ProductsAbaqus/CAE Preparing the Abaqus modelYou should take care to ensure that your Abaqus model is supported by structural optimization. Any restrictions imposed by the use of structural optimization, such as the supported element types, apply only to the design area; regions outside the design area do not play a role in the optimization.
Support for analysis typesThe following Abaqus analysis types are supported by topology, shape, sizing, and bead optimization:
Support for geometric nonlinearitiesYou 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. Support for multiple load casesIf 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. Support for multiple modelsA 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. Support for temperature loadingGeneral topology and sizing optimization support constant temperature loading. Support for acceleration loadingGeneral topology optimization supports prescribed acceleration loading from
Coriolis forces are not supported. Support for contact during the optimizationYou 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. Restrictions on an Abaqus model used for topology optimizationTopology 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. Restrictions on an Abaqus model used for shape optimizationAbaqus 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. Restrictions on an Abaqus model used for sizing optimizationAbaqus performs a sizing optimization by modifying the thickness of shell elements in the design region. The element thickness must be uniform, and only singlelayered shells are supported. Prescribed displacements are allowed in a static stress/displacement analysis; however, they are not supported in a frequency analysis. Restrictions on an Abaqus model used for bead optimizationAbaqus 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 singlelayered shells are supported. Prescribed displacements are allowed in a static stress/displacement analysis; however, they are not supported in a frequency analysis. Supported materials in the design areaThe material models supported by structural optimization in the elements in the design area depend on the type of optimization—conditionbased topology optimization, general topology optimization, or shape optimization. Materials supported by conditionbased topology optimizationConditionbased topology optimization in Abaqus supports linear elastic, plastic, and hyperelastic material models. Support for linear elastic material modelsThe following linear elastic material models are supported by conditionbased topology optimization:
Support for plastic material modelsMetal plasticity material properties—the plastic part of the material model for elasticplastic materials that use the Mises or Hill yield surface—are supported by conditionbased topology optimization. Isotropic hardening is supported; however, cyclic loading is not supported—each material point can be unloaded only once and should not become elastoplastic again. Support for hyperelastic material modelsAll of the hyperelastic material models are supported by conditionbased topology optimization, except for the Marlow material model and the hyperelastic material models with test data. Support for temperature and field variable dependencyConditionbased topology optimization supports materials that have temperature and field variable dependency. Materials supported by general topology optimizationGeneral topology optimization in Abaqus supports linear elastic, plastic, and hyperelastic material models. Support for linear elastic material modelsThe following linear elastic material models are supported by general topology optimization:
Support for plastic material modelsMetal plasticity material properties—the plastic part of the material model for elasticplastic materials that use the Mises or Hill yield surface—are supported by general topology optimization. Isotropic hardening is supported; however, cyclic loading is not supported—each material point can be unloaded only once and should not become elastoplastic again. Support for hyperelastic material modelsAll of the hyperelastic material models are supported by general topology optimization, except for the Marlow material model and the hyperelastic material models with test data. Support for temperature and field variable dependencyMaterials that have temperature and field variable dependency are supported by general topology optimization. Material support in shape optimizationAll of the Abaqus material models are supported by shape optimization. Material support in sizing optimizationNonlinear materials in the design area are not supported by sizing optimization. All of the Abaqus material models, including nonlinear materials, are supported outside the design area. Material support in bead optimizationNonlinear 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. Support for coordinate systemsIn most cases, you will use the same coordinate system to define your model and the optimization task. However, the Optimization module allows you refer to a different coordinate system when you are defining a design response. Supported element typesThe Abaqus elements that are supported as design elements by topology and shape optimization are listed in Table 1 through Table 4. The tables also list the Abaqus elements that support the reaction and internal force design responses. The shell elements that are supported as design elements by sizing and bead optimization are listed in Table 5 and Table 6, respectively. Unsupported elements are ignored during optimization and remain unchanged. Structural optimization does not place any restrictions on the type of elements that you use outside the design area. Supported twodimensional solid elementsTopology optimization (both conditionbased and general) and shape optimization support the twodimensional solid elements listed in Table 1.
Supported threedimensional solid elementsTopology optimization (both conditionbased and general) and shape optimization support the threedimensional solid elements listed in Table 2.
Supported axisymmetric solid elementsTopology optimization (both conditionbased and general) and shape optimization support the axisymmetric solid elements listed in Table 3.
Additional supported elementsTable 4 lists the general membrane, threedimensional conventional shell, and beam elements that are supported by optimization.
Supported threedimensional conventional shell elementsSizing optimization supports only the threedimensional conventional shell elements listed in Table 5.
Conditionbased bead optimization supports all Abaqus plate and shell elements. However, general bead optimization supports only the threedimensional conventional shell elements listed in Table 6.
