1D Library

specifies the type of library to be used. (Currently only GTpower and WAVE are available.)

1D Input File Name

specifies the name of the GT-POWER or WAVE input file.

Start

starts up GT-POWER or WAVE and generates Ansys Fluent user-defined functions for each boundary in the input file.

Stop

unlinks the shared library.

Cell Zones

contains a list of cell zones from which you can select the zone to be activated.

Activate

activates the selected cell zones.

(when setting up the Cell Distance predefined criterion under Boundary Layer...)

Boundary Zones

specifies the boundary zones where adjacent cell layers will be split for boundary layer adaption. The selections are used in a boundary register named boundary_cell_distance that is selected in the Refinement Criterion field in the Manual Mesh Adaption Dialog Box.

Cell Layers to Split

specifies the number of cell layers that will be split for boundary layer adaption. The value you enter is used in a boundary register named boundary_cell_distance that is selected in the Refinement Criterion field in the Manual Mesh Adaption Dialog Box.

(when setting up the Flame Indicator predefined criterion under Combustion...)

Include Vortex Indicator

specifies that the magnitude of vorticity is included as part of the criteria for refinement and coarsening.

Spark Region Refinement

enables refinement in a temporary spherical spark region at the start of the simulation (which will then later be coarsened back to the original mesh).

Time

sets the maximum time during which refinement is applied to the spark region, as part of the Spark Region Refinement option. The value you enter will automatically update an expression named spark_<ID>, which is a parameter in the flame_refinement_<ID> expression used in the Refinement Criterion field in the Manual Mesh Adaption Dialog Box or Automatic Mesh Adaption Dialog Box.

Centroid X

sets the x-coordinate for the center of the spark region as part of the Spark Region Refinement option. The value you enter will automatically update a cell register named spark_region, which is used in an expression named spark_<ID> that is a parameter in the flame_refinement_<ID> expression used in the Refinement Criterion field in the Manual Mesh Adaption Dialog Box or Automatic Mesh Adaption Dialog Box.

Centroid Y

sets the y-coordinate for the center of the spark region as part of the Spark Region Refinement option. The value you enter will automatically update a cell register named spark_region, which is used in an expression named spark_<ID> that is a parameter in the flame_refinement_<ID> expression used in the Refinement Criterion field in the Manual Mesh Adaption Dialog Box or Automatic Mesh Adaption Dialog Box.

Centroid Z

sets the z-coordinate for the center of the spark region as part of the Spark Region Refinement option. The value you enter will automatically update a cell register named spark_region, which is used in an expression named spark_<ID> that is a parameter in the flame_refinement_<ID> expression used in the Refinement Criterion field in the Manual Mesh Adaption Dialog Box or Automatic Mesh Adaption Dialog Box.

Radius

sets the radius of the spherical spark region as part of the Spark Region Refinement option. The value you enter will automatically update a cell register named spark_region, which is used in an expression named spark_<ID> that is a parameter in the flame_refinement_<ID> expression used in the Refinement Criterion field in the Manual Mesh Adaption Dialog Box or Automatic Mesh Adaption Dialog Box.

(when setting up the Volume of Fluid predefined criterion under Multiphase...)

Minimum Cell Length Scale

sets the minimum cell length scale for refinement. By default this is set to the minimum cell edge length in the initial mesh. It is used to automatically update the cell volume in an expression named vof_refinement_<ID> that is used in the Refinement Criterion field in the Manual Mesh Adaption Dialog Box or Automatic Mesh Adaption Dialog Box.

(when setting up the VOF-to-DPM [Generic] predefined criterion under Multiphase...)

Number of Cells Across Resolved Droplet

sets the number of cells across the resolved droplet (). It is used to automatically update the cell volume (as described in the definition that follows) used in the vof_to_dpm_refinement_<ID> expression that is used in the Refinement Criterion field in the Manual Mesh Adaption Dialog Box or Automatic Mesh Adaption Dialog Box.

Minimum Resolved Droplet Diameter

sets the minimum diameter of droplets that are resolved in the simulation (). By default this is set to the minimum cell edge length in the initial mesh. It is used (with the Number of Cells Across Resolved Droplet setting) to automatically update the cell volume used in the vof_to_dpm_refinement_<ID> expression, by setting it to . This expression is then used in the Refinement Criterion field in the Manual Mesh Adaption Dialog Box or Automatic Mesh Adaption Dialog Box.

(when setting up the VOF-to-DPM [Advanced] predefined criterion under Multiphase...)

Bulk Secondary Phase Edge Length

specifies an edge length that is cubed in order to define the minimum cell volume that initiates refinement in the secondary phase. This volume is used in an expression named vof_to_dpm_refinement_1 that is used in the Refinement Criterion field in the Manual Mesh Adaption Dialog Box or Automatic Mesh Adaption Dialog Box.

VOF Interface Refinement Edge Length

specifies an edge length that is cubed in order to define minimum / maximum cell volume that initiates refinement / coarsening at the VOF interface. This volume is used in expressions named vof_to_dpm_refinement_1 and vof_to_dpm_coarsening_1, which are then used in the Refinement Criterion and Coarsening Criterion fields, respectively, in the Manual Mesh Adaption Dialog Box or Automatic Mesh Adaption Dialog Box.

(when setting up the Overset predefined criterion)

Orphan Adaption

enables adaption that attempts to remove orphan cells. For details, see Marking for Orphan Adaption.

Size Adaption

enables adaption that reduces size mismatches between donor and receptor cells. For details, see Marking for Size Adaption.

Maximum Length Scale Ratio

sets the threshold () used as part of the Size Adaption option to determine which cells are marked for adaption based on donor-receptor cell size differences. This is set to 3 by default.

Gap Adaption

enables adaption that increases the mesh resolution in gaps as needed (in order to prevent the creation of orphan cells). For details, see Marking for Gap Adaption.

Gap Resolution

specifies the target (minimum) gap resolution used as part of the Gap Adaption option when marking cells for gap adaption. This is set to 4 by default.

Coarsening

enables the coarsening of the mesh when mesh refinement is no longer needed.

(when setting up the Goal-Based Error Indicator predefined criterion under Aerodynamics...)

Set Up Goal...

Opens the Adjoint Observables dialog box where you can select, edit, or create the desired observable.

Skip Initial Adjoint Advancement Before Adaption

When enabled, if the adjoint solution is calculated, the mesh adaption will ignore the computationally expensive initial adjoint iterations which are specified by Initial Adjoint Iterations before Adaption.

Initial Adjoint Iterations Before Adaption

This specifies the number of adjoint iterations in the initial adjoint calculation before the first mesh adaption.

Adjoint Iterations Before Adaption

This specifies the number of adjoint iterations during the adjoint calculation before each mesh adaption.

Number of Modes for Adjoint Advancement

This specifies the number of modes in the Krylov subspace used to approximate the solution. A larger value will help to converge the adjoint solution at the expense of memory cost and potentially more computational time.

Smoothing Steps Before Adaption

A larger value will lead to smoother adaption.

Reset Adaption History

Deletes any previous adaption history.

Print Adaption History

Prints the goal-based adaption history in the console.

Cell Zone(s)

contains a list of the cell zones for which you can find adjacent face zones.

Adjacent Face Zones

contains a list of the face zones that are adjacent to the selected cell zones.

Options

contains relevant options for adjacency.

Multiple Cell Zones

allows you to select multiple cell zones at once. The zones listed in Adjacent Face Zones will be the union of all zones adjacent to the selected cell zones.

Rename Face Zones

allows you to rename selected face zones based on adjacency, zone type, wild card, or add a prefix/suffix.

Rename Cell Zones

allows you to rename selected cell zones based zone type and ID, wild card, or by adding a prefix/suffix.

Draw Default Mesh

brings up the Mesh Display Dialog Box where you can specify zones of the mesh to be permanently displayed as you display or hide face zones from within the Adjacency dialog box. This can be helpful in cases where the mesh is very complex. If this option is not enabled, only the zones selected in Adjacent Face Zones will be displayed when you click Display Face Zones.

On Selected Face Zones

contains controls for renaming face zones that are selected in Adjacent Face Zones. For details on the renaming methods, refer to Renaming Zones Using the Adjacency Dialog Box.

Renaming By:

contains options for how you can rename surfaces.

Adjacency

renames the selected face zones incorporating the name of the adjacent cell zone and the face zone type when you click Rename.

Fluent Naming Convention

renames the selected surface to be a combination of the surface type and the surface ID when you click Rename. Cell zones are renamed to be a combination of the zone type and the zone ID.

Wildcard

renames the selected face zones or cell zones based on a pattern match string in the From field and a replacement string in the To field.

Add Suffix and/or Prefix

adds the provided text in the Suffix or Prefix field to either the beginning or end of the selected zone name(s). Click Add Suffix to add the provided text at the end of the name and click Add Prefix to add the provided text at the beginning of the name.

Abbreviate Types

uses abbreviations for the zone types when renaming rather than the full zone type text.

Exclude Custom Names

excludes from renaming any zones that do not match a recognized naming pattern. This can be useful to prevent inadvertently replacing a meaningful name.

Displace Face Zones

displays the face zones selected in Adjacent Face Zones.

Solution Stabilization

allows you to define solution stabilization settings for the gap model.

Stabilization Level

allows you to define the level of solution stabilization for the gap model simulation. For each level, the solver adjusts the numerical settings, discretization schemes, under-relaxations, AMG settings, and so on, and controls the flow behavior in vicinity of the gap regions. The cost of computation increases with higher levels. Note that these changes are applied globally to all gap regions, and a level other than None will override the local stabilization applied by default to flow-modeling regions that use the Sponge Layer method.

Check CFL Condition

enables the automatic determination of a desirable acoustic Courant (CFL) number based on the selected Stabilization Level, and then provides a warning message in the console if this CFL number would require you to specify a smaller time step for the calculation in order to improve the solver stability.

Extend Gap Regions

enables the extending of the gap regions by including additional cells in the vicinity of the gap interfaces during marking. This is useful when the default shape of the marked cells is negatively affecting solution stability or convergence behavior.

Name

specifies the name of the report definition.

Options

contains options for your aerodamping report definition.

Normalization

Sets the normalization factor for the damping value.

Report Files

lists all of the report files where you can write the report definition data.

Report Plots

lists all of the report plots where you can plot the report definition data (assuming this report has the same units as the other report definitions included in the selected report plot).

Create

Report File

creates a new report file that includes this report definition.

Report Plot

creates a new report plot that includes this report definition.

Frequency

specifies how frequently the report definition is written, plotted, or printed to the console.

Print to Console

prints the value of the report definition to the console.

Create Output Parameter

creates an output parameter for this report definition with the name <report definition name>-op.

OK

creates the report definition.

Compute

computes the value of the report definition at the selected zone(s) and prints to the console.

Name

specifies the name of the report definition.

Options

contains options for your aerodamping report definition.

Per Zone

If you are modeling multiple (main) blades, enables the damping value to be calculated for each dynamic mesh zone (which encompasses one main blade and possibly accompanying splitter blades).

Integrate Over

sets the number of time steps over which to integrate when calculating the damping value; a suggested value is the number of time steps per period..

Normalization

Sets the normalization factor for the damping value.

Report Files

lists all of the report files where you can write the report definition data.

Report Plots

lists all of the report plots where you can plot the report definition data (assuming this report has the same units as the other report definitions included in the selected report plot).

Create

Report File

creates a new report file that includes this report definition.

Report Plot

creates a new report plot that includes this report definition.

Frequency

specifies how frequently the report definition is written, plotted, or printed to the console.

Print to Console

prints the value of the report definition to the console.

Create Output Parameter

creates an output parameter for this report definition with the name <report definition name>-op.

Wall Zones

contains a selectable list of valid walls zones for aerodamping report.

OK

creates the report definition.

Compute

computes the value of the report definition at the selected zone(s) and prints to the console.

Name

name of the animation definition.

Realistic Rendering

option for enhancing the appearance of the animation object by using a raytracer for realistic lighting effects.

Raytracer Image

indicates that animation images will use a raytracing renderer for enhanced image quality. Refer to Realistic Rendering Using Raytracing for additional information on raytracing.

Animation Files

controls for how animation files are stored.

Record after every

specifies the frequency that images are captured during the calculation. You can select whether the frequency is Iteration, Time Step (transient only) or Flow Time (transient only) from the drop-down.

Storage Type

drop-down list with the available formats for storing the animation images.

None

no images are saved. This option is intended for use with embedded window dashboards (Embedded Graphics Window Dashboards).

In Memory

the image files associated with the animation will lost when you exit Fluent.

PPM Image

Fluent will save the animation images in PPM Image format (.ppm), which is 2D.

HSF File

Fluent will save the animation images in HSF file format (.hsf), which is 3D.

PNG Image

Fluent will save the animation images in PNG file format (.png), which is 2D.

JPEG Image

Fluent will save the animation images in JPEG file format (.jpg), which is 2D.

TIFF Image

Fluent will save the animation images in tagged image file format (TIFF—.tif), which is 2D.

Storage Directory

shows the location where the animation images will be stored if the Storage Type is set to any of the types other than In Memory.

---

Note:  Animation files are written to the same directory as the case file, by default. This is stored as a relative path, represented by a dot (.), so that when a case file is shared, animation files are written to an appropriate location.

If you manually specify a path, then what you are specifying is an absolute path that will not automatically be updated if the case file is shared or run from another directory.

---

Animation View

specifies the animation object orientation that will be used when the animation images are capture during the calculation.

views drop-down

list with all of the defined views.

Preview

displays the selected animation object in a reserved graphics window.

Use Active

saves the current view in the active graphics window and automatically selects it for use in the animation definition.

Append File Name with

indicates that the Name of the animation files will have either the time-step, flow-time, or iteration appended. The drop-down menu allows you to specify which one.

Precision

indicates the number of decimal places included when the flow-time is appended.

Animation Object

lists the defined graphics objects that may be selected for animation.

New Object

drop-down list allowing you to create new graphics objects for animating.

• Mesh... opens the Mesh Display Dialog Box.

• Contours... opens the Contours Dialog Box.

• Vectors... opens the Vectors Dialog Box.

• Pathlines... opens the Pathlines Dialog Box.

• Particle Tracks... opens the Particle Tracks Dialog Box.

• Scene... opens Figure 40.50: The Scene Dialog Box.

• XY Plot... opens the Solution XY Plot Dialog Box.

• Report Plot... opens the New Report Plot Dialog Box.

Edit Object...

allows you to edit the selected graphics object.

OK

creates the animation definition and/or saves settings changes and closes the dialog box.

Change Idle Timeout...

opens the Set Idle Timeout Dialog Box.

Method

contains a drop-down list of the recursive partition methods that can be used to create the mesh partitions. The choices include the Cartesian Axes, Cartesian Strip, Cartesian X-Coordinate, Cartesian Y-Coordinate, Cartesian Z-Coordinate, Cartesian R Axes, Cartesian RX-Coordinate, Cartesian RY-Coordinate, Cartesian RZ-Coordinate, Cylindrical Axes, Cylindrical R-Coordinate, Cylindrical Theta-Coordinate, Cylindrical Z-Coordinate, Metis, Polar Axes, Polar R-Coordinate, Polar Theta-Coordinate, Principal Axes, Principal Strip, Principal X-Coordinate, Principal Y-Coordinate, Principal Z-Coordinate, Spherical Axes, Spherical Rho-Coordinate, Spherical Theta-Coordinate, and Spherical Phi-Coordinate techniques, which are described in Mesh Partitioning Methods.

Case File

allows you to use a valid existing partition section in a case file (that is, one where the number of partitions in the case file divides evenly into the number of compute nodes). You need to turn off the Case File option only if you want to change other parameters in the Auto Partition Mesh dialog box.

Across Zones

allows partitions to cross zone boundaries (the default). If turned off, it will restrict partitioning to within each cell zone. This is recommended only when cells in different zones require significantly different amounts of computation during the solution phase, for example if the domain contains both solid and fluid zones.

Optimizations

contains an option to enable pre-testing.

Pre-Test

instructs Fluent to test all coordinate directions and choose the one which yields the fewest partition interfaces for the final bisection. Note that this option is available only when you choose Principal Axes or Cartesian Axes as the partitioning method.

Name

specifies the name of the adaption criteria.

Frequency

defines the frequency of the adaption that will be applied for this criteria during the calculation.

Refinement Criterion

specifies the cell register or expression that Fluent will use during the calculation to determine which cells to refine.

Coarsening Criterion

specifies the cell register or expression that Fluent will use during the calculation to determine which cells to coarsen.

Prismatic Adaption

specifies that prismatic cells are adapted anisotropically. This option is only available with the PUMA adaption method.

Predefined Criteria

allows you to select from a list of commonly used criteria for adapting the mesh (for a description of the list, see Predefined Criteria for Adaption); if one is selected, Fluent will automatically generate cell registers and/or expressions for refinement and coarsening, and define the settings in the Automatic Mesh Adaption dialog box and General Adaption Controls Dialog Box as needed. Depending on your selection, you may be prompted to complete the setup by defining fields in the Adaption Criteria Settings Dialog Box.

Cell Registers

allows you to create new cell registers and manage existing ones, which may then be selected from the Refinement Criterion and/or Coarsening Criterion drop-down lists.

List Criteria

prints to the console the number of cells marked for refinement, the number of cells marked for coarsening, and the number marked for both operations.

Display Options

opens the Display Options - Adaption Dialog Box.

General Adaption Controls

opens the General Adaption Controls Dialog Box, where you can specify the general settings that Fluent uses when adapting the mesh.

Name

specifies the name of the report definition.

Options

Per Surface

enables the reporting of the cell count individually for each of the selected zones (rather than reporting the sum from all of the selected zones).

Average Over

specifies the number of iterations / time steps over which the cell count is averaged when written, plotted, and/or printed. The default value of 1 means that no averaging is performed (that is, only the current cell count is reported), and higher values yields a running average. When the iteration / time step number is lower than the specified value, Fluent calculates the average of the available cell count values.

Retain Instantaneous Values

enables the retention of instantaneous values in any report file definition or report plot definition that is associated with this report definition. This option is only available if Average Over is set to a value greater than 1.

Report Files

allows you to select existing report file definitions to which you want to write cell count data from this report definition.

Report Plots

allows you to select existing report plot definitions to which you want to include cell count data from this report definition. Note that the units used in these report plots may not be suitable for the cell count data.

Create

Report File

creates a new report file definition for the data from this report definition.

Report Plot

creates a new report plot definition for the data from this report definition.

Frequency

specifies how frequently the report definition is written, plotted, and/or printed to the console.

Print to Console

enables the printing of the cell count data from this report definition to the console during the calculation.

Create Output Parameter

creates an output parameter for this report definition with the name <report_definition_name>-op.

Cell Zones

allows you to select the cell zones for which you want to report the number of cells.

OK

creates / saves the report definition.

Compute

computes the cell count within the selected zone(s) and prints to the console.

Options

contains check buttons that control the drawing of the mesh and the type of graphical tool used to display register cells.

Draw Mesh

toggles the ability to draw the mesh with the cell register display. This command opens the Mesh Display Dialog Box, which allows you to select the desired surface or zone meshes to be displayed with the register cells.

Wireframe

toggles the display of the cell wireframe.

Filled

toggles the solid shading of the cell wireframe.

Marker

toggles the display of the cell marker.

Color

is a drop-down list of colors for the wireframe or marker for the cells.

Symbol

is a drop-down list of symbols that can be used cell marker.

Size

is a real number entry for the size of the cell marker. A symbol of size 1.0 is 3.0% of the height of the display screen.

Source Files

contains a list of source files.

Header Files

contains a list of header files.

Add...

opens the Select File dialog box.

Delete

deletes the selected file from the list.

Library Name

specifies the name of the library to be created.

Use Built-In Compiler

enables the use of a built-in compiler (Clang) when the Build button is clicked. This option / compiler is available for Windows only, and is provided as part of the Fluent installation. It is recommended that you enable this option when the compiler you installed on your machine is older and no longer supported. Note that the built-in compiler is used automatically if Fluent determines that you have not installed Microsoft Visual Studio or Clang on your computer, whether this option is enabled or not.

Build

builds the library and compiles the user-defined function.

Load

opens the specified library and loads the user-defined function.

Shell Conduction

enables/disables shell conduction for the selected wall(s).

Number of Shell Conduction Layers

allows you to define the number of layers that make up the wall(s).

Primary Zone

sets a wall to copy conduction settings from to the other selected walls.

Layer 1, Layer 2...

allows you to define the settings for each layer. Note that Layer 1 refers to the layer closest to the fluid / solid adjacent to the wall zone, and layers with higher numbers are further away.

Thickness

sets the thickness of the layer for the calculation of the thermal resistance. Each layer must have a nonzero thickness. Note that non-shell walls with a specified Thickness will be treated as thin walls.

Material Name

sets the material type for the layer/wall. The conductivity of the material is used for the calculation of thermal resistance. Materials are defined using the Materials Task Page.

Heat Generation Rate

sets the rate of heat generation in the layer. Note that you have the option of defining the heat generation rate using a user-defined function (UDF) that utilizes the DEFINE_PROFILE macro; for more information on creating and using user-defined functions, see the Fluent Customization Manual.

Select Zones

contains the list of conduction zones (1d thin walls and 3d shell walls) and ordinary walls.

Wall Zones

contains a list of wall zones.

Settings...

opens the Conduction Layers Dialog Box, where you can define the conduction properties of the walls selected in the Wall Zones list.

Display

displays the selected walls in the graphics window.

Read...

allows you to define your conduction settings by reading a .csv file.

Write...

allows you to write your saved conduction settings to a .csv file.

Contour Name

is the name for a contour plot definition. You can specify a name or use the default name contour-id . This control appears only for contour plot definitions.

Options

contains the check buttons that set various contour display options.

Filled

toggles between filled contours and line contours.

Node Values

toggles between using scalar field values at nodes and at cell centers for computing the contours. When the Filled option is off, Node Values is always on. See Choosing Node or Cell Values and Node or Boundary Values and Node Values for details.

Boundary Values

enabling overwrites the node values (on boundaries) with a simple average of the boundary face values. Refer to Choosing Node or Cell Values and Node or Boundary Values for more information.

Contour Lines

combines filled contours with line contours. This option is only available when both the Filled and Node Values options are enabled.

Global Range

toggles between basing the minimum and maximum values on the range of values on the selected surfaces (off), and basing them on the range of values in the entire domain (on, the default).

Auto Range

toggles between automatic and manual setting of the contour range. Any time you change the Contours of selection, Auto Range is reset to on.

Clip to Range

determines whether or not values outside the prescribed Min/ Max range are contoured when using Filled contours. If selected, values outside the range will not be contoured. If not selected, values below the Min value will be colored with the lowest color on the color scale, and values above the Max value will be colored with the highest color on the color scale. See Specifying the Range of Magnitudes Displayed for details.

Draw Profiles

causes the addition of a profile plot to the contour plot. The Profile Options Dialog Box is opened when Draw Profiles is selected.

---

Note:   Draw Profiles is only available for the non-persistent/"global" version of the Contours dialog box that does not have a Name field. This version of the dialog box is opened by:

• Right-clicking Contours in the Outline View tree and selecting Edit... (located under the Results branch).

• Clicking Contours and selecting Edit... under Graphics in the Results ribbon tab.

---

Draw Mesh

toggles between displaying and not displaying the mesh. The Mesh Display Dialog Box is opened when Draw Mesh is selected.

Coloring

specifies how the contours appear.

Banded

the contour coloring features distinct color bands corresponding to the colormap.

Smooth

the contours feature a smooth transition between colors.

Colormap Options...

opens the Colormap Dialog Box, allowing you to customize the colormap for this graphics object.

Contours of

contains a list from which you can select the scalar field to be contoured.

Min

shows the minimum value of the scalar field. If Auto Range is off, you can set the minimum by typing a new value.

Max

shows the maximum value of the scalar field. If Auto Range is off, you can set the maximum by typing a new value.

Surfaces

contains a list from which you can select the surfaces on which to draw contours. For 2D cases, if no surface is selected, contouring is done on the entire domain. For 3D cases, you must always select at least one surface.

Display State

specifies the display state that is associated with this graphics object.

drop-down list of display states

selectable list of all the existing display states associated with this case.

Use Active

creates a display state that matches the settings of the active graphics window and assigns it to this graphics object (this association is only saved after you click Save/Display).

New Surface

is a drop-down list button that contains a list of surface options:

Point

opens the Point Surface Dialog Box.

Line/Rake

opens the Line/Rake Surface Dialog Box.

Plane

opens the Plane Surface Dialog Box.

Quadric

opens the Quadric Surface Dialog Box.

Iso-Surface

opens the Iso-Surface Dialog Box.

Iso-Clip

opens the Iso-Clip Dialog Box.

Structural Point

opens the Structural Point Surface Dialog Box.

Display

draws the contours in the active graphics window.

Compute

calculates the scalar field and updates the Min and Max values (even when Auto Range is off).

Save/Display

plots the contour in the active graphics window and saves the contour plot definition. This button appears only for contour plot definitions and replaces the Display button.

Active

check box for deactivating/activating individual convergence conditions.

Conditions

name of the convergence condition.

Report Definition

name of the report definition used in judging convergence.

Stop Criterion

specifies the criterion below which the solution is considered to be converged.

Ignore Iterations Before | Ignore Time Steps Before

ignores the first few iterations/time-steps if you expect the solution to fluctuate initially.

Use Iterations | Use Time Steps

specifies the number of previous iterations/time-steps to be included in the report definition convergence check.

Check For

specify whether Fluent checks for convergence at every time step or every iteration.

Solution Convergence

Fluent checks for solution convergence at every time step.

Time Step Convergence

Fluent checks for solution convergence at every iteration.

Choose Condition

to select the convergence conditions.

All Conditions are Met

The solution is considered to be converged if all of the convergence conditions’ criteria are satisfied, including those in the Residual Monitors Dialog Box.

Any Condition is Met

The solution is considered to be converged if any of the convergence conditions’ criteria is satisfied, including those in the Residual Monitors Dialog Box.

Every Iteration | Every Time-Step

to select how often convergence checks are done.

Mesh Interface Name Prefix

contains a text entry box in which you can specify the prefix used in the names of all the mesh interfaces created when you click the Create button, and a list from which you can select existing mesh interfaces.

Boundary Zone List 1, Boundary Zone List 2

allows you to select the zones that you want to pair up to make mesh interfaces. Note that mesh interfaces will be created for every possible combination between these two lists, regardless of whether the zones in question currently overlap. (You cannot edit the top fields; the names in these fields will be the name of the last zone you selected in the list below it.)

Create

creates mesh interfaces for every possible combination between the zones selected under Boundary Zone List 1 and Boundary Zone List 2, regardless of whether the zones in question currently overlap.

Delete

deletes the mesh interfaces selected from the list under Mesh Interface Name Prefix.

Display

allows you to display selected interface zones or mesh interfaces in the graphics window. Note that after you have selected a mesh interface, you can modify what zones are displayed by selecting / deselecting zones under Boundary Zone List 1 and/or Boundary Zone List 2.

List

prints information about the mesh interfaces selected in the list under Mesh Interface Name Prefix in the console.

Mesh Interface

contains a text entry box in which you can set the name of the mesh interface, and a list from which you can select an existing mesh interface.

Interface Zones Side 1, Interface Zones Side 2

contain selectable lists for the interface zones that make up the mesh interface and informational fields that show the names of the zones you selected in each list. (You cannot edit the top fields; the names in these fields will be the names of the zones you selected in the list below it.)

Interface Options

contains options related to the interface type.

Periodic Boundary Condition

allows you to create a non-conformal periodic boundary condition interface. Note that the Matching option is enabled by default with such periodic mesh interfaces.

Periodic Repeats

should be enabled when each of the two cell zones has a single pair of conformal or non-conformal periodics adjacent to the interface. This option is typically used in conjunction with the sliding mesh model, when simulating the interface between a rotor and stator; it allows Ansys Fluent to treat the interface between the sliding and non-sliding zones as periodic where the two zones do not overlap. For details, see The Periodic Repeats Option.

Coupled Wall

allows you to specify that the interface acts as a thermally coupled wall.

Matching

is relevant if only interface internal zones should be created (that is, interior or wall / shadow pairs), since the interface zones on both sides are aligned. With the Matching option, even interface zones that are not perfectly aligned are treated as if they are; however, if the discrepancy between the interface zones on both sides exceeds default thresholds, then warning messages will be displayed. Note that the Matching option is compatible with the Periodic Boundary Condition, Coupled Wall, and Static options. For more information about the recommended uses of this option, see Matching Option.

Mapped

enables an alternative approach for modeling coupled walls between zones. This approach is more robust than the standard non-conformal interface formulations when the interface zones penetrate each other or have gaps between them. It requires that at least one side of the interface consists of only solid zones.

---

Note:  The Mapped option is not compatible with shell conduction.

---

Static

reduces the memory usage and processing time (for interface creation and solution), especially when there are many zones on both sides of the interface. This option will only produce correct results if the interface zones do not move or deform relative to each other at the interface, and it is not compatible with the Periodic Boundary Condition, Periodic Repeats, or Mapped options.

Non-Overlapping Zones Side 1, Non-Overlapping Zones Side 2

display the names of any wall boundary zones created by Ansys Fluent during the process of creating the selected mesh interface. If the two interface zones overlap each other completely, then the wall boundaries are created but with zero faces.

Interface Wall Zones Side 1, Interface Wall Zones Side 2

display the names of any wall interface zones created by Ansys Fluent during the process of creating the selected mesh interface.

Interface Interior Zones

displays the names of any interface interior zones created by Ansys Fluent during the process of creating the selected mesh interface. This is used for embedded LES, when there is a need to be able to convert an interior zone into a RANS-LES interface.

Periodic Boundary Condition

Type

allows you to select a periodicity that is either Translational or Rotational.

Offset

is the offset coordinates or angle, depending on whether Translational or Rotational periodicity is selected. Note that when Auto Compute Offset is enabled, the Offset fields are not editable.

Auto Compute Offset

will result in Ansys Fluent finding the offset. If this option is disabled, then you will have to provide the offset coordinates or angle in the required fields, depending on whether Translational or Rotational periodicity is selected.

Mapped

Enable Local Tolerance

(when enabled) allows you to overwrite any value specified in the Tolerance group box in the Mapped Interface Options Dialog Box, and is used on the selected interface only.

Local Edge Length Factor

(when enabled) allows you to specify the multiplier that Fluent uses with the smallest edge length of the interface zones to calculate the tolerance for mapping. Disabling Local Edge Length Factor allows you to specify an absolute value for the tolerance.

Create/Edit...

performs one of the following:

• If you have entered a new Mesh Interface name and selected unassigned zones from the Interface Zones Side 1 and Interface Zones Side 2 selection lists, a new mesh interface is created.

• If you have made a selection from the Mesh Interface list, the Edit Mesh Interfaces Dialog Box will open so that you can revise the settings of existing mesh interfaces.

Delete

deletes the mesh interface selected under Mesh Interface.

Display

allows you to display interface zones or mesh interfaces in the graphics window. Note that you can only select and display an interface zone from Interface Zones Side 1 or Interface Zones Side 2 if it is not yet assigned to an existing mesh interface. After a Mesh Interface is created, you can select the appropriate mesh interface and click the Display button to display all of the zones under Interface Zones Side 1 and Interface Zones Side 2.

List

prints information about the selected Mesh Interface in the console. When you click this button, Ansys Fluent will list the two interface boundaries and (if you have initialized the solution) all new zones that were created (that is, wall and/or interior zones).

Mesh Interface

contains a text entry box in which you can set the name of the turbo interface, and a list from which you can select an existing mesh interface.

Interface Zones Side 1, Interface Zones Side 2

contain selectable lists for the interface zones that make up the turbo interface and informational fields that show the names of the zones you selected in each list. (You cannot edit the top fields; the names in these fields will be the names of the zones you selected in the list below it.)

Interface Options

contains options related to the interface type.

Periodic Boundary Condition

allows you to create a non-conformal periodic boundary condition interface. Note that the Matching option is enabled by default with such periodic mesh interfaces; for details about the Matching option, see Matching Option.

General Turbo Interface

(only available when the Turbo Model is enabled) connects two turbo zones. This option is typically used in conjunction with the sliding mesh model, when simulating the interface between a rotor and stator. These models permit for a pitch-change between the modeled blade rows.

Pitch-Change Types

Pitch-Scale

stretches or compresses the flow profiles between the cell zones to maintain the interaction between blade row passages. See Blade Row Interaction Modeling for details.

No Pitch-Scale

maintains the blade row interaction between blade row passages by creating virtual copies of the smaller pitch blade passage. See Blade Row Interaction Modeling for details.

Mixing Plane

uses a pitchwise averaging procedure to mix out the flow variation between the blade rows. See Blade Row Interaction Modeling for details.

Create/Edit...

performs one of the following:

• If you have entered a new Mesh Interface name and selected unassigned zones from the Interface Zones Side 1 and Interface Zones Side 2 selection lists, a new mesh interface is created.

• If you have made a selection from the Mesh Interface list, the Edit Mesh Interfaces Dialog Box will open so that you can revise the settings of existing mesh interfaces.

Delete

deletes the mesh interface selected under Mesh Interface.

Display

allows you to display interface zones or mesh interfaces in the graphics window. Note that you can only select and display an interface zone from Interface Zones Side 1 or Interface Zones Side 2 if it is not yet assigned to an existing mesh interface. After a Mesh Interface is created, you can select the appropriate mesh interface and click the Display button to display all of the zones under Interface Zones Side 1 and Interface Zones Side 2.

List

prints information about the selected Mesh Interface in the console. When you click this button, Ansys Fluent will list the two interface boundaries and (if you have initialized the solution) all new zones that were created (that is, wall and/or interior zones).

Name

specifies the name of the curvilinear coordinate system.

Cell Zones

specifies the cell zone whose geometry will be used to create the curvilinear coordinate system.

Direction 0 (1)

tabs to specify Direction 0 and 1 of the curvilinear coordinate system. Note that Direction 2 is calculated from the cross product of Direction 0 and 1.

Method

There are 2 options for specifying a direction.

• Diffusion - utilizes geometry to specify direction as determined by Boundary Specification.

  Start and End

  specifies the direction using a Start Face Zone and an End Face Zone.

  Jump

  for closed loop geometries, specifies the direction from Interior Zones (utilizing a coupled wall as a cross section, which is then split into start and end faces).

• Base Vector - specifies the direction using an X, Y, Z vector

Display Face Zones

displays currently selected face zones.

Visualize Direction Vectors

options to visualize the curvilinear coordinate system.

Direction 0

selects Direction 0 to display in the graphics viewer.

Direction 1

selects Direction 1 to display in the graphics viewer.

Direction 2

selects Direction 2 to display in the graphics viewer.

Auto Scale

scales the vectors to an appropriate size.

Draw Mesh

opens the Mesh Display dialog box.

Scale

specifies the size of the vectors for display.

Skip

Thins the number of vectors displayed to improve visibility.

Save

Saves the curvilinear coordinate system.

Display

Displays the curvilinear coordinate system according the settings under Visualize Direction Vectors.

Definition

displays the function that you are currently defining. As you select each item from the Field Functions list or the calculator keypad, it will appear in the Definition text entry box. You cannot edit the contents of this box directly; if you want to delete part of a function, use the Delete button on the keypad.

(Calculator Buttons)

are buttons that perform calculator operations. When you select a calculator button (by clicking on it), the appropriate symbol will appear in the Definition text entry box.

Select Operand Field Functions from

contains the available field functions and the means for selecting them.

Field Functions

contains a list from which you can select a variable to be used in the definition of a new function.

Select

enters the variable that is currently selected in the Field Functions list in the Definition field.

New Function Name

specifies the name of the function you are defining. Should you decide to change the function name after you have defined the function, you can do so in the Field Function Definitions Dialog Box, which you can open by clicking on the Manage... button.

Define

creates the function and adds it to the list of Custom Field Functions within the drop-down list of available field functions. The Define button is grayed out after you create a new function or if the Definition field is empty.

Manage...

opens the Field Function Definitions Dialog Box, which enables you to check, rename, save, load, and delete custom field functions.

First Law, Second Law, Third Law,...

contain drop-down lists in which you can choose a user-defined particle law to replace the standard law.

Switching

contains a drop-down list in which you can select a user-defined function that customizes the way Ansys Fluent switches between particle laws.

Name

is the name for a dashboard definition. You can specify a name or use the default name dashboard-id.

Base Window

specifies which window will be the background, upon which all other graphics and plot objects are embedded. You can also leave it set to none, allowing you to arrange the child windows without any overlap.

Pre-defined Layouts

controls how the embedded windows are arranged when they are displayed first displayed. You can manually move and resize the windows once they are displayed.

Available Objects

lists the available graphics and plot objects that can be included in the dashboard.

New Object

drop-down list allowing you to create additional graphics objects that can be included in the dashboard.

Save

saves the dashboard to the case file.

Display

saves the dashboard and displays it in the graphics window.

Cell Zones

contains a list of cell zones from which you can select the zone to be deactivated.

Deactivate

deactivates the selected cell zones.

Control Points

lists the control points you have created and allows you to modify and delete them.

Definition Tools

provides tools for defining the control points.

Mouse-Probe

allows you to create control points by probing (using the right mouse button, by default) in the graphics window.

Distribute Throughout Zone

allows you to quickly create a number of control points and distribute them on mesh nodes throughout a specific boundary zone.

Zones

allows you to select the boundary zone throughout which you want to distribute control points.

Approximate Number

allows you to specify the approximate number of control points you want to distribute throughout a zone. Note that due to the method by which the control points are distributed, the actual number may exceed the value you enter.

Distribute

creates a number of control points on mesh nodes throughout the specified zone (within the bounding box) with a distribution that is based on the distribution of the cell faces in that zone.

Coordinates

allows you to view and modify the coordinates of control points, as well as to create new control points and to delete existing control points.

X, Y, Z

displays the coordinates of the selected Control Point, and allows you to define new ones and edit existing ones.

Create

creates a new control point at the currently displayed X, Y, and Z coordinates.

Modify

revises the X, Y, and Z coordinates of the selected Control Point.

Delete

deletes the selected Control Point.

Cell Zones

contains a list of cell zones from which you can select the zone to be deleted.

Delete

deletes the selected cell zones.

Options

contains check boxes that controls the drawing of the mesh.

Draw Mesh

toggles the ability to draw the mesh with the adaption display. This command opens the Mesh Display Dialog Box, which allows you to select the desired surface or zone meshes to be displayed with the markings.

Refinement Cells

contains options related to the display of cells marked for refinement.

Faces

controls whether cell faces are displayed on the cells marked for refinement.

Edges

controls whether cell edges are displayed on the cells marked for refinement.

Centroid

controls whether the cell centroid is displayed on the cells marked for refinement.

Face Color

controls the color of the cell faces on the cells marked for refinement.

Edge Color

controls the color of the cell edges on the cells marked for refinement.

Edge Width

controls the thickness of the cell edges on the cells marked for refinement.

Coarsening Cells

contains options related to the display of cells marked for coarsening.

Faces

controls whether cell faces are displayed on the cells marked for coarsening.

Edges

controls whether cell edges are displayed on the cells marked for coarsening.

Centroid

controls whether the cell centroid is displayed on the cells marked for coarsening.

Face Color

controls the color of the cell faces on the cells marked for coarsening.

Edge Color

controls the color of the cell edges on the cells marked for coarsening.

Edge Width

controls the thickness of the cell edges on the cells marked for coarsening.

Common Cells

contains options related to the display of cells marked for both refinement and coarsening.

Faces

controls whether cell faces are displayed on the cells marked for both refinement and coarsening.

Edges

controls whether cell edges are displayed on the cells marked for both refinement and coarsening.

Centroid

controls whether the cell centroid is displayed on the cells marked for both refinement and coarsening.

Face Color

controls the color of the cell faces on the cells marked for both refinement and coarsening.

Edge Color

controls the color of the cell edges on the cells marked for both refinement and coarsening.

Edge Width

controls the thickness of the cell edges on the cells marked for both refinement and coarsening.

Display States

single selection listing of all defined display states.

New

create a new display state with the same settings as the active graphics window (or the last active user window if the current active window is displaying a 2D plot).

Copy

create a new display state the copies the properties of the selected display state.

Save

save the properties of the selected display state.

Delete

delete the selected state.

Read...

read in display states from a file.

Write...

write display states to a file.

Name

name of the selected display state.

Views...

opens the Views Dialog Box.

Views Drop-down List

list of views that can be associated with this display state.

General Settings

lists general graphics window settings.

Front Faces Transparency

controls whether the front faces are transparent.

Projection

specifies whether the display is in a perspective or orthographic view.

Axes

controls whether or not the axes triad is displayed.

Ruler

controls whether or not the ruler is displayed.

Boundary Markers

controls whether or not boundary markers are displayed. Note that boundary markers are only displayed on mesh, not other graphics objects like contours or vectors.

Title

controls whether or not the titles bar is displayed.

Edge Color

controls the color of the cell edges on the cells marked for refinement.

Lighting Effects

lists lighting settings.

Light ID

controls which light ID is saved. If more than one light ID is active when you click Use Active from a graphics object dialog box, this option is set to Don't Save.

Headlights

controls whether the headlight is on or off.

Lighting

specifies the lighting method that is used for the display.

Graphic Effects

lists the graphics effects.

Anti-Aliasing

controls whether or not lines and text are smooth.

Reflections

controls whether or not a reflection of the model is shown (with the axis of reflection being controlled in Preferences).

Static Shadows

controls whether or not static shadows are displayed.

Dynamic Shadows

controls whether or not dynamic shadows are displayed. These shadows move as you rotate your model and are computationally expensive to render.

Grid Plane

controls whether or not the grid plane is shown (with the axis for the grid being controlled in Preferences).

Apply

save the settings of the selected display state and apply these settings to the active graphics window display.

Use Active

update the currently-selected display state to inherit the display state settings of the active graphics window. This button is not available if the active graphics window is displaying a 2D plot.

Default

resets the selected display state to match the default settings.

Table 52.1: Default Display State Settings

Setting	State
View	isometric
Front Faces Transparent	Disable
Projection	Perspective
Axes	Enable
Ruler	Disable
Boundary Markers	Enable
Title	Disable
Light ID	0
Headlights	On
Lighting	Automatic
Anti-Aliasing	Enable
Reflections	Enable
Static Shadows	Enable
Dynamic Shadows	Disable
Grid Plane	Enable

---

Note:  The default graphics effects settings are dependent on the available graphics driver. If no modern graphics driver is available, graphics effects will be disabled.

---

Name

specifies the name of the report definition.

Average Over

(optional) To have Fluent calculate a running average for the DPM Report Definition you can enter a positive integer greater than 1 (the default) for Average Over.

Specifying a number greater than 1 means that Fluent will print, plot, and write the running average value of the selected variable instead of the current value of the same variable.

The value reported is averaged over the last iterations/time steps, where is your specified Average Over value. When the iteration/time step number is lower than , Fluent calculates the average of the available variable values.

Retain Instantaneous Values

appears when Average Over is set to a value greater than 1. If enabled when you are creating a new report definition, it ensures that all instantaneous values are saved in the new report file that is being created for this report definition. It also results in the Plot Instantaneous Values option being enabled in the newly created report plot.

Report Files

lists all of the report files where you can write the report definition data.

Report Plots

lists all of the report plots where you can plot the report definition data (assuming this report has the same units as the other report definitions included in the selected report plot).

Create

options you can choose when creating your report.

Report File

creates a new report file that includes this report definition.

Report Plot

creates a new report plot that includes this report definition.

Frequency

specifies how frequently the report definition is written, plotted, or printed to the console.

Print to Console

prints the value of the report definition to the console.

Create Output Parameter

creates an output parameter for this report definition with the name <report definition name>-op.

Output Quantity

quantities that can be applied to the output parameter.

Injected Mass

(unsteady particle tracking only) reports the total DPM mass injected into the domain.

Mass in Domain

(unsteady particle tracking only) reports the total DPM mass present in the domain.

Mass in Fluid

(unsteady particle tracking only) reports all DPM mass currently residing as free-stream particles in the domain. This option is available only with the wall-film DPM boundary condition.

Mass in Film

(unsteady particle tracking only) reports all DPM mass currently residing in Lagrangian wall-film. This option is available only with the wall-film DPM boundary condition.

Escaped Mass

reports the DPM mass that has left the domain through a certain boundary or boundaries.

Evaporated Mass

reports the total evaporated DPM mass for the selected injection(s). The quantity accounts for fully evaporated particles as well as all mass that has evaporated from any other particles. For unsteady tracking, this includes particles that are still present in the domain.

Penetration Length

(unsteady particle tracking only) reports the total penetration length in meters.

Injections

lists the injections that you can select for discrete phase reporting. For the Escaped Mass output quantity, this item is available only if you have enabled the report/dpm-zone-summaries-per-injection text command. Note that for unsteady particle tracking, if you want to report the mass of escaped particles per injection, this text command must be enabled before any particles are injected into the domain.

Boundaries

contains a selectable list of valid boundary zones for escaped mass reporting.

Show Mass Flow/Change Rate

(unsteady particle tracking only) if enabled, specifies that the mass flow rate will be reported (default). Otherwise the total mass will be reported. This item is not available for the Penetration Length report.

Particles Mass Fraction

the mass fraction expected between the injection nozzle and the penetration length. This item is available only for the Penetration Length reports.

User-Specified Origin and Direction

once enabled, it allows you to specify the Origin and Direction of the selected injection(s). This item is available only for the Penetration Length reports.

OK

creates the report definition.

Compute

computes the value of the report definition and prints to the console.

Name

specifies the name of the report definition.

Function

functions available for the source report definition.

DPM Mass Source

reports the mass contributions from the particle injections.

DPM Enthalpy Source

reports the heat contributions from the particle injections.

DPM Sensible Enthalpy Source

reports the sensible heat contributions from the particle injections.

Average Over

(optional) To have Fluent calculate a running average for the DPM Source Report Definition you can enter a positive integer greater than 1 (the default) for Average Over.

Specifying a number greater than 1 means that Fluent will print, plot, and write the running average value of the selected variable instead of the current value of the same variable.

The value reported is averaged over the last iterations/time steps, where is your specified Average Over value. When the iteration/time step number is lower than , Fluent calculates the average of the available variable values.

Retain Instantaneous Values

appears when Average Over is set to a value greater than 1. If enabled when you are creating a new report definition, it ensures that all instantaneous values are saved in the new report file that is being created for this report definition. It also results in the Plot Instantaneous Values option being enabled in the newly created report plot.

Report Files

lists all of the report files where you can write the report definition data.

Report Plots

lists all of the report plots where you can plot the report definition data (assuming this report has the same units as the other report definitions included in the selected report plot).

Create Output Parameter

creates an output parameter for this report definition with the name <report definition name>-op.

Create

options you can choose while generating a report.

Report File

creates a new report file that includes this report definition.

Report Plot

creates a new report plot that includes this report definition.

Frequency

specifies how frequently the report definition is written, plotted, or printed to the console.

Print to Console

prints the value of the report definition to the console.

Compute

computes the value of the report definition and prints to the console.

OK

creates the report definition.

Name

specifies the name of the report definition.

Options

options you can choose for the drag report.

Per Zone

specifies whether or not the drag for multiple walls zones should be monitored on each wall zone separately. When this option is turned off (the default), Fluent computes and monitors the total drag for all of the selected walls zones combined together.

Average Over (Time-Steps), Average Over (Iterations)

(optional) To have Fluent calculate a running average for the Drag Report Definition you can enter a positive integer greater than 1 (the default) for Average Over.

Specifying a number greater than 1 means that Fluent will print, plot, and write the running average value of the selected variable instead of the current value of the same variable.

The value reported is averaged over the last iterations/time steps, where is your specified Average Over value. When the iteration/time step number is lower than , Fluent calculates the average of the available variable values.

Retain Instantaneous Values

appears when Average Over is set to a value greater than 1. If enabled when you are creating a new report definition, it ensures that all instantaneous values are saved in the new report file that is being created for this report definition. It also results in the Plot Instantaneous Values option being enabled in the newly created report plot.

Force Vector

contains the components of the force vector.

X,Y,Z

are the components of the force vector along which the forces will be computed.

Report Files

lists all of the report files where you can write the report definition data.

Report Plots

lists all of the report plots where you can plot the report definition data (assuming this report has the same units as the other report definitions included in the selected report plot).

Create

options you can choose while generating a report.

Report File

creates a new report file that includes this report definition.

Report Plot

creates a new report plot that includes this report definition.

Frequency

specifies how frequently the report definition is written, plotted, or printed to the console.

Print to Console

prints the value of the report definition to the console.

Create Output Parameter

creates an output parameter for this report definition with the name <report definition name>-op.

Report Output Type

options you can choose relevant to report output.

Drag Coefficient

specifies the report definition as a unitless quantity.

Drag Force

specifies that the report definition has units of force.

Zones

lists the zones you can select for drag coefficient or drag force computation.

OK

creates the report definition.

Compute

computes the value of the report definition at the selected zone(s) and prints to the console.

Display Type

contains options for the different items you can display.

Cluster

specifies the display of clusters.

Ray

specifies the display of rays.

Options

contains check buttons that control display options.

Draw Mesh

toggles between displaying and not displaying the mesh. The Mesh Display Dialog Box is opened when Draw Mesh is selected.

Cluster Type

specifies whether Surface clusters or Volume clusters are to be displayed. This section of the dialog box appears when Cluster is selected as the Display Type.

Cluster Selection

contains options for cluster displays. This section of the dialog box appears when Cluster is selected as the Display Type.

Display All Clusters

enables the display of all surface or volume clusters in the domain.

Ray Parameters

contains controls for displaying rays. This section of the dialog box appears when Ray is selected as the Display Type.

Theta Divisions, Phi Divisions

control the number of rays being traced. (See Controlling the Rays.)

Nearest Point

specifies a point (X,Y,Z) near the cluster to be displayed (or the cluster from which the rays should start).

The Nearest Point controls are not available when Display All Clusters is selected under Cluster Selection.

Select Point With Mouse

is an alternative method for specifying the Nearest Point using your mouse, by clicking the button.

Display

displays the specified cluster(s) or rays.

Clustering

contains parameters for the clusters (see Clustering in the Theory Guide).

Cells Per Volume Cluster, Faces Per Surface Cluster

control the number of radiating surfaces and absorbing cells. (See the explanation in Controlling the Clusters.)

Angular Discretization

contains parameters for the ray traces (see Ray Tracing in the Theory Guide).

Theta Divisions, Phi Divisions

control the number of rays being traced. (Guidelines are provided in Controlling the Rays.)

Display Clusters

generates a graphical display of the clusters in the domain. (This item is available only after you have created or read a ray file.)

Gap Definition

contains input controls for editing an existing gap region.

Gap Name

specifies the name of the gap region. It cannot consist solely of numbers.

Face Zones

allows you to select the two or more face zones that constitute the gap region.

Proximity Threshold

defines the maximum distance between the face zones when flow blockage / deceleration occurs in the gap.

Gap Type

defines the type of the gap region. A Flow-Blocking type completely blocks the flow in the gap region, as a numerical zero-mass-flux boundary condition is applied at the boundary faces of the marked region so that the marked cells no longer participate in the solution. A Flow-Modeling type decelerates the flow in the cells of the marked region by manipulating the viscosity or source terms.

Method

defines the method used to scale the viscosity or to define source terms in the gap region. The Sponge Layer method specifies that the viscosity inside the gap regions is scaled based on the specified Gap Reynolds Number. The User-Defined Source method specifies the use of a compiled user-defined function (UDF) to define the source terms for the momentum and energy equations in the gap region. This drop-down list is only available when Flow-Modeling is selected for the Gap Type.

Resistance Type

specifies how the viscosity is scaled in the gap region. The Fictitious Viscosity approach scales the laminar viscosity inside the gap region during discretization of the viscous forces for the momentum equation; thus, its impact is explicitly seen in the velocity and pressure computation, and it has an implicit effect on the other solution fields through the changes in the velocity and pressure field. The Real Viscosity approach changes the actual laminar viscosity inside the gap region based on your specified Gap Reynolds Number; therefore, the effect of modeling will be seen not only in flow equation but also in other equations. This drop-down list is only available when Flow-Modeling is selected for the Gap Type and Sponge Layer is selected for the Method.

Gap Reynolds Number

defines the intended Reynolds number in the gap region, and thus determines the level of sealing. A lower Gap Reynolds Number results in better sealing. It can be estimated according to Equation 6–4. This drop-down list is only available when Flow-Modeling is selected for the Gap Type and Sponge Layer is selected for the Method.

Gap Source Terms

selects a compiled user-defined function (UDF) that specifies the source terms for the momentum and energy equations in the gap region using the DEFINE_GAP_MODEL_SOURCE macro. This drop-down list is only available when Flow-Modeling is selected for the Gap Type and User-Defined Source is selected for the Method.

Exclude Cell Zones

enables the ability to specify that cells in particular cell zones are not marked for flow blockage / deceleration as part of the gap region, in order to have greater control over the shape of the gap region.

Excluded Cell Zones

selects the cell zones in which cells are not marked for flow blockage / deceleration as part of the gap region.

Mesh Interfaces

allows you to select the mesh interfaces you would like to edit. Note that you can click the   button to group the interfaces in the list by their currently enabled interface option(s), which allows you to select / deselect all those of a particular type by simply clicking the top-level branch.

Interface Name

edits the name of the mesh interface. This is only available when a single interface is selected.

Interface Options

contains options related to the interface type. These options can be applied when a single or multiple interfaces are selected.

Periodic Boundary Condition

allows you to create a non-conformal periodic boundary condition interface.

Periodic Repeats

should be enabled when each of the two cell zones has a single pair of conformal or non-conformal periodics adjacent to the interface. This option is typically used in conjunction with the sliding mesh model, when simulating the interface between a rotor and stator; it allows Ansys Fluent to treat the interface between the sliding and non-sliding zones as periodic where the two zones do not overlap. For details, see The Periodic Repeats Option.

Coupled Wall

allows you to specify that the interface acts as a thermally coupled wall.

Matching

is relevant if only interface internal zones should be created (that is, interior or wall / shadow pairs), since the interface zones on both sides are aligned. With the Matching option, even interface zones that are not perfectly aligned are treated as if they are; however, if the discrepancy between the interface zones on both sides exceeds default thresholds, then warning messages will be displayed. Note that the Matching option is compatible with the Periodic Boundary Condition, Coupled Wall, and Static options. For more information about the recommended uses of this option, see Matching Option.

Mapped

enables an alternative approach for modeling coupled walls between zones. This approach is more robust than the standard non-conformal interface formulations when the interface zones penetrate each other or have gaps between them. It requires that at least one side of the interface consists of only solid zones.

---

Note:  The Mapped option is not compatible with shell conduction.

---

Static

reduces the memory usage and processing time (for interface creation and solution), especially when there are many zones on both sides of the interface. This option will only produce correct results if the interface zones do not move or deform relative to each other at the interface, and it is not compatible with the Periodic Boundary Condition, Periodic Repeats, or Mapped options.

Periodic Boundary Conditions

Type

allows you to select a periodicity that is either Translational or Rotational.

Offset

is the offset coordinates or angle, depending on whether Translational or Rotational periodicity is selected. Note that when Auto Compute Offset is enabled, the Offset fields are not editable.

Auto Compute Offset

will result in Ansys Fluent finding the offset. If this option is disabled, then you will have to provide the offset coordinates or angle in the required fields, depending on whether Translational or Rotational periodicity is selected.

Mapped

Enable Local Tolerance

(when enabled) allows you to overwrite any value specified in the Tolerance group box in the Mapped Interface Options Dialog Box, and is applied to the selected interface only.

Local Edge Length Factor

(when enabled) allows you to specify the multiplier that Fluent uses with the smallest edge length of the interface zones to calculate the tolerance for mapping. Disabling Local Edge Length Factor allows you to specify an absolute value for the tolerance.

Interface Zones

highlights the list of interface zones that make up the selected mesh interface and allows you to edit the list (provided that the zones you select are unassigned and located appropriately). This functionality is only available when a single interface is selected.

List

prints information in the console about the first mesh interface you selected. When you click this button, Ansys Fluent will list the interface boundaries and (if you have initialized the solution) all new zones that were created (that is, wall and interior zones).

Apply

saves the revised settings for the selected mesh interfaces.

Name

editable field displaying the name of the report file.

Active

check box (enabled by default) that determines if the file is written during the solution calculation.

Available Report Definitions

lists all of the existing report definitions not currently part of this report file.

Add>>

moves the selected report definition(s) to the Selected Report Definitions list.

<<Remove

moves the selected report definition(s) to the Available Report Definitions list.

File Name

allows you to specify the name used when the file is saved.

Browse...

opens the Select File dialog box, allowing you to specify the location where the report file will be saved.

Full File Name

displays the name and location of the report file once it has been saved. You can use the keyboard arrow keys to scroll within this field (<, >).

Get Data Every

indicates the frequency that the report definition data is written to the file. The default value of 1 allows you to write to the file at every iteration or time-step. If you select flow-time, then you must specify the frequency for writing the file in units of time. Time-step and flow-time are only a valid choices when you are calculating unsteady flow.

Print to Console

indicates whether or not the contents of the report file are printed to the console at the frequency specified in the Get Data Every field.

Selected Report Definitions

lists all of the existing report definitions currently included in this report file.

New

drop-down list allowing you to create new report definitions (surface, volume, force, flux, mesh, aeromechanics, dpm, expression, and user-defined).

Edit...

allows you to modify the highlighted report definition in the Selected Report Definition list.

Name

editable field displaying the name of the report plot.

Active

check box (enabled by default) that determines if the plot is plotted during the solution calculation.

Available Report Definitions

lists all of the existing report definitions not currently part of this report plot.

Add>>

moves the selected report definition(s) to the Selected Report Definitions list.

<<Remove

moves the selected report definition(s) to the Available Report Definitions list.

Options

Get Data Every

indicates the frequency that the report definition data is plotted. The default value of 1 allows you to write to the file at every iteration or time-step. If you select flow-time, then you must specify the frequency for plotting the data in units of time. Time-step and flow-time are only a valid choices when you are calculating unsteady flow.

Plot Title

provide a title for the plot.

X-Axis Label

choose whether the X-axis is flow-time or time-step.

Y-Axis Label

enter a label for the Y-axis.

Print to Console

indicates whether or not the contents of the report plot are printed to the console at the frequency specified in the Get Data Every field.

Selected Report Definitions

lists all of the existing report definitions currently included in this report plot.

New

drop-down list allowing you to create new report definitions (surface, volume, force, flux, mesh, aeromechanics, dpm, expression, and user-defined).

Edit...

allows you to modify the highlighted report definition in the Selected Report Definition list.

Curves...

opens the Curves Dialog Box.

Axes...

opens the Axes Dialog Box.

Execute on Demand

selects the user-defined function to be run.

Execute

runs the selected function.

Name

an editable field allowing you to name the expression. The Name field is not editable when the expression is in use.

Definition

displays the formula of the expression as you create it.

Current Value

Displays the current value of the expression.

Refresh Current Value  

Evaluates the expression and updates the Current Value field.

Details

This tab contains the optional description of the expression, as well as where the expression is used, and the options to set the expression as an input or output parameter.

Description

(Optional) allows you to provide more of a description of this expression beyond the name.

Used In

lists the locations where the expression is used.

Use as Input Parameter

allows you to define the expression as an input parameter.

Use as Output Parameter

allows you to define the expression as an output parameter.

Plot

This tab allows you to plot your expression to visualize and confirm its behavior.

Primary Independent Variable

allows you to select which variable is the independent variable.

Count

allows you to specify the number of plot points.

Min

sets the minimum value for the independent variable.

Max

sets the maximum value for the independent variable.

Secondary Independent Variable

allows you to select the secondary independent variable.

Curves

allows you to specify the number of lines or curves to include in the plot.

Min

sets the minimum value for the secondary independent variable.

Max

sets the maximum value for the secondary independent variable.

Copy to Clipboard

copies the current plot onto your clipboard.

Reset Zoom

resets to the default zoom. You can click and drag in the plot to change the zoom level.

Functions

lists the available functions (conditional, mathematical, and so on) that are available for constructing your expression.

Variables

lists all of the supported variables.

Cell Registers

lists the defined cell registers.

Constants

lists the available pre-defined constants.

Expressions

lists the defined expressions.

Report Definitions

lists the defined report definitions.

Locations

lists the available locations that you can include in your expression volume definition.

Current Value

Displays the current value of the expression.

Refresh Current Value  

Evaluates the expression and updates the Current Value field.

Primary Independent Variable

allows you to select which variable is the independent variable.

Count

allows you to specify the number of plot points.

Min

sets the minimum value for the independent variable.

Max

sets the maximum value for the independent variable.

Secondary Independent Variable

allows you to select the secondary independent variable.

Curves

allows you to specify the number of lines or curves to include in the plot.

Min

sets the minimum value for the secondary independent variable.

Max

sets the maximum value for the secondary independent variable.

Copy to Clipboard

copies the current plot onto your clipboard.

Reset Zoom

resets to the default zoom. You can click and drag in the plot to change the zoom level.

Functions

lists the available functions (conditional, mathematical, and so on) that are available for constructing your expression.

Variables

lists all of the supported variables.

Cell Registers

lists the defined cell registers.

Constants

lists the available pre-defined constants.

Expressions

lists the defined expressions.

Report Definitions

lists the defined report definitions.

Locations

lists the available locations that you can include in your expression volume definition.

Expression

Lists the defined named expressions.

Properties

Lists the properties of the selected expression in the Expression list. This list is blank when no expressions are selected or when more than one expression is selected.

New...

Opens the Expression Dialog Box, allowing you to create a new named expression.

Edit...

(Only available when a single expression is selected) Opens the Expression Dialog Box, allowing you to edit the selected expression.

Copy...

(Only available when a single expression is selected) Opens the Expression Dialog Box with the same definition as the selected expression. The Name field is automatically appended with a digit, but you may modify the name, if desired.

Delete

Deletes the selected expression(s). Note that some expressions cannot be deleted if they are included in the definitions of other expressions or if they are in use elsewhere in Fluent.

List

Prints the definition and description of all named expressions to the console.

Compute

Computes the value of the selected expression(s) and prints the value(s) to the console.

Import...

Opens the Select File dialog box so that you can read-in one or more expressions from a file.

Export...

Opens the Select File dialog box so that you can export the selected expression(s) to a file.

Name

an editable field allowing you to name the expression. The Name field is not editable when the expression is in use.

Definition

displays the formula of the expression as you create it.

Current Value

Displays the current value of the expression.

Refresh Current Value  

Evaluates the expression and updates the Current Value field.

Average Over

(optional) To have Fluent calculate a running average for the Expression Report Definition you can enter a positive integer greater than 1 (the default) for Average Over.

Specifying a number greater than 1 means that Fluent will print, plot, and write the running average value of the selected variable instead of the current value of the same variable.

The value reported is averaged over the last iterations/time steps, where is your specified Average Over value. When the iteration/time step number is lower than , Fluent calculates the average of the available variable values.

Retain Instantaneous Values

appears when Average Over is set to a value greater than 1. If enabled when you are creating a new report definition, it ensures that all instantaneous values are saved in the new report file that is being created for this report definition. It also results in the Plot Instantaneous Values option being enabled in the newly created report plot.

Report Files

lists all of the report files where you can write the report definition data.

Report Plots

lists all of the report plots where you can plot the report definition data (assuming this report has the same units as the other report definitions included in the selected report plot).

Create

Report File

creates a new report file that includes this report definition.

Report Plot

creates a new report plot that includes this report definition.

Frequency

specifies how frequently the report definition is written, plotted, or printed to the console.

Print to Console

prints the value of the report definition to the console.

Create Output Parameter

creates an output parameter for this report definition with the name <report definition name>-op.

Compute

prints the value of the expression report definition to the Console.

Functions

lists the available functions (conditional, mathematical, and so on) that are available for constructing your expression.

Variables

lists all of the supported variables.

Cell Registers

lists the defined cell registers.

Constants

lists the available pre-defined constants.

Expressions

lists the defined expressions.

Report Definitions

lists the defined report definitions.

Locations

lists the available locations that you can include in your expression report definition.

Name

an editable field allowing you to name the expression volume.

Definition

displays the formula of the expression volume as you create it.

Create

creates the expression volume.

Save

saves the changes you made to an existing expression volume.

Functions

lists the available functions (conditional, mathematical, and so on) that are available for constructing your expression.

Variables

lists all of the supported variables.

Cell Registers

lists the defined cell registers.

Constants

lists the available pre-defined constants.

Expressions

lists the defined expressions.

Report Definitions

lists the defined report definitions.

Locations

lists the available locations that you can include in your expression volume definition.

Name

specifies the name of the report definition.

Options

Per Surface

enables the reporting of the face count individually for each of the selected zones (rather than reporting the sum from all of the selected zones).

Average Over

specifies the number of iterations / time steps over which the face count is averaged when written, plotted, and/or printed. The default value of 1 means that no averaging is performed (that is, only the current face count is reported), and higher values yields a running average. When the iteration / time step number is lower than the specified value, Fluent calculates the average of the available face count values.

Retain Instantaneous Values

enables the retention of instantaneous values in any report file definition or report plot definition that is associated with this report definition. This option is only available if Average Over is set to a value greater than 1.

Report Files

allows you to select existing report file definitions to which you want to write face count data from this report definition.

Report Plots

allows you to select existing report plot definitions to which you want to include face count data from this report definition. Note that the units used in these report plots may not be suitable for the face count data.

Create

Report File

creates a new report file definition for the data from this report definition.

Report Plot

creates a new report plot definition for the data from this report definition.

Frequency

specifies how frequently the report definition is written, plotted, and/or printed to the console.

Print to Console

enables the printing of the face count data from this report definition to the console during the calculation.

Create Output Parameter

creates an output parameter for this report definition with the name <report_definition_name>-op.

Face Zones

allows you to select the face zones for which you want to report the number of faces.

OK

creates / saves the report definition.

Compute

computes the face count within the selected zone(s) and prints to the console.

Definition

displays the function selected in the Field Functions list. This display is for informational purposes only; you cannot edit it.

Field Functions

contains a selectable list of custom field functions. When you select a function, its definition will appear in the Definition box and its name will appear in the Name text entry box.

Name

displays the name of the currently selected field function. You can enter a new name in this box if you want to rename the function.

ID

reports the ID number of the selected function. The field function at the top of the list has an ID of 0, the second function has an ID of 1, and so on.

Rename

changes the name of the selected function to the name specified in the Name text entry box.

Delete

deletes the selected field function.

Save...

opens The Select File Dialog Box, where you can specify a file in which to save all of the functions in the Field Functions list.

Load...

opens the Select File dialog box, where you can specify a file from which to read custom field functions (that is, a file that you saved using the Save... button above).

Name

specifies the name of the report definition.

Options

Mass Flow Rate

specifies that the mass flow rate is computed for the selected boundary zones.

Total Heat Transfer Rate

specifies that the total heat transfer rate is computed for the selected boundary zones.

Total Sensible Heat Transfer Rate

specifies that the total sensible heat transfer rate is computed for the selected boundary zones. It reports the total energy flux as defined in Equation 5–5 in the Theory Guide.

Radiation Heat Transfer Rate

specifies that the radiation heat transfer rate is computed for the selected boundary zones.

Pressure Work Rate

specifies that the pressure work rate is computed for the selected boundary zones. This rate is the energy transfer due to pressure when a fluid zone undergoes normal zone motion relative to an adjacent solid zone (for further details, see Equation 25–1 in the Theory Guide). This pressure work is on the fluid side only, not on the solid side. This option is only available when the energy equation is enabled, the absolute velocity formulation is selected, and the Frame Motion and/or Mesh Motion option is enabled in the Fluid dialog box.

Viscous Work Rate

specifies that the viscous work rate is computed for the selected boundary zones, which is the integral of the product of viscous stress with velocity over the external boundary of the domain with the boundary normal directed inside (for further details, see Equation 25–2 in the Theory Guide). Note that after reading case and data files into Ansys Fluent, the viscous work rate is zero. You need to run at least one iteration or time step to obtain the viscous work rate value. This item is available only when the energy equation is enabled and the pressure-based solver is selected.

Film Mass Flow Rate

(available only when the Eulerian wall film model is enabled) specifies that the mass flow rate is computed for the selected boundary zone(s).

Film Heat Transfer Rate

(available only when the Eulerian wall film model is enabled) specifies that the film heat transfer rate is computed for the selected boundary zone(s).

Phase

contains a list of all of the phases in the problem that you have defined. This is available when the VOF, mixture, or Eulerian multiphase model is enabled.

Per Zone

specifies whether or not the chosen field variable is calculated from all of the selected boundary zones combined (default) or individually on each of the selected boundary zones.

Average Over (Time-Steps), Average Over (Iterations)

(optional) To have Fluent calculate a running average for the Flux Report Definition you can enter a positive integer greater than 1 (the default) for Average Over.

Specifying a number greater than 1 means that Fluent will print, plot, and write the running average value of the selected variable instead of the current value of the same variable.

The value reported is averaged over the last iterations/time steps, where is your specified Average Over value. When the iteration/time step number is lower than , Fluent calculates the average of the available variable values.

Retain Instantaneous Values

appears when Average Over is set to a value greater than 1. If enabled when you are creating a new report definition, it ensures that all instantaneous values are saved in the new report file that is being created for this report definition. It also results in the Plot Instantaneous Values option being enabled in the newly created report plot.

Report Files

lists all of the report files where you can write the report definition data.

Report Plots

lists all of the report plots where you can plot the report definition data (assuming this report has the same units as the other report definitions included in the selected report plot).

Create

Report File

creates a new report file that includes this report definition.

Report Plot

creates a new report plot that includes this report definition.

Frequency

specifies how frequently the report definition is written, plotted, or printed to the console.

Print to Console

prints the value of the report definition to the console.

Create Output Parameter

creates an output parameter for this report definition with the name <report definition name>-op.

Report Type

selects the integration method used on the selected cell zones. The available report types are the same as those in the Volume Integrals Dialog Box. See Volume Integration for details.

Boundaries

contains a selectable list of valid boundary zones for flux reporting.

OK

creates the report definition.

Compute

computes the value of the report definition at the selected zone(s) and prints to the console.

Name

specifies the name of the report definition.

Options

Per Zone

specifies whether or not the force for multiple walls zones should be monitored on each wall zone separately. When this option is turned off (the default), Fluent computes and monitors the total force for all of the selected walls zones combined together.

Average Over (Time-Steps), Average Over (Iterations)

(optional) To have Fluent calculate a running average for the Force Report Definition you can enter a positive integer greater than 1 (the default) for Average Over.

Specifying a number greater than 1 means that Fluent will print, plot, and write the running average value of the selected variable instead of the current value of the same variable.

The value reported is averaged over the last iterations/time steps, where is your specified Average Over value. When the iteration/time step number is lower than , Fluent calculates the average of the available variable values.

Retain Instantaneous Values

appears when Average Over is set to a value greater than 1. If enabled when you are creating a new report definition, it ensures that all instantaneous values are saved in the new report file that is being created for this report definition. It also results in the Plot Instantaneous Values option being enabled in the newly created report plot.

Force Vector

contains the components of the force vector.

X,Y,Z

are the components of the force vector along which the forces will be computed.

Report Files

lists all of the report files where you can write the report definition data.

Report Plots

lists all of the report plots where you can plot the report definition data (assuming this report has the same units as the other report definitions included in the selected report plot).

Create

Report File

creates a new report file that includes this report definition.

Report Plot

creates a new report plot that includes this report definition.

Frequency

specifies how frequently the report definition is written, plotted, or printed to the console.

Print to Console

prints the value of the report definition to the console.

Create Output Parameter

creates an output parameter for this report definition with the name <report definition name>-op.

Zones

lists the zones you can select for force computation.

OK

creates the report definition.

Compute

computes the value of the report definition at the selected zone(s) and prints to the console.