Abaqus/CAE ( ver. 6.9) Geometric Nonlinearity Tutorial
Problem Description The aluminum arch shown below is completely clamped along the flat faces. faces. The arch is to support a downward pressure of 600 MPa. The effects of geometric nonlinearities nonlinearities are to be included in the analysis, to determine if the arch will support the full load, and if it won’t what is the maximum pressure that can be applied.
Note: This is the same problem originally solved in “Shell Tutorial.” You may skip steps similar similar to the ones performed during linear elastic analysis.
©2008 Hormoz Zareh
1
Portland State University, Mechanical Engineering
Analysis Steps 1. Begin with the geometry from the shell tutorial
2. Create a set for the upper‐center vertex a. Expand the Assembly node in the model tree, and then double click on sets b. Name the set and select geometry for the type c.
Select the vertex at the top of the part and select “Done”
3. Double click on the “Steps” node in the model tree a. Name the step, set the procedure to “General”, and select “Static, General” b. On the “Basic” tab, give the step a description c.
Include the nonlinear effects of large displacements i. Nlgeom = On
d. On the “Incrementation” tab change the initial increment size to 0.1
©2008 Hormoz Zareh
2
Portland State University, Mechanical Engineering
4. Expand the Field Output Requests node in the model tree, and then double click on F‐Output‐1 (F‐Output‐1 was automatically generated when creating the step) a. Uncheck the variables “Strains” and “Contact”
5. Expand the History Output Requests node in the model tree, and then right click on H‐Output‐1 (H‐Output‐1 was automatically generated when creating the step) and select Delete
©2008 Hormoz Zareh
3
Portland State University, Mechanical Engineering
6. Double click on the History Output Requests node a. Name the history and select “Continue…” b. Set the domain to “Sets” and select the set created above c.
Leave the frequency set to every increment (n=1)
d. For the output variables select the U2 displacement
7. Because the part is symmetrical and the flat surfaces are fully restrained only a quarter of the arch needs to be modeled 8. Because the flat surfaces are assumed to be fully restrained we do not need to include them, and can instead fix just the edge
©2008 Hormoz Zareh
4
Portland State University, Mechanical Engineering
9. Double click on the “BCs” node in the model tree a. Name the boundary conditioned “Fixed” and select “Symmetry/Antisymmetry/Encastre” for the type
b. Select the edge shown below and click “Done”
c.
Select “ENCASTRE” for the boundary condition and click “OK”
©2008 Hormoz Zareh
5
Portland State University, Mechanical Engineering
10. Double click on the “BCs” node in the model tree a. Name the boundary conditioned “Zsymm” and select “Symmetry/Antisymmetry/Encastre” for the type
b. Select the edge shown below and click “Done”
c.
Select “ENCASTRE” for the boundary condition
d. Repeat for the other symmetry condition “Xsymm” 11. Double click on the “Loads” node in the model tree
©2008 Hormoz Zareh
6
Portland State University, Mechanical Engineering
a. Name the load “Pressure” and select “Pressure” as the type
b. Select the quarter of the arch surface with the boundary conditions applied to it c.
Select the color corresponding to the top surface
d. For the magnitude enter 600
©2008 Hormoz Zareh
7
Portland State University, Mechanical Engineering
12. In the model tree double click on “Mesh” for the Arch part, and in the toolbox area click on the “Assign Element Type” icon a. Select the portion of the geometry associated with the boundary conditions and load b. Select “Standard” for element type c.
Select “Linear” for geometric order
d. Select “Shell” for family e. Note that the name of the element (S4R) and its description are given below the element controls f.
Select “OK”
13. In the toolbox area click on the “Assign Mesh Controls” icon a. Select the portion of the geometry associated with the boundary conditions and load b. Change the element shape to “Quad”
©2008 Hormoz Zareh
8
Portland State University, Mechanical Engineering
14. In the toolbox area click on the “Seed Edge: By Number” icon
a. Select the shorter edges of the portion of the geometry associated with the boundary conditions and load i. Specify 5 seeds b. Select the longer curved edges of the portion of the geometry associated with the boundary conditions and load i. Specify 10 seeds
c.
Select “Done”
15. In the toolbox area click on the “Mesh Region” icon
a. Select the portion of the geometry associated with the boundary conditions and load b. Select “Done”
©2008 Hormoz Zareh
9
Portland State University, Mechanical Engineering
16. In the model tree double click on the “Job” node a. Name the job “Arch_geom_nonlinear” b. Give the job a description
©2008 Hormoz Zareh
10
Portland State University, Mechanical Engineering
17. In the model tree right click on the job just created and select “Submit” a. Ignore the message about unmeshed portions of the geometry b. While Abaqus is solving the problem right click on the job submitted, and select “Monitor”
c.
In the Monitor window check that there are no errors or warnings i. Abaqus exits with an error ii. Abaqus is unable to apply the full load iii. Observing the final time solved, Abaqus only solved for the first 97.5519% of the load iv. The results for the time steps Abaqus was successfully able to apply can still be viewed
©2008 Hormoz Zareh
11
Portland State University, Mechanical Engineering
18. In the model tree right click on the submitted job, and select “Results”
19. In the menu bar click on ViewportViewport Annotations Options a. Uncheck the “Show compass option” b. The locations of viewport items can be specified on the corresponding tab in the Viewport Annotations Options
20. Display the deformed contour of the (Von) Mises stress overlaid with the undeformed geometry a. In the toolbox area click on the following icons i. “Plot Contours on Deformed Shape” ii. “Allow Multiple Plot States” iii. “Plot Undeformed Shape”
©2008 Hormoz Zareh
12
Portland State University, Mechanical Engineering
21. In the toolbox area click on the “Common Plot Options” icon a. Note that when including the effects of geometric nonlinearities, the deformation scale factor defaults to a value of 1 b. Click “OK”
©2008 Hormoz Zareh
13
Portland State University, Mechanical Engineering
22. Click on the arrows on the context bar to change the time step being displayed a. Click on the three squares to bring up the frame selector slider bar
23. On the results tree, expand the History Output node and double click on the spatial displacement history created
Note the non-linear behavior of displacement vs. load. Horizontal axis (time) indicates the increment of load
©2008 Hormoz Zareh
14
Portland State University, Mechanical Engineering
