10.10.2 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.

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

General

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

Cell Zones Conditions

(a)   If the zone is rotating, or if you plan to specify cylindrical-velocity or flow-direction components at inlets to the zone, you will need to define the axis of rotation. In the Fluid dialog box or Solid dialog box, specify the Rotation-Axis Origin and Rotation-Axis Direction.

(b)   Also in the Fluid or Solid dialog box, select Moving Reference Frame in the Motion Type drop-down list 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.

Details about these inputs are presented in Section  7.2.1 for fluid zones, and in Section  7.2.2 for solid zones.

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 Section  10.10.1.

4.   Define the velocity at any velocity inlets and the flow direction and total pressure at any pressure inlets or mass flow inlets. 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 Section  7.3.5.

Details about these inputs are presented in Sections  7.3.3, 7.3.4, and 7.3.5.

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 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 (e.g., velocity inlet, pressure inlet, or mass flow inlet; pressure outlet). Keep in mind, however, that if mass conservation across the mixing plane is important, you need to use a mass flow inlet as the downstream boundary; 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  10.10.2).

Define $\rightarrow$ Mixing Planes...

Figure 10.10.2: The Mixing Planes Dialog Box

(a)   Specify the two zones that comprise 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 (i.e., that the boundary zones selected lie on the mixing plane interface). You can check this by displaying the mesh.

General Display...

(b)   (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, e.g., $p(r)$, $T(r)$. 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, e.g., $p(x)$, $T(x)$. This is the situation for a radial-flow device.

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.

(c)   (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 wish, 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.

(d)   Set the Global Parameters for the mixing plane.

i.   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 this section in the separate Theory Guide.

ii.   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

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

iii.   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.

(e)   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.

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 this section in the separate Theory Guide.

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.

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 $\rightarrow$ mixing-planes $\rightarrow$ set $\rightarrow$ fix-pressure-level

Conserving Swirl Across the Mixing Plane

Conservation of swirl is important for applications such as torque converters ( this section in the separate 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 $\rightarrow$ mixing-planes $\rightarrow$ set $\rightarrow$ 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 this equation (in the separate Theory Guide).

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 $\rightarrow$ mixing-planes $\rightarrow$ set $\rightarrow$ 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.