Contact Us
Problem: Using Patran/MSC Nastran, simulate a linear static model of how two deformable steel plates in the position shown below would behave when a 10 lb force is applied to the Y-direction to the right corners of the top plate. The dimensions of the plates are 4 in x 2 in x 0.1 in.
Horizontal spacer

1) Click on New from the File menu or from the Defaults Toolbar as shown.

2) Type the name of the new database as Deformable_Contact and click OK.

3) In the Approximate Maximum Model Dimensions box, input 10.0. Choose Structural for the analysis type. Click OK.





1) Under the Geometry tab, click on Solids and select XYZ.

2)Under Vector Coordinates List, enter <4 0.1 2> and under Origin Coordinates List enter [3 0 0] then click Apply. There are no units in Patran, and therefore it is important to stay consistent in units. (If Auto Execute is checked all you have to do is hit enter, do not click Apply, and it will create the geometry for you. Be careful not to create duplicate solid geometries.)

3) Create the second solid by changing the Origin Coordinates List input to [0.5 0.1 0], then click Apply.





1) Under the Properties tab, select Isotropic.

2) Input steel as the Material Name and then select Input Properties.

3) Input Elastic Modulus = 30E6, Poisson Ratio = 0.3. Click OK and Apply.



1) Click on Solid under the 3D Properties section.

2) Input Deformable_Solid as the Property Set Name and then click on Input Properties .

3)Click on Select Material and select steel. Click OK.

4) Click on Select Application Region and then click on the Select Members box. Screen pick Solids 1 and 2. Click Add, OK, then Apply



1) Under the Load/BCs tab, select Displacement Constraint.

2) Input New Set Name as the Fixed, and click on Input Data.

3) Enter Translations as <0,0,0>. Click OK.

4) Click on Select Application Region click on the Surface or Face. For the Application Region, screen select the left surface of Solid 1. Click Add, then screen select the right Surface of Solid 2. Click Add. Now click OK then Apply.







1) Click on Force. Enter New Set Name as Force and click on Input Data.

2) Enter <0,-10,0> as the Force and click OK.

3) Click on Select Application Region

4) Now,Click on the Select Geometry Entries box. In the filters toolbar, select Point. Screen select the 2 nodes as shown (you can click both nodes by holding down shift key). Click Add, OK then Apply.







1) Under the Meshing tab, set the Object as Mesh and Type as Solid.

2)Set the Elem Shape to Hex and Topology to Hex8. Click on the Input List box and screen select the bottom plate (Solid 1, in this case) as shown. Set the Global Edge Length to 0.25. Click on Apply.

3) Now, click on the Input List box and screen select the bottom plate (Solid 2, in this case) as shown. Set the Global Edge Length to 0.2. Click on Apply.





1) Under the Loads/BCs tab, click on Contact Bodies then choose Deformable.

2) For the name input Solid1 then choose 3D for the Target Element Type. Select Application Region, then screen pick Solid 1. Click Add, OK and Apply.

3) Now change the name to Solid2 then select Application Region , screen pick Solid 2. Click Add, OK and Apply.









1) Under the Analysis tab, select Entire Model. Input Deformable_Contact for the Job Name and click Solution Type. Choose LINEAR STATIC. Then click on Solution Parameters.

2) Click on Results Output Format.... Uncheck XDB, and choose MASTER/DBALL. Click OK, OK, and OK.

3) Now click on Subcases... and for the Available Subcases choose Default. Click on Subcase Parameters..., click on Contact Table.... Deselect the diagonal (to remove self-contact) by clicking on the T on the first column first row three times and by clicking on the second column second row three times. Click OK and OK.

4)Now click on Output Requests... and choose Contact Results on Select Result Type. Click OK, Apply, and Cancel. Now you are ready to run the model by clicking Apply.











1) Now click on MASTER/DBALL.

2) Ensure the appropriate Job Name is selected and click Apply.

3) Click the Results tab, select Fringe/Deformation for Object. Choose Displacements, Translational for Select Deformation Result, then click on Displacement, Translational.

4) Uncheck Show Undeformed then click Apply.









A deformable body is a physical body that deforms, this means that the body changes its shape or volume due to an external force.

In this problem forces are being applied to the top plate resulting in contact being created between the two plate.

A Hex 8 mesh is the suitable choice for a linear static deformable contact body.

In the model the outer surfaces of the 2 deformable bodies are fixed, this is what causes the deformation after a force is applied.