9.3.4. Setting Up a Multiple Moving Reference Frame Problem

To learn more about setting up a multiple reference frame problem, see the following sections:

9.3.4.1. Setting Up Multiple Reference Frames

To model a problem involving multiple reference frames, perform the following:


Important:  The mesh-setup constraints for a moving reference frame listed in Mesh Setup for a Single Moving Reference Frame apply to multiple reference frames as well.


  1. Select the Velocity Formulation to be used in the General Task Page: either Absolute or Relative. (For details, see Choosing the Relative or Absolute Velocity Formulation.)

     Setup →   General

    (Note that this step is irrelevant if you are using one of the density-based solution algorithms; these algorithms always use an absolute velocity formulation.)

  2. For each cell zone in the domain, specify its translational velocity and/or its angular velocity () and the axis about which it rotates.

     Setup →   Cell Zone Conditions

    1. If the zone is moving, or if you plan to specify cylindrical velocity or flow-direction components at inlets to the zone, you must define the axis of rotation of the frame of reference. In the Fluid or Solid dialog box, specify the Rotation-Axis Origin and Rotation-Axis Direction under the Reference Frame tab.

    2. In the Fluid (Figure 9.4: The Fluid Dialog Box Displaying Frame Motion Inputs) or Solid dialog box, enable the Frame Motion option. Set the Speed under Rotational Velocity and/or the X, Y, and Z components of the Translational Velocity in the expanded portion of the dialog box under the Reference Frame tab.

      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, described in DEFINE_TRANSIENT_PROFILE. Specifying the individual velocities as either a profile or a UDF allows you to specify a specific input of the frame motion individually. However, you can also specify the frame motion inputs via a single user-defined function that uses the UDF macro DEFINE_ZONE_MOTION. 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.


      Note:  If you decide to hook a UDF, then you will no longer have access to the rotation axis origin and direction, or the velocities.


      Details about these inputs are presented in Inputs for Fluid Zones and in Inputs for Solid Zones. Details about the zone motion UDF can be found in DEFINE_ZONE_MOTION in the Fluent Customization Manual.

    3. To switch between the MRF and moving mesh models, 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.

  3. Define the velocity boundary conditions at walls. You can choose to define either an absolute velocity or a velocity relative to the velocity of the adjacent cell zone specified in step 2.

    If the wall is moving at the speed of the moving frame (and hence stationary relative to the moving frame), it is convenient to specify a relative angular velocity of zero. Likewise, a wall that is stationary in the non-moving frame of reference should be given a velocity of zero in the absolute reference frame. Specifying the wall velocities in this manner obviates the need to modify these inputs later if a change is made in the rotational velocity of the fluid zone.

    An example for which you would specify a relative velocity is as follows: If an impeller is defined as wall-3 and the fluid region within the impeller’s radius is defined as fluid-5, you would need to specify the angular velocity and axis of rotation for fluid-5 and then assign wall-3 a relative velocity of 0. If you later wanted to model a different angular velocity for the impeller, you would need to change only the angular velocity of the fluid region; you would not need to modify the wall velocity conditions.

    Details about these inputs are presented in Velocity Conditions for Moving Walls.

  4. Define the boundary conditions at the inlets, as described in Boundary Conditions. For velocity inlets, you can choose to define either absolute velocities or velocities relative to the motion of the adjacent cell zone (specified in step 2). Likewise, the total pressure and flow direction can be prescribed in absolute or relative frames for pressure inlets.

    Details about these inputs are presented in Defining the Flow Direction and Defining the Velocity.

  5. Define the mesh interfaces using the Mesh Interfaces Dialog Box (Figure 10.10: The Mesh Interfaces Dialog Box).

     Setup → Mesh Interfaces New...

    To learn how to use the Mesh Interfaces dialog box, see Using a Non-Conformal Mesh in ANSYS Fluent.

  6. Initialize the solution using an absolute frame of reference (Figure 9.8: The Solution Initialization Task Page for Moving Reference Frames).

     Solution →   Initialization

    Select the Absolute option under Reference Frame. If the Relative to Cell Zone option is selected, the initial flow field can contain discontinuities, which can cause convergence problems in the first few iterations.

    Figure 9.8:  The Solution Initialization Task Page for Moving Reference Frames

    The Solution Initialization Task Page for Moving Reference Frames

9.3.4.2. Setting Up the Mixing Plane Model

The model inputs for mixing planes are presented in this section. Only those steps relevant specifically to the setup of a mixing plane problem are listed here. Note that the use of wall and periodic boundaries in a mixing plane model is consistent with their use when the model is not active.

  1. Select the Absolute or Relative Velocity Formulation in the General Task Page, when the pressure-based solver is enabled.

     Setup →   General


    Important:  When the density-based solver is enabled, only the Absolute Velocity Formulation can be used with the mixing plane model.


  2. For each cell zone in the domain, specify its angular velocity () and the axis about which it rotates.

     Setup →   Cell Zone Conditions

    1. If the zone is rotating, or if you plan to specify cylindrical-velocity or flow-direction components at inlets to the zone, you must define the axis of rotation for the frame of reference. In the Fluid dialog box or Solid Dialog Box, specify the Rotation-Axis Origin and Rotation-Axis Direction under the Reference Frame tab.

    2. In the Fluid (Figure 9.4: The Fluid Dialog Box Displaying Frame Motion Inputs) or Solid dialog box, enable the Frame Motion option and then set the Speed under Rotational Velocity and/or the X, Y, and Z components of the Translational Velocity in the expanded portion of the dialog box under the Reference Frame tab.


    Important:  It is important to define the axis of rotation for the cell zones on both sides of the mixing plane interface, including the stationary zone.


  3. Define the velocity boundary conditions at walls, as described in step 3 of Setting Up Multiple Reference Frames.

  4. Define the boundary conditions at the inlets, as described in Boundary Conditions. For velocity inlets, you can choose to define either absolute velocities or velocities relative to the motion of the adjacent cell zone (specified in step 2). For pressure inlets and mass-flow inlets, the specification of the flow direction and total pressure will always be absolute, because the absolute velocity formulation is always used for mixing plane calculations. For a mass-flow inlet, you do not need to specify the mass flow rate or mass flux. ANSYS Fluent will automatically select the Mass Flux with Average Mass Flux specification method and set the correct values when you create the mixing plane, as described in More About Mass Flux and Average Mass Flux.

    Details about these inputs are presented in Defining the Flow Direction, Defining the Velocity, and Inputs at Mass-Flow Inlet Boundaries.


    Important:  Note that the outlet boundary zone at the mixing plane interface must be defined as a pressure outlet, and the inlet boundary zone at the mixing plane interface must be defined as either a velocity inlet (incompressible flow only), a pressure inlet, or a mass-flow inlet. The overall inlet and exit boundary conditions can be any suitable combination permitted by the solver (for example, velocity inlet, pressure inlet, or mass-flow inlet; pressure outlet). Remember, however, that if mass conservation across the mixing plane is important, you must use a mass-flow inlet as the downstream boundary; strict mass conservation is not maintained across the mixing plane when you use a velocity inlet or pressure inlet.


  5. Define the mixing planes in the Mixing Planes Dialog Box (Figure 9.9: The Mixing Planes Dialog Box).

     Setting Up Domain → Mesh Models → Mixing Planes...

    Figure 9.9:  The Mixing Planes Dialog Box

    The Mixing Planes Dialog Box

    1. Specify the two zones that make up the mixing plane by selecting an upstream zone in the Upstream Zone list and a downstream zone in the Downstream Zone list. It is essential that the correct pairs be chosen from these lists (that is, that the boundary zones selected lie on the mixing plane interface). You can check this by displaying the mesh.

       Setup →   General → Display...

    2. (3D only) Indicate the geometry of the mixing plane interface by choosing one of the options under Mixing Plane Geometry.

      A Radial geometry signifies that information at the mixing plane interface is to be circumferentially averaged into profiles that vary in the radial direction, for example, , . This is the case for axial-flow machines, for example.

      An Axial geometry signifies that circumferentially averaged profiles are to be constructed that vary in the axial direction, for example, , . This is the situation for a radial-flow device.


      Important:  Note that the radial direction is normal to the rotation axis for the fluid zone and the axial direction is parallel to the rotation axis.


    3. (3D only) Set the number of Interpolation Points. This is the number of radial or axial locations used in constructing the boundary profiles for circumferential averaging. You should choose a number that approximately corresponds to the resolution of the surface mesh in the radial or axial direction. Note that while you can use more points if you want, the resolution of the boundary profile will only be as fine as the resolution of the surface mesh itself.

      In 2D the flow data is averaged over the entire interface to create a profile consisting of a single data point. For this reason you do not need to set the number of Interpolation Points or select a Mixing Plane Geometry in 2D.

    4. Set the Global Parameters for the mixing plane.

      1. Select the Averaging Method. The Area averaging method is the default method. For detailed information about each of the Area, Mass, or Mixed-Out options, see Choosing an Averaging Method in the Theory Guide.

      2. Set the Under-Relaxation parameter. It is sometimes desirable to under-relax the changes in boundary values at mixing planes as these may change very rapidly during the early iterations of the solution and cause the calculation to diverge. The changes can be relaxed by specifying an under-relaxation less than 1. The new boundary profile values are then computed using

        (9–1)

        where is the under-relaxation factor. Once the flow field is established, the value of can be increased.

      3. Click Apply to set the Global Parameters. If the Default button is visible to the right of the Apply button, clicking the Default button will return Global Parameters back to their default values. The Default button will then change to be a Reset button. Clicking the Reset button will change the Global Parameters back to the values that were last applied.

    5. Click Create to create a new mixing plane. ANSYS Fluent will name the mixing plane by combining the names of the zones selected as the Upstream Zone and Downstream Zone and enter the new mixing plane in the Mixing Plane list.

      If you create an incorrect mixing plane, you can select it in the Mixing Plane list and click the Delete button to delete it.

9.3.4.2.1. Modeling Options

There are two options available for use with the mixing plane model: a fixed pressure level for incompressible flows, and the swirl conservation described in Swirl Conservation in the Theory Guide.

9.3.4.2.1.1. Fixing the Pressure Level for an Incompressible Flow

For certain turbomachinery configurations, such as a torque converter, there is no fixed-pressure boundary when the mixing plane model is used. The mixing plane model is usually used to model the three interfaces that connect the components of the torque converter. In this configuration, the pressure is no longer fixed. As a result, the pressure may float unbounded, making it difficult to obtain a converged solution.

To resolve this problem, ANSYS Fluent offers an option for fixing the pressure level. When this option is enabled, ANSYS Fluent will adjust the gauge pressure field after each iteration by subtracting from it the pressure value in the cell closest to the Reference Pressure Location in the Operating Conditions Dialog Box.


Important:  This option is available only for incompressible flows calculated using the pressure-based solver.


To enable the fixed pressure option, use the fix-pressure-level text command:

define → mixing-planes → set → fix-pressure-level

9.3.4.2.1.2. Conserving Swirl Across the Mixing Plane

Conservation of swirl is important for applications such as torque converters (Swirl Conservation in the Theory Guide). If you want to enable swirl conservation across the mixing plane, you can use the commands in the conserve-swirl text menu:

define → mixing-planes → set → conserve-swirl

To turn on swirl conservation, use the enable? text command. Once the option is turned on, you can ask the solver to report information about the swirl conservation during the calculation. If you turn on verbosity?, ANSYS Fluent will report for every iteration the zone ID for the zone on which the swirl conservation is active, the upstream and downstream swirl integration per zone area, and the ratio of upstream to downstream swirl integration before and after the correction.

To obtain a report of the swirl integration at every pressure inlet, pressure outlet, velocity inlet, and mass-flow inlet in the domain, use the report-swirl-integration command. You can use this information to determine the torque acting on each component of the turbomachinery according to Equation 2–22 (in the Theory Guide).

9.3.4.2.1.3. Conserving Total Enthalpy Across the Mixing Plane

One of the options available in the mixing plane model is to conserve total enthalpy across the mixing plane. This is a desirable feature because global parameters such as efficiency are directly related to the change in total enthalpy across a blade row or stage.

The procedure for ensuring conservation of total enthalpy simply involves adjusting the downstream total temperature profile such that the integrated total enthalpy matches the upstream integrated total enthalpy.

If you want to enable total enthalpy conservation, you can use the commands in the conserve-total-enthalpy text menu:

define → mixing-planes → set → conserve-total-enthalpy

To turn on total enthalpy conservation, use the enable? text command. Once the option is turned on, you can ask the solver to report information about the total enthalpy conservation during the calculation. If you turn on verbosity?, ANSYS Fluent will report at every iteration the zone ID for the zone on which the total enthalpy conservation is active, the upstream and downstream heat flux, and the ratio of upstream to downstream heat flux.


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