• CFD, Fluid Flow, FEA, Heat/Mass Transfer
  • +91 987-11-19-383
  • amod.cfd@gmail.com

CFD Simulation approaches for Turbomachines

Multiple Reference Frame, Sliding Mesh Motion

CFD simulation approach for turbomachines as such centrifugal pump and blowers, appropriateness of various modeling approaches such as Single Reference Frame (SRF), Multiple Reference Frame (MRF) or Frozen Rotor Method, Sliding Mesh Motion (SMM) and application to industrial problems.

  • SRF: This method is used when the computational domain is axi-symmetric. This is called 'single' reference frame because only one reference frame (which is rotating) needs to be defined. This method can be used when whole geometry (the computational domain) can be assumed rotating.
  • MRF: This method uses more that one reference frames - at least one stationary and 1 rotating. This is also known as Frozen Rotor Method (FRM) as the rotating parts are kept frozen in position and rotation is accounted for by the additional source therms through inclusion of centrifugal and Coriolis forces. Even for the cases where transient simulation is required, MRF method is useful for attaining initial values for time-dependent simulations where the pseudo-steady state can be reached within a few revolutions starting from zero initial velocity.
    • MRF used simple local transformation of flow variables at the grid interfaces and hence the flow should be nearly uniform at the interface.
    • Result is influence by 'frozen' position of rotating components. Hence, the validity of result should be throughly checked when either the number of blade count is low or the speed of rotation is relatively low.
    • MRF result will be inaccurate when flow cross the interface from both direction - that is when flow enters and leaves the outer boundary of rotating domain.
  • Mesh: The mesh (elements and nodes) inside the rotating domain including external or internal boundaries rotate as a solid body with the rotation angular speed specified about the axis of rotation.
  • Walls: In order to account for wall shear, solver needs to know the speed of the wall. Any external or internal wall inside the rotating domain is assumed to rotate at the speed of the domain. If a wall defining the boundary of rotating domain is required to be defined stationary, it either needs to be specified as "counter-rotating wall" or its angular velocity needs to be defined as "0 [rad/s]". In FLUENT, this can be achieved using the feature motion "Relative to Adjacet Cell Zone" or 'Absolute'.
  • Governing Equations: In both SRF and MRF methods, the momentum conservation is governed by the Navier-Stokes equations, and the mass conservation is governed by the continuity equation. Both SRF and MRF methods are called steady-state approach (or pseudo-transient due to usage of psuedo time stepping) where the solution is time independent and rotation is achieved through mesh fixed in space and time.
  • SMM: In Sliding Mesh Motion the rotation is achieved through moving mesh functionality which is a time dependent process and hence known as transient simulation approach. This is specially true when (a)vortices of next blade (or wake behind the blade) that have just passed upwind affect the following blades or (b)flow unsteadiness due to pressure waves which propagate both upstream and downstream.
    • Note that the mesh motion can be constant speed or accelerating – the solver accommodate both situations.
    • In the SMM formulation, the motion(s) of moving zone(s) is tracked relative to the stationary reference frame where the motion of any point or node in the domain is given by a time rate of change of the position vector - known as grid speed.
    • SMM and DMM uses same equations where in case of DMM has additional feature for nodes to move relative to each other. Hence, SMM can be assumed to be a subset of more general DMM method.
    • For each time step, the meshes nodes are rotated and the fluxes at the sliding interfaces (interface at the stationary and rotating) are recomputed.
    • Time steps for transient simulation is a function of element size (Δs) at the sliding interface. The time steps should always be less that it requires a moving / rotating cells to cross past a stationary point at the interface that is Δt ≤ Δs/ω/r where ω is the rotational speed of moving domain and r is the radius of sliding interface.
    • The mesh interface between rotating and stationary domains must be situated such that there is no motion normal to it.
    • The common boundary or mesh interface can be any shape (including non-planar surfaces) provided the two interface boundaries are derived from a set of common geometrical entities (lines in 2D and surfaces in 3D).
    • By default, the velocity of wall is zero relative to the motion of the mesh or cell zone it is attached to. For walls bounding a moving mesh this imposes the "no-slip" condition in the reference frame of the mesh. Hence, one need to modify the wall velocity boundary conditions only if its stationary in the absolute frame and therefore moving in the relative frame. For example, shroud of fan is a stationary wall bounding the rotating reference frame defined for the blades. Hence, its velocity should be explicitly set to ZERO.
  • Selection of interface and its location
    • An interface is a MUST between rotating and stationary regions (domains or zones). Sometimes, such surface zones can be set as 'interior' instead of an interface.
    • However, such 'interfaces' must be a surface of revolution having axis of revolution coinciding with the axis of revolution of the rotating zones and walls.
    • The recommended practice (which is most obvious 1st guess sometimes) to chose the location of such interface(s) is the mid-way between the tip of rotating walls (or the blade tip) and the nearest stationary housing walls. Sometimes, the location of interfaces are also governed by meshing considerations (such as number of boundary layers on the walls of the blades) and free mesh size beyond this region.
    • For rotating domains embedded in relative large domains (such as a fan relative very small as compared to room), the recommendation is to have the interface at a location where flow is likely to be uniform.
    • Note that there is a significant difference between "Rotating Frame" and "Rotating Mesh".
  • DMM: In all the cases described above, the rotating and stationary parts do not change the shape or geometry. When the parts change shape and/or size, a Dynamic Mesh Model (DMM) method is required which allow changes to be made to the mesh (as solution progresses) such as remeshing, adding and removing grid cells where necessary. There are two types of mesh motions:
    1. prescribed translation (such as motion of piston and valves in engines), rotation (motion of teeth in gear pumps) or combination of translation and rotation (motion of teeth in helical pumps).
      • Since movement is known a priori, a sequence of meshes can be generated to accommodate the motion of the boundaries. In between those generated meshes the mesh can be deformed (for example stretching and compression) according to the prescribed boundary movement.
      • In situation where sliding interfaces need to be created in very tight clearances such as screw pumps, continuous mesh adaptation - even at every time step - might be required.
      • It is when the deformation of the mesh is excessive that the deformed mesh can be replaced with a new generated one (e.g. layer addition and deletion in case of translation of boundary or linear deformation of the fluid zone).
      • Note that the motion is prescribed at the solid boundaries and not at the mesh representing fluid volume which shape and size changes.
      • The motion of each point and cell in the mesh needs to be calculated so that the mesh remains topologically consistent to the changes in shape and size of the fluid domain.
      • During the mesh deformation process, a finite element method is used based to the Laplacian equation (∇.κ∇u = 0) for estimating the velocity and location of the mesh points, either with a constant or variable diffusivity κ. The added diffusivity controls the mesh deformation and quality.
    2. motion induced by flow field which is dependent of the solution of flow field itself such as aero-elesticity and fluid-structure interactions (FSI). A noticeable difference with prescribed mesh motion is that the deformation in this category of applications are low and mesh regeneration is rearely required.
    3. Typically, a DMM simulation can consist of up to 4 different zones. This is demonstrated by application of DMM for simulation of flow in an internal combusion engines.
      • Deforming zone: This refers to the mesh which will deform which the simulation. This zone or volume in 3D consists of cylinder volume bounded by piston, liner, head and valves. The zone deforms by the valve and piston motion.
      • Layering Zone: This zone represents the valve motion and it located above the valve, between valve curtain and valve stem. As the name suggest, mesh layers are added / deleted during the simulation. Whenever the mesh quality in the deforming zone or layering zone deteriorates beyond a pre-defined value, mesh is regenerated by adding or removing layers in the layering zone and remeshing the deforming zone by adding (refining) or removing (coarsening) cells (depending on if the cells are compressed or stretched during piston motion).
      • Rigid Motion Zone: This is located between the layering zone and the valve. This zone keeps its geometrical shape throughout the whole engine cycle, but follows the valve motion. The function of the rigid motion zone is to capture the concave valve shape without affecting the layering zone. In this way it is easier to make new meshes at different valve lifts by simply adding or removing layers of cells in the layering zone. It also helps to preserve the mesh quality in the area of the valve exit.
      • Static Zone: This zone consists of all volumes that are unaffected by boundary motion and as the name suggests they keep their geometry and shape during the whole engine cycle. This zone includes all remaining volumes in the intake and exhaust ports.
  • Immersed Solid Approach: ANSYS CFX uses an immersed solid approach to model to model steady-state or transient simulations involving rigid solid objects that can move through fluid domains such as lobe pump, gear pumps and axial flow fans. The immersed solid is represented as a moving walls (or two counter-rotating moving walls in case of gear pumps) and a source term in the fluid equations that drives the fluid velocity to match the solid velocity. Some of the limitations of this approach are: the immersed solid domain cannot undergo mesh deformation and the surfaces of the immersed solid body are not explicitly resolved by the mesh. In addition, a wall function cannot be applied to the boundary of an immersed solid and hence the accuracy of simulation results may be lower than can be obtained using mesh deformation methods or other techniques that support the use of wall boundaries to directly resolve solid surfaces.
  • Mixing Plane Method: MPM is available in ANSYS FLUENT. When a axial flow compressor or turbine stage needs to simulated with different values of periodic angles of rotor and stator, this approach becomes necessary. A "mixing plane" is defined at the interface of rotor and stator.
    • Like MRF, MPM is a steady-state approach, that is the mixing plane model is useful for predicting steady-state flow in a turbomachine stage when local interaction effects (such as wake and shock wave interaction) are weak.
    • After a prescribed number of iterations, the flow data at the mixing plane interface are (by default area-)averaged in the tangential (circumferential) direction at the interface: on both the rotor outlet and the stator inlet faces.
    • If rotor-stator interaction effects are important, then a transient sliding mesh calculation is required.
    • Note that the mass flux for the rotor portion and stator volume would be different as periodic angles are also different. However, for a complete 360° domain, the mass fluxes for rotor and stator should be equal.

    Flow inside a centrifugal blower for HVAC applications
    Centrifugal blowers have far too many applications. Automotive HVAC is one of them. Following picture demonstrates typical layout of blower inside the heating module for automobiles.
    Heating Module for Automotive Applications

    The purpose of this demonstration is:
    • to gain insight into the operation of a centrifugal blower, effect of casing on pressure recovery
    • develop an optimized throat shape, size and location
    • execute basic optimization using 2D simulation
    • use the 2D mesh to generate the 3D mesh, a novel use of mesh extrusion
    • assess the improvement in results using Sliding Mesh Model (SMM) over Multiple Reference Frame (MRF) model
    • study the effect of clearances between blade and casing on overall performance - 3D simulation
    • check for the issues observed when solution for SMM is initialized with a converged MRF solution vs. full transient start where flow field is uniform.
    The computational domain consists of a cascade of 40 forward-curved blades rotating at 50 Hz.
    2D Mesh - Centrifugal Blower

    The boundary condition, material properties and solver setting are
    • Incompressible air at 25 [C] and 1 [atm] resulting in density of 1.185 [kg/m3.
    • Realizable k-ε model with enhanced wall treatment
    • Coupled solver with 2nd order discretization schemes for mass, momentum and turbulence

    The results with Shear Stress Transport (SST) turbulence model is presented in following plots.
    The plots Y+, velocity contour and wall shear on top wall are shown here.
    Static Pressure Contour in a Centrifugal Blower
    Figure: Static Pressure Contour

    Velocity Contour in a Centrifugal Blower
    Figure: Velocity Contour

    Velocity Vector in a Centrifugal Blower
    Figure: Velocity vector plot

    Velocity Vector at Throat Region of Centrifugal Blower
    Figure: Velocity vector near discharge throat indicating small amount of back-flow

    New design of the throat of the Centrifugal Blower
    Figure: New design of the discharge throat
    • The calculated mass flow rate per unit [that is 1 m] depth of the blade is 4.72 [kg/s].
    • Small level of reverse flow observed near the throat area which has been handles by redesign of this section and extending the outlet. Free-slip wall boundaries can be applied to eliminate the effect of extended domain.
    • The location of throat is very close to the optimal design and there is no back flow into the blade cascade from the discharge region.

    Cyclone Separators

    • Cyclone separators are being used in industries for more than a century. This device falls under the category of what is called "Industrial Duct Collectors".
    • Dust separation process utilize different methods ranging from fabrics (such as Air Cleaners in Automotive Intake Systems) to Electrostatic Precipitators in Coal-fired power plants
    • Cyclone separators fall under the category of inertial separators which uses combination of the 3 most prevalent mechanical forces namely gravitational, centrifugal and inertial. In a cyclone, a high speed flow of fluid is established by tangential entry into a cylindrical geometry followed by a conical section. The tangential entry of fluid stream result in a rotating and translating (swirling) pattern, beginning at the top and ending at the bottom conical end. Heavier particles in the rotating stream gets thrown out due to centrifugal forces and strike the outside wall, falling along the wall then to the bottom exit of the cyclone where they are collected. In the conical section, due to conservation of angular momentum, as the rotational radius of the stream is reduced, the tangential component of velocity is increased throwing out lighter and smaller particles, leading to separating of smaller particles, even up to size of 5 microns.
    • The pressure loss and collection efficiency are two key performance parameters of this device.

      Cyclone Separators

      Design of Cyclone Separators

    • Despite such a long history of application in industry, the design principles so far as mostly based on empirical data. Recently, CFD techniques is being used to optimize the designs.
    • 4 geometrical parameter which is tightly linked with the performance of cyclone separators are
      • Vortex finder diameter
      • Inlet width
      • Inlet Height
      • Total Height of the Cyclone
    • The cone-tip diameter of the separator does not have noticeable effect on its performance.

    Gear Pumps

    Gear pumps with involute profile of Gerotor type and lobe pumps are two category of devices which require a dynamic mesh motion to solve the flow field.

    Gear Pump

    Gear pumps fall under the category known as "positive displacement pumps". The volume flow rates for such pumps and blowers are the volume created by the rotation of the moving cavity. The net volume flow rate is reduced by the leakage flow between the rotating / deforming cavity and leakage between the rotating walls and the stationary housing.

    Centrifugal Pumps

    Centrifugal Pump


    1. ANSYS FLUENT User Manual
    2. Study of mesh deformation features of an open source CFD package and application to a gear pump simulation: Alejandro Roger Ull, ETSEIAT 2012
Contact us
Disclaimers and Policies

The content on CFDyna.com is being constantly refined and improvised with on-the-job experience, testing, and training. Examples might be simplified to improve insight into the physics and basic understanding. Linked pages, articles, references, and examples are constantly reviewed to reduce errors, but we cannot warrant full correctness of all content.