Enter -0.08 for the X Velocity and -0.8 for the Y Velocity. Then click OK and OK again.

4) Enter -0.08 for the X Velocity and -0.8 for the Y Velocity. Then click OK and OK again.

5) Click on Add. Screen pick the Curves shown on the image below and to End list Right-Click on your mouse.

6) Click on Tools and choose Flip Curves.

7) Screen pick the Curves shown on the image below and to End list Right-Click on your mouse.

8) Click Identify.

9) Click on New and choose Deformable.

10) Enter rubber for the Name.

11)Click on Add. Screen pick the Elements shown on the image below. and to End list Right-Click on your mouse.











1) Click on the Arrow and then choose the Loadcases tab. Click on New and then choose Static.

2) Enter close_door for the Name.

3) Click on Properties. Choose Multi-Criteria and then click OK.





1) Click on the Arrow and then choose the Loadcases tab. Click on New and then choose Static.

2) Plot Displacement, Translational. Set Quantity to X Component. Click Apply. Repeat for Y Component.















1) Click on the Result tab. Choose Model Plot Results. Under the Deformed Shape choose Deformed Only for Style.

2) Under the Scalat Plot choose Countour Bands for Style. Click on Scalar and choose Equivalent of Total Strain. Then click OK.

3) Under the View Menu, select Plot Control...

4) Uncheck Nodes. Click Regen and then click OK.

5) Click Play to view simulation.