38.2.53. Mesh Morpher/Optimizer Dialog Box

The Mesh Morpher/Optimizer dialog box allows you to use the mesh morpher/optimizer to deform the mesh in order to solve shape optimization problems. You can deform the mesh manually, allow a built-in optimizer to define the deformation in order to minimize an objective function, or use Design Exploration in ANSYS Workbench to easily explore a variety of deformation scenarios. See Using the Mesh Morpher/Optimizer for further details.

 Design → Parameter-Based → Optimizer...

Controls

Regions

tab allows you to define the regions of the domain where the mesh will be deformed in order to optimize the shape.

Control Point Distribution

allows you to select the way in which you will define the locations of the control points, as well as the kinds of motions you can apply.

Regular

specifies that the control points will be spread in a regular distribution throughout the entire deformation region. The number of control points along each of the defining direction vectors will be specified in the Control Points group box. The motion of the control points will be limited to translations, as the ability to define rotational or radial motions will not be available.

Unstructured

specifies that control point locations will be specified by right-clicking with the mouse on boundary zones, distributing an approximate number throughout a zone, or by entering coordinates, using the Define Control Points Dialog Box. The motion of the control points will be able to be defined as translations, as rotations about a point / axis, or radially about a point / axis.

Name

provides controls for the deformation regions you are defining. The upper text-entry box defines the name of the region that is created when you click the Create button. The lower selection list allows you to select a region that has already been created, in order to display it in the graphics window, modify the settings via the Modify button, or delete the region via the Delete button.

Update from Zones

allows you to create a bounding box that defines the deformation region.

Boundary Zones

specifies the boundary zones that will be used to generate a bounding box for the deformation region when you click the Define button.

Define

updates the values in the Origin, Direction-1 Vector, Direction-2 Vector, and Size of Region group boxes based on a bounding box that encompasses the selections in the Boundary Zones list, and previews the bounding box in green in the graphics window.

Enlarge

increases the size of the bounding box created by the Define button, and previews the revised bounding box in green in the graphics window.

Reduce

decreases the size of the bounding box created by the Define button, and previews the revised bounding box in green in the graphics window.

Update from Plane Tool

updates the values in the Direction-1 Vector and Direction-2 Vector group boxes based on the settings in the plane tool. See Using the Plane Tool for information about the plane tool. This button is only available for 3D cases.

Update from Line Tool

updates the values in the Direction-1 Vector and Direction-2 Vector group boxes based on the settings in the line tool. See Using the Line Tool for information about the line tool. This button is only available for 2D cases.

Origin

allows you to define the Cartesian coordinates of the origin of the deformation region.

X

defines the x coordinate of the origin of the deformation region.

Y

defines the y coordinate of the origin of the deformation region.

Z

defines the z coordinate of the origin of the deformation region. This number-entry box is only available for 3D cases.

Direction-1 Vector

allows you to define a vector that acts as the first direction of the deformation region relative to the Origin.

X

defines the x component of the first direction vector of the deformation region.

Y

defines the y component of the first direction vector of the deformation region.

Z

defines the z component of the first direction vector of the deformation region. This number-entry box is only available for 3D cases.

Direction-2 Vector

defines a vector that is used to calculate the second direction of the deformation region relative to the Origin. For 2D cases, the values in the Direction-2 Vector group box are automatically defined by ANSYS Fluent to be perpendicular to the Direction-1 Vector. For 3D cases, the vector defined by the Direction-2 Vector group box is projected onto a plane that intersects the Origin and is perpendicular to the vector defined in the Direction-1 Vector group box, in order to calculate the second direction.

X

defines the x component of the vector used to calculate the second direction of the deformation region. This number-entry box is only editable for 3D cases.

Y

defines the y component of the vector used to calculate the second direction of the deformation region. This number-entry box is only editable for 3D cases.

Z

defines the z component of the vector used to calculate the second direction of the deformation region. This number-entry box is only available for 3D cases.

Size of Region

allows you to define the overall dimensions of the deformation region.

Direction-1

defines the length of the deformation region along the direction specified by the Direction-1 Vector group box.

Direction-2

defines the length of the deformation region along the direction specified by the Direction-2 Vector group box.

Direction-3

defines the length of the deformation region along the third axis (that is, the cross product of the vectors defined by the Direction-1 Vector and Direction-2 Vector group boxes). This number-entry box is only available for 3D cases.

Boundary Continuity

allows you to specify whether the mesh transitions are smooth or abrupt wherever the mesh intersects with the limits of the deformation region. This group box is only available when Unstructured is selected from the Control Point Distribution list.

Smooth Transitions

enables smooth mesh transitions wherever the mesh intersects with the limits of the deformation region, based on the creation of stationary control points at those intersections.

Display Control Points

displays the stationary control points created when the Smooth Transitions option is enabled.

Control Points

allows you to define the control points for the deformation regions.

Direction-1

defines the number of control points for the deformation region selected in the Name group box along the direction specified by the Direction-1 Vector group box. This number-entry box is only available when Regular is selected from the Control Point Distribution list.

Direction-2

defines the number of control points for the deformation region selected in the Name group box along the direction specified by the Direction-2 Vector group box. This number-entry box is only available when Regular is selected from the Control Point Distribution list.

Direction-3

defines the number of control points for the deformation region selected in the Name group box along the third axis (that is, the cross product of the vectors defined by the Direction-1 Vector and Direction-2 Vector group boxes). This number-entry box is only available for 3D cases when Regular is selected from the Control Point Distribution list.

Define...

opens the Define Control Points Dialog Box, which you can use to define the control points. This button is only available when Unstructured is selected from the Control Point Distribution list.

Preview

displays (in green) the bounding box that results from the current settings in the Origin, Direction-1 Vector, Direction-2 Vector, and Size of Region group boxes.

Create

creates a new deformation region with the name specified in the upper text-entry box of the Name group box and with the settings defined using the Origin, Direction-1 Vector, Direction-2 Vector, Size of Region, and (for regular control point distributions) Control Points group boxes. The newly created deformation region will be added to and selected in the lower Name selection list, and will be displayed (in blue) in the graphics window.

Modify

modifies the saved settings for the deformation region selected in the lower Name selection list and displays the modified region in the graphics window.

Delete

deletes the deformation region selected in the lower Name selection list.

Constraints

tab allows you to define the constraints on the boundary zones, in order to limit the freedom of particular zones that fall within the deformation region(s) during the morphing of the mesh.

Zones

allows you to select the boundary zones for which you are defining a constraint.

Option

specifies the constraint on the boundary zones selected from the Zones list.

Unconstrained

specifies that the boundary zones are completely free to be deformed according to the assigned parameters.

Passive

specifies that the nodes of the boundary zones are partially constrained to varying degrees, based on their proximity to adjacent boundary zones that are fixed. The nodes in a passive boundary zone behave in a similar manner to the interior mesh nodes, in order to ensure that there is a smooth transition between fixed and unconstrained boundary zones.

Fixed

specifies that the boundary zones are fixed and will not be deformed.

Display

displays the selected Zones in the graphics window.

Summary

prints a list in the console that summarizes the constraint definitions for all of the boundary zones.

Deformation

tab allows you to define the deformation.

Number of Parameters

defines the number of parameters available to define the motion of the control points.

Parameter Values

allows you to define either the magnitude of deformation associated with each parameter (when you are manually specifying the deformation or using Design Exploration in ANSYS Workbench to explore multiple deformation scenarios) or the bounds for each parameter (when you are using a built-in optimizer).

par1, par2...

specify the magnitude of deformation associated with each parameter. You can enter a numeric value in the field or use the   icon to create or assign an input parameter (see Select Input Parameter Dialog Box for details). These fields and icons are only available when none or workbench is selected from the Optimizer drop-down list in the Optimizer tab. Note that the value entered here will specify a length in meters for translations and radial motions, and will specify an angle in degrees for rotations; these units will be used regardless of what units you are using in the case.

Apply

saves definitions for the parameter fields in the Parameter Values group box. This button is only available when none or workbench is selected from the Optimizer drop-down list in the Optimizer tab.

Set Bounds...

opens the Parameter Bounds Dialog Box, where you can define strict minimum and maximum values for the parameters. Note that this button is not available when workbench is selected from the Optimizer drop-down list in the Optimizer tab.

Motion Settings...

opens the Motion Settings Dialog Box, where you can define the motion of the control points.

Deform

applies the current settings in the Parameter Values group box, modifies the mesh, and updates the mesh display in the graphics window. This button is only available when none is selected from the Optimizer drop-down list in the Optimizer tab.

Check

displays a mesh check report in the console for the mesh displayed in the graphics window. This button is only available when none is selected from the Optimizer drop-down list in the Optimizer tab. The mesh check report provides volume statistics, mesh topology and periodic boundary information, verification of simplex counters, and verification of node position with reference to the axis for axisymmetric cases, in the same manner as the Check button in the General task page (see Checking the Mesh for details).

Reset

undoes any modifications made to the mesh as a result of the Deform button and updates the mesh display in the graphics window.

Optimizer

tab allows you to define the settings for the optimizer.

Optimizer

specifies which optimizer is used. The choices include none (for manual deformation); compass, newuoa, powell, rosenbrock, simplex, and torczon (for optimization in ANSYS Fluent); and workbench (for optimizing using Design Exploration in ANSYS Workbench). Note that workbench is only available if you have launched your ANSYS Fluent session from ANSYS Workbench. For information about how the built-in optimizers function or how to use Design Exploration, see Design Analysis and Optimization in the User's Guide or Working With Input and Output Parameters in Workbench in the ANSYS Fluent in Workbench User's Guide, respectively.

Objective Function Definition...

opens the Objective Function Definition Dialog Box, where you can specify the format of the objective function that will be minimized during the optimization process. This button is not available if none or workbench is selected from the Optimizer drop-down list.

Optimizer Settings

allows you to specify the optimizer settings. This group box is not available if none or workbench is selected from the Optimizer drop-down list.

Maximum Number of Designs

defines the maximum number of design stages the optimizer will undergo to reach the specified objective function.

Maximum Iterations per Design

defines the maximum number of iterations ANSYS Fluent will perform for each design change.

Optimizer Convergence Criteria

defines the convergence criteria for the optimizer.

Initial Parameter Variation

defines how much the parameters will be allowed to vary during the initial calculations when newuoa is selected from the Optimizer drop-down list.

Mesh Quality

allows you to enable and define a mesh quality check: if the orthogonal quality (as defined in Mesh Quality) for any cell of a mesh is less than a specified value, no solution is calculated for the mesh and Fluent proceeds to the next design stage. This group box is not available if none is selected from the Optimizer drop-down list.

Reject Poor Quality Meshes

enables the consideration of orthogonal quality when determining whether a solution should be calculated for a mesh.

Minimum Orthogonal Quality

defines the minimum orthogonal quality value every cell must have in order for a solution to be calculated for a mesh. Values may range from 0–1 (where 0 represents the worst quality).

Case and Data File Sets

allows you to enable the automatic saving of intermediate case and data files at specified intervals during the optimization run, so that you can restart an interrupted solution in the same or a different Fluent session without increasing the overall number of design iterations needed to reach convergence. This group box is not available if none or workbench is selected from the Optimizer drop-down list.

Save Every

specifies the frequency (in number of design iterations) that you want intermediate case and data file sets saved. Note that the default value is 0, which specifies that no intermediate files will be saved.

Maximum Number Retained

specifies the maximum number of intermediate case and data files sets you want to retain. After the maximum limit of file sets has been saved, ANSYS Fluent begins overwriting the earliest existing intermediate file set.

File Name

specifies a root name for the intermediate case and data file sets, which will be appended with a number that represents the design iteration during which it was saved. Note that you can include a folder path in the file name if you want the files saved outside of the working folder.

Initialization

provides settings that determine how the solution variables are treated after the mesh is deformed during the optimization process. This group box is not available if none or workbench is selected from the Optimizer drop-down list.

Method

allows you to select one of the following:

Initialize Data After Morphing

specifies that the solution variables should be initialized to the values defined in the Solution Initialization task page after deformation.

Continue with Current Data

specifies that the solution variables should remain the values obtained in the previous design iteration.

Read Data File After Morphing

specifies that the solution variables are set to the values obtained from the data file specified in the Data File Name text-entry box after deformation. This selection is not available when newuoa is selected from the Optimizer drop-down list.

Data File Name

specifies the data file from which the solution variables are obtained when Read Data File After Morphing is selected.

Execute Commands

allows you to specify commands (text commands or command macros) that will be run during the optimization runs of the mesh morpher/optimizer. This group box is not available if none, newuoa, or workbench is selected from the Optimizer drop-down list.

Initial Commands

specifies the commands that will be run after the design has been modified, but before ANSYS Fluent has started to run the calculation for that design stage.

End Commands

specifies the commands that will be run after the solution has run and converged for a design stage.

Monitor...

opens the Optimization History Monitor Dialog Box, which allows you to plot and/or record how the value of the objective function varies with each design stage. This button is not available if none, newuoa, or workbench is selected from the Optimizer drop-down list.

Apply

saves the settings in the Optimizer tab.

Summary

displays a summary of the mesh morpher/optimizer settings in the console.

Optimize

initiates the optimization process using the settings saved in all of the tabs of the Mesh Morpher/Optimizer dialog box. This button is not available if none or workbench is selected from the Optimizer drop-down list.


Release 18.2 - © ANSYS, Inc. All rights reserved.