+1 800 942 2072 |Sign In|Contact Us|
Exercises

Plastic Deformation of a Cantilever Beam

Problem: In this exercise, a cantilever beam is subjected to a static load. The beam is initially analyzed using small deformation theory. However, after reviewing the results, it becomes apparent that small deformation theory is not appropriate for this problem. Subsequently, a large deformation analysis is performed and its results are compared to the small deformation analysis. Using Marc, Find the vertical displacement imposed by the load P by adjusting the nonlinear load case to account for plastic deformation. The load P is 6000 lb. The length L of the beam is 100 in. The dimensions of the beam Section A-A (a x b) are 1.0 in x 2.0 in. The Young's Modulus is 30 x 106 and the Poisson's Ratio is 0.3.
 
Download required Files here

Step 1 - Open Model.

1) Click on File and then Open.

2) Browse and Select tip_load.mud in working directory. and click Open.





Step 2 - Add Plastic Property Table.

1) Under Table & Coord. System, click on New and go to 1 Independent Variable.

2)Enter YieldStress_Table for the Name.

3) Then click on Type and select eq_plastic_strain.

4) Click on Data Points and then click on Add.

5) In the Dialog Box, enter 0 65000 0.5 1.565E6.

6) Then click Fit.

(65000 is Yield Stress and 30E6 is Young Modulus, considering plastic range slope 10% slope of Elastic range so another point on the curve can be calculated as follows for the table 0.1*30E6*0.5+65E3 = 1.565E6)







Step 3 - Add Plastic Property to the Material.

1) Under Material Properties, click Show Menu.

2) Under Data Categories, Click on Structural.

3)Click on Plasticity.

4) Enter Yield Stress as 1.

5) Then click on YieldStress_Table and then click OK and OK.



Step 4- Subdivide the Mesh.

1)Under Windows, change back to Model (View 1) to change back to the Beam Model if you are still on Table (View 1).

2) Under Geometry & Mesh - Operations, click on Subdivide.

3) Enter Divisons as 2 and 4.

4) Then click on Elements.

Select All Elements



Step 5 - Adjust the Boundary Conditions.

1) Under Boundary Conditions.

2) Click on Edit.

3) Click on Fixed, then click on OK.

4)Under Nodes, click on Add.

5) Select the Left Edge Nodes as shown and click on End List. Check number of numbers to be 5, if not then click on Sweep under Geometry & Mesh and go to Nodes and and select the same left edge and click on End List to remove the duplicate Nodes and Elements.





Step 6 - Adjust the Nonlinear Job.

1) Click on Temperature under the Nodal section.

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

3) Input 100 as the Boundary Temperature. Click OK.

4) Click on Select Application Region and then screen select the left edge of the surface. Click Add, OK then Apply.



Step 7 - Run the Analysis.

1) In the Jobs tab, click Run.

2)Click Submit.

3) When the Status indicates Complete, click on Open Post File (Result Menu).



Step 8 - Plot Deformation.

1) Click on the Results tab and click on Model Plot.

2)Under Deformed Shape set style to Deformed & Original.

3)Under Scalar Plot set the style to Contour Bands.

4)Click Scalar and select Displacement Y. Click OK.

5) Click Play.

6) Click FILL.





Step 9 - Plot Total Strain and Global Plastic Strain.

1) To plot the Total Strain, while still in the Model Plot tab, under Scalar, click on Equivalent of Total Strain. Then click OK.

2) To plot the Global Plastic Strain, while still in the Model Plot tab, under Scalar, click on Equivalent of Global Plastic Strain Layer. Then click OK.









 

Share this page