2.6. Define Design Objectives

An Objective object is added by default for optimization systems. This object displays the Worksheet in order for you to specify the optimization goal.

Go to a section topic:

Application

To apply an Objective object: On the Environment Context tab: select Objective, or right-click the Environment tree object or in the Geometry window and select Insert > Objective.

Objective Worksheet Overview

When you select the Objective object, the Worksheet displays by default, as illustrated in the images shown below. You use the Worksheet to specify Response Type, Formulation, Goal, and Weights for the steps/modes of the upstream analysis. A Structural Optimization analysis supports one or more upstream Harmonic Response, Modal, Static Structural, or Steady-State Thermal analyses. For the Shape Optimization method, nonlinear Static Structural analyses are also supported.

Whenever you link a Harmonic Response, Modal, Static Structural, or Steady-State Thermal analysis to a Structural Optimization analysis in the Project Schematic, a new row is added to the Worksheet. The default Response Type setting for a Static Structural analysis is Compliance, for a Modal analysis it is Frequency, and for a Steady-State Thermal analysis it is Thermal Compliance. There is not default setting for a Harmonic Response analysis.

Single Static Structural System

Single Modal System

Single Thermal System

You can insert additional rows into the Worksheet to specify multiple response types for multiple systems and Weight values for a single step or multiple steps (by disabling or enabling the Multiple Sets option).

Note:

For the Topology Optimization - Density Based method, Objective objects of different types are always normalized. Here, the option only applies for Objective objects of same type.

For the Topology Optimization - Level Set method, when you have multiple Objective objects specified, you can choose to normalize them with their initial response to give equal weightage for all objectives. To do so, set the Normalized Sum property to Yes.

Multiple Systems

Worksheet Properties

You set the values for properties in the Worksheet columns to define the Objective object as follows:

Enabled

This option is checked by default. When checked the application includes the specifications of the row in the solution. Unchecking the row excludes it from the solution.

Response Type

The options for this column depend upon the analysis you are optimizing. Supported options include:

Mass/Volume
Stress
Compliance
Criterion
Accumulated Plastic Strain
Frequency
Thermal Compliance

Review the Objective and Response Constraint Capability Map for a complete listing of the supported analysis types, response constraint you want to specify, and the optimization method you are using.

Limitation: When you select a criterion that is scoped to Remote Point or remote boundary condition (Remote Force or Remote Displacement), the Base Result property options Reaction Force and Reaction Moment are not supported for the Density Based and Lattice Optimization methods.

Goal

The options for this property depend upon the selection made in the Response Type column.

If constraint is...	Then this entry can be set to...
Mass/Volume Stress Accumulated Plastic Strain	Minimize.
Frequency	Maximize.
Criterion Compliance	Minimize or Maximize.
Thermal Compliance	Minimize or Maximize.

Note: Generally, you set static and thermal compliance constraints to Minimize, however, the application also supports the Maximize setting.

Formulation

This column is applicable only when the Response Type is set to Compliance (Static Structural analysis), Stress (Static Structural analysis), or Thermal Compliance (Steady-State Thermal Analysis).

Compliance

For the Density Based optimization method, when you select Compliance (Static Structural analysis), this column is used to specify the formulation method by which maximum stiffness can be attained to minimize the compliance.

Program Controlled: This default setting selects either the Force or Displacement formulation based on whether a force load or a displacement load exists in the Static Structural analysis.
Force: If you have not applied a displacement load and a force load is applied, then the displacement, with respect to this force load, is minimized during the optimization.
Displacement: If you have a non-zero displacement load and no force load is applied, then the force that leads to the given displacement is maximized during the optimization.
Note: For the Topology Optimization - Level Set Based and Shape Optimization methods, the Compliance option uses a unique formula regardless of the context. That is, it executes in the presence of surface loads, acceleration, prescribed displacement, and/or thermal expansion.

Stress

When Stress is the specified Response Type, Formulation options include:

Equivalent von-Mises Stress (default). This option is supported for density based, level set, and shape optimization methods.
Local Equivalent von-Mises Stress. This option is only supported for shape optimization methods.
Maximum Principal Stress. This option is supported for density based, level set, and shape optimization methods.
Local Strain Energy. This option is supported for level set and shape optimization methods.
The strain energy computed only over the optimization region of interest.
Important: The Local Strain Energy calculation is exactly twice the Compliance if, and only if:
1. Local Strain Energy is computed over the entire model, and,
2. There are only loads in the upstream structural analysis.
As a result, Ansys recommends that you keep this in mind when specifying this stress option. For example, if you apply a prescribed-displacement and minimize the Local Strain Energy, you could experience an unwanted (but expected) disconnection.
While the Local Strain Energy is by nature, a scalar value, the Equivalent von-Mises Stress and Maximum Principal Stress options are elemental scalar-fields. Before being consumed by the optimizer, those two stress-norm are scalarized in a way to mimic the maximum and to stay derivable.

As summarized below, the application monitors all elements of the optimization region, however, based on the method and criterion, some elements may be ignored. This table describes the supported methods only.

Criterion	Methods^[a]
Criterion	Density Based	Level Set Based	Shape Optimization
Equivalent von-Mises Stress	Scoping elements: All elements except those lying in the Exclusion Region.	Scoping elements: All elements except those lying in the Exclusion Region.	Scoping elements: All.
Local Equivalent von-Mises Stress	Not Available	Not Available	Scoping elements: All elements except those lying in the Exclusion Region.
Maximum Principal Stress	Scoping elements: All elements except those lying in the Exclusion Region.	Scoping elements: All elements except those lying in the Exclusion Region.	Scoping elements: All.
Local Strain Energy	Not Available	Not Available	Scoping elements: All.

^[a]For the mixable density and topography methods, no elements are monitored.

Thermal Compliance

For Thermal Compliance, this column is used to specify the formulation method by which heat transfer is maximized. Options include Program Controlled (default), Thermal Load, and Temperature. The Thermal Load option includes all thermal loads (Convection, Heat Flux, etc.) exceptTemperature. For this Worksheet property, note the following behaviors:

Program Controlled: This default setting selects either the Temperature or Thermal Load formulation based on whether a temperature load or a thermal load exists in the Steady-State Thermal analysis.
Thermal Load: If you have not applied a Temperature load and a Thermal Load is applied, then the average temperature, with respect to this thermal load, is minimized during the optimization.
Temperature: If you have Temperature load and no Thermal Load is applied, then the thermal load that leads to the given temperature is maximized during the optimization.
Note: For the Topology Optimization - Level Set Based and Shape Optimization methods, the Thermal Compliance option uses a unique formula regardless of the context. That is, it executes in the presence of Heat Flux, Heat Flow, prescribed Displacement, Convection conditions, and/or Internal Heat Generation.

Environment Name

From the drop-down list, select the environment associated with the entries of the Response Type and Goal properties. Note that geometric criteria (mass, volume, etc) does not need to be associated to an environment.

Criterion

From the drop-down list, select the desired criterion.

Weight

The default value for this option is 1. The Weight can be any real number.

If you define multiple responses, they are aggregated into a weighted sum, using:

Where:

is the design of the k^th iteration.

is the i^th Objective response.

is the effective weight of the i^th Object response.

is the aggregated Objective.

When the Normalized Sum option is set to No, then , where is the entered weight.

When the Normalized Sum option is set to Yes, then . This indicates that it is scaled using the value at the first iteration.

Multiple Sets

The values for this option are Enabled (default) or Disabled.

If Enabled, you can specify Start Step and End Step values within the boundaries of the maximum number of steps defined in the upstream Static Structural analysis.
If Disabled, only the Step column is available to define the Weight for a single step.

Start Step

This option is available when the Environment Name column is set to either Static Structural or Steady-State Thermal. This option requires the Multiple Sets option to be set to Enabled in order to define the Start Step from the upstream solution.

End Step

Step

This option is supported when the Environment Name column is set to either Static Structural or Steady-State Thermal. This option specifies the step number used from the upstream solution. This field is read-only when the Multiple Sets option is set to Enabled, and the entry for this option can also be Multiple or All, if the Start and End Step values cover more than one step or the entire analysis from the upstream solution. Otherwise, you can specify the weight for single steps using this option.

Start Mode

Only supported when Modal system is selected in the Environment Name column. This field requires the Multiple Sets option to be set to Enabled in order to define the Start Mode for the selected Modal analysis solution.

End Mode

Mode

Only supported when Modal system is selected in the Environment Name column. This option specifies the mode number used from the upstream solution. This field is read-only when the Multiple Sets option is set to Enabled and the entry for this option can also be Multiple or All, if the Start Mode and End Mode values cover more than one mode or all of the modes from the upstream solution. Otherwise, you can specify the weight for single modes using this option.

Refer to the Objective object reference page for additional information.