The Abaqus Topology Optimization Module provides a variety of settings that allow you to configure a topology optimization task. The configuration settings depend on whether you are configuring an optimization task for a general topology optimization or a condition-based topology optimization. The following topics are covered:
A general topology optimization is a flexible, sensitivity-based optimization that allows you to apply a range of constraints and objective functions to your model. You use the optimization task editor to customize various aspects of a general topology optimization. To locate the editor, select Task
Editoptimization task name from the main menu bar. To specify a general topology optimization, select the Advanced tab and choose General optimization (sensitivity-based).
The following topics are covered:
To configure basic settings:
In the optimization task editor, click the Basic tab.
Choose whether to freeze load and/or boundary condition regions.
It is recommended that you freeze regions to which prescribed conditions are applied because you do not want these regions to be removed during the optimization. Freezing these regions stabilizes the optimization and often leads to a significantly lower number of iterations.
To configure density settings:
In the optimization task editor, click the Density tab.
Select the Density update strategy.
This setting controls the rate at which the Abaqus Topology Optimization Module updates the relative material density of design elements during the optimization. In most cases you should accept the default setting (Normal). However, if the design responses are very sensitive and you have problems fulfilling the constraints, you may need a more conservative rate that requires more optimization iterations.
Enter the Initial density (0.0 < initial density ≤ 1.0). You should use this option only if volume is selected as an objective function and not as a constraint.
When the volume is selected as an objective function, each element has an initial relative density of 50%. However, you may need to set the initial density to a larger or smaller value to fulfill other constraints, such as displacement constraints.
Enter the Minimum density , the Maximum density, and the Maximum change per design cycle.
The minimum density must be greater than 0.0, and the maximum density must be less than or equal to 1.0. Changing the density bounds is not recommended, in particular the upper bound. You may need to increase the lower bound if the default value leads to a nearly singular stiffness matrix.
Numerical experiments indicate that a value of 0.25 (default) is acceptable for the maximum change in density. A lower limit in the change of density, such as 0.1, is recommended for complicated design responses and optimization formulations. However, a lower limit often leads to a higher number of optimization iterations.
To configure the perturbation settings:
In the optimization task editor, click the Perturbation tab.
Enter the number of eigenmodes to track. The default value is five, which means that the Abaqus Topology Optimization Module will try to track the five lowest eigenfrequencies.
In some cases many local modes having a low eigenfrequency appear during the optimization iterations, which leads to a high number of modes to track and degrades performance. You can avoid tracking a high number of modes by choosing the lower bound of the eigenfrequencies to be 25% of the eigenfrequency of interest in the first optimization iteration.
Mode tracking is not required if your design response will use the Kreisselmaier-Steinhauser formulation to evaluate the eigenfrequencies. Your Abaqus model must include an output request for at least the number of eigenfrequencies you are tracking.
Select the region over which the Abaqus Topology Optimization Module should track the eigenmodes.
To configure 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 Abaqus Topology 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.
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 Abaqus Topology Optimization Module will use to delete elements:
Choose Standard deletion 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 Abaqus Topology Optimization Module does not remove the soft elements. In addition, the Abaqus Topology 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.
Choose Aggressive deletion to delete soft elements regardless of continuity.
If desired, enter the value of the Relative material density threshold. An element is considered “soft” if its relative material density that is less than this value, and the Abaqus Topology Optimization Module removes it from the analysis.
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.
By default, the Abaqus Topology Optimization Module selects the SIMP interpolation scheme for static problems and the RAMP interpolation scheme if at least one dynamic load case appears in your model.
Specify the Convergence Criteria. The following options allow you to specify the convergence criteria for a general topology optimization:
Specifying when to start checking for convergence
You can specify the iteration during which the Abaqus Topology Optimization Module will begin to check the two convergence criteria. The optimization will always continue at least until this value has been reached. The default value is 4.
Specifying which convergence criterion to check
You can specify whether the optimization should end when either of the convergence criterion has been fulfilled or both of the criteria have been fulfilled. The default value is that both criteria must be fulfilled.
Convergence based on the change in optimization function
You can specify that the optimization will end based on the change in the objective function from one iteration to the next. The default value is 0.001.
Convergence based on the change in element densities
Element density is the design variable for a topology optimization. You can specify that the optimization will end based on the average change in the element density from one iteration to the next. The default value is 0.005.
A condition-based topology optimization uses a strain energy objective function and a volume constraint. You use the optimization task editor to customize various aspects of the condition-based topology optimization. To locate the editor, select TaskEditoptimization task name from the main menu bar. To specify a condition-based topology optimization, select the Advanced tab and choose Condition-based optimization.
The following topics are covered:
To configure basic settings:
In the optimization task editor, click the Basic tab.
Choose whether to freeze load and/or boundary condition regions.
It is recommended that you freeze regions to which prescribed conditions are applied because you do not want these regions to be removed during the optimization. Freezing these regions stabilizes the optimization and often leads to a significantly lower number of iterations.
To configure advanced options:
In the optimization task editor, click the Advanced tab.
Select the Condition-based optimization algorithm.
Choose whether to Delete soft elements in region.
During the topology optimization process, the Abaqus Topology 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.
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 choose the method that the Abaqus Topology Optimization Module will use to delete elements:
Choose Standard deletion 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 Abaqus Topology Optimization Module does not remove the soft elements. In addition, the Abaqus Topology 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.
Choose Aggressive deletion to delete soft elements regardless of continuity.
If desired, enter the value of the Relative material density threshold. An element is considered “soft” if its relative material density that is less than this value, and the Abaqus Topology Optimization Module removes it from the analysis.
Select the rate at which the Abaqus Topology Optimization Module will modify the element properties during a topology optimization. You can select the rate (Very small, Small, Moderate, Medium, or Large) and allow the Abaqus Topology Optimization Module to calculate the number of design cycles required to meet this rate.
Alternatively, you can select Dynamic and enter the maximum number of design cycles. The minimum number of design cycles is 10, and the default value is 15. A reduction in the number of design cycles can lead to undesired effects in the optimization. Although the resulting structures have the same stiffness (the sum of the strain energy is almost equal for the different results), changing the optimization speed can cause a different truss configuration in the solution.
Select the volume deleted after the first cycle. You can enter a percentage or an absolute value.
By default, the Abaqus Topology Optimization Module removes 5% of the optimization region volume in the first iteration. In some cases increasing this starting value will accelerate the optimization without influencing the solution, especially for models where relatively low stresses are present in large areas. Conversely, the Abaqus Topology Optimization Module may remove too many elements in the first iteration if the starting value is too high, leading to a failure in the optimization or a coarse structure.