1) Click Structures.

1) Check in the lower right-hand corner for the current system of units.

2) If the current system of units is not English units (in, lb, s), click on the box to bring up the User Options form.

3) Click Standard Units.

4) Scroll down and select the line with units in, lb, s,…

5) Click OK and OK.

1) Go to Geometry > Surfaces > Planar.

2) Enter Origin Point as 0,0,0.

3) Enter 4 for Length.

4) Enter 1 for Width.

5) Click OK.

1) Activate Top view, by clicking on the "Cube" icon and clicking on Top.

2) Plot Geometry Wireframe, by going to the "Cube" icon and selecting Geometry Wireframe.

3) Select Meshing > Automesh > Seed.

4) Select Curves on the left and right of the surface as shown.

5) Enter 9 for the Number of Elements and click OK.

1) Select Meshing > Automesh > Seed.

2) Select Curve on the bottom of the surface as shown.

3) Select One Way Bias Type.

4) Check Display Curve Orientation Marker Box.

5) Activate Number of Elements and L2/L1 Method.

6) Enter 27 for the Number of Elements.

7) Enter 0.2 for L2/L1 and click Apply.

1) Select Curve on the top of the surface

2) Select One Way Bias Type.

3) Check the Display Curve Orientation Markers Box.

4) Activate Number of Elements and L2/L1 Method.

5) Enter 27 for the Number of Elements.

6) Enter 5 for L2/L1.

7) Click Apply.

1) Select Meshing > Automesh > Surface.

2) Select Surface on the bottom of the surface

3) Select Quad Dominant for the MeshType.

4) Select Mapped for the Mesh Method and click OK.

1) Under the Materials and Properties tab, click Isotropic in the Material group.

2) Enter Material Name Aluminum.

3) Enter 1e7 for Young’s Modulus.

4) Enter 0.33 for Poisson’s Ratio.

5) Activate Advanced.

6) Click on the Add Constitutive Model button.

7) Select Elasto-Plastic.

8) Select Stress-Strain Data.

9) Click on the Stress-Strain Data Arrow > New > Strain Dependent (Structural).

10) A new Window will open with Strain Dependent table.

11) Select Total Strain for the Strain Type.

12) Click "+" button to add Points Data.

13) Fill the Table with all points define to create plasticity curve.

14) Click the Update Plot button to visualize the curve and click OK.

15) Stress-Strain Data has been implemented. Click OK.

1) Click Plane in the 2D Properties group.

2) Click in the Entities text box.

3) Select the part PART_1 from the Model browser.

4) Click in the Material textbox.

5) Select Aluminum from the Model Browser. 6) Click Advanced.

7) Check Non Linear box in the Advanced Part.

8) Verify Aluminum is define as Material.

9) Define 1 for the Thickness.

10) Define Implicit Structural for the Analysis type and click OK

1) Under the LBCs tab, click General in the Constraints group.

2) Enter Symmetry_vertical for the LBC Name.

3) Click in the Entities text box and select the curve filter only.

4) Select the left curve.

5) Check T1, R2, R3 boxes and uncheck T2, T3, R1, click OK.

6) Under the LBCs tab, click General in the Constraints group.

7) Enter Symmetry_horizontal for the LBC Name.

8) Click in the Entities text box and select the curve filter only.

9) Select the Top curve.

10) Check T2, R1, R3 boxes and uncheck T1, T3, R2 and click OK.

11) Under the LBCs tab, click General in the Constraints group.

12) Enter Pull_at_end for the LBC Name.

13) Click in the Entities text box and select the curve filter only

14) Select the Right curve.

15) Enter 1.4 for T1, check T2 and T3 and uncheck R1, R2, R3 and click OK.

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

2) Enter Prob7_necking as the Job Name.

3) Select General Nonlinear Analysis (SOL400).

4) If desired, click the folder icon to the right of the Solver Input File text box and select the location to save the analysis files and click OK.

1) Right click Solver Control and select Properties.

2) Highlight Analysis Options.

3) Select Large Displacement and Follower Force.

4) Uncheck Assumed Strain box.

5) Uncheck Assumed Strain box.

6) Click Apply and click Close.

1) Right-click Load Case Control and select Properties.

2) Highlight Stepping Control Parameters.

3) Define an Adaptive Stepping type.

4) Define Time stepping parameters.

5) Select Every computed load increment for the Output control.

6) Click Apply and click Close.

1) Right-click Output Requests and select Elemental Output Requests > Create Sol400 Nonlinear Stress Output Request.

2) Select Stress and Strains and check Cauchy Stress, Total Strain, Elastic Strain, Plastic Strain.

3) Select Equivalents and check Equivalent von Mises Stress, Equivalent Plastic Strain and click OK.

1) Right click on Prob7_necking and select Run.

2) Select File > Attach Results.

3) Click the folder icon for File Path.

4) Navigate to and select the file WS03_necking.op2.

5) Click OK.

1) Under the Results tab, click Deformation.

2) Highlight Results Case Time = 1.

3) Highlight Results Type Displacements, Translational.

4) Under the Deformation tab, Check the Show undeformed check box.

5) Activate True Deformation scaling to 1.

6) Click Update.

7) Click Fill.

8) Click the Plot Data tab.

9) Pull down the Plot type to Fringe.

10) Click Update. The maximum deformation should be 1.40 in.

1) Select to Plot the von Mises component of the Cauchy Stress, Nonlinear Output for the time = 1.

2) Click Update. The maximum tress should be 19390 psi.

1) Select to Plot the Equivalent Plastic Strain, Nonlinear for the time = 1.

2) Click Update. The maximum plastic strain should be 1.777.

1) Select File > Save As…

2) For filename, enter Prob7_necking.SimXpert.

3) Click Save.

4) Select File > Exit.