Product: Abaqus/CAE
For each design cycle the optimization process:
generates new material and element properties during topology optimization;
modifies nodal coordinates during shape optimization;
sends the modified model to an Abaqus analysis; and
reads the results of the analysis.
You 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.
You must ensure that your Abaqus model can be analyzed and produces the expected mechanical results before you attempt to optimize your model.
You should account for nonlinearities only if your model is truly nonlinear; the optimization will be significantly less expensive computationally if your Abaqus model is linear. You may want to ensure that an optimization of a linear version of your model produces reasonable results before you introduce geometric or material nonlinearities.
An optimization takes multiple design cycles to complete, and the time required to reach an optimized solution can be significant. As a result, you must configure your Abaqus model to minimize computational time; for example, by removing small details that are not important to the optimization.
The Abaqus/CAE Topology Optimization Module does not support the use of parts and assemblies in the Abaqus input file. When you run an optimization task, the Abaqus/CAE Topology Optimization Module generates a flattened input file that does not use parts and assemblies.
The Abaqus/CAE Topology Optimization Module reads data from the output database (.odb) file. The Abaqus/CAE Topology Optimization Module requests data only from the end of each step. To minimize the size of the output database file, you should also request data only from the end of each step.
The following Abaqus analysis types are supported by both topology and shape 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.
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.
General topology optimization supports prescribed acceleration loading from
gravity,
rotational body forces, and
centrifugal forces.
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 Abaqus/CAE Topology 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 Abaqus/CAE Topology 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 Abaqus/CAE Topology 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 Abaqus/CAE Topology 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.
The material models supported by structural optimization in the elements in the design area depend on the type of optimization—stiffness-based topology optimization, general topology optimization, or shape optimization.
Stiffness topology optimization in Abaqus supports linear elastic, plastic, and hyperelastic material models.
The following linear elastic material models are supported by stiffness topology optimization:
Linear elastic materials with isotropic behavior.
Linear elastic materials with fully anisotropic behavior.
Linear elastic materials with orthotropic behavior. All of the behavior models are supported, except for orthotropic shear behavior for warping elements and coupled and uncoupled traction behavior for cohesive elements.
Metal plasticity material properties—the plastic part of the material model for elastic-plastic materials that use the Mises or Hill yield surface— are supported by stiffness 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.
General topology optimization in Abaqus supports linear elastic, plastic, and hyperelastic material models.
The following linear elastic material models are supported by general topology optimization:
Linear elastic materials with isotropic behavior.
Linear elastic materials with fully anisotropic behavior.
Linear elastic materials with orthotropic behavior. All of the behavior models are supported, except for orthotropic shear behavior for warping elements and coupled and uncoupled traction behavior for cohesive elements.
Metal plasticity material properties—the plastic part of the material model for elastic-plastic 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.
In most cases, you will use the same coordinate system to define your model and the optimization task. However, the Abaqus/CAE Topology Optimization Module allows you refer to a different coordinate system when you are defining a design response.
The Abaqus elements that are supported as design elements by topology and shape optimization are listed in Table 13.2.3–1 through Table 13.2.3–4. The tables also list the Abaqus elements that support the reaction and internal force design responses. 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.
Topology optimization (both stiffness and general) and shape optimization support the two-dimensional solid elements listed in Table 13.2.3–1.
Table 13.2.3–1 Supported two-dimensional solid elements.
| CPE31, CPE3H, CPE41, CPE4H, CPE4I, CPE4IH, CPE4R1, CPE4RH, |
| CPE6H, CPE6M, CPE6MH |
| CPE81, CPE8H, CPE8R1, CPE8RH |
| CPS31, CPS41, CPS4I, CPS4R1, CPS61, CPS6M, CPS6MT, CPS81. CPS8R1 |
| CPEG3, CPEG3H, CPEG4, CPEG4H, CPEG4I, CPEG4IH, CPEG4R, CPEG4RH, CPEG6, CPEG6H, CPEG6M, CPEG6MH, CPEG8, CPEG8H, CPEG8R, CPEG8RH |
| CPE3T, CPE4T, CPE4HT, CPE4RT, CPE4RHT, CPE6MT, CPE6MHT, CPE8T, CPE8HT, CPE8RT, CPE8RHT |
| CPS3T, CPS4T, CPS4RT, CPS8T, CPS8RT |
| CPEG3T, CPEG3HT, CPEG4T, CPEG4RT, CPEG4RHT, CPEG6MT, CPEG6MHT, CPEG8T, CPEG8HT, CPEG8RHT |
| 1 Can include reaction and internal force design responses. |
Topology optimization (both stiffness and general) and shape optimization support the three-dimensional solid elements listed in Table 13.2.3–2.
Table 13.2.3–2 Supported three-dimensional solid elements.
| C3D41, C3D4H, C3D81 |
| C3D61, C3D6H |
| C3D8H, C3D8I, C3D8IH, C3D8R1, C3D8RH |
| C3D101, C3D10H, C3D10M, C3D10MH |
| C3D151, C3D15H |
| C3D201, C3D20H, C3D20R1, C3D20RH |
| C3D4T, C3D6T, C3D8T, C3D8HT, C3DHRT, C3D8RHT, C3D10MT, C3D10MHT, C3D20T, C3D20HT, C3D20RT, C3D20RHT |
| 1 Can include reaction and internal force design responses. |
Topology optimization (both stiffness and general) and shape optimization support the axisymmetric solid elements listed in Table 13.2.3–3.
Table 13.2.3–3 Supported axisymmetric solid elements.
| CAX31, CAX3H, CAX41, CAX4H, CAX4I, CAX4IH, CAX4R1, CAX4RH |
| CAX81, CAX8H, CAX8R1, CAX8RH |
| CGAX3, CGAX3H, CGAX4, CGAX4H, CGAX4R, CGAX4RH, CGAX8, CGAX8H, CGAX8R, CGAX8RH |
| CAX3T, CAX4T, CAX4HT, CAX4RT, CAX4RHT, CAX8T, CAX8HT, CAX8RT, CAX8RHT |
| CGAX3T, CGAX3HT, CGAX4T, CGAX4HT, CGAX4RT, CGAX4RHT, CGAX8T, CGAX8HT, CGAX8RT, CGAX8RHT |
| 1 Can include reaction and internal force design responses. |
Table 13.2.3–4 lists the general membrane, three-dimensional conventional shell, and beam elements that are supported by optimization.
Table 13.2.3–4 Additional supported elements
| General membrane elements (topology and shape optimization) | M3D31, M3D41, M3D4R1, M3D61, M3D81, M3D8R1 |
| Three-dimensional conventional shell elements (topology optimization only) | STRI3, S3, S3R, STRI65, S4, S4R, S4R5, S8R, S8R5, S8RT |
| Three-dimensional conventional shell elements (shape optimization only) | STRI31, S31, S3R1, S41, S4R1, S8R1 |
| Beam elements (shape optimization only) | B212, B21H2, B312, B31H2 |
| 1 Can include reaction and internal force design responses. | |
| 2 You can include beam elements in shape optimization only to define a neighboring component that is used to restrict the movement of nodes in the optimized region. | |