• 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 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 shere, 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-rotatig 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 Zonne" 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 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 vortices of next blade (or wake behind the blade) that have just passed upwind affect the following blades or 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.
  • 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)s such as remeshing, adding and removing grid cells where necessary. For transonic and supersonic flows, this method is a must as unsteadiness is inherent due to shocks waves striking downstream blade (moving or stationary) row.
  • 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".


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.
  • 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.
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.