Configuring advanced options

In the optimization task editor, click the Advanced tab.
Select the General optimization algorithm.
Choose whether to Delete soft elements in region.
During the topology optimization process, the Optimization module distributes a given mass within the design area while it tries to satisfy the constraints and optimize the objective. At the end of the optimization, the structure contains hard (filled) and soft (void) elements. The soft elements have a negligible influence on the stiffness of the structure; but they are still relevant for the number of degrees of freedom of the structure and, hence, influence the speed of the optimization process. The Delete soft elements option allows you to select a region from which soft elements that have only soft neighboring elements will be removed. The deleted elements are reactivated if needed; for example, if the force flow changes during the optimization.

Choosing to delete soft elements can help Abaqus converge on a solution because those elements would otherwise degenerate or collapse and is recommended when you are optimizing a nonlinear model. In addition, selecting a Conservative density update strategy and a small change in density per design cycle will improve the accuracy of the results. See Configuring the density settings, for more information.
If you chose to delete soft elements, you can prevent isolated soft elements from being removed by choosing to delete only soft elements that have neighboring soft elements. You can define a neighboring element as being within the radius specified by the Average edge length (default) or specified by a value that you enter. If the element edge length varies considerably within the mesh, the radius calculated from the average edge length can be misleading.
If you chose to delete soft elements, you can select the method that the Optimization module will use to delete elements:

Favor continuity (Standard)

Choose Favor continuity (Standard) and enter a Relative material density threshold to check for continuity before deleting soft elements. If the optimized model contains an island of hard elements that are separated from the rest of the model by soft elements, the Optimization module does not remove the soft elements. In addition, the Optimization module retains soft elements that are preventing hard elements from moving with respect to each other; for example, hard elements that share a common edge but not a common face. An element is considered soft if its relative material density is less than the threshold value, and the Optimization module removes it from the analysis.

Favor continuity (Aggressive)

Choose Favor continuity (Aggressive) and enter a Relative material density threshold to remove soft elements regardless of continuity. An element is considered soft if its relative material density is less than the threshold value, and the Optimization module removes it from the analysis.

Maximum shear strain

Choose Maximum shear strain and enter a Maximum shear strain threshold. The Optimization module removes elements from the analysis that have a shear strain larger than the threshold.

Minimum principal strain

Choose Minimum principal strain and enter a Minimum principal strain threshold. The Optimization module removes elements that have a principal strain lower than the threshold.

Maximum elastoplastic strain

Choose Maximum elastoplastic strain and enter a Maximum elastoplastic strain threshold. The Optimization module removes elements that have an elastoplastic strain larger than the threshold.

Volume compression

Choose Volume compression and enter a Relative volume compression. The Optimization module removes elements that are compressing and have a relative volume that is lower than the threshold. The relative volume $V_{r e l}$ is defined as $\frac{V_{d e f o r m} - V_{o r g}}{V_{o r g}}$ , where $V_{d e f o r m}$ is the deformed element volume and $V_{o r g}$ is the original element volume.

You should choose Volume compression if your model uses shell or membrane elements or if your model is experiencing large deformations.

Note:
The soft delete method that you select is dependent on the material behavior and the element type, and you might have to experiment to determine the best method and its threshold value. The file, TOSCA.OUT, contains information about the elements that are being removed and will help you determine the best soft delete method and threshold value. The Favor continuity methods provide a default Relative material density threshold of 0.05. In contrast, the strain and volume methods do not provide a default threshold because the appropriate value depends on your model; for example, on the properties of the materials.
Choose the Material interpolation technique and the Penalty factor.
Optimization generates hard elements with a density close to one or void elements with a density close to zero. Topology optimization introduces elements with a density between one and zero, and the material interpolation technique calculates the relationship between density and stiffness for these intermediate elements. The SIMP (solid isotropic material with penalization) interpolation scheme defines an exponential relationship between the density and the stiffness of an element and is suitable for static problems. The penalty factor should be greater than 1, and numerical experiments indicate that the default value of 3 produces good results. The RAMP (rational approximation of material properties) interpolation scheme is suitable for dynamic problems. The penalty factor should be greater than 0, and numerical experiments indicate that the default value of 3 produces good results. The MIMP material interpolation is a combination of the SIMP for the constitutive material interpolation and a new material interpolation for the physical density.

By default, the Optimization module selects the SIMP interpolation scheme for static problems and the interpolation scheme is switched to PEDE automatically by TOSCA if at least one dynamic load case appears in your model.
You can choose Use Abaqus sensitivities when possible to use Abaqus to compute the design responses and their sensitivities whenever possible. This workflow modification improves the optimization process performance.
Select Use Group Operator when possible to use large groups of more than 5000 elements or nodes in the design response definition in an efficient way. This workflow modification uses a new algorithm based on Abaqus sensitivities.