2.7. Define Response Constraints

The Structural Optimization analysis requires and automatically inserts a response constraint. The available response types include:

Volume Constraint
Mass Constraint (default)
Center of Gravity Constraint
Moment of Inertia
Compliance Constraint (Static Structural)
Displacement Constraint (Static Structural)
Reaction Force Constraint (Static Structural)
Global Stress Constraint (Static Structural)
Local von-Mises Stress Constraint (Static Structural)
Natural Frequency Constraint (Modal)
Thermal Compliance (Steady-State Thermal)
Temperature Constraint (Steady-State Thermal)
Criterion Constraint (Harmonic Response, Modal, Static Structural)

Note: Shell Body Stress Constraints

When you apply a Global Stress Constraint or a Local von-Mises Stress Constraint to a shell body, the application optimizes the body using the elemental mean of the top and bottom surfaces.

Note: 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.

Application

To apply a Response Constraint:

On the Environment Context tab, open the Response Constraint drop-down menu and select the desired response constraint, or, right-click the Environment (Structural Optimization) object or in the Geometry window and select Insert>[desired Response Constraint menu option].
The application inserts the appropriate object matching the selected response option.
Additional properties display based on the setting of the Response property setting, and include:
Geometric-Based Analyses
Mass Constraint/Volume Constraint: Based on how you define the constraint, modify the percentage or the value as needed.
Center of Gravity Constraint: Specify the upper and/or the lower limit (Maximum Value/Minimum Value) and desired Axis.
Moment of Inertia Constraint: Based on how you define the constraint, modify the percentage or the value as needed and specify a desired Coordinate System and Axis.
Criterion Constraint: Specify the Criterion, Lower Bound, and Upper Bound properties.
Harmonic Response Analyses
Criterion Constraint: Specify the Criterion, Lower Bound, and Upper Bound properties.
Modal Analyses
Natural Frequency Constraint: Specify the values for the Mode Number, Minimum Frequency, and Maximum Frequency properties. Modify the Environment Selection property as needed.
Criterion Constraint: Specify the Criterion, Lower Bound, and Upper Bound properties.
Static Structural Analyses
Global Stress Constraint: Specify a Stress Type, either Equivalent von-Mises Stress (default), Local Equivalent von-Mises Stress, Maximum Principal Stress, or Local Strain Energy, and the Maximum stress value. Modify the Environment Selection property as needed.
Local von-Mises Stress Constraint: Define the Scoping Method as either Geometry Selection or Named Selection and then specify the geometry. Also specify the Maximum stress value. Modify the Environment Selection property as needed.
Displacement Constraint: Specify the X/Y/Z Component (Max) properties. Modify the Environment Selection property as needed.
Reaction Force Constraint: Specify the Axis Selection, Criteria, Bound Type, and X/Y/Z Component properties. Modify the Environment Selection property as needed.
Compliance: Specify the maximum value. Modify the Environment Selection property as needed.
Criterion Constraint: Specify the Criterion, Lower Bound, and Upper Bound properties.
Thermal Analyses
Temperature Constraint: Specify the Temperature (Abs Max) property. Modify the Environment Selection property as needed.
Thermal Compliance: Specify the maximum value. Modify the Environment Selection property as needed.
Note: Where applicable, the application automatically specifies a (read-only) Coordinate System property.

Renaming Based on Definition

The Response Constraint object provides the context menu (right-click) option Rename Based on Definition. This option automatically renames the object based on your Response property selection. That is, it renames the object "Mass Constraint,""Volume Constraint,""Global Stress Constraint," or "Natural Frequency Constraint" accordingly. This feature supports all of the options of the Response property.

Details View Properties

The Details view for this object includes the following properties.

Category Properties/Options/Description

Scope

Scoping Method: The option for this property is based upon the type of Response Constraint you specify.

For the Mass Constraint, Volume Constraint, Center of Gravity, and Moment of Inertia response types, the available Scoping Method options include:

Geometry Selection: This option indicates that the design region is applied to a geometry or geometries (body selection only), which are chosen using the graphical selection tools. When you specify Geometry Selection for the Scoping Method, the Geometry property displays.
In this case, use selection filters on the Graphics Toolbar to pick your geometric entities, and then click Apply. Once complete, the property displays the type of geometry and the number of selected geometric entities (for example: 1 Body).
Named Selection: This option indicates that the design region is applied to a body-based (only) Named Selection. When you specify Named Selection for the Scoping Method, the Named Selection property displays. This property provides a drop-down list of available user-defined Named Selections.
Optimization Region (default): This option indicates that the design region is applied to the specified Optimization Region. When Optimization Region is specified for the Scoping Method, the Optimization Region Selection property also displays. This property contains a default value: Optimization Region.
All Optimization Regions: When you have multiple Optimization Region objects defined, this option indicates that the constraint is applied to all of them.

For Local von-Mises Stress Constraint, Displacement Constraint, and Reaction Force Constraint response types, supported by a linked Static Structural analysis, and the Temperature Constraint, supported by a linked Steady-State Thermal analysis, the available options, as described above, include:

Geometry Selection: Not restricted to body-based scoping only.
Named Selection: Not restricted to body-based scoping only.

For the Global Stress Constraint (Static Structural only) response type, the only available option is Optimization Region and All Optimization Regions.

Note: There is no Scope category for the Natural Frequency Constraint response type.

Definition

Type: This is a read-only property that indicates the object as a Response Constraint.

Response

The options for this property include:

Mass (default)/Volume^[a]: When you select either of these options, the Define By property displays. Define By properties include:
- Constant (default): When this option is used, the Percent to Retain property also displays. The Percent to Retain property defines the upper bound (in percentage) of the Volume/Mass constraint. The default value is 50. The entry range for this property is between 1 and 99.
  Note: For the Density Based Optimization method, this constraint is handled as an equality constraint.
- Range: When this option is selected, the Percent to Retain (Min) and Percent to Retain (Max) properties also display. You use these two properties to define the range, namely lower and upper bound, in percentage, of the Volume/Mass constraint. The default value for each is 50. The entry range for these properties is between 1 and 99.
- Absolute Constant: When selected, the Maximum Value property also displays. The Maximum Value property defines the units-based upper bound of the Mass/Volume constraint. The default value is Free.
  Note: For the Density Based Optimization method, this constraint is handled as an equality constraint.
- Absolute Range^[a]: When selected, the Minimum Value and Maximum Value properties also display. You use these two properties to define the units-based range, namely lower and upper bound, of the Mass/Volume constraint. The default value for each is Free.
Center of Gravity^[a]: When this option is selected, the Max Value and Min Value properties also display and enable you to specify an upper and lower bound for the constraint. The default value is Free. You will note a value contained in the field when you select it. This is a infinite value to indicate a free state.
Moment of Inertia^[a]: When you select this option, the Define By property displays. Define By properties include:
- Constant (default): When this option is used, the Percent to Retain property also displays. The Percent to Retain property defines the upper bound (in percentage) of the Moment of Inertia. The default value is 50. The entry range for this property is between 1 and 99.
- Range: When this option is selected, the Percent to Retain (Min) and Percent to Retain (Max) properties also display. You use these two properties to define the range, namely the lower and upper bound, in percentage, of the Moment of Inertia. The default value for each is 50. The entry range for these properties is between 1 and 99.
- Absolute Constant: Specify the upper bound in the appropriate Unit system.
- Absolute Range: Specify the upper and lower bound in the appropriate Unit system.
Natural Frequency^[a]: This option is only available when there is at least one upstream Modal system. By using this property, the analysis ensures the specified mode and the range of frequencies are supported by the optimized body. When selected, the following associated properties will be shown:
- Mode Number: This property defines the mode number used to create the optimized body.
- Minimum Frequency: This property defines the minimum frequency for the selected mode number.
- Maximum Frequency: This property defines the maximum frequency for the selected mode number.
You can use multiple Natural Frequency objects that specify different Mode Numbers and corresponding frequency ranges for each upstream Modal system.
Global Stress: This option is only available when there is at least one upstream Static Structural system. You use this property to make sure that the optimized geometry or structure always supports a specified maximum stress. When selected, the following reassociated properties also display:
- Stress Type: Options include Equivalent (Von-Mises) Stress, Local Equivalent von-Mises Stress, Maximum Principal Stress, and Local Strain Energy. These options have optimization method support requirements. See the Worksheet Properties topic in the Objective section for more information about the stress options.
- Maximum: Enter a stress value as a Constant or using Tabular Data entries.
Local von-Mises Stress: This option is only available when there is at least one upstream Static Structural system. You use this property to make sure that the geometry or structure always supports a specified maximum stress using the Maximum property that also displays when you select the Local von-Mises Stress option. You specify the stress value of the Maximum property as either a Constant (default) or using Tabular Data entries (via fly-out menu). The application supports multiple Local von-Mises Stress constraints. You can apply this constraint on supported elements that may or may not be included in the Optimization Region.
Displacement^[a]: This option is only available when there is at least one upstream Static Structural system. You use this property to make sure that the optimized geometry or structure always support a specified maximum displacement using the X/Y/Z Component (Max) properties that also display when you select the Displacement option. A read-only Coordinate System property also displays and is automatically set to Nodal Coordinate System. You specify the displacement value of the X/Y/Z Component (Max) properties as either a Constant (default), Free, or using Tabular Data entries (via fly-out menu). The application supports multiple Displacement constraints.
Important: If you apply a Displacement to more than one node, the absolute value for the constraint is met and negative numbers are no longer allowed. For example, if you enter a value of 100N, the constraint is satisfied if it meets a value between -100 and 100.

Reaction Force^[a]: This option is only available when there is at least one upstream Static Structural system. You use this constraint to make sure that the optimized geometry or structure always support a specified maximum reaction force. The application supports multiple Reaction Force constraints.

During the solution process, the application calculates a reaction force for each node used in the Reaction Force constraint (if scoped to more than one node or a vertex, edge, face, or body). Based on the Criteria property setting, the reaction forces are either summed or normalized. Neither of these calculated values can exceed the entries you make in the Component properties for the specified direction(s). Reaction Force has the following distinct properties:

Axis Selection: Options include All (default), X Axis, Y Axis, and Z Axis.
Criteria: Options include Sum (default) and Absolute Maximum (when scoped to more than one node or a vertex, edge, face, or body).
Note: For legacy databases, release 2019 R1 or earlier, that include Reaction Force constraints, the default setting for this property is Absolute Maximum.
Bound Type: Options include Upper Bound (default) and Lower Bound.

X/Y/Z Component (Sum or Max): Component entries are either Constant or based on Tabular Data entries.

When the Criteria property is set to Sum:

Positive values are treated as upper (maximum) bounds. Therefore, the constraint is satisfied if the constraint value is less than the value you specify.

Negative values are considered as lower (minimum) bounds. Therefore, the constraint is satisfied if the constraint value is greater than the value you specify.

A read-only Coordinate System property also displays and is automatically set to Nodal Coordinate System.

Important: If you apply a Reaction Force to more than one node, and the Criteria property is set to Absolute Maximum, the absolute value for the constraint is met and negative numbers are no longer allowed. For example, if you enter a value of 100N, the constraint is satisfied if it meets a value between -100 and 100.

Temperature: This option is only available when the upstream system is Steady-State Thermal. You use this constraint to put an upper bound on the temperatures using Temperature (Abs Max) property. This value can be define as a Constant or using Tabular Data.
Compliance: This option is only available when there is at least one upstream Static Structural system. You use this property to make sure that the optimized geometry or structure is stiff enough. When selected, the Maximum property also displays. Enter a value in the Maximum property as a Constant or using Tabular Data entries. When selected, the Compliance Limit property also displays. The Compliance Limit property enables you to specify an upper boundary on the Compliance value.
Criterion: This option is available when there is at least one upstream Static Structural system. The Criterion constraint enables you to evaluate relative displacements, such as the difference between the displacements of two nodes. And it enables you to make sure that the value of a certain criterion is above or below a given boundary value or that it is within a given range. When selected, the following additional properties need to be specified:
- Criteria: This property displays a drop-down list of available Primary Criterion and Composite Criterion objects evaluated in the upstream Static Structural analysis.
- Lower Bound: Specify this value or set to Free (default).
- Upper Bound: Specify this value or set to Free (default).
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.

Suppressed

Include (No, default) or exclude (Yes) the response constraint.

Environment Selection

The application displays this property when you select the Global Stress, Local von-Mises Stress, Natural Frequency, Displacement, Reaction Force, or Temperature options for the Response property. The entry depends upon your upstream analysis type. Per the upstream system, the default entry is All Structural, All Modal, or All Steady-State Thermal. Also included in the drop-down list are the specific upstream systems. You can select from one of these systems to specify individual values for stress, frequency, etc.

Note: If your Structural Optimization analysis includes multiple upstream analyses, any constraint that sets the Environment Selection property to All Static Structural or All Steady State Thermal, the application only applies the minimum number of steps as determined from the upstream analyses. That is, whichever upstream system has the least number of load steps specified, that is the value the application uses. Selecting a specific analysis from the property drop-down list applies the constraint for all load steps of the selected upstream analysis.

Location and Orientation

When you specify the Response property as Center of Gravity or Moment of Inertia, the Axis property displays in order to specify a desired axis to constrain. Options include X-Axis, Y-Axis, and Z-Axis.

In addition, for the Moment of Inertia option, a Coordinate System property displays so that you can specify the appropriate Cartesian coordinate system for the constraint.

^[a]Ansys recommends that you use User Defined Criterion to define your criterion of interest and then specify the criterion in the Objective or Response Constraint object of your optimization analysis.

Refer to the Response Constraint object reference page for additional information.