Problem: Two types of interference fit modeling are demonstrated in this workshop. Interference fits can be modeled geometrically or by specifying an Interference Closure amount in the MSC Marc Contact Table and using congruent geometry. This workshop will show that the same results are achieved for both methods. The two main objectives for this problem are to investigate contact table parameters. and use interference Analysis using deformable-deformable contact. The following properties of the lug are given: Young's Modulus of 30 x 106, Poisson's Ratio of 0.3, and Mass Density of 0.00074.
Horizontal spacer
Download required files here

1) Click on File. Click on Import and go to Patran...

2) Select lug_pin_if.out and click Open.

3) Click Fill.







1) Under Material Properties and under Material Properties, click on New - Structural.

2) For Name, enter steel.

3) Click on Structural.

4) Enter 3e7 for the Young's Modulus and enter 0.3 for the Poisson's Ratio and click OK.

5) Under Elements, click Add.

6) Click All Existing and click on End List.







1) Under Geometric Properties, click on New and go to Planar and Plane Strain.

2) Under Name, enter all.

3) Click Properties.

4) For Thickness, enter 1. Click OK.

5) Under Elements, click Add

6) Click on the All Existing icon, and click on End List.







1) Under Boundary Conditions, go to New (Structural) and then go to Fixed Displacement.

2) Under Name, enter Fixed.

3) Click on Properties.

4) Make sure that Displacement X and Displacement Y are checked and click OK.

5) Under Nodes, click Add.

6) Select the left edge nodes as shown and then click on End List.







1) Under Contact in Contact Bodies, go to New - Deformable.

2) Under Name, enter lug.

3) Click Properties.

4) For Friction Coefficient, enter 0.05. Click OK.

5) Go to Select and then Selection Control.

6) Under Method, select Flood.

7) Click Elements and then click anywhere on the lug surface. Then click OK.

8) Under Elements, click Add.

9) Then click on All Selected and then click on End List.









1) Under Contact in Contact Bodies, go to New - Deformable.

2) Under Name, enter upper_pin.

3) Click Properties.

4) For Friction Coefficient, enter 0.05. Click OK.

5) Go to Select and then Selection Control.

6) Click Clear, under Elements.

7) Click Elements and then select any element in the Upper Pin as shown. Then click OK.

8) Under Elements, click Add.

9) Then click on All Selected and then click on End List.









1) Under Contact in Contact Bodies, go to New - Deformable.

2) Under Name, enter lower_pin.

3) Click Properties.

4) For Friction Coefficient, enter 0.05. Click OK.

5) Go to Select and then Selection Control.

6) Click Clear, under Elements.

7) Click Elements and then select any element in the Lower Pin as shown. Then click OK.

8) Under Elements, click Add.

9) Then click on All Selected and then click on End List.









1) Click on the Contact tab and then click on New in Contact Tables.

2) Click Properties.

3) Click the box 2-1 as (between lug and upper_pin) as shown.

4) For Contact Type select, Touching.

5) For Interference Closure, enter 0.01. and click OK.

6) Click the box 3-1 (between lug and lower_pin) as shown.

7) For Contact Type, select Touching.

8) For Distance Tolerance, enter 0.015 and click OK.







1) Under the Loadcases tab, go to New - Static.

2) Click Properties.

3) Click Contact.

4) Click Contact Table and select ctable1 and click OK.

5) Select Multi-Criteria and click on Parameters.

6) For Initial Fraction of Loadcase Time, enter 1. For Maximum Fraction of Loadcase time, enter 1. Click OK and OK.







1) Click on Jobs tab and click on Elements Types.

2) Under Analysis Dimension, then Click Planar, and then click Solid.

3) Select 27.

4) Click on the All Existing icon and click OK.

5) Click on ID Types to verify the elements.





1) Click on the Jobs tab and then click on New - Structural.

2) Then, click Properties.

3) Select lcase1.

4) For Analysis Dimension select Plane Strain.

5) Click Contact Control.

6) For Type, select Coulomb Bilinear (Displacement) and click OK.

7) Click Analysis Options.

8) Make sure Small Strain is selected and click OK.

9) Now click on Job Results.

10) Select Element Scalar: Equivalent Von Mises Stress.

11) Select Element Tensor: Stress. Click OK and OK.











1) Click Run.

2) Click Save Model.

3) Click Submit(1).

4) Click Monitor.

5) Click Open Post File (Results Menu).



1) Under Deformed Shape, for Style, select Deformed Only.

2) Under Scalar Plot, for Style, select Contour Bands.

3) Click Scalar.

4) Select Equivalent of Stress, and click OK.

5) Click Monitor Results File to view the results.