1. ANALYSIS OF A RUBBER SEAL
WORKSHOP 2
ANALYSIS OF A RUBBER SEAL
MAR 120, Workshop 2, December 2001

3. Model Description:
In this Exercise we analyze a trunk door seal. The purpose of the analysis is to examine the stresses and deflections created during the closing of a door. The seal is made of a rubber material and therefore will be modeled using hyperelastic material properties. The trunk door is considered very stiff relative to the rubber seal and can be modeled using a rigid body.

4. Objectives: Required: Large displacement/ Large strain analysis
Contact analysis using a rigid body contact model
Hyperelastic material model
Required:
A file named rubber_seal.ses in your working directory (Ask your instructor for it if you don’t see it before starting.)

5. Suggested Exercise Steps:
Build the seal geometry and mesh from a session file.
Model the contact surfaces with LBC contact.
Create the element properties.
Create the Loads and BCs.
Submit the job to analysis.
Evaluate the results.

6. CREATE NEW DATABASE a d e f c b
MSC.Marc q e f
Create a new database. Name it Pin_Insert.db.
File / New.
Enter Rubber_seal as the file name.
Click OK.
Select MSC.Marc as the Analysis Code.
Select Structural as the Analysis Type.
Rubber c
Rubber_seal b

7. Step 1. Run the Provided Session Filea b
Rubber
Run the provided session file.
File / Session.
Click Play.
Select rubber_seal.ses as the File name.
Click -Apply-. (This action will run the session file. Please do not interrupt it.) c
Rubber_seal.ses d
When the session file is done the viewport will contain all the geometry for the rubber seal and trunk rigid body. Additionally, 2 groups have been created, one containing the seal and the other containing the trunk.

8. Step 2. Elements / Mesh Seed / Curvesa
Create Mesh Seed for Curves.
Elements : Create / Mesh Seed / Uniform.
Select Element Length.
Enter 0.06 as the Element Length.
Uncheck Auto Execute.
Click in Curve List panel.
Select Curve icon.
Pick curves 2,3 and 4 (Hold on to the Shift Key when you are selecting the curves. It will let you choose multiple curves.)
Click –Apply-. g b c
0.06 d e
Curve 2:4 h f

9. Step 3. Elements / Create Mesh / Curves
3470
Create Mesh for Curves.
Create / Mesh / Curve.
Select Bar2.
Click in Curve List panel.
Select Curve or Edge icon.
Pick all three curves.
Enter 0.1 as the Value.
Click –Apply-.
3090 b c
Curve 2:4 e f
0.01 g d

10. Step 4. Elements / Create / Mesh / Surface2
Mesh the seal.
Create / Mesh / Surface.
Select IsoMesh as the Mesher.
Click in Surface List panel.
Select Surface or Solid Face icon.
Pick all three surfaces. (Surface 1:3)
Uncheck Automatic Calculation.
Enter as the Value.
Click –Apply-. 1 b e c
Surface 1:3 f g
0.015 h d
We use IsoMesh to mesh the top part only.
Continue working in Elements form on next page.

11. i j k n m o l p We use Paver to mesh the bottom part.
Create / Mesh / Surface.
Select Paver as the Mesher.
Click in Surface List panel.
Select Surface or Solid Face icon.
Select Surface 4.
Uncheck Automatic Calculation.
Enter as the Value.
Click –Apply-. i
1604
1401 j k
Surface 4 n m o
0.015 l p

12. Step 5. Elements / Equivalence / All / Tolerance Cube
Equivalence the model.
Equivalence / All / Tolerance Cube.
Enter .005 as the Equivalencing Tolerance.
Click –Apply-. a b
0.005 c
Equivalence any duplicate nodes created during meshing. This process will delete all the overlapped nodes (where the pink circles are), and have only one nodes left.

13. Step 6. Elements / Verify / Element / Normalsd a
Verify the elements’ normals.
Verify / Element / Normals.
Select Draw Normal Vectors.
Click –Apply-.
Click on Iso 1 View icon.
Select Reverse Elements.
Enter Elm 314 as the Guiding Element. (Pick any element pointing in the positive Z-direction as guiding element.) b e f
Elm 314 c g
Wrong orientation.
Since this is a 2-D solid model, all element normals must point in the positive Z direction. Verify the elements’ normals, and correct those whose normals point the wrong direction.

14. Step 7. Elements / Create / Node / Edit
9999
Coord 0
[0 0 0] a b d e g c f
Creating a node for future reference.
Create / Node / Edit.
Click on Node ID List panel.
Enter 9999 as the Node ID List.
Uncheck Auto Execute.
Enter [ ] as the node location.
Click on Front View icon.
Click -Apply-.
Location of the node 9999.

15. Step 8. Material / Create / Isotropic / Manual Input*
rubber a b c k
Define the rubber material.
Materials: Create / Isotropic / Manual Input.
Enter rubber as the Material Name.
Click on Input Properties.
Select Hyperelastic as the Constitutive Model.
Select Mooney-Rivlin as the Model.
Select Time as the Domain Type.
Select 1 as the Number of Terms.
Enter 80 as the Strain Energy Function, C10.
Enter 20 as the Strain Energy Function, C01.
Click OK.
Click Apply. 80 20 d e f g h i j
The material’s constitutive model used in this analysis is an Incompressible Mooney Rivlin hyperelastic formulation. Make sure that the analysis code is set for MSC.Marc under Preferences- Analysis.

16. Step 9. Properties: Create / 2D / 2D Solid
seal a b c e d
Define the Element Properties.
Properties: Create / 2D / 2D Solid.
Enter seal as the Property Set Name.
Select Plane Strain as the Option.
Select Herman/Reduced Integration.
Click on Input Properties.
Click on Material Property Sets panel.
Select rubber as the Material Name.
Enter 1 as the Thickness.
Click OK.
M:rubber 1
rubber
Real Scalar q f g h i

17. In this step, you will be defining the element properties for the rubber seal. The seal will be modeled using a 2-D Solid (Plane Strain) Hermann/Reduced Integration element formulation. The rubber material will be assigned to this property. Incompressible hyperelastic materials require the use of the Hermann formulation.
Click in Select Members panel.
Select Surface or face icon.
Select all four surfaces as the Application Region.
Click Add.
Click –Apply-.
seal
seal l k j
Surface 1:4 m
Surface 1:4 n

18. Step 10. Loads/BCs: Create / Contact / Element Uniform
Node 9999
<-0.06, -0.60, 0 > f g h i j
Create the rigid contact object.
Loads/BCs: Create / Contact / Element Uniform.
Select Rigid Body as the Option.
Enter door as the New Set Name.
Select 1D as the Target Element Type.
Click on Input Data.
Check Flip Contact Side. (This is needed because the rigid surface bounds an actual body –a car’s door in this problem- which, the way we created these curves will otherwise to be on the wrong side. See page 2-17.)
Select Velocity as the Motion Control.
Enter <-0.06, -0.60, 0.> for the Velocity.
Pick Reference Point: Node 9999 (See next page for location of this node. You do not really need to enter a node here if no rotation of the rigid surface is to be used; we have you entering a node so you later can more easily experiment with forcing a rotation of the rigid surface; therefore, if you wish, ignore this instruction for now.)
Click OK.
Click on Select Application Region form.
door a b c d e k

19. Notice: Location of Rotation Reference Point (Node 9999)
Rigid Surface
Curve 2
Curve 3
Curve 4 n
Choose Geometry as the Geometry Fitter.
Click in Select Curves panel.
Select all three curves defining the rigid surface (Curve 2:4) using Curve or Edge. These curves are not meshed; yet one node has been created at one end for MSC.Marc to use as a reference point.
Click Add.
Click OK.
Curve 2:4 l m o p
Notice: Location of Rotation Reference Point (Node 9999)

20. The rigid contact markers points in the direction toward the inside of the rigid body –think of them as tickmarks representing a wall.
Click –Apply-.
Rigid Contact Markers
door q
The -Apply- action actually saves the rigid contact body in the MSC.Patran database. You should then see the contact (pink) markers in the viewport and the name of the object in the Existing Sets panel..

21. Step 11. Loads/BCs: Create / Contact / Element Uniform
After you Apply you will see the contact markers (pink circles) in viewport. a b
Create the deformable contact object.
Create / Contact / Element Uniform.
Select Deformation Body as the Option.
Enter rubber as the New Set Name.
Select 2D as the Target Element Type.
Click on Select Application Region form.
Choose Geometry as the Geometry Fitter.
Click on Select Surfaces panel.
Select all four surfaces using the Surface or face icon.
Click Add.
Click OK.
Click –Apply-. i h
Surface 1:4 f g j i c
rubber d e k

22. Step 12. Loads/BCs : Create / Displacement / Nodal
Create the Boundary Condition fixing the bottom of the rubber seal.
Create / Displacement / Nodal.
Enter Base fix as the New Set Name.
Click on Input Data.
Enter <0,0, > for the Translation.
Enter < , , > for the Rotation.
Click OK.
Click on Select Application Region form.
Base fix a b c g
<0, 0, >
< , , > 1.
Coord 0 d e f

23. j h i m k l Choose Geometry as the Geometry Fitter.
Base fix m
Choose Geometry as the Geometry Fitter.
Click on Select Geometry Entities panel.
Select the bottom edge of the surface using the Curve or Edge icon.
Click Add.
Click OK.
Click –Apply-. j
Surface 4.1 h i k l

24. Step 13. Analysis: Analyze / Entire Model / Full Run
Setup and launch the Analysis.
Analysis: Analyze / Entire Model / Full Run.
Enter Rubber_job1 as the Job Name.
Click on Load Step Creation form.
Enter Close door as the Job Step Name.
Click on Solution Parameter panel.
Rubber_job1
Full Run q
Entire Model q a b c
Default Static Step
Close door d e

25. f i j g k h l m n o p Select Nonlinear for the Linearity.
Select Large Displacements/Large Strains.
Click on the Load Increment Parameters form.
Select Adaptive as the Increment Type.
Select None.
Enter 5 as the Number of Cutbacks.
Enter 0.1 as the Trial Time Step.
Enter 2.0 as the Time Step Scale Factor.
Enter 100 as the Max Number Of Step.
Enter 1 as the Total Time.
Click OK. f g h 5
0.1
2.0
100 1 i j k l m n o p

26. q s
Note that the rubber seal can make contact with itself and the rigid body. The rigid body on the other hand, cannot contact itself.
Click on Contact Table.
Click OK. (We are not changing anything here, just wanted you to take a look at this table.)
Click OK.
Click Apply.
Click Cancel.
Default Static Step
Close door t u
rubber
rubber
door
door r

27. w x v z y The Step Select form looks like this when you open it.
Default Static Step
Close door w
Rubber_job1
Full Run q
Entire Model q v z x
Click on Load Step Selection form.
Select Close Door from the Existing Job Steps.
Deselect Default Static Step.
Click OK.
Click Apply.
Default Static Step
The Step Select form should look like this when you close it.
Close door
Default Static Step
Close door
Monitor the job while it runs as explained in Workshop 1. y

28. Step 14. Analysis: Read Results / Result Entities / Attach
Read (Attach) results.
Analysis: Read Results / Result Entities / Attach.
Select Rubber_job1 from the Available Jobs.
Click on Select Results File form.
Select Rubber_job.
Click OK.
Click Apply.
Rubber-job1
Rubber-job2
Result Entities
Attach q a b c f
Rubber-job1.t16
Rubber-job2.t16 d e

29. Step 15. Results: Create / Quick Plot
1.0 a b c d e f
Post-process results.
Results: Create / Quick Plot.
Click on Deform Attributes icon.
Select True Scale as the Scale Interpretation.
Enter 1.0 as the Scale Factor.
Uncheck Undeformed.
Click Apply.

30. g h i j k l After you Apply the viewport will look like this.
Click on Select Result icon.
Select the last result case available.
Select Strain, Total as the Fringe Result.
Select von Mises as the Quantity.
Select Displacement, Translation as the Deformation Result.
Click Apply.
Notice the self-contact in the seal.

31. Step 16. Results: Read Results
Use any text editor (such as Notepad) and open the file. Then search for second occurrence of text “body number 2”. The editor pointer should find this record:
This section of the job.out file describes the rigid surface as defined by a sequence of (straight) line segments or polygonal; the points in the polygon are the nodes of the one dimensional mesh you created on the three curves defining the “door”. The value of “analytical form” is 0 (no use of analytical geometry). Other data define the (translational) “velocity” and (rotational) “angular velocity” of the rigid surface, friction coefficient.
You can open this file from the Analysis form using Action: Monitor.
(more like this…)

32. Step 17. Elements: Delete / Mesh / Curve
Delete the 1-D Mesh on the rigid surface
Elements: Delete / Mesh / Curve.
Uncheck Auto Execute.
Click on the Curve List panel.
Select Curve 2:4 using Curve or Edge picking icon.
Click –Apply-. d
Curve 2:4 a b c e
The rigid surface still exists after having deleted the 1-D mesh; however the rigid surface is now defined by geometric entities, the curves 2, 3, and 4.

33. Step 18. Analysis: Analysis / Entire Model / Full Run
Rubber_job2
Rubber-job1
Full Run q
Entire Model q a b c d
Analyze.
Analysis: Analyze / Entire Model / Full Run.
Select rubber_job1 from the Available Jobs.
Enter rubber_job2 as the Job Name.
Click Apply.
By selecting the existing job name and then editing the name you are copying all the setup done for the first job into the second job. (which you may later edit if you so desire.)
This way the new job will not override the files created by the first job so you may compare the two sets later.
Monitor the job while it runs as explained in Workshop 1.

34. Step 19. Analysis: Read Results / Result Entities / Attach
Read (Attach) results.
Read Results / Result Entities / Attach.
Select rubber_job2 from the Available Jobs.
Click on Select Results File form
Select rubber_job2.
Click OK.
Click Apply.
Rubber-job1
Rubber-job2
Result Entities q
Attach q a b c f
Rubber-job1.t16
Rubber-job2.t16 d e

35. Step 20. Results : Create / Quick Plot
1.0 a b c d f e
Visualize Result.
Results: Create / Quick Plot.
Click on Deform Attributes icon.
Select True Scale as the Scale Interpretation.
Enter 1.0 as the Scale Factor.
Uncheck Show Undeformed.
Click Apply.

36. Compare these results with the ones obtained using a meshed rigid surface; in this case you will hardly find any difference. (The minimum strain is slightly different.) h g i j k l
Click on Select Result icon.
Select the last result case available.
Select Strain, Total as the Fringe Result.
Select von Mises as the Quantity.
Select Displacement, Translation as the Deformation Result.
Click Apply.

37. Step 21. Read the rubber_job2.out File
Use any text editor (such as Notepad) and open the file. Then search for second occurrence of text “body number 2”. The editor pointer should find this record:
This section of the job.out file describes the rigid surface as defined by Nurbs curves; These are used after you deleted the one dimensional mesh on the three curves defining the “door”. The value of “analytical form” is 1 (use of Nurbs analytical geometry). Compare this with the definition of the rigid geometry in section 17 of this workshop.
You can open this file from the Analysis form using Action: Monitor.
continue
(more like this…)

38. Step 22. Experiment Rotating the Rigid Surface
This is a challenge for you. Back in section 11 you created the rigid surface using the reference node Take advantage of that by introducing a rotation of – radians (10 degrees) of the rigid surface at the same time you move it down (and slightly to the left) with the same Velocity of <-0.06, -0.60, 0.> used before.
How to: Use Loads/BCs, Modify Contact, Option: Rigid Body, select, the “door” set, open the Modify Data form, enter the “Angular Velocity” value given above (in radians), OK the form, Apply. Notice you need the rotation reference node 9999 in the definition of the rigid surface discussed earlier.
Run the analysis again changing the name of the job to Rubber_job3 as you did in section 21. Read the results and visualize and compare them with previous results.