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

Two-equation turbulent models: low re airfoils

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 14, 2011, 17:46
Default
  #41
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 10
Josh is on a distinguished road
Quote:
Originally Posted by truffaldino View Post
I am still confused: At figure 4 of that reference they list k-w sst, k-w sst trans., gamma-re-theta. So it sems that they distinguish between k-w sst trans and gamma-re-theta. At that figure k-w SST is close to k-w SST trans, which is drastically different from gamma-re-theta. It seems what they call k-w sst trans. is not SST transitional, but SST with k-omega options "Transitional Flows" from Fluent 6.3.
I believe this is a typo or Fluent-based nomenclature. The k-w SST transitional must mean the low-Reynolds-number SST model (i.e., without a wall function - the grid resolves the viscous sublayer, y+ < 1), the k-w SST is the classic SST with a wall function, and the gamma-theta is the SST gamma-Re_theta model.

Observing the graph, the k-w SST model provides the worst result, with the k-w SST-trans providing slightly better, though still poor, results. The gamma-theta provides much better results, so my above assumption makes sense.
Josh is offline   Reply With Quote

Old   March 15, 2011, 17:00
Default
  #42
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 469
Rep Power: 11
Martin Hegedus is on a distinguished road
Quote:
Originally Posted by truffaldino View Post
Martin,

Have you tried to run laminar? Is it really turbulent at RE=5000 and alpha=7? At such a low speed the transition can be delayed up to the trailing edge.
No, I did not run laminar. The flow is sub critical and, as can be seen from the Re 5000, a big bubble exists. If I run laminar the bubble will pop, resulting in unsteady flow.

In my opinion, at these Reynolds number the concept of turbulence takes on a different meaning than at higher Reynolds numbers. At these Re numbers the turbulent eddies are largish in scale. They are more macro than micro. The SA turbulence model is just picking up on the vorticity in the problem and creating eddy viscosity. The eddy viscosity then dampens out the problem and provides steadiness.

As the Re number increases, micro unsteadiness builds up on the bubble facilitating the bubble's reattachment and the macro unsteadiness goes away, leaving only micro turbulence. At this point I guess turbulence models become more relevant.

Or, another way of viewing reattachment is that by going from Re 5,0000 to 50,000 one has given more surface length (10 times) for the bubble to reattach itself. Thus, macro and micro are relative. Maybe the eddies actually remain sort of on the same real scale as the airfoil is stretched to 10 X, but relative to the airfoil length they are 10 times smaller?
adilio likes this.
Martin Hegedus is offline   Reply With Quote

Old   March 15, 2011, 17:52
Default
  #43
Senior Member
 
truffaldino's Avatar
 
Join Date: Jan 2011
Posts: 246
Blog Entries: 5
Rep Power: 9
truffaldino is on a distinguished road
Quote:
Originally Posted by Martin Hegedus View Post
No, I did not run laminar. The flow is sub critical and, as can be seen from the Re 5000, a big bubble exists. If I run laminar the bubble will pop, resulting in unsteady flow.
But flow might be really unsteady and laminar at this reynolds number with foil shedding vortices and without steady bubble?

It is interesteresting at this reynolds numbers the turbulence is indeed "macroscopic" in a sence that Kolmogorov lenght Re^-3/4 is of orer of 10^-3 which is .1% of the wing chord.
truffaldino is offline   Reply With Quote

Old   March 15, 2011, 18:09
Default
  #44
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 469
Rep Power: 11
Martin Hegedus is on a distinguished road
Quote:
Originally Posted by truffaldino View Post
But flow might be really unsteady and laminar at this reynolds number with foil shedding vortices and without steady bubble?
I do agree that the flow is unsteady. Unfortunately I'm running these on my laptop which doesn't have the horse power to adequately model the unsteady flow.
Martin Hegedus is offline   Reply With Quote

Old   March 15, 2011, 18:23
Default
  #45
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 10
Josh is on a distinguished road
Chances are the flow is laminar and unsteady and that while laminar separation occurs, neither transition nor reattachment do. Like you said, the eddy viscosity dampens the effect.
Josh is offline   Reply With Quote

Old   March 17, 2011, 14:36
Default
  #46
Senior Member
 
Raashid Baig
Join Date: Mar 2010
Location: Bangalore, India
Posts: 136
Rep Power: 8
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, 16:28
Default
  #47
Senior Member
 
truffaldino's Avatar
 
Join Date: Jan 2011
Posts: 246
Blog Entries: 5
Rep Power: 9
truffaldino is on a distinguished road
Quote:
Originally Posted by cfd_newbie View Post
Hi,
Please let me know your thoughts on the same and are there any other methods which can give more accurate and consistent results ???????????
At these reynolds numbers ( RE around 10^6 and lower) I would try x-foil, it is much simpler and highly validated.
truffaldino is offline   Reply With Quote

Old   March 16, 2012, 01:10
Default Flow over stepped airfoil
  #48
New Member
 
Join Date: Feb 2012
Posts: 1
Rep Power: 0
lazer is on a distinguished road
Quote:
Originally Posted by truffaldino View Post
The problem here that there is no experimental results for stepped vortex-trapping airfoils, analysys of which is a final goal of thisn work. I wanted to compare performance of this type of airfoils with best conventional ones (and now trying to analyse only conventional ones using CFD code). For conventional airfoils one can establish correlations etc, but these data are of no use in different geometry of vortex-trapping airfoils.

As for x-foil: it uses viscous-nviscid interaction for boundary layer through integral BL methods, transition is predicted by e^n method. Program seems to use some othrer correlations (I am not copletely sure).
Hey there Pal..
I've been reading some of your post and found out that you've worked on flow over stepped airfoils. I've also been working on stepped model airfoils for the past 3 weeks but with no luck.
Now the problem is I'm stuck up in selecting a viscous model in Fluent.

The problem description is as follows:
airfoil chord: 0.25 m
Reynolds number: 67000
domain: c-grid; 10c semicircle, 20c chordwise, 10c total height.


I'm using Low Re airfoils namely Eppler 61 and NACA 4415. I've tried SA, K-E and all but the results are not matching with WT results.
I doubt that the flow over the airfoil would be either laminar or fully turbulent. it sure must be in the transition region. Although I've not used any transition model and I dont know what parameters for the transition model to set.

The problem is, the solution converges but doesn't give the correct values (doesn't match with published results). This is only about normal airfoils. Second step would to be make a step and run the simulation again.
I hope you will share some of your experiences in solving this problem.

TIA
Hemant
lazer is offline   Reply With Quote

Old   March 16, 2012, 03:56
Default
  #49
Senior Member
 
truffaldino's Avatar
 
Join Date: Jan 2011
Posts: 246
Blog Entries: 5
Rep Power: 9
truffaldino is on a distinguished road
Hi Hemant,

I have tried different turbulence models without much success: It sems that only LES should give something more or less close to reality.

I have also tried the following thing with stepped airfoils: At low angles of attack and in the case when the step is close enough to the leading edge, transition will happen at the step. So, I have written a user defined function which switches the turbulence model on over top surface of the foil at the step location. At the bottom surface the model is switched on at the trailing edge (see image attached).

Truffaldino
Attached Images
File Type: jpg v_trapping.jpg (91.2 KB, 68 views)
truffaldino is offline   Reply With Quote

Old   March 19, 2012, 18:09
Default
  #50
New Member
 
Abdelkader
Join Date: Jan 2012
Location: Algeria
Posts: 9
Rep Power: 6
Abdelkader_Aero is on a distinguished road
Send a message via Skype™ to Abdelkader_Aero
hello for everybody
i'm just biginner in cfd and i want specially to ask Martin Hegedus , why u used turbulence model and u r sur that the flux around airfoil is still laminar [Re=70000<5e5] , it's not clear for me , can you explan me please
thank you
Abdelkader_Aero is offline   Reply With Quote

Old   March 19, 2012, 18:11
Default
  #51
New Member
 
Abdelkader
Join Date: Jan 2012
Location: Algeria
Posts: 9
Rep Power: 6
Abdelkader_Aero is on a distinguished road
Send a message via Skype™ to Abdelkader_Aero
hello for everybody
i'm just biginner in cfd and i want specially to ask Martin Hegedus , why u used turbulence model and u r sur that the flux around airfoil is still laminar [Re=70000<5e5] , it's not clear for me , can you explan me please
thank you
Abdelkader_Aero is offline   Reply With Quote

Old   March 19, 2012, 19:57
Default
  #52
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 469
Rep Power: 11
Martin Hegedus is on a distinguished road
Yikes, this thread is almost a year old. I did quickly scan it, but can't say I remember all the details.

At 70,000 I don't think a RANS model is appropriate, but it goes give you insights into what the flow is doing. Also, since SA tends to be on the stable side, it gets you steady state solutions. Less expensive than time accurate. As the Re for a RANS model decreases, so does the eddy viscosity. As the eddy viscosity decreases the RANS solution becomes more like a laminar one. The RANS solution is only "turbulent" once the eddy viscosity has had a chance to build up. As the Re drops, I believe, the skin friction drag for RANS approaches laminar. This is true only if there isn't separation of one sort or another (flat plate is an example). However, separation is a different issue. Even for low Res, a RANS model has enough eddy viscosity to dampen out or greatly affect the unsteadiness so it will not behave like a laminar result. One thing that can be done with a RANS model is to limit the amount of eddy viscosity to see what it takes to make the solution go unsteady. This can give you an idea of how appropriate the RANS model is.
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
Use of k-epsilon and k-omega Models Jade M Main CFD Forum 13 June 24, 2016 11:57
low reynolds number models in Fluent doug Main CFD Forum 6 August 4, 2012 14:39
Adding source terms to turbulent models makaveli_lcf OpenFOAM Running, Solving & CFD 0 June 8, 2009 09:34
Turbulent Heat Transfer Transport Equation Flo.duck Main CFD Forum 0 May 6, 2009 03:37
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12


All times are GMT -4. The time now is 08:51.