To model a problem involving a single moving reference frame, follow the steps outlined below.
Select the Velocity Formulation to be used when solving: either Relative or Absolute. (See Choosing the Relative or Absolute Velocity Formulation for details.)
Setup →
General
(Note that this step is irrelevant if you are using one of the density-based solvers; these solvers always use an absolute velocity formulation.)
For each cell zone in the domain, specify the translational
velocity of the reference frame and/or the angular velocity () of the reference
frame and the axis about which it rotates.
Setup →
Cell Zone Conditions
In the Fluid or Solid dialog box, specify the Rotation-Axis Origin and Rotation-Axis Direction for the frame motion to define the axis of rotation.
Also 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. 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, 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.
If you need to switch between the moving reference
frame 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.
Important: For solid zones, you only need to enable the Frame Motion option if you intend to include the convective terms in the energy equation for the solid (Equation 5–11 in the Theory Guide). Normally, this is not required if you want to do a conjugate heat transfer problem where the solid and fluid zones are moving together.
Define the velocity boundary conditions at walls. You can choose to define either an absolute velocity or a velocity relative to the moving reference frame (that is, 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 in 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 velocity of the fluid zone.
Details about these inputs are presented in Velocity Conditions for Moving Walls.
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.
It is recommended that you use the velocity formulation that will result in most of the flow domain having the smallest velocities in that frame, thereby reducing the numerical diffusion in the solution and leading to a more accurate solution.
The absolute velocity formulation is preferred in applications where the flow in most of the domain is not moving (for example, a fan in a large room). The relative velocity formulation is appropriate when most of the fluid in the domain is moving, as in the case of a large impeller in a mixing tank.
A problem with stationary outer walls and a rotating impeller can be solved in a single reference frame. The example is illustrated in Figure 9.5: Geometry with the Rotating Impeller.
In case A, it is expected that only the flow near the impeller would be rotating and that much of the flow away from the impeller would have a low velocity magnitude in the absolute frame. Therefore, solving using the absolute velocity formulation is recommended. In case B, most of the flow is expected to be rotating with a velocity close to that of the impeller. Hence, the relative velocity formulation is appropriate.
In a situation between case A and case B, either of the formulations may be used.
If the velocity formulation is switched during the solution process, ANSYS Fluent will not transform the current solution to the other frame, which can lead to large jumps in residuals. If changing the frame is necessary, it is recommended that you first reinitialize, and then solve.
When one of the density-based solution algorithms is used, the absolute formulation is always used; the relative velocity formulation is not available in the density-based solvers.
For velocity inlets, pressure inlets, mass-flow inlets, and walls, you may specify velocity in either the absolute or the relative frame, regardless of whether the absolute or relative velocity formulation is used in the computation.
For pressure outlets, the specified static pressure is independent of frame. However, when there is backflow at a pressure outlet, the specified static pressure is used as the total pressure. For calculations using the absolute velocity formulation, the specified static pressure is used as the total pressure in the absolute frame; for the relative velocity formulation, the specified static pressure is assumed to be the total pressure in the relative frame. As for the flow direction, ANSYS Fluent assumes the absolute velocity to be normal to the pressure outlet for the absolute velocity formulation; for the relative velocity formulation, it is the relative velocity that is assumed to be normal to the pressure outlet.