CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

General question: turbulence and laminar models

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 11, 2011, 12:23
Default General question: turbulence and laminar models
  #1
New Member
 
Join Date: Mar 2011
Posts: 1
Rep Power: 0
fluentmonkey is on a distinguished road
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!
fluentmonkey is offline   Reply With Quote

Old   March 11, 2011, 20:03
Default
  #2
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9
Martin Hegedus is on a distinguished road
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.
Martin Hegedus is offline   Reply With Quote

Old   March 11, 2011, 22:32
Default
  #3
Senior Member
 
Raashid Baig
Join Date: Mar 2010
Location: Bangalore, India
Posts: 136
Rep Power: 7
cfd_newbie is on a distinguished road
Quote:
Originally Posted by Martin Hegedus View Post
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
cfd_newbie is offline   Reply With Quote

Old   March 11, 2011, 23:02
Default
  #4
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9
Martin Hegedus is on a distinguished road
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.
Martin Hegedus is offline   Reply With Quote

Old   March 12, 2011, 07:10
Default
  #5
Senior Member
 
Raashid Baig
Join Date: Mar 2010
Location: Bangalore, India
Posts: 136
Rep Power: 7
cfd_newbie is on a distinguished road
Quote:
Originally Posted by Martin Hegedus View Post
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
cfd_newbie is offline   Reply With Quote

Old   March 14, 2011, 14:40
Default
  #6
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9
Martin Hegedus is on a distinguished road
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.
Martin Hegedus is offline   Reply With Quote

Old   March 15, 2011, 00:43
Default
  #7
Senior Member
 
Raashid Baig
Join Date: Mar 2010
Location: Bangalore, India
Posts: 136
Rep Power: 7
cfd_newbie is on a distinguished road
Quote:
Originally Posted by Martin Hegedus View Post
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.
cfd_newbie is offline   Reply With Quote

Old   March 15, 2011, 16:13
Default
  #8
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9
Martin Hegedus is on a distinguished road
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.
Martin Hegedus is offline   Reply With Quote

Old   March 15, 2011, 21:18
Default
  #9
Senior Member
 
Julien de Charentenay
Join Date: Jun 2009
Location: Australia
Posts: 229
Rep Power: 9
julien.decharentenay is on a distinguished road
Send a message via Skype™ to 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.
__________________
---
Julien de Charentenay
julien.decharentenay is offline   Reply With Quote

Old   March 16, 2011, 06:11
Default
  #10
New Member
 
Vic
Join Date: Feb 2011
Posts: 5
Rep Power: 6
solique is on a distinguished road
Quote:
Originally Posted by julien.decharentenay View Post
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
solique is offline   Reply With Quote

Old   March 17, 2011, 05:06
Smile
  #11
Senior Member
 
mohammad
Join Date: Dec 2010
Location: Seoul, South korea
Posts: 210
Rep Power: 7
mohammad is on a distinguished road
Quote:
Originally Posted by Martin Hegedus View Post
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,
mohammad is offline   Reply With Quote

Old   March 17, 2011, 14:49
Default
  #12
Senior Member
 
Raashid Baig
Join Date: Mar 2010
Location: Bangalore, India
Posts: 136
Rep Power: 7
cfd_newbie is on a distinguished road
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 ???????????
cfd_newbie is offline   Reply With Quote

Old   March 17, 2011, 15:47
Default
  #13
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9
Martin Hegedus is on a distinguished road
Quote:
Originally Posted by mohammad View Post
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.
Martin Hegedus is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Is this understanding of turbulence models correct? 3kha Main CFD Forum 3 January 31, 2011 22:31
How to determinate turbulence scale in LES (laminar simulation)? Franciswu21 ANSYS 0 October 22, 2009 12:48
turbulence model question Jason Wei Main CFD Forum 1 May 6, 2003 00:45
Turbulence models pop Main CFD Forum 3 May 31, 2001 00:16
turbulence modeling questions llowen Main CFD Forum 3 September 11, 1998 04:24


All times are GMT -4. The time now is 02:52.