김경종
24 KiB
= \mathrm{Max} \left| \frac {\left(\sigma_ {v M i s e s}\right) ^ {2}}{\left(f \left(\rho_ {i}\right) \sigma_ {y}\right) ^ {2}} \cdot \sigma_ {y} \right|,
where \sigma _ { v M i s e s } is the element centroidal von Mises stress, \sigma _ { y } is the reference stress, and \rho _ { i } is a factor for interpolating the stresses of elements that have a reduced current relative density because of the topology optimization. The weighting factor and the interpolation are required for convergence during the optimization.
The von Mises stress is calculated at the centroid of the element to avoid stress singularities that might be present in the initial model or might appear in an optimized structure before it is smoothed. You cannot compare the scaled element centroidal von Mises stress with the von Mises stress calculated by Abaqus. The two measures are equal only when the element is solid and has a relative density of 1.0.
You can provide the reference stress when you create the objective function, or the Optimization module can calculate the reference stress during the initial optimization iteration. If you provide the reference stress, the value should not be too low or numerical singularities will result. The reference stress is given as
\sigma_ {\mathrm{y}} = \mathrm{Min} \left\{\alpha_ {1} \mathrm{Max} \left| \frac {\left(\sigma_ {v M i s e s}\right) ^ {2}}{\left(f \left(\rho_ {i}\right) \sigma_ {r e f _ {1}}\right)}. \sigma_ {r e f _ {1}} \right| + \alpha_ {2} \mathrm{Max} \left| \frac {\left(\sigma_ {v M i s e s}\right) ^ {2}}{\left(f \left(\rho_ {i}\right) \sigma_ {r e f _ {2}}\right) ^ {2}}. \sigma_ {r e f _ {2}} \right| \right\}.
You can define multiple load cases for the scaled element centroidal von Mises stress measure. Static linear analysis is supported. Static nonlinear analysis supports only contact nonlinearities. Nonlinear materials and geometrical nonlinearities, such as large deformations, are not supported.
Abaqus/CAE Usage: Optimization module: Task→general topology task, Design Response→Create: Single-term, Variable: Stress
Strain energy
The compliance of a structure is a measure of its overall flexibility or stiffness and is defined as the sum of the strain energy of all the elements, \textstyle \sum u ^ { t } k u for linear models, where is the displacement vector and is the global stiffness matrix. Compliance is the reciprocal of stiffness, and minimizing the compliance is equivalent to maximizing the global stiffness. If a load case is driven by forces or pressures, you should choose to minimize the strain energy to maximize the global stiffness. However, if a load case is driven by a thermal field, strain energy decreases when the optimization modifies the structure to make it softer. As a result, you should always choose to maximize the strain energy because attempting to minimize the strain energy can result in a stiff structure. In addition, you should always choose to maximize the strain energy if prescribed displacements are applied to your model.
Topology optimization considers the total strain energy for all of the elements; therefore, if you choose strain energy as an objective function, you must apply the objective to the entire model. You cannot use strain energy as a constraint in your optimization.
Abaqus/CAE Usage: Optimization module: Task→condition-based topology or general bead task, Design Response→Create: Single-term, Variable Strain energy
Volume
The volume is defined as the sum of the volume of the elements in the design area, \sum V _ { e } , where V _ { e } is the element volume. During a topology optimization, the elements are scaled with the current relative density defined in your Abaqus model. For most optimization problems, you must apply a volume constraint. For example, if you are trying to minimize the strain energy (maximize the stiffness) and do not apply a volume constraint, the Optimization module simply fills the entire design area with material.
Abaqus/CAE Usage: Optimization module: Task→condition-based topology task, Design Response→Create: Single-term, Variable: Volume
Weight
The weight is defined as the sum of the weight of all the elements in the design area, \sum W _ { e } , where W _ { e } is the element weight. The Optimization module scales elements using the current relative density. For most optimization problems, you must apply either a volume or a weight constraint. Using weight instead of volume allows you to constrain the optimized model to a specified physical weight and accounts for regions composed of materials with different densities. The Optimization module uses only supported element types when calculating the weight.
Abaqus/CAE Usage: Optimization module: Task→general topology or sizing task, Design Response→Create: Single-term, Variable: Weight
Design response operators
You must specify the operation that the Optimization module will use to arrive at a single scalar value for the design response, although some restrictions apply. For example, a volume design response can only use the sum of the volume within the design area. A design response that calculates the von Mises stress must use the maximum value of the stress within a region of the model. (None of the operators are relevant when the Optimization module calculates a dynamic frequency design response.) The following design response operators are provided by the Optimization module:
• Minimum or maximum: The minimum or maximum value within the selected region. The Optimization module allows only the maximum operator for stress, contact stress, and strain design responses.
• Sum: The sum of all the values within the selected area. The Optimization module allows only the sum operator for volume, weight, moment of inertia, and gravity design responses.
The available design responses for each type of optimization
The design responses you can create are dependent on the type of structural optimization you are performing—topology, shape, sizing, or bead. The type of optimization also controls whether you can use a design response as an objective, as a constraint, or as both.
Table 13.2.1–4 Design responses for condition-based topology optimization.
| Design response | Objective | Constraint |
| Strain energy | √ | |
| Volume | √ |
Table 13.2.1–5 Design responses for general topology optimization.
| Design response | Objective | Constraint |
| Center of gravity | √ | √ |
| Displacement and rotation | √ | √ |
| Eigenfrequency from Kreisselmaier-Steinhauser formula | √ | |
| Eigenfrequency from modal analysis | √ | √ |
| Energy stiffness measure | √ | √ |
| Internal and reaction forces and moments | √ | √ |
| Moment of inertia | √ | √ |
| Scaled centroidal von Mises stress | √ | √ |
| Strain energy | √ | |
| Volume | √ | |
| Weight | √ | √ |
Table 13.2.1–6 Design responses for shape optimization.
| Design response | Objective | Constraint |
| Contact stress | √ | |
| Damage | √ |
| Design response | Objective | Constraint |
| Eigenfrequency from Kreisselmaier-Steinhauser formula | √ | |
| Equivalent strain | √ | |
| Equivalent stress | √ | |
| Nodal strain energy density | √ | |
| Volume | √ | |
| Weight | √ |
Table 13.2.1–7 Design responses for sizing optimization.
| Design response | Objective | Constraint |
| Center of gravity | √ | √ |
| Displacement and rotation | √ | √ |
| Eigenfrequency from Kreisselmaier-Steinhauser formula | √ | |
| Eigenfrequency from modal analysis | √ | √ |
| Energy stiffness measure | √ | √ |
| Internal and reaction forces and moments | √ | √ |
| Moment of inertia | √ | √ |
| Strain energy | √ | |
| Volume | √ | |
| Weight | √ | √ |
Table 13.2.1–8 Design responses for general bead optimization.
| Design response | Objective | Constraint |
| Center of gravity | √ | √ |
| Displacement and rotation | √ | √ |
| Eigenfrequency from Kreisselmaier-Steinhauser formula | √ | |
| Eigenfrequency from modal analysis | √ | √ |
| Internal and reaction forces and moments | √ | √ |
| Moment of inertia | √ | √ |
| Strain energy | √ |
Table 13.2.1–9 Design responses for condition-based bead optimization.
| Design response | Objective | Constraint |
| Bead height | √ | |
| Eigenfrequency from Kreisselmaier-Steinhauser formula | √ | |
| Eigenfrequency from modal analysis | √ | |
| Strain energy | √ |
Operating on design responses
You can define a design response that is a combination of the single values generated by multiple design responses; for example, you can add values or find the maximum of several values. You can also define a design response that is the result of an operation on another design response; for example, the difference between the value of the design response at different nodes.
For example, you can create two design responses that correspond to the displacement in the 1- direction of two selected vertices. Alternatively, you can create a design response that is the difference between the displacement in the 1-direction of two selected vertices. You can then define a constraint that
forces the design response to be close to zero. In effect, the constraint forces the two selected vertices to move together in the 1-direction.
Abaqus/CAE Usage: Optimization module: Design Response→Create: Combined-term
Additional references
• Bakhtiary, N., P. Allinger, M. Friedrich, F. Mulfinger, J. Sauter, O. Müller, and J. Puchinger, “A New Approach for Size, Shape and Topology Optimization,” SAE International Congress and Exposition, Detroit, Michigan, USA, February 26–29, 1996.
• Bendsøe, M. P., E. Lund, N. Ohloff, and O. Sigmund, “Topology Optimization - Broadening the Areas of Application,” Control and Cybernetics, vol. 34, pp. 7–35, 2005.
• Bendsøe, M. P., and O. Sigmund, Topology Optimization: Theory, Methods and Applications, Springer-Verlag, Berlin Heidelberg New York, 2003.
• Bendsøe, M. P., and O. Sigmund, “Material Interpolations in Topology Optimization,” Archive of Applied Mechanics, vol. 69, pp. 635–654, 1999.
• Clausen, P. M., and C. B. W. Pedersen, Non-Parametric Large Scale Structural Optimization, ECCM 2006 III European Conference on Computational Mechanics, Lisbon, Portugal, June 5–9, 2006.
• Cook, R. D., D. S. Malkus, and M. E. Plesha, Concepts and Applications of Finite Element Analysis, John Wiley & Sons Inc., 1989.
• Emmrich, D., “Entwicklung einer FEM-basierten Methode zur Gesaltung von Sicken für biegebeanspruchte Leitstützstrukturen im Konstruktionsprozess,” Forschungsberichte des Instituts für Produktentwicklung, 13. Karlsruhe, 2004.
• Hansen, L. V., “Topology Optimization of Free Vibrations of Fiber Laser Packages,” Structural and Multidisciplinary Optimization, vol. 29(5), pp. 341–348, 2005.
• Olhoff, N., and J. Du, Topology Optimization of Vibrating Bi-Material Plate Structures with Respect to Sound Radiation, IUTUAM Symposium on Topological Design Optimization of Structures, Machines and Materials: Status and Perspectives, M. P. Bendsøe, N. Olhoff, and O. Sigmund, eds., pp. 147–156, Springer, 2006.
• Pedersen, C. B. W., and P. Allinger, Industrial Implementation and Applications of Topology Optimization and Future Needs, IUTUAM Symposium on Topological Design Optimization of Structures, Machines and Materials: Status and Perspectives, M. P. Bendsøe, N. Olhoff, and O. Sigmund, eds., pp. 147–156, Springer, 2006.
• Sigmund, O., and J. S. Jensen, “Systematic Design of Phononic Band Gap Materials and Structures by Topology Optimization,” Philosophical Transactions of the Royal Society: Mathematical, Physical and Engineering Sciences, vol. 361, pp. 1001–1019, 2003.
• Stolpe, M., and K. Svanberg, “An Alternative Interpolation Scheme for Minimum Compliance Optimization,” Structural and Multidisciplinary Optimization, vol. 22, pp. 116–124, 2001.
• Svanberg, K., “The Method of Moving Asymptotes—A New Method for Structural Optimization,” International Journal for Numerical Methods in Engineering, vol. 24, pp. 359–373, 1987.
13.2.2 OBJECTIVES AND CONSTRAINTS
Product: Abaqus/CAE
References
• “Structural optimization: overview,” Section 13.1.1
• “Creating objective functions,” Section 18.8 of the Abaqus/CAE User’s Guide
• “Creating constraints,” Section 18.9 of the Abaqus/CAE User’s Guide
• “Configuring geometric restrictions,” Section 18.10 of the Abaqus/CAE User’s Guide
• “Creating local stop conditions,” Section 18.11 of the Abaqus/CAE User’s Guide
Overview
For an optimization problem:
• an objective function defines the objective of the optimization;
• a constraint imposes limitations on the optimization and defines a feasible design;
• geometric restrictions impose limitations on the topology or shape of the structure that can be generated by the optimization; and
• stop conditions define when an optimization task is considered complete.
Objective functions
Objective functions define the objective of the optimization. An objective function is a single scalar value that is formulated from a set of design responses. For example, if the design responses are defined from the strain energy of the nodes in a region, the objective function could minimize the sum of the design responses; i.e., minimize the sum of the strain energy, in effect maximizing the stiffness of the region.
An optimization problem can be stated as:
\min \left(\Phi \left(U (x), x\right)\right),
where is the objective function that depends on the state variables, , and the design variables, .
The formula for the objective function that tries to minimize design responses can be stated as:
\Phi_ {\mathrm{min}} = \min \left(\sum_ {i = 1} ^ {N} W _ {i} \left(\varphi_ {i} - \varphi_ {i} ^ {r e f}\right)\right),
where each design response, \varphi _ { i } , is given a weight, W _ { i } , and a reference value, \varphi _ { i } ^ { r e f } . The formula for the objective function that tries to maximize design responses can be stated as:
\Phi_ {\mathrm{max}} = \max \left(\sum_ {i = 1} ^ {N} W _ {i} \left(\varphi_ {i} - \varphi_ {i} ^ {r e f}\right)\right).
The default weighting factor is 1.0. For a topology optimization the default reference value is 0.0; for shape and sizing optimization the default reference value is calculated by the Optimization module. For the most common optimization problems you do not need to change the default values of the weighting factor and the reference value. However, in some cases you may have to change the weighting factor to balance the effect of an objective function that is dominating the optimization. You should be aware that changing the weighting factor can have a significant impact on the final design. In addition, a design response that is dominant at the start of the optimization may have less effect as the Optimization module modifies your model.
An objective function that tries to minimize the maximum design response is an important optimization formulation. During each design cycle the Optimization module first determines which of the set of weighted design responses has the maximum value and then tries to minimize that design response. In many problems, minimizing the maximum design response provides a satisfactory solution because it reduces the maximum of a number of design responses. For example, if your design responses are defined from the stress in multiple regions of your model, minimizing the maximum design response attempts to minimize the stress in the region that is exhibiting the maximum stress. The formula can be stated as:
\Phi_ {m i n m a x} = \min \left(\max _ {i} \left\{W _ {i} \left(\varphi_ {i} - \varphi_ {i} ^ {r e f}\right) \right\}\right).
The design responses provided with the Optimization module are listed in “Design responses,” Section 13.2.1.
Defining the target of an objective function
The target of an objective function can be minimized or maximized. Alternatively, the target of an objective function can be set to minimize the maximum, such that the design response targets the maximum value, and the objective attempts to minimize that maximum value. In all cases, the weighting and reference values of the design responses are accounted for.
Abaqus/CAE Usage: Optimization module: Objective Function→Create: Target
Constraints
As outlined in the previous section, an optimization problem can be stated as:
\min \left(\Phi (U (x), x)\right),
where is the objective function that depends on the state variables, , and the design variables, . Constraints, , can be applied to the optimization problem, and constraints, K _ { i } , can be applied to the design variables:
\begin{array}{l} \Psi_ {i} (U (x), x) \leq 0, \\ K _ {i} (x) \leq 0, \\ \end{array}
where \Psi _ { i } \left( U \left( x \right) , x \right) \leq \Psi _ { i } ^ { * } and \Psi _ { i } is the design response that is constrained by the value \Psi _ { i } ^ { * } . In addition, K _ { i } \left( x \right) \leq K _ { i } ^ { * } , where K _ { i } is an expression for the layout of the design variables, such as manufacturability, and K _ { i } ^ { * } is the constraint on the design variables.
The Optimization module can arrive at a solution that optimizes the objective function; however, if the constraints are not satisfied, the result of the optimization may not be a feasible design. A constraint is based on a design response and, similar to a design response, is formulated from a single scalar value. Most optimizations have constraints that prevent the optimization from arriving at a trivial solution. For example, if you are trying to maximize the stiffness of a structure, the Optimization module will simply fill the entire design area if you do not apply any constraints. However, if you apply a weight constraint that limits the weight to 50% of its initial value, the Optimization module is forced to seek an optimum solution that both optimizes the stiffness objective and satisfies the weight constraint. You can apply only volume constraints to both topology optimization and to shape optimization; you cannot use volume as an objective function. You cannot apply multiple constraints of the same type, such as volume, to the whole model or to a single region.
Abaqus/CAE Usage: Optimization module: Constraint→Create
Applying constraints to regions
You can apply different constraints to different regions of your model. In addition, those regions can have different material properties or a material property can vary within a region. When the Optimization module calculates the design response, it considers varying material properties within the region. You cannot apply multiple volume constraints to the whole model or to a single region.
Geometric restrictions
Geometric restrictions are constraints that are applied directly to the design variables. Geometric restrictions allow you to model design limitations and manufacturing limitations.
Defining a frozen area
You can specify that a region within the optimization region is excluded from the optimization by freezing the region. For example, you could exclude a circular shaft that forms a bearing surface or a boss that is used to attach the structure to a rigid surface. You must freeze regions that are used to apply prescribed conditions. To simplify this operation, you can request that the Optimization module automatically freeze regions that are used to apply prescribed conditions and loads when you create an optimization process.
Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Frozen area
Specifying minimum and maximum member size
In most cases you should try to avoid the generation of thin trusses in the structure by defining a minimum member size. However, the Optimization module cannot ensure that the optimized structure will not contain regions with a diameter that is smaller than the minimum member size. The minimum member
size must be larger than the average element edge length. The maximum member size must be larger than twice the element length; otherwise, the optimization algorithm may experience issues with element connectivity. A coarse mesh and a fine mesh lead to an optimization with the topological equivalent result if you specify the same minimum member size for both cases. The Optimization module will not generate a thin region where prescribed conditions have been applied to the structure. Removing material from these regions may result in the structure collapsing.
If your structure will be cast, you may want to avoid the generation of overly thick parts by specifying a region with a maximum member size. The optimization process will avoid creating a thick region by generating several thinner regions. You do not need to specify both a maximum and a minimum member size. The Optimization module assumes the value that you enter for the maximum member size also applies to the minimum member size and will generate trusses of the specified size. The combination of a maximum member size constraint with a restraint that imposes a pull direction, such as a moldable or stampable manufacturing constraint, is allowed only for a general topology optimization. (The “pull direction” is the direction in which the two halves of a mold separate or the direction in which a stamping tool moves.)
Computational time increases significantly when you specify regions with a minimum or maximum member size. Therefore, you should apply the member size restrictions only to regions where thin or thick members must be avoided. You should run an optimization without member size restrictions to identify such regions.
Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Member size
Applying manufacturing restrictions
The topology optimization process always creates a structural layout that satisfies the objective function and the constraints; however, the design may be impossible to create using standard manufacturing techniques, such as casting and forging. You can apply geometric restrictions that force the topology optimization process to consider only designs that can be manufactured. For example, when you are using topology optimization you can force the Optimization module to create a castable shape that can be extracted from a mold or a stampable shape that can be created with a tool and die.
Maintaining a moldable structure
In cases where bending and torsion loads are applied, topology optimization is likely to generate a model with hollow areas or with undercuts that cannot be manufactured. You can prevent the topology optimization from generating cavities and undercuts by specifying the following:
• A forgeable structure that can be removed from the forging die, as shown in Figure 13.2.2–1.
• A moldable structure that can be removed from two halves of a mold, as shown in Figure 13.2.2–2. In contrast, Figure 13.2.2–3 illustrates parts with a cavity and an undercut that are not moldable.
Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Demold control; Demold technique, Demolding with a central plane