6.2.1. Fluid Conditions

A fluid zone is a group of cells for which all active equations are solved. The only required input for a fluid zone is the type of fluid material. You must indicate which material the fluid zone contains so that the appropriate material properties will be used.


Important:  If you are modeling multiphase flow, you will not specify the materials here; you will choose the phase material when you define the phases, as described in Defining the Phases for the VOF Model.



Important:  If you are modeling species transport and/or combustion, you can specify the material as either a mixture or a fluid. The mixture material has to be the same as that specified in the Species Model dialog box when you enable the model. The fluid zones, being of different material types, must not be contiguous.


Optional inputs allow you to set sources or fixed values of mass, momentum, heat (temperature), turbulence, species, and other scalar quantities. You can also define motion for the fluid zone. If there are rotationally periodic boundaries adjacent to the fluid zone, you must specify the rotation axis. If you are modeling turbulence using one of the -  models, the -  model, or the Spalart-Allmaras model, you can choose to define the fluid zone as a laminar flow region. If you are modeling radiation using the DO model, you can specify whether or not the fluid participates in radiation.

Warning:  In general, disabling Participates in Radiation for fluid zones is not recommended, as it can produce erroneous results. There are rare cases when it is acceptable: for example, if the domain contains multiple fluid zones, disabling this option for zones where radiation is negligible may save computational time without affecting the results.


Important:  For information about porous zones and 3D fan zones, see Porous Media Conditions and 3D Fan Zones, respectively.


6.2.1.1. Inputs for Fluid Zones

You will set all fluid conditions in the Fluid Dialog Box (Figure 6.8: The Fluid Dialog Box), which is accessed from the Cell Zone Conditions task page (as described in Setting Cell Zone and Boundary Conditions).

Figure 6.8:  The Fluid Dialog Box

The Fluid Dialog Box

6.2.1.1.1. Defining the Fluid Material

To define the material contained in the fluid zone, select the appropriate item in the Material Name drop-down list. This list will contain all fluid materials database) in the Create/Edit Materials Dialog Box. If you want to check or modify the properties of the selected material, you can click Edit... to open the Edit Material dialog box; this dialog box contains just the properties of the selected material, not the full contents of the standard Create/Edit Materials dialog box.


Important:  If you are modeling species transport or multiphase flow, the Material Name list will not appear in the Fluid dialog box. For species calculations, the mixture material for all fluid zones will be the material you specified in the Species Model Dialog Box. For multiphase flows, the materials are specified when you define the phases, as described in Defining the Phases for the VOF Model.


6.2.1.1.2. Defining Sources

If you want to define a source of heat, mass, momentum, turbulence, species, or other scalar quantity within the fluid zone, you can do so by enabling the Source Terms option. See Defining Mass, Momentum, Energy, and Other Sources for details.

6.2.1.1.3. Defining Fixed Values

If you want to fix the value of one or more variables in the fluid zone, rather than computing them during the calculation, you can do so by enabling the Fixed Values option. See Fixing the Values of Variables for details.

6.2.1.1.4. Specifying a Laminar Zone

When you are calculating a turbulent flow, it is possible to “turn off” turbulence modeling in a specific fluid zone. To disable turbulence modeling, turn on the Laminar Zone option in the Fluid dialog box. This is useful if you know that the flow in a certain region is laminar. For example, if you know the location of the transition point on an airfoil, you can create a laminar/turbulent transition boundary where the laminar cell zone borders the turbulent cell zone. This feature allows you to model turbulent transition on the airfoil.

By default, the Laminar Zone option will set the turbulent viscosity, , to zero and disable turbulence production in the fluid zone. Turbulent quantities will still be transported through the zone, but effects on fluid mixing and momentum will be ignored. If you want to keep the turbulent viscosity, you can do so using the text command define/ boundary-conditions/fluid. You will be asked if you want to Set Turbulent Viscosity to zero within laminar zone?. If your response is no, ANSYS Fluent will set the production term in the turbulence transport equation to zero, but will retain a nonzero .

Disabling turbulence modeling in a fluid zone can be applied to all the turbulence models except the Large Eddy Simulation (LES) model.

6.2.1.1.5. Specifying a Reaction Mechanism

If you are modeling species transport with reactions, you can enable a reaction mechanism in a fluid zone by turning on the Reaction option and selecting an available mechanism from the Reaction Mechanism drop-down list. See Defining Zone-Based Reaction Mechanisms for more information about defining reaction mechanisms.

6.2.1.1.6. Specifying the Rotation Axis

If there are rotationally periodic boundaries adjacent to the fluid zone or if the zone is rotating, either the mesh or its reference frame, you must specify the rotation axis. To define the axis for a moving reference frame problem, set the Rotation-Axis Direction and Rotation-Axis Origin under the Reference Frame tab. To define the axis for a moving mesh problem, set the Rotation-Axis Direction and Rotation-Axis Origin under the Mesh Motion tab.


Note:  If a frame motion and a mesh motion are specified at the same zone and this zone has rotationally periodic boundaries adjacent to it, then both axes have to be coaxial. Otherwise, the periodicity assumption is not valid and you will receive a warning message. In addition, the mesh check will fail.


The cell zone axis is independent of the axis of rotation used by any adjacent wall zones or any other cell zones. For 3D problems, the axis of rotation is the vector from the Rotation-Axis Origin in the direction of the vector given by your Rotation-Axis Direction inputs for the frame of reference and the mesh motion. For 2D non-axisymmetric problems, you will specify only the Rotation-Axis Origin; the axis of rotation is the -direction vector passing through the specified point. (The direction is normal to the plane of your geometry so that rotation occurs in the plane.) For 2D axisymmetric problems, you will not define the axis: the rotation will always be about the axis, with the origin at (0,0).

6.2.1.1.7. Defining Zone Motion

To define zone motion for a moving reference frame (MRF), enable the Frame Motion option in the Fluid dialog box. Set the appropriate parameters in the expanded portion of the dialog box, under the Reference Frame tab.

To define zone motion for a moving (sliding) mesh, enable the Mesh Motion option in the Fluid dialog box. Set the appropriate parameters in the expanded portion of the dialog box, under the Mesh Motion tab. See Setting Up the Sliding Mesh Problem for details.

For cases that do not contain zones with motion specified in a relative frame to another zone, select absolute from the Relative To Cell Zone drop-down list. Here, the velocity and rotation components are specified in an absolute reference frame, which is the default setting, as shown in Figure 6.9: Rotation Specified in the Absolute Reference Frame. If no moving zones are present in the simulation, then absolute will be the only available selection. See The Multiple Reference Frame Model for more information.

Figure 6.9:  Rotation Specified in the Absolute Reference Frame

Rotation Specified in the Absolute Reference Frame

For cases where you have a moving zone specified relative to another moving zone, select the cell zone carrying the primary motion from the Relative To Cell Zone drop-down list under the Reference Frame tab or the Mesh Motion tab. Note that for such cases, Rotation-Axis Origin (Relative) will appear in the interface, signifying coordinates relative to the zone selected from the Relative To Cell Zone drop-down list.

Figure 6.10: Rotation Specified Relative to a Moving Zone illustrates that the rotational axis origin of the small rotating zone is specified relative to the cell zone carrying the primary motion (having local coordinate system ).

Figure 6.10:  Rotation Specified Relative to a Moving Zone

Rotation Specified Relative to a Moving Zone


Note:  The Relative To Cell Zone list will consist of all moving cell zones with an absolute motion specification (that is zones that are moving, but their motion is not relative to some other zone), excluding the current cell zone.


For problems that include linear, translational motion of the fluid zone, specify the Translational Velocity by setting the X, Y, and Z components under the Mesh Motion tab. For problems that include rotational motion, specify the rotational Speed under Rotational Velocity. The rotation axis is defined as described above. Note that the speed can be specified as a constant value or a transient profile. The transient profile may be in a file format, as described in Defining Transient Cell Zone and Boundary Conditions, or a UDF macro (DEFINE_TRANSIENT_PROFILE). Specifying the individual velocities as either a profile or a UDF allows you to specify a single component of the frame motion individually. However, you can also specify the frame motion using a user-defined function. This may prove to be quite convenient if you are modeling a more complicated motion of the moving reference frame, where the hooking of many different user-defined functions or profiles can be cumbersome.


Important:  If you need to switch between the MRF and moving mesh models, simply click the Copy To Mesh Motion for zones with a moving frame of reference and Copy to Frame Motion for zones with moving meshes to transfer motion variables, such as the axes, frame origin, and velocity components between the two models. The variables used for the origin, axis, and velocity components, as well as for the UDF DEFINE_ZONE_MOTION will be copied. This is particularly useful if you are doing a steady-state MRF simulation to obtain an initial solution for a transient Moving Mesh simulation in a turbomachine.


See Modeling Flows with Moving Reference Frames for details about modeling flows in moving reference frames. Details about the frame motion UDF can be found in DEFINE_ZONE_MOTION in the Fluent Customization Manual.

6.2.1.1.8. Defining Radiation Parameters

If you are using the DO radiation model, you can specify whether or not the fluid zone participates in radiation using the Participates in Radiation option. See Defining Boundary Conditions for Radiation for details.


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