[fluentmonkey]

Quick question: What happens when you use a turbulent model in a system where the flow is laminar? Apart from computational costs, how would this affect the result? Would the result be exactly the same as using a laminar model?

The reason I ask this is, in my limited time with CFD, I have just modelled systems that have had some turbulence in them. I modelled a system and, as I usually do, turned on the turbulent parameters within the software without really thinking. I ran the analysis, did mesh studies, y+ etc. However, after all this, when I looked at the boundary inlet, and did some 'hand calculations', I realised, in this particular case, the flow entering had a Reynolds number of 2130, which is laminar. The crunch is, do I have to go back and re-run the analysis with a laminar model, or does it not matter? I used a k-omega model.

Cheers!

[Martin Hegedus]

Your Reynolds number is quite small. The use of a turbulence model will have an effect, how much depends on the level of the eddy viscosity compared to your laminar viscosity. If the ratio is greater than 5, definitely expect differences. But, considering your low Reynolds number, it might not be. It is also a function of your incoming turbulence. Best thing to do is plot up your eddy viscosity and see what it looks like. Also, run a sample set of laminar runs and see how they compare to the ones when using a turbulence model.

[cfd_newbie]

Originally Posted by Martin Hegedus

Your Reynolds number is quite small. The use of a turbulence model will have an effect, how much depends on the level of the eddy viscosity compared to your laminar viscosity. If the ratio is greater than 5, definitely expect differences. But, considering your low Reynolds number, it might not be. It is also a function of your incoming turbulence. Best thing to do is plot up your eddy viscosity and see what it looks like. Also, run a sample set of laminar runs and see how they compare to the ones when using a turbulence model.

Here is what i believe -
(Someone please correct me if I am wrong here)
It's always safe to run a turbulent simulation, because the flow might be laminar at the inlet, but it might turn turbulent after interacting with the geometry. If that is the case I don't think laminar simulation will be able to capture it properly. Can someone elaborate on this topic ?
Raashid

[Martin Hegedus]

Because of the small Reynolds number, I am assuming that the flow features are large-ish when compared to geometry scales.

Fluentmonkey should say more about what he is modeling to give a better answer.

[cfd_newbie]

Originally Posted by Martin Hegedus

Because of the small Reynolds number, I am assuming that the flow features are large-ish when compared to geometry scales.

Fluentmonkey should say more about what he is modeling to give a better answer.

This is a more general doubt that I have.

1. Is there a definite way by which we can say a flow is laminar/turbulent or in transition ? Is it not dependent heavily on the geometry shape and it is more difficult to define weather a flow is laminar or turbulent for bodies with complicated geometry (like flow over a terrain or flow over an oil rig where there is no single fixed reference length).

2. If we know for sure that a flow is turbulent but we run it as a turbulent simulation, will not the artificial numerical turbulence die on it's own ?
In other words what are the pits falls of our choice.

Thanks in advance to anyone who enlighten me with these doubts.
Raashid

[Martin Hegedus]

Truthfully, I'm not sure what the pitfalls of our choices are.

1) yes defining the reference length is challenging. I don't think there is a good answer. That is part of the art.

2) The eddy viscosity doesn't necessarily die out, or at least die out where it should.

[cfd_newbie]

Originally Posted by Martin Hegedus

Truthfully, I'm not sure what the pitfalls of our choices are.

1) yes defining the reference length is challenging. I don't think there is a good answer. That is part of the art.

2) The eddy viscosity doesn't necessarily die out, or at least die out where it should.

Hi Martin,
Thanks for the reply.
I want to ask weather there is a easy way of predicting weather a flow is laminar or turbulent. To determine if a flow is separated or not there is a very easy way of using surface streamlines (or oil flow patterns) in any major CFD post-processing software. Is there a similar way by which we can determine this ?

I have had some past experience in high speed external aerodynamic flow for such problems, laminar to turbulence transition is of relatively lower importance (Since the flow becomes turbulent very easily) than flow separation. But for low speed problems transition occurs much later is is more difficult to predict. So I want to know is there a definitive and easy way of analyzing if the flow is laminar or turbulent.

[Martin Hegedus]

I usually look at the eddy viscosity since eddy viscosity is created where the turbulence model thinks there is turbulence. Of course the turbulence model could be wrong...

You can also check out the parameters used as variables for the turbulence source model, such as vorticity for the SA model.

[julien.decharentenay]

Hi,

Imposing a turbulence model to a laminar scenario usually results in higher dissipation. But, as Martin pointed out, it is best to put it to the test.

On the subject, have a look at the poster presentation http://www.cats.rwth-aachen.de:8080/...er-FDA2009.pdf . The Re 500 scenario is laminar. The simulations conducted with turbulence model show a sharper decrease in centreline velocity.

[solique]

Originally Posted by julien.decharentenay

Hi,

Imposing a turbulence model to a laminar scenario usually results in higher dissipation. But, as Martin pointed out, it is best to put it to the test.

On the subject, have a look at the poster presentation http://www.cats.rwth-aachen.de:8080/...er-FDA2009.pdf . The Re 500 scenario is laminar. The simulations conducted with turbulence model show a sharper decrease in centreline velocity.

According to my knowledge, the laminar model is best imposed to those fully developed low Re flow. But there are more chances to model those with lots of entries and complext structures, where we cannt simply say the flow is fully developed. At this time, even the Re is very low, what model we should use? I was told that using turbulence model only cost more time in calculation but the result will be right also? Is it right?

Also for some instances, the Re range in a scenario could vary from hundreds to thousands, but as we can only use one model in the calculation, we have to choose the turbulence?

Am I right?

Victor

[mohammad]

Originally Posted by Martin Hegedus

Your Reynolds number is quite small. The use of a turbulence model will have an effect, how much depends on the level of the eddy viscosity compared to your laminar viscosity. If the ratio is greater than 5, definitely expect differences. But, considering your low Reynolds number, it might not be. It is also a function of your incoming turbulence. Best thing to do is plot up your eddy viscosity and see what it looks like. Also, run a sample set of laminar runs and see how they compare to the ones when using a turbulence model.

Hello Martin, hello all,
I have a problem with the values of "eddy viscosity" and "laminar viscosity".
I run one wind turbine file in CFX and at the end of the output file i got two eddy viscosity values( max. and min.) for each domain. Since the model contains two domains, I have 4 totally different values for eddy viscosity ranging from 8.81E-21 to 1.79 e-3.
Would you please tell me about this problem?

Regards,

[cfd_newbie]

Hi,
I will like to take forum's attention to a very similar problem that I faced while trying to simulate wind turbine NREL phase VI simulations. It's a low speed flow problem where the Reynolds numbers are around 1e06 or below.
Experimental results are available for the base aerofoil S809 (See the attached images).

These experimental oil flow lines show that they have all the problems associated with low speed laminar flows (Laminar separation, bubble formation and turbulent reattachment).

But just today I found a paper by Dr Menter -
"Predicting 2D Airfoil and 3D Wind Turbine Rotor Performance using a Transition Model for General CFD Codes",
R. Langtry, J. Gola and F. Menter, ANSYS CFX, Otterfing, Germany, AIAA-2006-0395 44th AIAA Aerospace Sciences Meeting and Exhibit

It uses the SST -Transitional model and surprisingly these are the most consistent set of results that I have seen for this set of experiments. The results may not be very accurate but they manage to give consistency and are always around 10% of the experimental values.

Please let me know your thoughts on the same and are there any other methods which can give more accurate and consistent results ???????????

[Martin Hegedus]

Originally Posted by mohammad

Hello Martin, hello all,
I have a problem with the values of "eddy viscosity" and "laminar viscosity".
I run one wind turbine file in CFX and at the end of the output file i got two eddy viscosity values( max. and min.) for each domain. Since the model contains two domains, I have 4 totally different values for eddy viscosity ranging from 8.81E-21 to 1.79 e-3.
Would you please tell me about this problem?

Regards,

In general I like to plot contours of non-dimensionalized eddy viscosity. Since you may be close to sea level, you can non-dimensionalize your eddy viscosity by the sea level value of the dynamic viscosity (1.78938E-5 kg/(m*s)). I assume this matches your units of eddy viscosity.

The eddy viscosity at the surface will essentially be zero. A little off the surface the non-dimensional value can range from 10 to 100. The value increases as Reynolds number goes up and your inlet turbulence value is increased. The value also increases getting closer to trailing edge. In the wake of a blunt body the non dimensional eddy viscosity can get extremely large, such as 1e4 to 1e5.