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
2D simulations are often used in the early design phase in order to obtain a typical 2D section of a blade. For cases with many long blades or vanes, like low-pressure turbines, a 2D simulation can also provide reasonable results. If the area of the flow-path changes significantly in the axial direction it might be necessary to instead make a Quasi-3D simulation. A quasi-3D simulation is a 2D simulation in which extra source terms are used to account for the acceleration/decelleration caused by a changing channel height or growing endwall boundary layers. Codes focused on turbomachinery applications often have the possibility to perform quasi-3D simulations, but most general purpose commercial CFD codes can not do this type of simulations, or require user coding to implement the correct source terms in the equations. Please contact your software distributor if your code does not have this possibility and you require it. Many codes require special routines or hidden commands to enable the quasi-3D feature.
Full 3D simulations are necessary if a true 3D geometry is needed to obtain correct secondary flows and/or shock locations. For low-aspect-ratio cases with only a few short blades, like for example structurally loaded turbine outlet guide vanes, the secondary flow development is important and a 3D simulation is often necessary in order to obtain reasonable results. For applications where the endwall boundary layers grow very quickly and interact with a large part of the flow-field it is necessary to perform a full 3D simulation. This is often the case in compressors and fans, where the negative pressure gradients make the boundary layers grow much quicker than what they do in for example turbines. For cases where the shock location is very critical, like in transonic compressors, it is also often necessary to perform a 3D simulation in order to obtain reasonable shock locations.
Inviscid or viscid
For attached flows close to the design point and without any large separations it is often sufficient with an inviscid Euler simulation in order to obtain reasonable blade loadings and pressure distributions. Note that inviscid Euler simulations should only be used it the boundary layers are judged to not have a significant effect on the global flow-field. A viscid Navier-Stokes simulation is necessary in order to predict losses, secondary flows and separations. As soon as separations are of interest it is of course also necessary to do a viscid simulation.
Transient or Stationary
Most turbomachinery simlation are performed as stationary simulations. Transient simulations are done when some kind of transient flow behaviour has a strong influence on the global flow field. Examples of transient simulations are detailed simulations of rotor-stator interaction effects, simulations of large unsteady separations etc. Sometimes when you perform a steady stationary simulation you can see tendencies of unsteady behvaiour like for example periodic vortex shedding behind blunt trailing edges. This is often first seen as periodical variations of the residuals. If the unsteady tendencies are judged to not affect the overall simulation results if might be necessary to coarsen the mesh close to the vortex shedding or run a different turbulence model in order to make the simulation converge. Sometimes you are still forced to run a transient simulation and average the results if you don't obtain a converged steady solution.
Meshing
In turbomachinery applications structured muli-block hexahedral meshes are most often used for flow-path simulations. In most solvers a structured grid requires less memory, provides superior accuracy and allows a better boundary-layer resolution than an unstructured grid. By having cells with a large aspect ratio around sharp leading and trailing edges a structured grid also provides a better resolution of these areas. Many companies have automatic meshing tools that automatically mesh blade sections with a structured mesh without much user intervention.
Unstructured meshes are used for more complex and odd geometries where a structured mesh is difficult to create. Typical examples where unstructured meshes are often used are blade tip regions, areas involving leakage flows and secondary air systems, film cooling ducts etc.
Mesh size guidelines
It is difficult to define, a priori, the mesh size. The required mesh size depends on the purpose of the simulation.
If the main goal is to obtain static pressure forces a coarse mesh is often able to obtain a good solution, especially when an accurate resolution of the boundary layers is not required. For 2D inviscid simulations a mesh with say 3,000 cells is most often sufficient. For 3D inviscid simulations a mesh size of about 40,000 cells is usually sufficient. On inviscid Euler simulations the cells should be of fairly equal size and no boundary layer resolution should be present.
For loss prediction and cases where boundary layer development and separation is important the mesh needs to have a boundary layer resolution. The boundary layer resolution can either be coarse and suitable for a wall function simulation or very fine and suitable for a low-Re simulation. 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 3D 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 20,000 cells and a good low-Re mesh with resolved boundary layers has around 50,000 cells.
Along the suction and pressure surfaces it is a good estimate to use about 100 cells in the streamwise direction. In the radial direction a good first approach is to use something like 40 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 20 and 200. For more accurate simulations with resolved boundary layers the mesh should have a y+ for the first cell which is below 1. Some new codes are now using a hybrid wall treatment that allows a smooth transition from a coarse wall-function mesh to a resolver low-Re mesh. Use some extra care when using this type of hybrid technique since it is still fairly new and unproven.
Otside of the first cell at a wall a good rule of thumb is to use a growth ratio nomral to the wall 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 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. This model has become more popular in the last years due to the many inherent problems in more refined two-equation models. The big advantage with both the Baldwin-Lomax model and the Spalart-Allmaras model over more advanced models is that they are very robust to use and rarely produce completely unphysical results.
In order to accurately predict more difficult cases, like separating flows, rotating flows, flows strongly affected by secondary flows etc. it is often necessary to use a more refined turbulence model. Common choices are two-equation models like the 
model.
Two-equation models are based on the Boussinesq eddy viscosity assumption and this often leads to an over-production of turbulent energy in regions with strong acceleration or deceleration, like in the leading edge region, regions around shocks and in the suction peak on the suction side of a blade. To reduce this problems it is common to use a special model variant using, for example, Durbin's realizability constraint or the Kato-Launder modification. Note that different two-equation models behave differently in these problematic stagnation and acceleration regions. Worst is probably the standard model. 
model are slightly better but still do not behave well. More modern variant like the Menter's SST k-omega model also have problems wheras the more v2f model by Durbin behaves better.
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 deceleration. In the last few years Menter's low-Re 
model has gained increased popularity.
Transition prediction
Transition refers to the process when a laminar 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
Use at least a second order accurate scheme for the flow variables. Some codes require a first order scheme for the turbulent variables (
and 
) in order to converge well. It is often sufficient with a first order scheme there, but a second order scheme is of course preferable.
Round-off errors
With todays computers and cheap memory prices it often does not cost much extra to run in double precision. Before using single precision you should first investigate how your software and hardware works with double precision. If the extra time and memory needed for double precision is negligible you should of course always run in double precision. With double precision you never have to worry about round-off errors. So always using double precision is one way of avoiding one type of pit-falls in the complex world of CFD simulations.
When using single precision care needs to be taken to avoid round-off errors. Inviscid Euler simulations and simulations using wall-function meshes can most often be performed in single precision. For well resolved boundary layers with Y plus close to 1 it is often necessary to use double precision. If using double precision for very fine mesh resolutions make sure that you also create the mesh in double precision and not just run the solver in double precision. Sometimes a single precision solver converges slower than a double precision solver due to numerical errors caused by round-off errors. When using advanced physical models like combustion, free-surface simulations, spray and transient simulations with quick mesh motions it is also often necessary to use double precision.
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
