Best practice guidelines for turbomachinery CFD
From CFD-Wiki
Contents |
Introduction
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
Meshing
In general, for turbomachinery blading simulations a structured grid, especially in the boundary layers, is preferable and will most often provide superior accuracy over an unstructured grid.
Mesh size guidelines
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.
It is important to resolve leading and trailing edges well. Typically at least 10 cells, preferably 20 should be used around the leading and tralining edges. For very blunt and large leading edges, like those commonly found on HP turbine blades, 30 or more cells can be necessary.
Cases which are difficult to converge with a steady simulation and which show tendencies of periodic vortex shedding from the trailing edge, can sometimes be "tamed" by using a coarse mesh around the trailing edge. This, of course, reduces the accuracy but can be a trick to obtain a converged solution if time and computer resouces does not allow a transient simulation to be performed.
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.
If you are uncertain of which wall distance to mesh with you can use a y+ estimation tool to estitmate the distance needed to obtain the desired y+.
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
Describe different types of boundary conditions and when they should be used:
- 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 
. 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.
For off-design simulation, or simulations involving complex secondary flows and separations, it is often necessary to use a low-Re model. There exists many low-Re models that have been used with success in turbomachinery simulations. A robust and often good choice is to use a one-equation model, like for example the Wolfstein model, in the inner parts of the boundary layer. There are also several Low-Re models that work well. Just make sure they don't suffer from the problem with overproduction of turbulent energy in regions with strong acceleration or decelleration. In the last few years Menter's low-Re 
model has gained increased popularity.
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.
Tone noise possible. Often run with linearzised solvers in the frequency domain.
Jet noise possible. Often run with LES or DES simulations that either also resolve the sound waves or couples to a separate acoustic solver.
Turbomachinery broadband noise not possible yet, or at least a great challenge.
What to trust and what not to trust
CFD is generally quite good at predicting surface static pressure distributions. With care CFD can also be used to predict performance, total-pressure losses and blade turning.
Predicting separation, stall and off-design performance can be a challenge and results with non-attached flows should be interpreted with care.
Heat transfer is often very difficult to predict accurately and it is common to obtain heat-transfer coefficients that are 100% wrong or more. Validation data is critical in order to be able to trust heat transfer simulations.
Transition is almost impossible to predict accurately in general. However, there exist models that have been tuned to predict transition and these tend to give acceptable results for cases close to the ones they were tuned for.
External links
QNET-CFD Best Practise Advice for Turbomachinery Internal Flows
