Best practice guidelines for turbomachinery CFD

From CFD-Wiki

Revision as of 14:53, 23 February 2007

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 example. For cases with many long blades or stators, like low-pressure turbines, a 2D simulation can also provide reasonable results. If the area of the flow-path changes 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 this type of simulations, or require user coding to implement the correct source terms in the equations.

Full 3D simulations are necessary if a true 3D geometry is needed to obtain correct secondary flows and/or shock locations. For cases with only a few short blades, like for example structurally loaded turbine outlet guide vanes, 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.

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. 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 a few type of effects are of interest. 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 periodic vortex shedding behind blunt trailing edges etc. This is often first seen as periodical variations of the residuals. If the periodic vortex shedding is 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.

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 geometries and cases where a structured mesh is difficult to create. Typical examples are features like 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. 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.

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 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

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