Creating Abaqus Optimization Models

The following Abaqus analysis types are supported by topology, shape, sizing, and bead optimization:

• Static stress/displacement, general analysis

• Static stress/displacement, linear perturbation analysis

• Extract natural frequencies and modal vectors

You can specify that geometric nonlinearity should be accounted for only during static stress/displacement analyses.

Elements that have limited stiffness, such as elements with hyperelastic material properties, can deform excessively during topology optimization in a nonlinear analysis. This deformation can lead to an adverse effect on the convergence and result in the termination of the analysis. You should be aware of this potential issue when applying topology optimization using hyperelastic materials.

Sizing optimization supports geometric nonlinearity only if the maximum elemental effective total strain for the design elements is less than 2%. Sizing optimization supports geometric nonlinearity outside the design area where any magnitude of total strain for an element is allowed.

Bead optimization does not support geometric nonlinearity.

If your model is undergoing a sequence of loads, you can significantly reduce the computational cost by defining a multiple load case analysis within a single step.

A design response can include steps or load cases from multiple Abaqus models. You can incorporate multiple models into your optimization when linear perturbations about a base state are no longer sufficient as load cases. For example, you can simulate nonlinear load cases (which are not supported by Abaqus/CAE) by creating multiple copies of your nonlinear model and by creating a step in each model during which different loads and boundary conditions are applied. For a meaningful optimization, it is expected that each model will have the sameAbaqus/CAE geometry and the same mesh.

General topology and sizing optimization support constant temperature loading.

General topology optimization supports prescribed acceleration loading from

• gravity,

• rotational body forces, and

• centrifugal forces.

Coriolis forces are not supported.

You can avoid contact in optimized regions of your model by defining geometric restrictions, such as casting or minimum member size restrictions. In some cases, you cannot specify the exact boundary conditions early in the design phase. In addition, nonlinear boundary conditions, such as contact definitions, can change if the Optimization module changes the topology of the model.

The optimization process is more efficient if you create an Abaqus model with the appropriate contact definitions and allow Abaqus to calculate the contact. The contact conditions are included in the optimization through the forces at the nodes and the stresses in the elements, and both topology and shape optimization permit contact conditions in the Abaqus model.

You can define a contact surface directly on the edge of the design space in topology optimization. However, if the design edge belongs to a contact surface in shape optimization, you must invert the shape optimization algorithm by entering a negative growth scale factor. You may encounter convergence difficulties in your Abaqus model if you have a complex contact problem or if the optimization results in large changes in the model.

Topology optimization determines the optimal material distribution in the design space, given the prescribed conditions applied to the model along with the objective function and constraints. Your optimization must apply appropriate constraints and restrictions; otherwise, the Optimization module can extensively alter the topology of the component. The resolution of the structure that has been optimized with topology optimization is very dependent on the discretization. A fine mesh produces a structure with a higher resolution than a coarse mesh; however, it will also substantially increase the processing time required. You must determine the appropriate compromise between structural resolution and processing time.

During topology optimization the Optimization module modifies the material definition of the elements in the design area. As a result, you must provide the initial density of the materials in the design area, even if it is not required by the Abaqus analysis.

Abaqus performs a shape optimization by modifying the boundaries or surfaces of a component. The optimization uses the stress condition to calculate new coordinates for nodes on the surface of the component and then adjusts the underlying mesh accordingly. The mesh quality must be sufficient to ensure that the analysis results are mostly unchanged by the movement of the surface nodes. High stress gradients must not be present within an element.

When the Optimization module is performing a shape optimization on a shell structure, it optimizes the form of the shell structure and not its thickness. The nodal position along shell edges can be modified; however, Abaqus does not modify the shell definition.

Abaqus performs a sizing optimization by modifying the thickness of shell elements in the design region. The element thickness must be uniform, and only single-layered shells are supported. Prescribed displacements are allowed in a static stress/displacement analysis; however, they are not supported in a frequency analysis.

Abaqus performs a bead optimization by moving nodes of shell elements in the direction of the shell normal in the design region. The element thickness must be uniform, and only single-layered shells are supported. Prescribed displacements are allowed in a static stress/displacement analysis; however, they are not supported in a frequency analysis.

Condition-based topology optimization in Abaqus supports linear elastic, plastic, and hyperelastic material models.

General topology optimization in Abaqus supports linear elastic, plastic, and hyperelastic material models.

All of the Abaqus material models are supported by shape optimization.

All of the Abaqus material models, including nonlinear materials, are supported inside and outside the design area. However, cyclic loading is not permitted.

Nonlinear materials in the design area are not supported by bead optimization. All of the Abaqus material models, including nonlinear materials, are supported outside the design area.

Topology optimization (both condition-based and general) and shape optimization support the two-dimensional solid elements listed in Table 1.

Topology optimization (both condition-based and general) and shape optimization support the three-dimensional solid elements listed in Table 2.

Topology optimization (both condition-based and general) and shape optimization support the axisymmetric solid elements listed in Table 3.

Table 4 lists the general membrane, three-dimensional conventional shell, and beam elements that are supported by optimization.

Sizing optimization supports only the three-dimensional conventional shell elements listed in Table 5.

Condition-based bead optimization supports all Abaqus plate and shell elements. However, general bead optimization supports only the three-dimensional conventional shell elements listed in Table 6.