Best practice guidelines for turbomachinery CFD

From CFD-Wiki

Revision as of 10:23, 9 April 2007

This article contains a summary of the most important knowledge and experience a CFD engineer needs in order to perform CFD simulations of turbomachinery components. The guide is mainly aimed at axial turbomachinery. The goal is to give a CFD engineer, who has just started working with turbomachinery simulations, a head start and avoid some of the most difficult pit-falls. Experienced turbomachinery CFD engineers can also use the guidelines in order to learn what other experts consider best practice. The intended audience is expected to know basic CFD terminology and have a basic turbomachinery knowledge, but no detailed knowledge about CFD for turbomachinery is needed.

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 if 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 of one blade a mesh with say 3,000 cells is most often sufficient. For 3D inviscid blade simulations a mesh size of about 40,000 cells is usually sufficient. On inviscid Euler simulations the cells should be fairly equal in size and no boundary layer resolution should be present. Avoid having too skewed cells.

For loss predictions 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. For further information about selecting the near-wall turbulence model please see the turbulence modeling section. In 3D single-blade simulations 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 of a blade section 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 blade simlations 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 use about 100 cells in the streamwise direction. In the radial direction a good first approach is to use something like 30 cells for a wall-function mesh and 100 cells for a low-Re mesh.

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. The outer limit is dependent on the actual Re number of the simulations. For cases with fairly low Re numbers make sure to keep the maximum y+ as low as possible. 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 resolved 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 normal to the wall in the boundary layer of maximum 1.25. For a low-Re mesh this usually gives around 40 cells in the boundary layer whereas a wall-function mesh does not require more than 10 cells in the boundary layer.

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+. These estimation tools are very handy if you have not done any previous similar simulations.

As a rule of thumb a wall-function mesh typically requires areound 5 to 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
• ...

Turbulence inlet conditions

Prescribing realistic turbulence inlet conditions is important and usually difficult. For two-equation turbulence models two different turbulence values need to be specified on the inlet. The most common way of specifying the inlet turbulence variables is to give an inlet turblence level and length-scale. For simulations where the incoming boundary layers are estimated to not have any significant effect on the secondary flows and global flow-field downstream it is usually sufficient to specify a constant incoming turbulence level and length-scale.

The incoming turbulence level is dependent on which component is analyzed. Best is of course to have measurments from a similar application in order to be able to prescribe a fairly realistic value. Without measurements it is necessary to make an educated guess. Simulations with very complex and turbulence-generating components upstream will have a very high incoming turbulence level. For example, a high-pressure turbine just downstream of a turbulence generating combustor might have incoming turbulence levels up to 20%. Fans and low-pressure compressors with not many components upstream might have as low incoming turbulence level as 1%. For components between these two extreme examples, like high-pressure compressors, low-pressure turbines etc. a turbulence level of around 5% might be realistic. If you do not have any measurements and are unsure about which incoming turbulence level to prescribe it is always a good idea to run a few different simulations with say one half and one double incoming turbulence level in order to estimate how important it is for the simulation results.

The incoming turbulence length-scale is often even more difficult to guess than the incoming turbulence level. Measurements might sometimes include the incoming turbulence level, but very seldom also include the incoming turbulent length-scale. The best way of guessing a realistic incoming length-scale is to use the geometrical properties of the upstream components. The incoming turbulence length-scale can be estimated as say the thickness of upstream blades or somewhere between 2% and 20% of the incoming channel heigth. Fortunately the incoming turbulence length-scale is usually not that important for the end results. However, some k-omega models can have an unrelisticly strong influence on the incoming turbulence length-scale. Hence, be extra carefull about the length-scale when using k-omega models. Note that the SST k-omega model does not have this unrealistic sensitivity to the inlet turbulence length-scale.

Instead of specifying an incoming turbulence length-scale it is sometimes more convenient to specify an incoming eddy viscosity ratio. For low-turbulence cases with no well-specified turbulence generating components upstream it can be difficult to estimate a turbulence length-scale. Specifying an eddy viscosity ratio instead gives a more direct control over how large the effect of the incoming turbulence is. The eddy viscosity ratio describes how large the turbulence viscosity is related to the molecular viscosity. In turbomachinery the eddy viscosity ratio can vary from say 10 in low-turbulence components like fans up to say 1,000 or in rare cases even 10,000 in high-turbulence components like high-pressure turbines. In components between these extremes a typical eddy viscosity ration might be about 200. Even if specifying an inlet turbulence length scale it can still be good to compute what eddy viscosity ratio this corresponds to in order to estimate if it sounds reasonable.

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.

Errors and uncertainties

CFD is still a tool which requires that a user has a good understanding of uncertainties and errors in a CFD similation. Without some knowledge about possible errors and how they can be handled a CFD simulation can not be trusted. Errors can occur at different places:

• Definition of the problem - What needs to be analyzed.
• Selection of the solution strategy - What physical models and what numerical tools should be used.
• Development of the computational model - How should the geometry and the numerical tools be set up.
• Analysis and interpretation of the results - How should the model be analyzed and the results be interpreted.

There exists many different definitions on errors. In this guide the errors are classified into three different types of errors:

• Model errors

Errors related to the computational model. This can be either the selection of the type of simulation to perform, errors in the supplied boundary contitions or the used geometry.

• Numerical errors

Errors related to the numercial solution of the developed model. Typical examples of numerical errors are discretization errors, convergence errors and round-off errors.

• User and code errors

Errors related to bugs in the code used or misstakes made by the CFD engineer.

The chapters below describe these types of errors and give some guidelines on how to avoid them.

Model errors

Wrong type of simulation

When starting a CFD simulation it is essential to get an overview of the physics involved and how the problem can best be analyzed. Running a 2D simulation in order to understand secondary flows or running a steady simulation in order to understand transient behaviour is of course no use. To select the most appropriate type of simulation to perform it is good to consider the following points:

1. 2D or 3D
2. Transient or steady
3. Single or multi-stage

Wrong physical models

Once the type of similation has been selected the next step is to select what type of physical models the simulation should use. The following points should be considered:

1. Gas data
2. Turbulence modeling
3. Other models (combustion, sprays, ...)

Boundary condition errors

Geometrical errors

Numerical errors

Discretization errors

Convergence errors

Round-off errors

User and code errors

External links

QNET-CFD Best Practise Advice for Turbomachinery Internal Flows