Problem: Create a Contact Demonstration of 2 deformable contact bodies to perform a linear static analysis of surface to surface touch contact in SimXpert.

1) Click Structures.

1) Select Tools > Options.

2) Highlight Units Manager.

3) Click Standard Units.

4) Scroll down and select the line with in, lb, s, rankine.

5) Click OK.

6) Click OK.

1) Under the Geometry tab, select Planar from the Surface group.

2) Choose 2 Points.

3) Enter 0,0,0;0,0,1 for Points.

4) Enter 10 for Length and Enter 6 for Width.

5) Click OK.

1) Select Curve from the Curve group.

2) Choose Polyline and 2 Points.

3) For X,Y,Z Coordinate enter 3, -2, -0.1;3, 2, -0.1.

4) Click OK.

5) Turn ON Transparency.

6) Select Sweep from the Surface group.

7) Click in the Along text box and choose Axis.

8) For Reference Coordinate System enter 0 0 0.

9) For Axis, select the X axis.

10) For Length of Sweep enter 10.

11) For Entities choose Curve 5 the curve on the middle of the geometry.

12) Check Delete entities to sweep then Click OK.

1) Under the Meshing tab, select Surface from the Automesh group.

2) Select the first (top) surface as shown.

3 Uncheck Calculate.

4) Enter 1 for Size.

5) Click Apply.

1) Select the second (bottom) surface as shown.

2) Enter 0.75 for Size.

3) Click OK.

1) Under the Materials and Properties tab, select Isotropic from the Material group.

2) Enter Aluminum for Name.

3) Enter 10e6 for Young’s Modulus, 0.3 for Poisson’s Ratio.

4) Click Apply.

5) Enter Plastic for Name.

6) Enter 1e6 for Young’s Modulus, 0.3 for Poisson’s Ratio.

7) Click OK.

8) Check for the newly created materials in the Model Browser.

1) Select Shell from the 2D Properties group.

2) Enter Aluminum Plate for Name.

3) Click in the Entities textbox. Deselect Pick Elements and Parts on the Pick Filters.

4) Select the first surface as shown.

5) Click in the Material text box and select Aluminum from the Model Browser.

6) Enter 0.06 for Part thickness. Click Apply.

7) Pull down the pick arrow to the right of the Entities text box and select Clear.

8) Click Apply.

9) Click in the Entities textbox and Deselect Pick Elements and Parts on the Pick Filter.

10) Select the second surface as shown.

11) Click in the Material text box and select Plastic from the Model Browser.

12) Enter 0.06 for Part thickness.

13) Click OK.

1) Under the LBCs tab, select Fixed from the Constraints group.

2) Click in the Entities text box and select Pick Curves from the Pick Filters.

3) Select the two curves as shown.

4) Click OK.

5) Turn ON Detailed Rendering to visualize the constraints.

1) Select Pressure from the Pressure group.

2) Click in the Entities text box. Deselect Pick Elements on the Pick Filter.

3) Select the second surface as shown.

4) Enter -0.5 for Pressure value.

5) Click OK.

1) Select Deformable Body from the Contact group.

2) Enter AluminumContact for Name.

3) Select Deformable Surface for Type.

4) Click in the Pick Entities text box.

5) Select Pick Surfaces on the Pick Filters toolbar.

6) Select the first surface as shown.

7) Click Apply.

8) Enter PlasticContact for Name.

9) Enter Deformable Surface for Type.

10) Select Clear to clear out the entities ont he Pick Entities box.

11) For the Pick Entities, select the second surface as shown.

12) Click OK.

13) Select Table from the Contact group.

14) Make sure the values in the contact table cells are all T.

15) Click OK.

1) Right click on FileSet and select Create new Nastran Job.

2) Enter SurfaceContact for Job Name.

3) Click OK.

4) In the Model Browser, right click on Loads/Boundaries and pick Select Contact Table.

5) Click in the Selected BCTable text box.

6) Select the BCTABLE_1 from the Model Browser.

7) Click OK.

8) Right click on Output Requests. In the Nodal Output Requests select Create Contact Output Request.

9) Click OK.

10) In the Model Browser, Right click on Solver Control and select Properties.

11) Highlight Output File Properties.

12) Select Master / DBALL for Nastran DB Options.

13) Select XDB for Binary Output.

14) Click Apply.

15) Click Close.

1) Right click on SurfaceContact and select Run.

1) Select File and choose Attach Results.

2) Click Browse.

3) Select the file surfacecontact.MASTER.

4) Click Open.

5) Click OK.

1) Under the Results tab select Deformation from the Results group.

2) Make sure the State plot property editor by default is setup to show translational displacement.

3) Click Update.

4) Click Update.

5) Select Displacements, Translational for the Result type.

6) Click Update.

7) Highlight Stress Tensor for the Result type.

8) Highlight von Mises for Derivation.

9) Click Update.

10) Click Clear after viewing results.

br />