text_image

Pull direction Back plane

Figure 13.2.2–1 A forgable part. 

text_image

Pull directions Center plane Pull direction (normal to every surface)

Figure 13.2.2–2 A moldable part. Optimization module: Geometric Restriction→Create: Demold control; Demold technique, Demolding at the region surface Optimization module: Geometric Restriction→Create: Demold control; Demold technique, Forging 

text_image

Pull directions - Center plane Pull directions - Center plane

Figure 13.2.2–3 Cavities and undercuts prevent a part from being moldable. # Maintaining a stampable structure You can specify that the structure is to be manufactured by a stamping process. If the optimization process removes one element from the structure, it also removes all elements positioned either behind or in front of the element (with respect to the pull direction), as shown in Figure 13.2.2–4. 

text_image

Elements removed during optimization Pull directions Center plane

Figure 13.2.2–4 A stampable structure. The rate at which the Optimization module modifies the element properties should not be set too high if the stamping restriction is activated in a condition-based topology optimization; otherwise, supports or trusses generated by the optimization may become unattached from the rest of the structure. Abaqus/CAE Usage: Use the following option to create a stamping geometric restriction in a topology optimization: Optimization module: Geometric Restriction→Create: Demold control; Demold technique, Stamping Use the following option to create a stamping geometric restriction in a shape optimization: Optimization module: Geometric Restriction→Create: Stamp control Use the following option to specify the rate at which the Optimization module modifies the element properties: Optimization module: Task→Create: Advanced , Size of increment for volume modification # Specifying bounds on shell thickness You can specify upper and lower bounds on the thickness of shell elements when you are configuring a sizing optimization. The value can be an absolute thickness or a fraction of the initial thickness. Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Thickness control # Specifying a symmetric structure Introducing symmetry constraints into your model can significantly increase the speed at which the Optimization module calculates the optimized structure. You can use the Optimization module to apply the following symmetry constraints: • Symmetry about an axis or plane (reflection symmetry) • Symmetry about a point • Rotational symmetry • Cyclic symmetry (replication of an area with a given distance) You can apply a symmetry restriction to unstructured meshes or to tetrahedron meshes in a topology optimization. The elements should be approximately the same size because the resulting symmetry is based on the resolution of the coarsest part of the mesh. In addition, the Optimization module may fail to create the symmetric conditions if the difference in the element size is too large. To define symmetry for a shape optimization, the Optimization module assembles nodes that are approximately symmetric into a symmetry group (normally there are two symmetric nodes in each symmetry group). The Optimization module then determines the master node of the symmetry group and calculates the design displacements of the client nodes in such a way that they move symmetrically to the plane of the master node. If you are performing a topology optimization, your meshed Abaqus model does not have to be symmetric before the optimization starts. Conversely, if you are performing a shape optimization, your meshed Abaqus model should be symmetric before the optimization starts to allow the Optimization module to identify symmetric nodes and maintain their symmetry when the surface nodes are moved. Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Planar symmetry, Point symmetry, Rotational symmetry, or Cyclic symmetry # Specifying the minimum width A sizing optimization determines the optimal element thickness when modeling a sheet metal structure with shell elements. Specifying the minimum width of a region containing elements of the same thickness prevents narrow slivers of elements with equal thickness appearing in the solution after a sizing optimization. Specifying a minimum width also prevents oscillations in the shell thickness or a “checkerboard” pattern of element thicknesses. A coarse mesh and a fine mesh lead to the same optimized solution if the same minimum width is specified in both cases; thus, the optimized solution is independent of the mesh resolution. However, in all cases the minimum width must be larger than the average length of the element edges. Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Thickness control # Specifying clustering You can specify that selected regions contain clusters of shell elements of equal thickness after a sizing optimization. You can use clustering to generate strengthening ribs or rings in the sheet metal structure you are optimizing or to define borders between regions of equal thickness. Clustered regions can be reproduced in manufacturing using sheets of constant thickness; for example, a vehicle “body in white” formed by welding and stamping individual sheet metal structures. To allow for maximum design flexibility, you should first optimize your structure without specifying clustering and use the initial design to decide which regions to cluster in your final optimization. Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Cluster areas # Applying additional restrictions during a shape optimization Shape optimization determines the displacement of each surface node in an effort to homogenize the stress on the surface and satisfy the objective function and any constraints. The Optimization module does not couple the displacement of neighboring nodes; each of the design nodes can move independently of the other design nodes. For example, during the optimization a planar surface can develop into a nonplanar free-form surface. By coupling the design nodes you can force the optimization to maintain the regularity of a plane. Coupling conditions restrict the range of solutions for the system and reduce the optimization potential. In addition, defining the appropriate coupling conditions can be very time consuming. To simplify your optimization, you should start with an optimization with as few restrictions as possible and only a few coupling conditions and introduce additional coupling conditions only if they are required. You can apply additional restrictions while the Optimization module is moving surface nodes during a shape optimization: • The optimized shape can be manufactured by a tool on a lathe cutting into the model along a specified direction. • The optimized shape can be manufactured by a tool drilling into the model along a specified direction. The hole created by the tool is symmetric about the axis of the tool. In addition, the tool can be withdrawn from the hole. • Selected faces in the optimized shape can slide along each other and/or cannot penetrate each other. • Nodes are restricted to move: – along a specified vector, – a specified distance either inward or outward (shrinkage or growth), – along a specified direction, – only along selected degrees of freedom, and – only in the direction of applied loads. Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Turn control, Drill control, Penetration check, Slide region control, or Vector # Combining geometric constraints Each geometric constraint that you apply reduces the possibility of Abaqus arriving at an optimized solution. In addition, if you apply too many geometric restrictions, the solution that Abaqus generates may not be the most optimal solution available. Therefore, you should start by allowing Abaqus to perform an optimization with no geometric restrictions applied or with only a limited number. After you have studied the results of the unrestricted, or less-restricted, optimization, you should apply only the restrictions that are required to solve the problem. You can combine geometric constraints; however, only certain combinations are permissible. Abaqus processes geometrical constraints in the following order: • Minimum member size • Symmetry constraints • Manufacturing constraints • Maximum member size Applying one constraint may weaken the effect of another constraint. For example, you cannot define symmetry about a plane in conjunction with a demold pull direction that is not parallel with the axis or plane of symmetry. The following manufacturing restriction combinations are permissible: • You can combine symmetry about a plane with a pull direction provided the pull direction is perpendicular or parallel to the plane of symmetry. • You can combine rotational symmetry with a pull direction provided the pull direction is parallel to the axis of rotation. • You can combine two symmetries about a plane provided the planes are perpendicular. • You can specify a minimum member size that is greater than the maximum member size. Abaqus first processes the minimum member size requirement and creates relatively thick supports. The thick supports are subsequently divided into smaller parallel members when Abaqus processes the maximum size requirement. # Stop conditions Stop conditions are examined after each design cycle and determine whether an optimization should end because the maximum number of design cycles has been reached or because the optimization has converged on an optimal solution. The Optimization module provides both global and local stop conditions; however, local stop conditions are supported only by shape optimization and are rarely required. # Global stop conditions The global convergence stop condition defines the maximum number of design cycles that should be performed. To limit the number of design cycles, you must define a global stop condition for each optimization task. The default value for the maximum number of design cycles depends on the type of optimization, as shown in Table 13.2.2–1. Table 13.2.2–1 Default maximum number of design cycles.

Optimization Type	Default maximum number of design cycles
Condition-based topology optimization	15
General topology optimization	50
Shape optimization	10
Sizing optimization	50
Condition-based bead optimization	3
General bead optimization	20

Abaqus/CAE Usage: Job module: Optimization→Create: Maximum cycles # Local stop conditions Local stop conditions indicate if a shape optimization has converged on an optimal solution. Local stop conditions apply to the displacements or stresses in a region of your model and define when the goals of an optimization have been reached. A local stop condition compares a single scalar value of displacement or equivalent stress to a reference value. The single scalar value can be either the maximum or minimum value over a region or the sum of all the values. The reference value can be taken from the value of the single scalar value after the previous iteration or after the first iteration. In addition, you can modify the reference value by a fixed amount or by a percentage. For example, you can specify a local stop condition that ends the optimization if the sum of the displacements within a region is smaller than 1% of the sum of the displacements after the first optimization cycle. You can define one or two local stop conditions, and you can specify if either or both (default) of the local stop conditions must be met for the Optimization module to end the optimization. Examples of local stop conditions include the following: • If you have specified that the displacement or stress should be minimized (or maximized), a local stop condition can end the optimization if the value of the displacement or stress increases (or decreases) after an optimization cycle. • When the optimization approaches the optimum solution, you can expect only small changes in the value of the displacement or stress. A local stop condition can end the optimization if the relative change in the displacement or stress falls below a tolerance limit after an optimization cycle. • When the optimization approaches the optimum solution, you can expect only small changes in the sum of the displacements and, therefore, only minor modifications to the model. A local stop condition can end the optimization if the change in the sum of the displacements falls below a tolerance limit after an optimization cycle. You can use the sum of the displacements as a stop condition for optimizations with and without constraints. In addition, this stop condition is suitable for a variety of objective functions, such as stress or frequency. Abaqus/CAE Usage: Optimization module: Stop Condition→Create # 13.2.3 CREATING Abaqus OPTIMIZATION MODELS # Product: Abaqus/CAE # References • “Structural optimization: overview,” Section 13.1.1 • “Understanding optimization,” Section 18.3 of the Abaqus/CAE User’s Guide # Overview 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. # Preparing the Abaqus model 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 Optimization module does not support the use of parts and assemblies in the Abaqus input file. When you run an optimization task, the Optimization module generates a flattened input file that does not use parts and assemblies. • The Optimization module reads data from the output database (.odb) files that are created during each design cycle. The Optimization module requests data only from the end of each step. To minimize the size of the output database files, you should also request data only from the end of each step. # Support for analysis types 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 # Support for geometric nonlinearities 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. # Support for multiple load cases 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. # Support for multiple models 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. # Support for temperature loading General topology and sizing optimization support constant temperature loading. # Support for acceleration loading General topology optimization supports prescribed acceleration loading from • gravity, • rotational body forces, and • centrifugal forces. Coriolis forces are not supported.