1. Introductory FLUENT Training
Moving Zones
Introductory FLUENT Training
Welcome to the Moving Zones lecture.
The purpose of this lecture is to introduce new Fluent users to the capabilities of the solver for modeling moving domains. Due to the limited length of this presentation, we will only be able to provide a brief overview of this topic. However, additional material is provided in the Appendix as well as in the Fluent User’s Guide.

2. Outline Introduction and Overview of Modeling Approaches
Single-Reference Frame (SRF) Model
Multiple Zones and Multiple-Reference Frame Model (MRF)
Mixing Plane Model (MPM)
Sliding Mesh Model (SMM)
Dynamic Mesh (DM) Model
Summary
Appendix
The presentation is divided into topic areas as shown in this slide. After a brief introduction, we will cover the five modeling approaches for moving domains, progressing from the simplest approach (the Single Reference Frame model) to the most complex (the Dynamic Mesh approach). Again, the goal is to introduce the new user to these topics and provide some guidance about their setup and use.

3. Introduction
Many engineering problems involve flows through domains which contain translating or rotating components.
Examples – Translational motion:
Train moving in a tunnel, longitudinal sloshing of fluid in a tank, etc.
Examples – Rotational motion:
Flow though propellers, axial turbine blades, radial pump impellers, etc.
There are two basic modeling approaches for moving domains:
If the domain does not change shape as it moves (rigid motion), we can solve the equations of fluid flow in a moving reference frame.
Additional acceleration terms added to the momentum equations
Solutions become steady with respect to the moving reference frame
Can couple with stationary domains through interfaces
If the domain changes shape (deforms) as it moves, we can solve the equations using dynamic mesh (DM) techniques.
Domain position and shape are functions of time.
Solutions are inherently unsteady.
Computational fluid dynamics (or CFD) has been used to examine problems involving moving domains ever since the advent of computer simulation in the 1960s. The motions can either be:
Translational – such as the cyclic oscillation of liquid in a tank or a train moving through a tunnel. Or
Rotational – which is perhaps the most common. Examples include flows though turbomachines (pumps, turbines, compressors, and related equipment), electric motors, spinning objects such as car tires, and so forth.
There are two basic approaches to modeling flows in moving domains.
The first approach involves referring the problem to a moving reference frame. For example, we can define a reference frame which is spinning in concert with a rotating tank. The flow is described with respect to the spinning reference frame. However, the fact that the reference frame itself is moving gives rise to “non-inertial” effects – that is, the equations of motion now have additional acceleration terms added to them to account for the moving frame (more about that later).
The benefit of using a moving reference frame is often a problem which is inherently unsteady in the stationary frame becomes steady-state in the moving frame of reference. Moreover, we can couple adjacent zone to the moving zone though grid interfaces to create a simplified model of a complex moving zone system (for example a pump impeller coupled with a scroll casing).
The second approach solves the equations using a mesh which is moving with respect to a fixed frame, and we refer all flow variables to the fixed frame. In this case, the solution is inherently unsteady. The main advantage of this approach is that we can allow the mesh (and hence the domain) to deform with time, thus permitting a wide range of problems involving moving and deforming boundaries.

4. Moving Reference Frame vs. Dynamic Meshx
Domain
Moving Reference Frame – Domain moves with rotating coordinate system
This slide illustrates the two approaches. Notice that in the moving reference frame approach, the axes are attached to the moving domain and are rotate with it. Therefore the axes always remain in the same position with respect to the moving domain. Again, because the frame is accelerating, additional terms are added to the equations of motion of the fluid.
In contrast, the moving/deforming domain approach permits a time-dependent deformation of the computational domain, which requires tracking the mesh with respect to a fixed frame of reference.
Dynamic Mesh – Domain changes shape as a function of time

5. Overview of Modeling Approaches
Single Reference Frame (SRF)
Entire computational domain is referred to a moving reference frame
Multiple Reference Frame (MRF)
Selected regions of the domain are referred to moving reference frames
Interaction effects are ignored  steady-state
Mixing Plane (MPM)
Influence of neighboring regions accounted for through use of a mixing plane model at rotating/stationary domain interfaces
Circumferential non-uniformities in the flow are ignored  steady-state
Sliding Mesh (SMM)
Motion of specific regions accounted for by a mesh motion algorithm
Flow variables interpolated across a sliding interface
Unsteady problem - can capture all interaction effects with complete fidelity, but more computationally expensive than SRF, MRF, or MPM
Dynamic Mesh (DM)
Like sliding mesh, except that domains are allowed to move and deform with time
Mesh deformation accounted for using spring analogy, remeshing, and mesh extrusion techniques
Now, we will begin discussing the five approaches for modeling moving zones, as listed in this slide. Again we will only be able provide a brief overview of each topic, and you are encouraged to seek out additional information which is available in the User’s Guide and from additional publications available from ANSYS.

6. Outline Introduction and Overview of Modeling Approaches
Single-Reference Frame (SRF) Model
Multiple Zones and Multiple-Reference Frame Model (MRF)
Mixing Plane Model (MPM)
Sliding Mesh Model (SMM)
Dynamic Mesh (DM) Model
Summary
Appendix
Let us now begin with the simplest approach for modeling moving zones – the Single Reference Frame Model or SRF.

7. Introduction to SRF Modeling
SRF assumes a single fluid domain which rotates with a constant speed with respect to a specified axis.
Why use a rotating reference frame?
Flow field which is unsteady when viewed in a stationary frame can become steady when viewed in a rotating frame
Steady-state problems are easier to solve...
simpler BCs
low computational cost
easier to post-process and analyze
NOTE: You may still have unsteadiness in the rotating frame due to turbulence, circumferentially non-uniform variations in flow, separation, etc.
example: vortex shedding from fan blade trailing edge
Wall boundaries must conform to the following requirements:
Walls which move with the fluid domain may assume any shape
Walls which are stationary (with respect to the fixed frame) must be surfaces of revolution
Can employ rotationally-periodic boundaries for efficiency (reduced domain size)
The single reference frame model is the simplest approach for moving zone modeling. In this approach, a single, non-deforming fluid domain is referred to a moving frame of reference. As mentioned previously, the equations of motion are modified to account for the non-inertial motion of the moving frame. In addition, boundary conditions are defined relative to the moving zone.
Why use a rotating frame to begin with? The reason is that, for many common classes of moving zone problems, a flowfield which is unsteady when viewed from the stationary frame becomes steady in the moving frame. Steady-state problems are desirable as they are (1) easier and less expensive to solve, (2) possess simpler BCs, and (3) are more straightforward to post-process and analyze.
Please note that you may still model natural unsteadiness in the moving frame – for example, vortex shedding from the trailing edge of a rotating fan blade.
Now, when you model a rotating zone with the SRF approach, it is important to note that the walls must conform to the following requirements:
Walls which move with the reference frame can be any shape (3-D)
Walls which are to modeled as stationary (with respect to the fixed frame) must be surfaces of revolution! If your domain does not meet this requirement, you must break your model up into multiple zones and use an approach which supports multiple zones.
Finally, it is very common to employ rotationally periodic boundaries in SRF models as it reduces the mesh size from an entire rotating geometry to a single periodic passage. Of course, both your geometry and your flowfield must be rotationally periodic, which can be an issue if, for example, your inflow BC is not periodic.

8. Stationary Walls in SRF Models
baffle
stationary wall
rotor
In this slide, we show the difference between a domain which can be modeled with SRF (the figure on the left) and a zone which can not (the figure on the right). In this case, the baffles prevent the stationary wall from being a surface of revolution. If one wanted to model the system with the baffles, you would, as mentioned before, need to separate the tank into a rotating zone in the vicinity of the rotor and a stationary zone which encompasses the baffles.
Wrong!
Correct
Wall with baffles not a surface
of revolution!

9. N-S Equations: Rotating Reference Frames
Equations can be solved in absolute or rotating (relative) reference frame.
Relative Velocity Formulation (RVF)
Obtained by transforming the stationary frame N-S equations to a rotating reference frame
Uses the relative velocity and relative total internal energy as the dependent variables
Absolute Velocity Formulation (AVF)
Derived from the relative velocity formulation
Uses the absolute velocity and absolute total internal energy as the dependent variables
Rotational source terms appear in momentum equations.
Refer to Appendix for a detailed listing of equations x y z
stationary
frame
rotating
axis of
rotation
CFD domain
Let us now briefly examine the forms of the Navier-Stokes equations appropriate for moving reference frames. Basically, the transformation from the stationary frame to the moving frame can be done mathematically in two different ways. In the first form, the momentum equations are expressed in terms of the velocity relative to the moving frame. This form is known as the Relative Velocity Formulation. The second form utilizes the velocities referred to the absolute frame of reference in the momentum equations, and is known as the Absolute Velocity Formulation. In both cases, additional acceleration terms result from the transformations. In addition, for compressible flows, the energy variables that are solved for will depend on the forumlation.
A complete list of the equations is provided in the Appendix.

10. The Velocity Triangle
The relationship between the absolute and relative velocities is given by
In turbomachinery, this relationship can be illustrated using the laws of vector addition. This is known as the Velocity Triangle
It is important to understand the relationship between the velocity viewed from the stationary and relative frames. This relationship is often called the “velocity triangle,” and can be expressed by the simple vector equation:
Here, V is the velocity in the stationary or absolute frame ,W is the velocity viewed from the moving frame, and U is the frame velocity. For a rotating reference frame, U is simply
Notice from the picture of the moving turbine blade that a flow approaching the blade in the x direction appears to be moving with a positive angle due to the downward motion of the blade.

11. Comparison of Formulations
Relative Velocity Formulation: x-momentum equation
Coriolis acceleration
Centripetal acceleration
Absolute Velocity Formulation: x-momentum equation
Let’s now compare the two formulations. To do this we will simply consider the x momentum equation.
For the relative velocity formulation, we observe that the x component of the relative velocity is being solver for, and that the convecting velocity is the relative velocity. It should be noted here that in a moving frame, scalars are convected along relative streamlines and we will employ a similar kind of convection term for such scalar equations as turbulence kinetic energy and dissipation rate, and species transport. Also note the presence of additional acceleration terms, which have been placed on the right hand side. The first acceleration is called the Coriolis acceleration (2w x W), and has the property of acting perpendicular to the direction of motion of the fluid and to the axis of rotation. The second term is called the Centripetal acceleration, which acts in the radial direction. Both of these accelerations act as momentum source terms in the momentum equations, and can lead to difficulties if the rotational speed is very large.
For the absolute velocity formulation, we now solve for the x component of the absolute velocity. Note that the relative velocity is still the convecting velocity, and that the accerlation terms can be collapsed into a single term (w x V), due to the fact that the Corilolis acceleration becomes (w x W).
It should be stressed that these equations are equivalent representations of the flow in the moving frame, and that either form can be used for CFD. However, since the numerical errors are different for each form, on a finite grid there may be an advantage in using one form over another. We will return to this point shortly.
Coriolis + Centripetal accelerations

12. SRF Set-up: Solver Solver Choice recommendations:
Pressure Based – Incompressible, low-speed (subsonic) compressible flows
Density Based – High-speed (transonic, supersonic) compressible flows
Velocity Formulation recommendations:
Use absolute velocity formulation (AVF) when inflow comes from a stationary domain
Use relative velocity formulation (RVF) with closed domains (all surfaces are moving) or if inflow comes from a rotating domain
NOTE: RVF is only available in the segregated solver
Gradient Option
Use Node-Based gradients for tet/hybrid meshes
Use Least Squares gradients for polyhedral cells
Let us now look at some practical aspects of setting up SRF problems in the Fluent CFD solver.
First, the choices for solver type and the gradient option should follow existing best practices – that is, use the pressure-based solver (in general) for low speed through mildly compressible flows, and the density-based solver for high speed flows. Other physical model choices may also influence this choice (for example, to use either the real gas or wet steam models, you must use the density-based solver). Also, the gradient option recommendation is tied to the cell types employed in your mesh as indicated in the slide.
For the velocity formulation, the best practice is to use the AVF for cases where the flow conditions are best represented in the stationary frame (for example, flow entering a compressor from a stationary plenum), and the RVF where the flow is represented best in the relative frame (such as, flow in a closed, rotating tank). Please note that the RVF is only available for the pressure-based solver.

13. SRF Set-up: Fluid BCs
Use fluid BC panel to define rotational axis origin and direction vector for rotating reference frame
Direction vectors should be unit vectors but Fluent will normalize them if they aren’t
Select Moving Reference Frame as the Motion Type for SRF
Enter Rotational Velocity
Rotation direction defined by right-hand rule
Negative speed implies rotation in opposite direction
Once the solver, physical model, and material selections have been made, you can activate a moving reference frame in the BC panel for the fluid zones. The parameters which must be set as follows:
Enter first the rotational axis origin and direction. The origin (x,y,z) corresponds to the origin of the moving frame, while the direction is a unit vector pointing in the direction of the axis. Rotation of the frame is defined using the right-hand-rule.
Next, under “Motion Type”, select “Moving Reference Frame”. This indicates to Fluent that the entire cell zone is moving with the translational and rotational speeds you provide.
Finally, enter the moving zone velocities – most typically a rotational velocity, though a translational velocity may be employed under special circumstances. Note that the rotational velocity may be positive or negative, a negative speed implying a sense of rotation opposite to the right hand rule.

14. SRF Set-up: Inlet/Outlet Boundaries
Velocity Inlets:
Absolute or relative velocities may be defined regardless of formulation.
Pressure Inlet:
Definition of total pressure depends on velocity formulation:
Pressure Outlet:
For axial flow problems with swirl at outlet, radial equilibrium assumption option can be applied such that:
Specified pressure is hub pressure
Other BCs for SRF problems
Non-reflecting BCs
Target mass flow outlet
incompressible, AVF
incompressible, RVF
Flow boundaries require some special attention for SRF models.
First, velocity inlets permit specification of velocity directions or components in either the absolute or relative frames. Use the form which is relevant to the problem at hand.
Pressure inlet specifications, however, are closely tied with the velocity formulation. Specifically, if you are using the AVF, the total pressure which is entered into the GUI is the absolute total pressure, which is shown here in the incompressible form. Note that the dynamic term involves the absolute velocity, ½ r V^2. In addition, the direction vector is defined in the absolute frame. In contrast, if you are using the RVF, the total pressure that is entered is assumed to be a relative total pressure, which has a dynamic term that involves the relative velocity, ½ r W^2. The direction vector in this case is defined in the relative frame. These comments also apply to reverse flow specifications at pressure outlets, where the pressure outlet behaves like a pressure inlet.
The pressure outlet also has an option for “radial equilibrium”. This option permits a radial variation in pressure due to swirl, as given by the simplified radial equilibrium equation. This condition holds only for cases with axial outflow (flow is parallel to the axis of rotation) – for example, at the outlet of an axial compressor or turbine stage.
Other BCs which may be of interest for turbomachinery applications include:
Non-reflecting BCs
Target mass flow outlet
More information about these models can be found in the manual.

15. Wall BCs
For moving reference frames, you can specify the wall motion in either the absolute or relative frames.
Recommended specification of wall BCs for all moving reference frame problems…
Activate “Moving Wall” option
Set Rotation-Axis Origin and Direction same as fluid zone
For stationary surfaces (in the absolute frame) use zero Rotational speed, Absolute
For moving surfaces, use zero Rotational speed, Relative to Adjacent Cell Zone
Wall boundary conditions also require some special attention in rotating machinery applications. First, it should be pointed out that the default setting for walls (stationary wall) takes on a new meaning when the cell zone to which it’s attached becomes a MRF zone. For MRF zones, “stationary” wall means “stationary relative to the MRF” – that is, the wall is moving with the reference frame! If that is the desired condition for all walls in your MRF zone, then you can leave the wall BC alone. However, if you wish to have a surface of revolution be considered as a stationary wall (in the absolute frame) then you must turn on the Moving Wall option, set the specification mode to “Rotational”, set the axis origin and direction to be the same as the cell zone MRF specification, set the rotational speed to 0, then finally set the “Motion” option to “Absolute”. For convenience, it is desirable to set all walls this way. For rotating wall select the “Relative to Adjacent Cell Zone” option for walls moving with the MRF and “Absolute” for stationary walls.

16. Solution Strategies for SRF Problems
SRF problems may be more difficult to solve because of large flow gradients resulting from the rotation of the fluid domain.
May require a finer mesh to resolve steep gradients due to rotational effects.
Some things to consider for troublesome cases:
Make sure the mesh quality is good (max cell skewness < 0.9 – 0.95).
Start problems using first order discretizations.
Reduce underrelaxation factors / Courant numbers to enhance stability.
Use FMG initialization for hard-to-start problems.
Especially desirable for compressors, pumps, and similar applications .
Consider running the problem as a transient calculation.
Can provide more robust convergence versus the standard steady-state approach.
Use first order discretization in time and about 2-3 time steps per iteration.
Run until steady-state is achieved.
The solution strategies for SRF problems mirror the best practices for general fluid flow problems. Specifically, the use of high quality meshes, appropriate under-relaxation factors and Courant numbers, and first order discretizations early in the calculation can help prevent unstable solution behavior. In addition, a finer mesh may be necessary in order to resolve steep gradient which may arise due to rotational effects.
Initialization is always important for CFD; but, for problems like compressors and pumps where the flow sustains a pressure rise, it can be very important. This is because the higher exit pressure tends to promote reverse flow at the outlet, which can lead to unstable behavior. One way to avoid this is to employ the FMG initialization scheme, which is available in the TUI. This procedure pre-calculates an approximate flow solution for use as an initial condition, and has been found in many cases to greatly accelerate convergence. For more information on this feature, please consult the User’s Guide.
Finally, some especially troublesome cases have been solved by treating the problem as an unsteady or transient calculation. That is, you activate the unsteady solver, choose an appropriate time step, set the number of time steps per iteration to a low number (say 2-3), and time-march the calculation until steady-state is achieved. As an estimate for the time step size, use the ratio of an average cell size in your model with a velocity scale related to the rotational speed (for example, the rotational speed of a compressor blade times the tip radius).

17. Outline Introduction and Overview of Modeling Approaches
Single-Reference Frame (SRF) Model
Multiple Zones and Multiple-Reference Frame Model (MRF)
Mixing Plane Model (MPM)
Sliding Mesh Model (SMM)
Dynamic Mesh (DM) Model
Summary
Appendix
Let us now turn our attention to multiple zone, steady-state models, starting with the simplest approach that we call the Multiple Reference Frame or MRF approach.

18. Multiple Zone Modeling
Many rotating machinery problems involve stationary components which cannot be described by surfaces of revolution (SRF not valid).
Systems like these can be solved by dividing the domain into multiple fluid zones – some zones will be rotating, others stationary.
The multiple zones communicate across one or more interfaces.
The way in which the interface is treated leads to one of following approaches for mutiple zones models:
Multiple reference frame model (MRF)  Steady-state solution
Simplified interface treatment - rotational interaction between reference frames is not accounted for.
Mixing plane model (MPM)  Steady-state solution
Interaction between reference frames are approximated through circumferential averaging at fluid zone interfaces (mixing planes).
Sliding mesh model (SMM)  Unsteady solution
Accurately models the relative motion between moving and stationary zones at the expense of more CPU time (inherently unsteady).
There are many moving zone problems which cannot be solved using the SRF approach alone – specifically, applications with stationary components with walls that are not surfaces of revolution. For example, a centrifugal pump impeller typically is situated next to a scroll-shaped casing or volute. Since the casing is not a surface or revolution about the axis of rotation, you cannot include that region in the moving reference frame zone.
To address these kinds of problems, you must break up the domain into multiple fluid zones, some which are moving and others which are stationary. The zones communicate across one or more interfaces, thereby permitting a specific degree of interaction between the zones. The way in which the interface is treated leads to one of the following multiple zone approaches:
The multiple reference frame model
The mixing plane model
The sliding mesh model

19. Single Versus Multiple Component Modeling
interface
This slide illustrates the difference between a single blade passage case on the left, which can be solved using the SRF approach by assuming rotational periodic boundary conditions, versus a multiple zone model on the right, which consists of a blower wheel and casing. Note the interface which separates the two zones. Again, the interface can be treated in a number of ways, each with it’s own inherent assumptions and limitations.
Single Component
(blower wheel blade passage)
Multiple Component
(blower wheel + casing)

20. Introduction to the MRF Model
The computational domain is divided into stationary and rotating fluid zones.
Interfaces separate zones from each other.
Interfaces can be Conformal or Non-Conformal.
Flow equations are solved in each fluid zone.
Flow is assumed to be steady in each zone (clearly an approximation).
SRF equations used in rotating zones.
At the interfaces between the rotating and stationary zones, appropriate transformations of the velocity vector and velocity gradients are performed to compute fluxes of mass, momentum, energy, and other scalars.
MRF ignores the relative motions of the zones with respect to each other.
Does not account for fluid dynamic interaction between stationary and rotating components.
For this reason MRF is often referred to as the “frozen rotor” approach.
Ideally, the flow at the MRF interfaces should be relatively uniform or “mixed out.”
Let’s now discuss the MRF approach. This is perhaps the simplest possible way of treating interfaces between moving and stationary zones.
To use this approach, you must divide your mesh into separate fluid zones with interfaces between zones. The interfaces may be conformal or non-conformal – we’ll talk about that further in the next slide.
We then assume steady-state conditions in each fluid zone and solve the appropriate equations in those zones (either stationary or MRF). At the interfaces, the algorithm simply apply a change of frame for the for velocity vector and related quantities.
It should be noted that the fluxes computed in this fashion are local to the interface and ignore the relative motions of the zones with respect to each other. It is as if the rotating zones are “frozen” in place with respect to the stationary zones. Hence, this approach is often referred to as the “frozen rotor approach”
Another way of thinking about MRF is as a instantaneous “snapshot” of the flowfield. If the temporal variations at the interface are small – that I, the flow is relatively uniform or mixed out - then this becomes a reasonable approximation.

21. Interfaces in MRF Models
Conformal interfaces
An interior mesh surface separates cells from adjacent fluid zones.
Face mesh must be identical on either side of the interface.
Non-conformal interfaces
Cells zones are physically disconnected from each other.
Interface consists of two overlapping surfaces (type = interface)
Fluent NCI algorithm passes fluxes from on surface to the other in a conservative fashion (i.e. mass, momentum, energy fluxes are conserved).
User creates interfaces using DefineGrid Interfaces…
Interfaces may be periodic
Require identical translational or rotational offset.
Conformal interface
The MRF approach can accommodate two types of interfaces – conformal and non-conformal.
Conformal interfaces are simply interior face zones which separate individual fluid zones. By definition, a single face zone divides the cells and the faces and nodes match across the interface.
In contrast, non-conformal interfaces consist of cell zones which are physically disconnected from each other. The zones communicate across overlapping interface boundaries. Fluxes are passed conservatively from one side to the other. Clearly, the advantage of this approach is that is permits much more flexibility in the mesh generation with very little penalty in accuracy. In addition, as we will see later, it is easy to change an MRF model with non-conformal interfaces to a sliding mesh model if desired. Thus non-conformal interfaces recommended in general over conformal interfaces.
Non-conformal interface

22. Interface Shapes
Walls which are contained within the rotating fluid zone interfaces are assumed to be moving with the fluid zones and may assume any shape.
Stationary walls are permitted if they are surfaces of revolution.
The interface between a the two zones must be a surface of revolution with respect to the axis of rotation of the rotating zone.
Periodic interfaces are permitted but the periodic angles (or offsets) must be identical for all zones.
stationary zone
rotating zone
Consider a mixing impeller inside a rectangular vessel:
- Problem can be described with two reference frames or zones.
It is important to recognize that the interface shape must adhere to a simple rule when used in MRF (or even sliding mesh calculations). Specifically, the interface surface must be a surface of revolution about the axis of rotation. Another way to think of this is that a moving mesh zone must not become disconnected from the adjacent stationary zone at the non-conformal interface boundary. Clearly, a shape such as the oval shown on the right would not be permissible.
In addition, if a periodic interface in used, the periodic angles or offsets must be the same for all zones.
Interface is not a surface
or revolution
Correct
Wrong!

23. Example of Rotationally Periodic Interface
Each zone has
same periodic
angle (40 deg)
periodic
non-conformal
interface
An example of a periodic MRF problem is shown in this slide. As can be seen, the periodic non-conformal interface can handle the angular offset correctly provided the periodic angles are identical. If your geometry does not permit this, you may need to slightly alter the geometry (for example, add or subtract a blade) and stretch the geometry in the periodic direction to obtain equal angles.
Centrifugal compressor stage

24. MRF Set-Up
Generate mesh with appropriate stationary and rotating fluid zones
Can choose conformal or non-conformal interfaces between cell zones
For each rotating fluid zone (Fluid BC), select Moving Reference Frame as the Motion Type and enter the rotational speed.
Identical to SRF except multiple zones
Stationary zones remain with Stationary option enabled
Set up for other BCs and Solver settings same as SRF model.
To set up an MRF problem, you will first need to decide what types of interfaces are to be used (that is, conformal or non-conformal). This decision will impact how the mesh is generated in your preprocessor.
When the multiple zone mesh is read into Fluent, you will be able to selectively apply the moving reference frame option to the rotating zones.
Boundary conditions, physical models, materials, and solver settings will be the same as for SRF problems.

25. Solution Strategies for MRF Problems
Like SRF problems, MRF problems may be difficult to solve because of large flow gradients resulting from the rotation of one or more fluid zones.
Interactions between adjacent cell zones may need to use lower under-relaxations than default.
Some things to consider for troublesome cases:
Make sure the mesh quality is good (max cell skewness < 0.9 – 0.95), particularly in the vicinity of grid interfaces.
Use FMG initialization.
Can employ unsteady time-marching as a means of achieving a stable steady-state solution.
NOTE: MRF is a steady-state method - transient solutions are not meaningful!
If MRF is producing unstable or unrealistic results, you may want to run the case using the unsteady, sliding mesh model.
Solution strategies for MRF problem largely mirror those for SRF problem. Difficult to converge cases may respond to reductions in URFs and Courant numbers and improvements in mesh quality. Also, FMG initialization can be used to generate a reasonable starting guess for the model.
It is important to note that the MRF approach is an inherently steady-state method and so unsteady solutions are not meaningful. However, you can employ an unsteady time-marching approach as a means of achieving a stable steady-state solution.
Finally, if your MRF model is producing inaccurate or unphysical results, you may wish to activate the sliding mesh model. Well talk more about the sliding mesh approach later.

26. Outline Introduction and Overview of Modeling Approaches
Single-Reference Frame (SRF) Model
Multiple Zones and Multiple-Reference Frame Model (MRF)
Mixing Plane Model (MPM)
Sliding Mesh Model (SMM)
Dynamic Mesh (DM) Model
Summary
Appendix
For applications involving multistage turbomachinery, you may wish to consider another steady-state method, namely the mixing plane model.

27. Introduction to Mixing Plane Model (MPM)
The MPM was originally implemented to accommodate rotor/stator and impeller/vane flows in axial and centrifugal turbomachines.
Can also be applied to a more general class of problems.
Domain is comprised of multiple, single-passage, rotating and stationary fluid zones
Each zone is “self contained” with a inlet, outlet, wall, periodic BCs (i.e. each zone is an SRF model).
Steady-state SRF solutions are obtained in each domain, with the domains linked by passing boundary conditions from one zone to another.
The BC “links” between the domains are called the mixing planes.
BCs are passed as circumferentially averaged profiles of flow variables, which are updated at each iteration.
Profiles can be radial or axial.
As the solution converges, the mixing plane boundary conditions will adjust to the prevailing flow conditions.
The mixing plane model is a method which was developed within the turbomachinery community as a way of dealing with multiple blade row compressor and turbine analyses. It has since become more widely applied to pumps, fans, and similar systems.
The basic idea is to consider a system of single passage, SRF models which are aligned such that the outlet of an upstream zone feeds the inlet of a downstream zone. We can obtain a steady-state solution to this system in the following manner. First, we establish links between adjacent boundary conditions so that flow data from one domain is passed as a boundary condition to the adjacent zone. We then obtain a provisional solution in each SRF zone in the usual way. At the end of the solution step, we average the flow properties at the interface flow boundaries in the circumferential direction, thereby obtaining a simple radial or axial profile. Profiles are create for each variable required by the adjacent zone’s boundary condition. These profiles are then applied to the adjacent zones (much like one would apply a profile file to a standard Fluent model). By continuously updating the boundary conditions in this fashion, a coupled, steady-state flow solution will be obtained at convergence.

28. MRF vs MPM
MRF can be used only if we have equal periodic angles for each row.
Flow properties are passed locally along the interface, which may lead to some unphysical behavior.
Odd blade numbers may require modeling the entire (360 deg.) geometry in order to have equal periodic angles for each blade row.
The MPM requires only a single blade passage per blade row regardless of the number of blades.
This is accomplished by mixing out (averaging) the circumferential non-uniformities in the flow at the mixing plane interface.
MRF
Since both MRF and the mixing plane models are steady-state solution techniques, it is useful to contrast these two approaches.
As was mentioned previously, the MRF model can be used to couple multiple SRF zones together. Instead of using boundary conditions, however, the flow properties are transferred across non-conformal interfaces. There are two disadvantages with this approach. First, the flow properties are applied locally along the interface, thereby leading to some dependency of the solution on the relative positions of the zones, and possibly giving rise to some unphysical behavior. Second, since the adjacent passages must have equal periodic angles, systems with odd blade counts may require using the entire 360 deg geometry, leading to a much larger mesh.
In contrast, the MPM only requires a single blade passage per blade row. This is due to the circumferential averaging that is performed, which permits boundary conditions to be matched to any passage periodic angle. As a result, the meshes for mixing plane problems can be very modest in size.
MPM

29. Mixing Plane Configurations
radial machines
A mixing plane is an interface that consists of the outlet of an upstream domain and the inlet to the adjacent downstream domain.
The inlet/outlet boundaries must be assigned BC types in one of the following combinations:
Pressure-Outlet / Pressure-Inlet
Pressure-Outlet / Velocity-Inlet
Pressure-Outlet / Mass-Flow-Inlet
The MPM has been implemented for both axial and radial turbomachinery blade rows.
For axial machines, radial profiles are used.
For radial (centrifugal) machines, axial profiles are used.
axial machines
The mixing plane interface consist of an upstream pressure outlet boundary which is linked to a downstream inlet boundary . The inlet type can be a pressure inlet, and velocity inlet, or a mass flow inlet. It should be noted that if a mass flow inlet is used, Fluent will automatically match the downstream mass flux with the upstream mass flux, thus ensuring total mass flow conservation.
There are two types of profiles which are possible, depending on the geometry of the interface boundaries. If the boundaries are radial, as one would expect in an axial turbomachine, then a radial profile is defined (that is, the pressure, temperatures, flow directions, etc. are function of the radial coordinate). For centrifugal compressors and similar geometries, an axial profile may be defined (where the flow variables are functions of the axial coordinate).

30. MPM Setup
Set fluid zones as Moving Reference Frames and define zone velocities.
Assign appropriate BC types to inlet- outlet boundary pairs.
Select upstream and downstream zones which will comprise mixing plane pair.
Set the number of points for profile interpolation.
Should be about the same axial/radial resolution as the mesh.
Mixing Plane Geometry determines method of circumferential averaging.
Choose Radial for axial flow machines.
Choose Axial for radial flow machines.
Mixing plane controls
Under-Relaxation - Profile changes are underrelaxed using factor between 0 and 1
Setting up a mixing plane is accomplished in the DefineMixing Planes GUI. The steps are as follows.
First, you select the upstream and downstream zones from the lists shown. You should visually check these zones so that their radial or axial extent matches.
Next, you choose the type of profile under the Mixing Plane Geometry option box. Select Radial for a radial profile or Axial for an axial profile.
The Interpolation Points is entered next. This parameter is the number of points which comprise the profile (which is sampled uniformly along the boundary). This number should roughly correspond to the number of mesh elements in the radial or axial directions at the mixing plane boundaries. However, choosing a number such as 50 – 100 should be sufficient for most problems, and there is no penalty for choosing a number which is larger than the mesh size.
Finally, you may provide an under-relaxation factor for the mixing plane. This will reduce the changes in the boundary condition values from one iteration to the next, thereby enhancing the stability of the calculation.

31. Solution Strategies for Mixing Plane Models
Because the mixing plane model involves modifying boundary conditions at the mixing plane interface, rapid changes in flow conditions at the mixing plane may cause convergence difficulties.
Try reducing the mixing plane under-relaxation factor to to help stabilize the solution.
Some other things to consider for troublesome cases
Make sure the mesh quality is good (max cell skewness < 0.9 – 0.95).
Use FMG initialization for hard-to-start problems.
FMG initialization is compatible with the mixing plane model.
Reduce under-relaxation factors and/or Courant numbers.
Run you case with fixed BCs for some interations, then enable the mixing planes.
The solution strategies for mixing plane problem again mirror the SRF recommendations with regard to mesh quality, solution controls, and the use of FMG initialization.
Because the mixing plane is constantly updating the boundary conditions values at the mixing plane interface, rapidly changing and complex flows near the mixing plane interface can cause convergence difficulties. For such cases, using a mixing plane underrelaxation factor of between 0.1 and 0.5 may help.

32. Outline Introduction and Overview of Modeling Approaches
Single-Reference Frame (SRF) Model
Multiple Zones and Multiple-Reference Frame Model (MRF)
Mixing Plane Model (MPM)
Sliding Mesh Model (SMM)
Dynamic Mesh (DM) Model
Summary
Appendix
We will now consider the first of the two inherently unsteady methods for moving zones – namely, the sliding mesh model.

33. Introduction to Sliding Mesh Model (SMM)
The relative motion of stationary and rotating components in a turbo-machine will give rise to unsteady interactions. These interactions are generally classified as follows:
Potential interactions (pressure wave interactions)
Wake interactions
Shock interactions
Both MRF and MPM neglect unsteady interaction entirely and thus are limited to flows where these effects are weak.
If unsteady interaction can not be neglected, we can employ the Sliding Mesh Model to account for the relative motions of the stationary and rotating components.
wake interaction
Shock
interaction
potential interaction
stator
rotor
In the MRF and mixing plane approaches, we assume that interactions between components are weak and therefore could be neglected in the analysis. This, of course, is clearly an approximation. The motion of a moving blade, for instance, past a stationary vane will give rise to unsteady interactions as shown in this slide. These interactions can be classified as follows:
First we have potential interactions (or pressure waves). These are a result of hydrodynamic interactions, and are a two-way effect – that is, the waves are felt both upstream and downstream.
Next we wake interactions, which are a result of wakes from upstream objects impacting downstream components. Unlike potential interactions, this is a one-way effect.
If the flow is compressible and Mach numbers are high enough, we may also have shock wave interactions. Like wake effects, this is a one-way interaction.
If the components are sufficiently remove from one another, these interaction effects are small and can often be ignored, thus permitting the use of MRF or mixing plane techniques. However, interaction between closely spaced components is usually very large and cannot be ignored. In addition, there can be complex flows occurring in the vicinity of the interfaces between moving and non-moving zones such that the MRF or mixing plane models will be sensitive to the interface location.
When interaction effects cannot be ignored, we can employ the sliding mesh model to simulate the unsteady interaction effects.

34. How the Sliding Mesh Model Works
Like the MRF model, the domain is divided into moving and stationary zones, separated by non-conformal interfaces.
Unlike the MRF model, each moving zone’s mesh will be updated as a function of time, thus making the mathematical problem inherently unsteady.
Another difference with MRF is that the governing equations have a new moving mesh form, and are solved in the stationary reference frame for absolute quantities (see Appendix for more details).
Moving reference frame formulation is NOT used here (i.e. no Coriolis, centripetal accelerations).
Equations are a special case of the general moving/deforming mesh formulation.
Assumes rigid mesh motion and sliding, non-conformal interfaces.
cells at time t
cells at time t+Dt
moving mesh zone
The sliding mesh model can be thought of as an extension of the MRF approach, in that we define stationary and moving zones separated by non-conformal interfaces. As the calculation proceeds, the moving zone meshes are updated as a function of time, thereby making the problem inherently unsteady. It should be noted that the meshes are moved in a rigid (non-deforming) manner and communication with adjacent zones will be maintained provided the grid interfaces maintain an overlap with one another (hence the name sliding mesh).
Another difference that the sliding mesh model has with MRF is the equations that are used. In the sliding mesh model, a moving mesh formulation is used which refers all flow variables to the stationary or inertial frame, and solves for absolute quantities. More details about this formulation are provided in the Appendix. The primary implication is that, unlike SRF, MRF, and MPM, the momentum equations do not contain Coriolis and centripetal acceleration terms – however, the geometry (mesh) is now a function of time, which wasn’t the case with the Moving Reference Frame approach. It should also be noted that the equations employed for sliding mesh models are a special case of the general moving/deforming mesh formulation which assumes rigid mesh motion and sliding, non-conformal interfaces.

35. Sliding Interfaces
Sliding interfaces must follow the same rules as MRF problems:
Any translation of the interface cannot be normal to itself.
The interface between a rotating zone and an adjacent stationary/rotating zone must be a surface of revolution with respect to the axis of rotation of the rotating subdomain.
Many failures of sliding mesh models can be traced to interface geometries which become disconnected as the mesh is moved!
Sliding interfaces can be partially-overlapping.
Can either be:
Periodic
Walls
If periodic, boundary zones must also be periodic and have identical offsets.
time t = 0
t + Dt
Sliding interfaces should follow the same rules mentioned previously for MRF models. In particular, for rotating zones it is important that the sliding interface be a surface of revolution about the axis of rotation. It should come as no surprise that any mesh motion which results in the sliding interfaces becoming disconnected will result in a failure of the calculation.
It was shown earlier that a rotationally-periodic interface can be partially overlapping, since the non-overlapping parts can be defined using the offset angle. For non-periodic zones, you can also have a partial overlap – however, in this case, the non-overlapping zones will be assumed to be walls.
Elliptic interface is not a surface of revolution.

36. Sliding Mesh Setup Enable unsteady solver.
Define sliding zones as Interface BC types.
For moving zones, select Moving Mesh as Motion Type in Fluid BC panel.
For each interface zone pair, create a non-conformal interface
Enable Periodic option if sliding/rotating motion is periodic.
Enable Coupled for conjugate heat transfer.
Other BCs are same as SRF, MRF models.
Setting up a sliding mesh model is relatively straightforward. The geometry, mesh, physical model, materials, and surface boundary condition set up will be identical to an MRF calculation. For a sliding mesh calculation, you will need to turn on the unsteady solver and define appropriate option depending on the flow solver selected (pressure-based vs density-based). Next, you will select the Moving Mesh option as the Motion Type in the Fluid BC panel for all moving cell zones (stationary zones remain with the Stationary option). You will need to set up all non-conformal interfaces as well (remembering to select Periodic if the interface is adjacent to periodic zones).
You will also need to set up your monitors to track the solution as a function of time rather than iteration.

37. Solution Strategies for SMM Problems
Choose appropriate Time Step Size and Max Iterations Per Time step to ensure good convergence with each time step.
Time Step Size should be no larger than the time it takes for a moving cell to advance past a stationary point:
Advance the solution until the flow becomes time-periodic (pressures, velocities, etc., oscillate with a repeating time variation).
Usually requires several revolutions of the grid.
Good initial conditions can reduce the time needed to achieve time-periodicity.
Ds = average cell size
wR = characteristic velocity of the moving zone (R = mean radius of interface surface)
One of the most important parameters associated with sliding mesh models is the time step size. For rotating problems, we often observe solutions which repeat themselves over some time period (for example, the blade passing period). To capture this time periodicity accurately, we need to choose an appropriate time step. One way of doing this is to choose a time step which is the ratio of an average cell size with a characteristic velocity (e.g. the velocity of the moving zone interface). You may also choose a time step which is some fraction of the passing period of the moving zone.
Since a sliding mesh calculation is unsteady, the solution we seek is not a single flow field, but rather a time-varying flow field. The results of interest may be an instantaneous result at a given point in time or a time-averaged result determine over a specified period. Solution results can be time-averaged using the “Data Sampling for Time Statistics” option in the Iterate GUI panel. The time-averaged results will be saved in the data file along with the latest instantaneous results.
Finally, the time required to obtain a time-periodic results will vary from problem to problem This time can be reduced by employing a good initial condition. Perhaps the best way to initialize sliding mesh models is to first run an MRF solution. You can easily switch to the sliding mesh model after computing the MRF solution.

38. Outline Introduction and Overview of Modeling Approaches
Single-Reference Frame (SRF) Model
Multiple Zones and Multiple-Reference Frame Model (MRF)
Mixing Plane Model (MPM)
Sliding Mesh Model (SMM)
Dynamic Mesh (DM) Model
Summary
Appendix
We will now discuss the most sophisticated moving zone approach available in Fluent 6 – the Dynamic Mesh Model.

39. What is the Dynamic Mesh (DM) Model?
A method by which the solver (FLUENT) can be instructed to move boundaries and/or objects, and to adjust the mesh accordingly.
Examples:
Automotive piston moving inside a cylinder
A flap moving on an airplane wing
A valve opening and closing
An artery expanding and contracting
The dynamic mesh model is the name given to a general modeling framework which permits flow solutions in arbitrarily moving and deforming domains. The user defines the boundary motions of the domain, and Fluent will determine the positions of the mesh nodes as a function time. If required the mesh can even be regenerated to accommodate large deformations of the domain. The equations which are solved account for the time varying mesh motions, and are a generalization of the equations used for the sliding mesh model.
This powerful technique has been applied to a wide range of problems, including:
Automotive piston moving inside a cylinder
A flap moving on an airplane wing
A valve opening and closing
An artery expanding and contracting
We will give a brief over overview of the methods and capability of the dynamics mesh approach in this section.
Volumetric fuel pump

40. Dynamic Mesh (DM) Model: Features
Internal node positions are automatically calculated based on user specified boundary/object motion, cell type, and meshing schemes
Spring analogy (smoothing)
Local remeshing
Layering
2.5 D
User defined mesh motion
Boundaries/Objects motion can be moved based on:
In-cylinder motion (RPM, stroke length, crank angle, …)
Prescribed motion via profiles or UDF
Coupled motion based on hydrodynamic forces from the flow solution, via FLUENT’s 6 DOF model.
Different mesh motion schemes may be used for different zones. Connectivity between adjacent zones may be non-conformal.
The dynamic mesh model in Fluent is comprised of a “toolbox” of methods for controlling the mesh motion. There are three general-purpose methods for dealing with mesh deformations, and these are:
Spring analogy
Local Remeshing
Layering
For specific classes of mesh motion and geometries, there are the several specialized approaches, specifically:
The 2.5D method
The user-defined mesh motion approach
The in-cylinder motion package (design with automotive in-cylinder applications in mind)
The 6 degree-of-freedom package
It should be noted that these schemes are very flexible, and one can utilize more than one approach in a single model, including the use of stationary and sliding non-conformal interfaces. We will show an example of this ability in a later slide.

41. Spring Analogy (Spring Smoothing)
The nodes move as if connected via springs, or as if they were part of a sponge.
Connectivity remains unchanged;
Limited to relatively small deformations when used as a stand-alone meshing scheme.
Available for tri and tet meshes;
May be used with quad, hex and wedge mesh element types, but that requires a special command.
Let’s begin our overview of the basic moving mesh methods with a discussion of the spring analogy approach.
Suppose we have a moving boundary that imparts only a relatively minor deformation on the domain. In this case, the mesh count and connectivity remain the same, while the cells respond to the boundary motion by deforming individually, like tiny sponges. The nodes of the cells are in fact updated as if the edges which connect them were springs with a prescribed spring constant. This is what gives this method its name – the spring analogy approach. The user may modify the effective spring constant of this system to control the deflection of the nodes, which may be helpful in maintaining good mesh quality.
This method is available all cells types, though quad, hex, wedge, and pyramidal elements require a special command to activate spring analogy. In all cases, you need to examine the range of boundary motion to see if any unacceptable mesh distortion occurs.

42. Local Remeshing
As user-specified skewness and size limits are exceeded, local nodes and cells are added or deleted.
As cells are added or deleted, connectivity changes.
Available only for tri and tet mesh elements.
The animation also shows smoothing (which one typically uses together with remeshing).
If the range of boundary deformation is so large that cells will become highly skewed or collapse to zero volume, Fluent has the capability of remeshing the domain. As shown in this animation, cells are either added or deleted as part of remeshing process, thereby leading to a change in connectivity of the cells.
The remeshing is triggered when user-specified size and skewness limits are exceeded. The user has full control over these threshholds. In addition, the mesh can be smoothed to improve mesh quality after the remeshing. Once a new mesh is created, the solution is updated with full conservation on the new mesh.
Remeshing is only available for tri and tet elements, as these are the only types of cells for which a robust, automated meshing procedure has been developed.
It should be noted also that the fluid domain can never collapse entirely to zero volume, nor can the domain topology change.

43. Layering Cells are added or deleted as the zone grows and shrinks.
As cells are added or deleted, connectivity changes.
Available for quad, hex and wedge mesh elements.
The third method in the dynamic mesh toolbox is the layering approach. Here, cell layers are added of removed in response to the boundary motion. Again, the addition or removal of cell layers is triggered by mesh quality requirements, specifically cell aspect ratio and size. The user can adjust these triggers to control the layer process.
Layering is available for quad, hex, and wedge elements only.

44. Combination of Approaches
Initial mesh needs proper decomposition;
Layering:
Valve travel region;
Lower cylinder region.
Remeshing:
Upper cylinder region.
Non-conformal interface between zones.
For complex models, it is common to utilize more than one approach to handle the variety of boundary motions which may occur. Fluent permits the spring analogy, remeshing, and layering methods to operate together on a zone-specific basis. This use of multiple methods is demonstrated in the animation shown in this slide, which from a simulation of an automotive in-cylinder flow.

45. Dynamic Mesh Setup Enable unsteady solver.
Enable Dynamic Mesh model in DefineDynamic Mesh.
Activate desired Mesh Methods and set parameters as appropriate.
Define boundary motion in the Dynamic Mesh Zones GUI.
UDF may be required.
Other models, BCs, and solver settings are same as SRF, MRF models.
Mesh motion can be previewed using SolveMesh Motion utility.
Fluent will identify mesh quality problems if they occur during the preview.
Because of the complexity of the dynamic mesh modeling, setting up a dynamic mesh model in Fluent is more involved than other moving zone models.
You will first need to turn on the unsteady solver and define appropriate options depending on the flow solver selected (pressure-based vs density-based). Next, you will enable the dynamic mesh model in the GUI using DefineDynamic Mesh. You will then define the Mesh methods you wish to apply and set the parameters as appropriate. The boundary motions are defined in a separate GUI. Note that you may need to create a user-defined function to define the mesh motion. Other models, boudary conditions, and solver settings are the same as other moving zone models.
It is recommended that prior to running your model, you preview the mesh motion using SolveMesh Motion feature. You can run your mesh through a defined range of physical time, and thereby identifying problems with the mesh motion before you begin the actual CFD calculation.

46. Other Dynamic Mesh Options
2.5 D Mesh Motion
Special remeshing approach for extruded geometries.
Permits tri mesh to be extruded as wedge elements through volume.
Advantage – can handle small gaps better than tet elements.
User-Defined Mesh Motion
Mesh motion controlled through a UDF.
No change in mesh topology can occur.
Advantage – can provide for general mesh motions not possible with spring analogy, remeshing, or layer approaches.
6 DOF Model
Permits moving mesh surfaces to represent moving objects with defined mass, moments of inertia.
Motions of surfaces respond to pressures ans stresses computed by the CFD solution.
Gravitational and other forces can be added to force balance.
Additional information on these options are provided in the Appendix and the User’s Guide.
There are several other options and packages available for the dynamic mesh model.
The 2.5 Mesh Motion model is a special remeshing approach for extruded geometries. It makes use of 2-D triangle remeshing and applies this to one end of the geometry. The triangles are then extruded through the geometry to create the volume mesh. This approach is much more robust that 3-D tetrahedral remeshing (especially configurations with small gaps) but has the limitation that the geometry must permit extruded cells.
The User-Defined Mesh Motion approach permits you to handle mesh motion entirely through a UDF. This permits general mesh motions which are not possible with spring analogy, remeshing, or layering. One limitation of this approach is that you cannot change the mesh topology.
Finally, the 6 degree of freedom model (or 6 DOF) permits moving mesh surfaces to represent objects with defined masses and moments of inertia. The motions of the surfaces are determined by a force balance and therefore respond to the pressures and viscous stresses computed by the CFD solution. Gravitation and other forces can be added to the force balance for the objects, if desired.
For additional information on these features, please consult the Appendix of this presentation and the User’s Guide.

47. Outline Introduction and Overview of Modeling Approaches
Single-Reference Frame (SRF) Model
Multiple Zones and Multiple-Reference Frame (MRF) Model
Mixing Plane Model (MPM)
Sliding Mesh Model (SMM)
Dynamic (Moving and Deforming) Mesh Model
Summary
Appendix
We will now summarize the main points of this presentation.

48. Summary
Five different approaches may be used to model flows over moving parts.
Single (Rotating) Reference Frame Model
Multiple Reference Frame Model
Mixing Plane Model
Sliding Mesh Model
Dynamic Mesh Model
First three methods are primarily steady-state approaches while sliding mesh and dynamic mesh are inherently unsteady.
Enabling these models, involves in part, changing the stationary fluid zones to either Moving Reference Frame or Moving Mesh.
Most physical models are compatible with moving reference frames or moving meshes (e.g. multiphase, combustion, heat transfer, etc.)
Follow best practice guidelines provided in the previous slides.
In this presentation, we have covered the five different approaches for modeling moving zones. These are:
The single reference frame model
The multiple reference frame model
The mixing plane model
The sliding mesh model
The dynamic mesh model
Note that the first three approaches are primarily steady-state approaches while the sliding and dynamic mesh approaches are inherently unsteady.
Enabling these models primarily involves enabling either Moving Reference Frame or Moving mesh in the BC specification for the Fluid zones. Also note that any model which invokes Moving Mesh must employ the unsteady solver.
Most physical models are compatible with moving reference frames or moving meshes. This includes multiphase, combustion, heat transfer and other models.
Finally, to obtain robust solutions for most problems, it is suggested that you follow the best practice guidelines outlined in the previous slides.

49. Appendix Navier-Stokes equations for moving reference frames
Relative Velocity Formulation
Absolution Velocity Formulation
Navier-Stokes equations for moving mesh problems

50. N-S Equations: Rotating Reference Frame
Two different formulations are used in Fluent
Relative Velocity Formulation (RVF)
Obtained by transforming the stationary frame N-S equations to a rotating reference frame
Uses the relative velocity as the dependent variable in the momentum equations
Uses the relative total internal energy as the dependent variable in the energy equation
Absolute Velocity Formulation (AVF)
Derived from the relative velocity formulation
Uses the absolute velocity as the dependent variable in the momentum equations
Uses the absolute total internal energy as the dependent variable in the energy equation
NOTE: RVF and AVF are equivalent forms of the N-S equations!
Identical solutions should be obtained from either formulation with equivalent boundary conditions

51. Reference Frames y x z y x z rotating frame stationary frame axis of
CFD domain x
rotating
frame z
stationary
frame x z
axis of
rotation
Note: R is perpendicular
to axis of rotation

52. Assumptions and Definitions
No translation ( )
Steady rotation (w = constant) about specified axis
axis passes through origin of rotating frame
Ignore body forces due to gravity and other effects (for the equations shown)
Ignore energy sources (for the equations shown)
Definitions
Absolute velocity ( ) - Fluid velocity with respect to the stationary (absolute) reference frame
Relative velocity ( ) - Fluid velocity with respect to the rotating reference frame
3-D compressible, laminar forms of the equations presented in the following slides (other forms are similar)

53. Relative Velocity Formulation
(Continuity)
(Momentum)
(Energy)

54. Relative Velocity Formulation (2)
(Relative total internal energy)
(Viscous stress)
(Fourier’s Law)

55. RVF Accelerations Due to Rotating Frame
Coriolis
acceleration
centrifugal
acceleration

56. Rothalpy
Consider steady, adiabatic, inviscid flow within a flow passage in a rotating reference frame. The energy equation reduces to:
The quantity is known as the rothalpy.
From the above, it is seems that rothalpy is conserved for steady, inviscid flow in a rotating frame.
Rothalpy is also conserved for viscous flows if the flow passage walls are moving with the rotating frame (such that the relative velocity is zero on the rotating wall).

57. Absolute Velocity Formulation
(Continuity)
(Momentum)
(Energy)

58. Absolute Velocity Formulation (2)
(Relative total internal energy)
(Viscous stress)
(Fourier’s Law)

59. AVF Accelerations Due to Rotating Frame
Acceleration reduces to single term involving
rotational speed and absolute velocity

60. Velocity Formulation Recommendations
Use AVF when inflow comes from a stationary domain
Absolute total pressure or absolute velocities are usually known in this case
Example: Flow in a ducted fan system, where inlet is a stationary duct
Use RVF with closed domains (all surfaces are moving) or if inflow comes from a rotating domain
Relative total pressure or relative velocities are usually known in this case
Example: Swirling flow in a disk cavity
As noted previously, RVF and AVF are equivalent, and therefore either can be used successfully for most problems
Discrepancies on the same mesh can occur if the magnitude of absolute velocity gradients are very different than magnitude of the relative velocity gradients
Differences between solutions should disappear with suitable mesh refinement

61. Scalar Equations in a Moving Reference Frame
General form for a scalar transport equation referred to a moving frame can be written as follows:
Equation shows that scalars are convected along relative streamlines.
Gradients, source terms are defined with respect to the moving control volume.
Examples: turbulence model equation, species conservation equations, etc.

62. N-S Equations: Moving Mesh Form
The sliding mesh (aka moving mesh) and the dynamic mesh formulations assume that the computational domain moves relative to the stationary frame.
No reference frame is attached to the computational domain.
The motion of any point in the domain is given by a time rate of change of the position vector ( ).
is also known as the grid speed
For rigid body rotation at constant speed
Equations will be presented in integral form.

63. Moving Mesh Illustrationy
Moving CFD domain
stationary
frame x z
axis of
rotation

64. N-S Equations: Moving Mesh (1)
(Continuity)
(Momentum)
(Energy)

65. N-S Equations: Moving Mesh (2)
In the foregoing equations, W and are the volume and boundary surface of a moving control volume, respectively.
For the sliding mesh model, W remains constant since the mesh is not deforming.
For the moving/deforming mesh model, W = W (t), and is determined using the geometric conservation law (GCL):
The time derivative (d/dt) represents differentiation with respect to time following the moving control volume.
All spatial gradients are computed with respect to the stationary frame.

66. The 2.5 D Model
The 2.5D mesh essentially is a 2D triangular mesh which is extruded along the normal axis of the specific dynamic zone that you are interested in modeling.
Rigid body motion is applied to the moving boundary zones.
Triangular extrusion surface is assigned to a deforming zone with remeshing and smoothing enabled.
The opposite side of the triangular mesh is extruded and assigned to be a deforming zone as well, with only smoothing enabled.

67. User Defined Mesh Motion
Mesh motion is defined by the user through a User Defined Function (UDF).
No connectivity change is allowed if using UDF to move the mesh.
Useful applications include:
Vane pumps
Gerotor pumps
Bearing
Rotary compressors

68. 6 DOF Coupled Motion
Objects move as a result of aerodynamic forces and moments acting together with other forces, such as the gravity force, thrust forces, or ejector forces (i.e., forces used to initially push objects away from an airplane or rocket, to avoid collisions).
In such cases, the motion and the flow field are thus coupled, and we call this coupled motion.
Fluent provides a UDF (user-defined function) that computes the trajectory of an object based on the aerodynamic forces/moments, gravitational force, and ejector forces. This is often called a 6-DOF (degree-of-freedom) solver , and we refer to it as the 6-DOF UDF.
The 6-DOF UDF is fully parallelized.
Flowmeter2d.AVI

69. 6 DOF Coupled Motion (cont’d)
Store dropped from a delta wing (NACA 64A010) at Mach 1.2.
Ejector forces dominate for a short time.
All-tet mesh.
Smoothing - remeshing with size function.
Fluent results agree well with wind tunnel results!
Flowmeter2d.AVI