Problem: Create a steel semi-cylinder with a radius of 5” is pressed against a 2” deep aluminum base. The problem is linear except for the contact condition between the two parts.

1) On the main menu click on File and choose Save As....

2) Enter hertz for the File name and click Save.

3) On the main menu click on Tools and choose Procedures.... Find the file name hertz.proc and then click Open. Then click on Load.

4) Click on Start/Cont.

5) Click OK on the Procedure File.

1) Under the Material Properties tab, click on New and then choose Standard.

2) For the Name enter Steel and then click Structural.

3) For the Young's Modulus, enter 3e7 and for the Poisson's Ration, enter 0.3. Click OK.

4) Click Add for the Elements, and then Screen Select the Elements shown on the image below.

5) Click on New and then choose Standard.

6) For the name enter ALUM and then click Structural.

7) For the Young's Modulus, enter 1e7 and for the Poisson's Ration, enter 0.33. Click OK.

8) Click Add for the Elements, and then Screen Select the Elements shown on the image below.

1) Click on New (Structural) and then choose Planar. Click Plane Strain.

2) Click on Add and then click on the All Existing Elements icon.

3) Click Run.

4) Click on Save Model and then click on Submit. Click on Monitor to monitor the status.

5) Click on Open Post File to open the result menu.

1) Under the Boundary Conditions Tab, click on Fixed Displacement.

2) Enter Sim_X for the Name. Click on Properties. Choose Displacement X and then click OK.

3) Click Add for the Nodes. Then Screen Pick the nodes showns on the image below then Right Click to end the list.

4) Under the New (Structural) click on Fixed Displacement.

5) Enter Fix_Base_Y for the Name. Click on Properties.

6) Choose Displacement X and then click OK.

7) Click Add for the Nodes. Then Screen Pick the nodes showns on the image below then Right Click to end the list.

8) Under the Boundary Conditions tab click on New. Choose Independent Variable and then choose Time for the Type. Make sure Data Points is selected.

9) Click Add then enter 0 0 when "Enter independent variable V1 value" is prompted. Then click Enter.

10) Enter 1 1 when "Enter independent variable V1 value" is prompted. Then click Enter. Under the Boundary Conditions tab click on Edge Load. Enter PUSH_IT_DOWN for the Name. Click on Properties. Make sure that Pressure is selected and enter 200000 for the pressure.

11) Click on Table and make sure that table 1 is listed on the Currently Defined Tables. Click OK.

12) Then click OK.

13) Click Add for the Edges. Then Screen Pick the element edge showns on the image below then Right Click to end the list.

>

1) Under the Contact tab, click on New, then choose Deformable.

2) Enter Plate for the Name. Click on Add for the Elements.

3) Then Screen Pick the nodes showns on the image below then Right Click to end the list.

4) Click on New, then choose Deformable. Enter Cylinder for the Name.

5) Click on Add for the Elements. Then Screen Pick the nodes showns on the image below then Right Click to end the list.

1) Under the Loadcases tab, click on New, then choose Static.

2) Click on Properties. Make sure that Multi-Criteria is selected.

3) Now, click on the Solution Control. Make sure that Non-Positive Definite is selected. Then click OK for Solution Control and Loadcase Properties.

1) Under the Jobs tab, click on New, then choose Structural.

2) Click on Element Types and then choose Planar for the Analysis Dimension.

3) Click on Solid choose Quad 11 and then click OK.

4) Make sure that ID Types is selected. Then click All Unselected Quad 11 elements will show up on the display.

5) Now click on Close.

6) Click on Properties. Then click on lcase1.

7) Choose Plane Strain for the Analysis Dimension, then click on Analysis Options.

8) Click on Advanced Options. Make sure that Assumed Strain is selected. Then click on OK.

9) Click on Initial Loads. For the Boundary Conditions click Clear select Sim_X & Fix_Base_Y. Then click on OK.

10) Click on Job Results. Select Stress and Equivalent Von Mises Stress.

11) Then click on Custom and then select Displacement. Click OK.

12) Click on Save Model and then click on Submit. Click on Monitor to monitor the status. Click on Open Post File to open the result menu.

1) Choose Deformed Only for the Style under Deformed Shape.

2) Under Scaler Plot choose Contour Bands. Click on Scalar, then choose Equivalent of Total Strain, and then click OK.

3) Click on the Monitor Result File icon to monitor the result file.

4) Under View menu click on Plot Control....

5) Uncheck Nodes. Click Redraw, and then click OK.