You can use the field and history output generated by Abaqus to view the results generated by your optimization process. You can also use the output to diagnose any problems with the optimization; for example, to determine if the optimization is converging on an objective or to study the rate of convergence. You view the results by clicking Results in the Optimization Process Manager.
When you submit an optimization process for analysis, Abaqus creates an output database that contains data from each design cycle of the optimization. The output database is stored in the jobname\ATOM_POST directory. The behavior of the Visualization module depends on whether the output database was created from a topology optimization or a shape optimization.
Topology optimization
When you view the results of a topology optimization, Abaqus/CAE automatically displays a view cut superimposed on the current view that represents the optimized design surface. The isosurface variable of the view cut is the normalized material property that the Abaqus Topology Optimization Module uses to “add” or “remove” elements from the analysis. By default, Abaqus/CAE displays the view cut with the normalized material property set to 0.3. You can use the view cut manager to modify the value of the isosurface variable and to view the resulting boundary of the isosurface. Boundary conditions are not displayed while an optimization view cut is active. For more information, see “Managing view cuts,” Section 80.2.
Shape optimization
When you view the results of a shape optimization, Abaqus/CAE displays the model in its optimized shape using the new position of the surface nodes.
Each design cycle in the optimization process is saved as a frame in the output database, and you can open the Step/Frame dialog box to display the results from each design cycle. You can view the results of an optimization process while it is still in progress. As the optimization process moves toward completion, the lists of completed steps and frames are updated every time you close and reopen the Step/Frame dialog box. For more information, see “Selecting a specific results step and frame,” Section 42.3.1, and “Stepping through frames,” Section 42.3.2.
You can perform a time history animation of a deformed or contour plot and view the progress of the optimization as Abaqus attempts to satisfy the objective functions while respecting the constraints. For a topology optimization you can view the progressive removal of elements from the analysis and the resulting effect on the mechanical behavior of the model, such as the change in deformation or stress. Turning on translucency allows you to see the progression of the optimization through interior elements; for example, the removal of interior elements to create voids. For more information, see “Changing the translucency,” Section 77.3. For a shape optimization you can view the incremental change in the position of the surface nodes as the optimization progresses; and, similar to a topology optimization, you can view the resulting effect on the mechanical behavior of the model.
In addition, the optimization process writes history data in the ATOM_OPTIMIZATION that you can use to track the design variables. As a result, you can create an X–Y plot showing how the objective functions and constraints change after each design cycle. The resulting plot indicates how the Abaqus Topology Optimization Module tries to meet the specified objective functions while satisfying the constraints. You can use an X–Y plot of the objective functions and constraints as a diagnostic tool to view the progression of the optimization after each design cycle and to determine if the optimization is converging on a solution, as shown in Figure 18–2.
The Abaqus Topology Optimization Module also saves output databases in the jobname\SAVE.odb directory. These output databases contain the data generated by the Abaqus analyses during each design cycle; however, they do not contain data related to the optimization, such as the value of the normalized material property.
If you performed an eigenfrequency optimization, the output database stored in the jobname\ATOM_POST directory contains only results corresponding to the first eigenfrequency. However, the jobname\SAVE.odb output database contains results from the last optimization step for all eigenfrequencies.
