

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) 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 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) 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.


