CFD Online Logo CFD Online URL
Home > Wiki > Best practice guidelines for turbomachinery CFD

Best practice guidelines for turbomachinery CFD

From CFD-Wiki

Revision as of 23:42, 13 February 2007 by Frmonto (Talk | contribs)
Jump to: navigation, search



This guide is mainly aimed at axial turbomachinery. Feel free to extend it to other types of turbomachinery though.

Deciding what type of simulation to do

2D, Quasi-3D or 3D

Inviscid or viscid

Transient or Stationary


In turbomachinery application, generally, structured meshes are used for the analysis fo flow path, generally during the design process. The main advantace using structured meshes is the time required by the operator to generate the mesh (a lot of companies have in house mesh generators able to mesh a standard blade in few seconds); in addition coupling a structured solver and a structured mesh is it possible to have a very fast design tools. The unstructured meshes are used generally to study the blade and other features like blade tip, wheel space, film cooling ducts etc. In the second case generally the computational time required with the same number of elements is higher (if in the first case a structured solver is chosen) related to the elements connections (in a structured mesh is trivial, in an unstructured grid an array is required to store the connectivity).

Mesh size guidelines

It is difficult to define, a priori, the mesh size. Mainly this depends on the purpose of the simulation. If the main goal is to obtain pressure forces a coarse mesh is able to obtain a good solution and not an accurate resolution of boundary layer is required (an inviscid calculation with a kutta condition on trailing edge is able to detect quite well the loading of a blade, if separations are not presents).

For losses prediction the mesh have to be denser in the BL region. Check if the BL is currently represented by the solution. For the heat transfer is really difficult to give a general rule. In all simulation the distance of first node to the wall is related to the turbulence closure but this is really important in heat transfer prediction.

In 3D a decent wall-function mesh typically has around 100,000 cells. This type of mesh size is suitable for quick design iterations where it is not essential to resolve all secondary flows and vortices. A good wall-function mesh intended to resolve secondary flows well should have at least 400,000 cells. A good low-Re mesh with resolved boundary layers typically has around 1,000,000 cells.

In 2D a good wall-function mesh has around 10,000 and a good low-Re mesh with resolved boundary layers has around 30,000 cells.

Boundary layer mesh

For design iteration type of simulations where, a wall function approach is sufficient, y+ for the first cell should be somewhere between 30 and 300. For more accurate simulations with resolved boundary layers the mesh should have a y+ for the first cell which is below 1. A good rule of thumb is to use a growth ratio in the boundary layer of 1.2 - 1.25.


As a rule of thumb a wall-function mesh typically requires about 10 cells in the boundary layer whereas a resolved low-Re mesh requires about 40 cells in the boundary layer.

Boundary conditions


  • Total pressure in, static pressure out
  • Absorbing boundary conditions
  • ...

Describe how to select inlet turbulence level and length-scale

Turbulence modeling

Selecting a suitable turbulence model for turbomachinery simulations can be a challenging task. There is no single model which is suitable for all types of simulations. Which turbulence model CFD engineers use often has as much to do with beliefs and traditions as with knowledge and facts. There are many diffrent schools. However, below follows some advices that most CFD engineers in the turbomachinery field tend to agree upon.

For attached flows close to the design point a simple algebraic model like the Baldwin-Lomax model can be used. Another common choice for design-iteration type of simulations is the one-equation model by Spalart-Allmaras. The big advantage with both the Baldwin-Lomax model and the Spalart-Allmaras model over more advanced models are that they are very robust to use and rarely produce complete unphysical results.

In order to accurately predict more difficult cases, like flows that are close to or even fully separated, rotating flows, flows strongly affected by secondary flows etc. it is often necessary to use a more refined turbulence model. Common choices are a two-equation models like the k-\epsilon. k-\epsilon models can give good results but this type of models need to include some form of correction to avoíd over-production of turbulent energy in regions with strong acceleration or decelleration. Typical such corrections are some form or realizability constraint or the Kato-Launder modification. Antoher common choice in turbulence model is Menter's SST k-omega model or the slightly more elaborate v2f model by Durbin.

Near-wall treatment

For on-design simlations without any large separated regions it is often sufficient to use a wall-function model close to the wall, preferably using some form of non-equilibrium wall-function that is sensitised to streamwise pressure gradients.


Transition prediction

Transition refers to the process when a lamainar boundary layer becomes unstable and transitions to a turbulent boundary layer. There are two types of transition - natural transition, where inherent instabilities in the boundary layer cause the transition and by-pass transition, where convection and diffusion of turbulence from the free-stream into the boundary layer causes transition.

Numerical considerations

Multi-stage analysis

Types of analysis:

  • Frozen rotor
Frozen rotor defines the domain interface to transfer flow and thermal data across the interface between the stationary and rotating domain. Frozen rotor interface connects the two doamins (rotating and stationary) in such a way that these two domains have a fixed relative position throughout the solution, but with desired frame transformation occurring across the interface. Transient effects cannot be modelled with this interface. This the the only disadvantage of the frozen rotor interface.
  • Mixing-plane

In the Mixing-plane also called as "Stage-Interface" approah in the commercial code CFX, variables are circumferentially averaged before passing from one domain to the other, say for instance from stator to rotor. This is used typically when there are blade rows on either sides of the interface. The advantage in this approach is that only one blade passage need to be modeled. One situation where this is less appropriate is while simulating impeller and a volute in a pump/ compressor. Transient effects are completely ignored and often this approach closely matches test data near design point.

  • Sliding-mesh
  • Time-inclinded
  • Adamszyk stresses ...

Describe how to scale blade-sections when doing sliding-mesh computations

Heat transfer predictions

Acoustics and noise

A whole separate research subject, difficult.




What to trust and what not to trust





External links

QNET-CFD Best Practise Advice for Turbomachinery Internal Flows

My wiki