Design Responses

The Optimization module provides a number of different design responses.

Bead Height

The bead height has the most significant effect on the stiffness of a shell structure that is being optimized with bead optimization. Usually, the greater the bead height the greater the stiffness, although manufacturing restrictions will limit how deep you can draw a bead. When the optimization starts, the bead height is initially zero. As the optimization proceeds, it moves the nodes in the shell normal direction until they reach the bead height. A bead height design response is available only as a constraint in a condition-based beam optimization.

Abaqus/CAE Usage

Optimization module: Taskcondition-based bead task, Design ResponseCreate: Single-term, Variable: Bead height

Center of Gravity

You can use the center of gravity of a selected region as a design response in an optimization. You can choose the center of gravity in the three principal directions:

\begin{matrix} x_{g} = \frac{\int ρ x d V}{\int ρ d V}, \\ y_{g} = \frac{\int ρ y d V}{\int ρ d V}, and \\ z_{g} = \frac{\int ρ z d V}{\int ρ d V} \end{matrix}

When the Optimization module calculates the center of gravity, the elements are scaled with the current relative density defined in your Abaqus model.

For example, you might want to constrain the center of gravity in the Y-direction so that it remains within a minimum and maximum range during the optimization. The design response can consider the center of gravity of the whole model or a region of the model.

If you select a local coordinate system, the Optimization module uses both the direction of the axes and the position of the origin to recalculate the center of gravity. The Optimization module applies the global coordinate system if you do not select a local coordinate system.

When the Optimization module calculates the center of gravity, it treats shell and membrane regions as three-dimensional regions by applying the thickness of the region. The Optimization module calculates the center of gravity using only the element types that are supported by topology optimization. As a result, the center of gravity calculated by the Optimization module might not be the same as the center of gravity calculated by Abaqus/Standard or Abaqus/Explicit; for example, if your model contains wire regions.

Abaqus/CAE Usage

Optimization module: Taskgeneral topology or sizing task, Design ResponseCreate: Single-term, Variable: Center of gravity

Damage

Typically, you use shape optimization to modify the surface geometry of a component to minimize stress concentrations. In most cases reducing the stress levels leads to a significant increase in durability. However, it is possible that the regions of peak stress identified by a static analysis differ from the regions of maximum damage identified from a durability (or damage) analysis, and using shape optimization alone to modify the surface geometry may decrease the durability. To avoid this situation, you can incorporate a durability solver in the optimization loop to ensure that you are both reducing stress levels and increasing durability.

You can create a design response that uses damage only in a shape optimization, and it can be used only as an objective function—minimization of the maximum damage in the critical areas. The Optimization module provides damage values as equivalent stress values. You can create a damage design response where the durability analysis runs only once in the optimization loop. Alternatively, you can create a damage design response when the durability analysis contains load case information and runs multiple times in the optimization loop.

Abaqus/CAE Usage

Optimization module: Taskshape task, Design ResponseCreate: Single-term, Variable: Damage (single)

Optimization module: Taskshape task, Design ResponseCreate: Single-term, Variable: Damage (multiple)

Displacement and Rotation

In most optimization problems you will use displacement and/or rotation to define your objective function or constraints. For example, the maximum displacement of a vertex could be either an objective or a constraint of an optimization. The performance of the optimization is improved if you apply displacements and rotations to only vertices or to small regions. In addition, performance is improved if you assign regions that are used to define displacements or reactions as frozen regions (the Optimization module will not remove elements from frozen regions during the optimization).

Table 1 lists the available displacement and rotation variables.

Table 1. Displacement and rotation variables for a general and sizing topology optimization.
	Displacement	Rotation
i-direction	$u_{i}$	$θ_{i}$
Absolute	$\sqrt{u_{i}^{2} + u_{j}^{2} + u_{k}^{2}}$	$\sqrt{θ_{i}^{2} + θ_{j}^{2} + θ_{k}^{2}}$
Absolute in i-direction	$\sqrt{u_{i}^{2}}$	$\sqrt{θ_{i}^{2}}$

Abaqus/CAE Usage

Optimization module: Taskgeneral topology, general bead, or sizing task, Design ResponseCreate: Single-term, Variable: Displacement

Energy Stiffness Measure

The energy stiffness is a measure that has no physical meaning but can be used as an objective function or a constraint in an optimization to optimize the stiffness of a structure that is subjected to both external loading and prescribed displacements.

To optimize the stiffness of a structure with only external loading, the strain energy should be minimized:

min (\frac{P \cdot u}{2}),

where $P$ is the external loading and $u$ is the resulting deflection of the loaded nodes. If only external loading is present, the energy stiffness measure is equal to the total strain energy, also called the compliance.

In contrast, if a load case is driven by prescribed displacements, the elastic energy, or compliance, will decrease only if the structure is made softer. To optimize a structure with only prescribed displacements, the strain energy should be maximized:

max (\frac{R \cdot u *}{2}),

where $u$ is the prescribed displacement at the nodes and $R$ is the resulting reaction force at the displaced nodes. If only prescribed displacements are present, the energy stiffness measure is equal to the negative of the total strain energy.

The strain energy with both external loads and prescribed displacements is given as

θ = \frac{P \cdot u}{2} + \frac{R \cdot u *}{2} .

The energy stiffness measure is used only for optimization (it has no physical meaning) and is given as

min (\frac{P \cdot u}{2} - \frac{R \cdot u *}{2}) .

You cannot use the energy stiffness measure as a design response in a model that is experiencing thermal loading or mass-dependent loading, such as gravity. An energy stiffness design response must be applied to the entire model. When energy stiffness is used as an objective function, you must select a target that tries to minimize the sum of the weighted differences between the design response and the reference value, regardless of whether an external load and/or prescribed displacements are being applied to the structure.

Abaqus/CAE Usage

Optimization module: Taskgeneral topology or sizing task, Design ResponseCreate: Single-term, Variable: Energy stiffness measure

Equivalent Strain

If your model is undergoing large deformations, a measure of the stress is not always a good indicator of the model's response. For example, a structure undergoing plastic deformation will, for an ideal plastic material, experience a large constant stress over the plastic area. In these circumstances a measure of the strain is a more reliable indicator of the model's response. You can choose from the following equivalent strains:

Equivalent plastic (PEEQ, calculated by Abaqus)
Elastic
Plastic (calculated by the Optimization module)
Total (the sum of the elastic and plastic)

Abaqus/CAE Usage

Optimization module: Taskshape task, Design ResponseCreate: Single-term, Variable: Strain

Equivalent Stresses

Equivalent stresses are the most commonly used objective function of a shape optimization. All of the stress values that are calculated by the Optimization module, whether nodal or from Gauss points or elements, are interpolated to the nodes. For example, you can try to optimize your model with an objective function that tries to minimize the maximum von Mises stresses in a region with stress concentrations or tries to minimize contact pressure in a region with contact. The Optimization module considers only the maximum value of an equivalent stress within a region. The Optimization module issues warnings for nodes that do not have the appropriate stress values. For example, if you select an objective response of contact stress, the Optimization module issues warnings about nodes of elements that are not in contact. If your Abaqus model contains multiple load cases, the design response is evaluated by summing the stress values from each load case.

You can choose from the following equivalent stresses:

von Mises
Maximum principal and absolute maximum principal
Minimum principal and absolute minimum principal
Second principal
Beltrami
Drucker Prager
Galilei
Kuhn
Mariotte
Mises
Sandel
Sauter
Tresca

You can choose from the following equivalent contact stresses:

Contact stress pressure
Total shear contact stress
Shear contact stress in the 1-direction
Shear contact stress in the 2-direction
Total contact stress

Abaqus/CAE Usage

Optimization module: Taskshape task or sizing task, Design ResponseCreate: Single-term, Variable: Stress or Contact stress

Internal Forces and Moments

You can use nodal internal forces and moments of the whole model or a region of the model as an objective function or a constraint in a general topology or sizing optimization.

Table 2 lists the available nodal internal force and moment variables.

Table 2. Nodal internal force and moment variables for a general and sizing topology optimization for the elements e attached to the nodes i.
	Nodal internal force	Nodal internal moment
i-direction	$\sum K_{e} u_{i}$	$\sum K_{e} u_{i}$
Absolute	$\| \sum K_{e} u_{i} \|$	$\| \sum K_{e} u_{i} \|$
Absolute in i-direction	$\sqrt{u_{i}^{2}}$	$\sqrt{u_{i}^{2}}$

You must use the global coordinate system with an absolute internal force or with absolute internal moment. Your structure must have stiffness in the direction of the force used in the optimization; otherwise, the internal force will be zero in this direction.

Abaqus/CAE Usage

Optimization module: Taskgeneral topology, general bead, or sizing task, Design ResponseCreate: Single-term, Variable: Internal force or Internal moment

Modal Eigenfrequency Analysis

Modal eigenvalues are the simplest dynamic responses in structural analysis. Typical uses of data from an eigenfrequency analysis during a topology optimization include the following:

maximize the lowest eigenfrequencies,
maximize a selected eigenfrequency,
constrain an eigenfrequency to be higher or lower than a given value,
maximize or minimize an eigenfrequency at a certain mode, and
perform a bandgap optimization that force modes away from a certain frequency.

The Optimization module supports two approaches for optimizing the eigenfrequencies:

single eigenfrequencies from modal analysis and
the Kreisselmeier-Steinhauser formulation.

The Kreisselmeier-Steinhauser formulation is the more efficient of the two approaches and should be used whenever possible. The only advantage of optimizing single eigenfrequencies is that you can use the sum of the eigenfrequencies as a constraint in a general topology or sizing optimization, which you cannot do with the Kreisselmeier-Steinhauser formulation.

When you are trying to maximize the lowest eigenfrequency, it is recommended that you consider not only the first eigenfrequency but also at least the next two highest natural frequencies. During the optimization, the various natural frequencies are weighted by their distance from the lowest natural frequency—the closer a natural frequency approaches the first natural frequency during the optimization, the more it is weighted. You should use the Kreisselmeier-Steinhauser eigenvalue formulation if you are trying to maximize the lowest eigenfrequency or, in particular, if you are trying to maximize more than one of the lowest eigenfrequencies. You do not need to use mode tracking if you are using the Kreisselmeier-Steinhauser formulation to maximize the lowest eigenfrequency, but you should use mode tracking for the higher modes because the modes might switch. For example, while the model is being optimized, the frequency of the first mode is maximized and the second eigenmode can become the mode with the lowest frequency.

Abaqus/CAE Usage

Optimization module: Taskgeneral topology, general bead, or sizing task, Design ResponseCreate: Single-term, Variable: Eigenfrequency from modal analysis or Eigenfrequency calculated with Kreisselmeier-Steinhauser formula

Moment of Inertia

You can use a moment of inertia design response in an optimization to minimize the rotational inertia about a selected axis. You can use the sum of the moment of inertia of the whole model or a region of the model as an objective function or a constraint in a general topology or sizing optimization.

You can choose the moment of inertia in the three principal directions or the three principal planes:

\begin{matrix} I_{x} = \int ρ (y^{2} + z^{2}) d V, \\ I_{y} = \int ρ (x^{2} + z^{2}) d V, \\ I_{z} = \int ρ (x^{2} + y^{2}) d V, \\ I_{x y} = I_{y x} = - \int ρ x y d V, \\ I_{x z} = I_{x z} = - \int ρ x z d V, \\ I_{y z} = I_{y z} = - \int ρ y z d V . \end{matrix}

If you select a local coordinate system, the Optimization module uses the direction of the axes to recalculate the center of gravity. The Optimization module applies the global coordinate system if you do not select a local coordinate system.

When the Optimization module calculates the moment of inertia, it treats shell and membrane regions as three-dimensional regions by applying the thickness of the region. The Optimization module calculates the moment of inertia using only the element types that are supported by topology optimization. As a result, the moment of inertia calculated by the Optimization module might not be the same as the moment of inertia calculated by Abaqus/Standard or Abaqus/Explicit; for example, if your model contains beam or truss elements (wire regions in Abaqus/CAE).

The moment of inertia with respect to any two orthogonal axes is zero if you have selected either of the axes to be an axis of symmetry.

Abaqus/CAE Usage

Optimization module: Taskgeneral topology, general bead, or sizing task, Design ResponseCreate: Single-term, Variable: Moment of inertia

Nodal Strain Energy Density

The nodal strain energy density, $u = σ_{i j} ε_{i j}$ , is a local point-wise strain energy that can provide a better representation of failure than stresses in nonlinear materials.

Abaqus/CAE Usage

Optimization module: Taskshape task, Design ResponseCreate: Single-term, Variable: Strain energy density

Reaction Forces and Moments

Nodal reaction forces and moments can be used as a design response only in general and sizing topology optimization. As with displacements, the performance of the optimization is improved if you apply reaction forces or moments to only vertices or to small regions and assign those regions as frozen regions (the Optimization module will not remove elements during the optimization).

Table 3 lists the available nodal reaction force and moment variables.

Table 3. Nodal reaction force and moment variables for a general and sizing topology optimization for the elements e attached to the nodes i.
	Nodal reaction force	Nodal reaction moment
i-direction	$\sum K_{e} u_{i}$	$\sum K_{e} u_{i}$
Absolute	$\| \sum K_{e} u_{i} \|$	$\| \sum K_{e} u_{i} \|$
Absolute in i-direction	$\sqrt{u_{i}^{2}}$	$\sqrt{u_{i}^{2}}$

You cannot use a reference coordinate system with an absolute reaction force or with an absolute reaction moment. Your structure must have stiffness in the direction of the force used in the optimization; otherwise, the reaction force will be zero in this direction.

Abaqus/CAE Usage

Optimization module: Taskgeneral topology, general bead, and sizing task, Design ResponseCreate: Single-term, Variable: Reaction force or Reaction moment

Scaled Centroidal Von Mises Stress

You can use the scaled element centroidal von Mises stress of the whole model or a region of the model as an objective function in an optimization. You must avoid regions with stress singularities caused by external loads or boundary conditions.

The scaled element centroidal von Mises stress is defined as

​ = Max | \frac{{(σ_{v M i s e s})}^{2}}{{(f (ρ_{i}) σ_{y})}^{2}} \cdot σ_{y} |,

where $σ_{v M i s e s}$ is the element centroidal von Mises stress, $σ_{y}$ is the reference stress, and $ρ_{i}$ 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

σ_{y} = Min {α_{1} Max | \frac{{(σ_{v M i s e s})}^{2}}{(f (ρ_{i}) σ_{r e f_{1}})} . σ_{r e f_{1}} | + α_{2} Max | \frac{{(σ_{v M i s e s})}^{2}}{{(f (ρ_{i}) σ_{r e f_{2}})}^{2}} . σ_{r e f_{2}} |} .

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: Taskgeneral topology task, Design ResponseCreate: 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, $\sum u^{t} k u$ for linear models, where $u$ is the displacement vector and $k$ 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: Taskcondition-based topology or general bead task, Design ResponseCreate: 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: Taskcondition-based topology task, Design ResponseCreate: 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: Taskgeneral topology or sizing task, Design ResponseCreate: Single-term, Variable: Weight

Design Responses