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

Drag over-prediction

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 22, 2010, 06:00
Default Drag over-prediction
  #1
Senior Member
 
MadsR's Avatar
 
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 8
MadsR is on a distinguished road
Hi.

I get drag overprediction from CFX simulations of an 2D airfoil

Setup info:
1. I have an 2D airfoil setup in CFX
2. Mesh is created in ICEM Hexa. 200k->900k mesh dependent tests done
3. max(y+)<1
4. turbulence model is k-omega-SST
5. fully turbulent, no transition
6. angle of attacks investigated 0-15deg
7. Re is 3e6
8. domain extents sensitivity is investigated, 60chords of domain extent is found sufficient
9. butterfly/O-mesh, inlet (bottom/left)-outlet(top/right) BC's
10. high-resolution and specified blend factor of 1.0 is investigated
11. convergence to 1e-6 (max residuals) and lift/drag convergence monitored

I compare these CFX results with an academic code which has a good track record. I get less than 1% discrepancy on the lift coefficient, which is quite good. But drag (which I know is harder to resolve) is off by up to 20% (more than the academic code).

Any suggestions on what to check? Help would be greatly appreciated.

/Mads
__________________
Online free airfoil-mesher for OpenFOAM here
MadsR is offline   Reply With Quote

Old   February 22, 2010, 20:37
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,651
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
What accuracy did your mesh and boundary proximity tests show?

What turbulence model does the academic code have? What about turbulence inlet conditions? Is a turbulence transition model needed?
ghorrocks is offline   Reply With Quote

Old   February 23, 2010, 03:34
Default
  #3
Senior Member
 
MadsR's Avatar
 
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 8
MadsR is on a distinguished road
Hi Glenn. Thanks for your feedback. I am in the process of doing formal grid dependence tests but proximity-tests showed that I needed around 60-chord-lengths of extent to get best results. Drag was 40-50% off when using a 40-chord-extent mesh and now down to 20% when using 60-chord-extent. 80-chord-extent doesn't improve anything.

The turbulence model used by the academic code is the same as mine, mentioned above (k-omega-SST). Transition model is needed but this case is run with and without and I am currently testing without and comparing to academic results without transition.

It is my experience that setting a turbulence level does not change solution as it is so far away from the airfoil that it will dissipate way before reaching the airfoil. Do you experience otherwise? Turbulence inlet level is zero in the academic simulations and set to "low" in mine.

Thanks, and please continue to ask such questions, there might be something else I have missed :-)

/Mads
__________________
Online free airfoil-mesher for OpenFOAM here
MadsR is offline   Reply With Quote

Old   February 25, 2010, 20:33
Default
  #4
New Member
 
Join Date: Jun 2009
Posts: 8
Rep Power: 8
Bak_Flow is on a distinguished road
Hi MadsR,

This is interesting. I did a bunch of cases back about 5 years ago with CFX and found about the same over-prediction. I was doing simple NACA uncambered airfoils ie 0012, 0009, 0012, etc.

At the time the transition models had not been full implimented and the story was that the difference between experiments and predictions were due to the lower skin friction from leading edge to tranition point in the experiments. The other major issue was that stall was predicted late and under-predicted.

I actually found that smaller domains upstream could be used reliably if you are careful about setting k and epsilon at the inlet. As you point out k dies away if you have a finite epsilon at the inlet. What you have to do is ensure that you have turbulent viscosity = 0 or some constant by the time the flow gets to the leading edge. AND be consistient between different domains!

Another thing you have to be careful with for turbulence quantities is that most codes never let k=0 because of divide by zero for terms like (eps/k) which is used in all the linearizations, etc. So each code will have some different arbitrary number. You just have to make sure that you are consistient.

Yet another thing in CFX is that k and epsilon are solved first order by default (since wiggles can produce negative numbers and stability problems....divergence). So you can get some unexpected things happening near the leading edge where k~0 upstream.

I have not revisited these cases which were pretty disappointing for such simple cases ~ 5 years ago! There probably are some new settings, etc to fix things up by now. The interesting lesson from these cases is that you really learn what is important when you apply a code to such a simple geometry. The drag on the airfol(unstalled) is all skin friction....and if you don't get the models set-up right.....look out! A 3-D case with flaps, separation, etc. "hides" some of these details.

What academic code are you using?

Let us know how you make out!

Regards,

Bak_Flow
Bak_Flow is offline   Reply With Quote

Old   February 26, 2010, 03:36
Default
  #5
Senior Member
 
MadsR's Avatar
 
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 8
MadsR is on a distinguished road
Hi Bak_flow and thanks a lot for your valuable input. I can't comment much on the academic code since I am not using it and are referring to to results which have been kindly handed to me by the academic institution. I am sure they don't mind, but you never know.

Nice points about the inlet turbulence and turbulence is still solved by first order numerics in CFX by default. Also zero values causes issues.

At the moment I am following two paths: 1) mesh dependency study with different meshes to observe truncation error and 2) two mesh-domains in ICEM, i.e. one for the near-profile-domain and one for the outer part. They end up being one domain, but in this way I can ensure that the boundary-layer cells do not move when I expand my domain.

I will get back with more results and/or indications later.
/Mads
__________________
Online free airfoil-mesher for OpenFOAM here
MadsR is offline   Reply With Quote

Old   February 26, 2010, 05:46
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,651
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
CFX V12 has high order numerics for the turbulence model as an option. You might need this for your application.

Does the academic code have the SST model? While the basic idea of the SST model is published in the open literature there are lots of under-the-hood bits of it which are proprietary. I don't think the turbulence models will be the same unless you choose something like k-e, and even then you have to be careful about the issues Bak-flow mentions and the order of the turbulence numerics.
ghorrocks is offline   Reply With Quote

Old   February 26, 2010, 07:36
Default
  #7
Senior Member
 
MadsR's Avatar
 
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 8
MadsR is on a distinguished road
Thanks for your feedback, Glenn :-)

I will look into the second order numerics for turbulence.

SST: Yes, and both results are with SST model. I am also thinking that the academic code might feature some "tuning" of parameters and I have to investigate this further.

Keep posting such valuable info.

/Mads
__________________
Online free airfoil-mesher for OpenFOAM here
MadsR is offline   Reply With Quote

Old   February 26, 2010, 09:40
Default
  #8
Senior Member
 
MadsR's Avatar
 
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 8
MadsR is on a distinguished road
Initial experience with high resolution numerics on turbulence is that it won't converge...In my grid dependence study I have three meshes and with highres turbulence numerics I can't get convergence on the coarsest mesh. Actually normally you would convergen more easily on coarse meshes due to the high numerical diffusion, but I guess not when it comes to this case.

/Mads
__________________
Online free airfoil-mesher for OpenFOAM here
MadsR is offline   Reply With Quote

Old   February 28, 2010, 18:41
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,651
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Of course the high resolution numerics will be harder to converge. Use the results you already have as an initial condition, that should help a lot.
ghorrocks is offline   Reply With Quote

Old   March 1, 2010, 04:25
Default
  #10
Senior Member
 
MadsR's Avatar
 
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 8
MadsR is on a distinguished road
@Glenn: Well I guess not necessarily so. The "high resolution" in CFX is just a automatic blending function so in theory it should give good convergence. At least that's how it works for the advection numerics. In case of "trouble" it switches to first order, else it is second order central differencing.

Naturally, I started out from a previous simulation with pure upwind on the turbulence terms, and it just doesn't converge. Well, it does converge to in-between 1e-3 - 1-e4 but not in a smooth way as the turbulence-upwind which converges to machine precision in one smooth swoop. Neither does it converge from a complete restart, which makes sense.

/Mads
__________________
Online free airfoil-mesher for OpenFOAM here
MadsR is offline   Reply With Quote

Old   March 1, 2010, 17:29
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,651
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Have you run through the suggestions here:

http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Now you are resolving the turbulence more accurately you are probably picking up smaller and possibly transient features and these are causing convergence difficulties.
ghorrocks is offline   Reply With Quote

Old   March 2, 2010, 03:49
Default
  #12
Senior Member
 
MadsR's Avatar
 
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 8
MadsR is on a distinguished road
Hi Glenn. Thanks a lot for that pointer - I will look through it.

I found that changing between zero pressure at the outlet or averaged zero pressure at the outlet changed roboustness (the averaged being the most robust, which seems reasonable).
__________________
Online free airfoil-mesher for OpenFOAM here
MadsR is offline   Reply With Quote

Old   March 8, 2010, 20:48
Default
  #13
New Member
 
Join Date: Jun 2009
Posts: 8
Rep Power: 8
Bak_Flow is on a distinguished road
Hi Mads,

another option you might look at is setting the blend factor for the turbulence equation discretization yourself.

I am a bit of a doubter and don't always like the code making decisions for me....and in some cases have seen some wierd things going on to back it up....with hi-res!!

You have to play a few tricks since the gui does not have the blend factor option. You can either edit the .ccl yourself and inject it into the def file or you can use the def file editor starting with a .def for hi-res. for turbulence and then adding the appropriate parameters ie switch the parameter for turbulence to specified blend factor and then adding the blend factor you want.

Usually something like 0.9 or 0.95 will give you near second order for convergence of turbulence quantities and should be as robust as hi-res...and you know what you have got!

Let us know how the results look and if you need any more pointers.

Regards,

Bak_Flow
Bak_Flow is offline   Reply With Quote

Old   March 9, 2010, 03:39
Default
  #14
Senior Member
 
MadsR's Avatar
 
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 8
MadsR is on a distinguished road
Hi Bak. I totally agree with you, I also prefer to explicitly specify such figures. Thanks for the info.

/Mads
__________________
Online free airfoil-mesher for OpenFOAM here
MadsR is offline   Reply With Quote

Old   March 24, 2010, 01:05
Default
  #15
New Member
 
Dr. Flow Squad
Join Date: Mar 2009
Posts: 14
Rep Power: 8
Dr. Flow Squad is on a distinguished road
Hi Mads.
What was the outcome of this? Still difficult drag predictions?
Dr. Flow Squad is offline   Reply With Quote

Old   March 24, 2010, 04:29
Default
  #16
Senior Member
 
MadsR's Avatar
 
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 8
MadsR is on a distinguished road
Hello Dr Flow Squad :-)

Well, I am still trying and now I tested for sensitivity of y+. I have varied max(y+) from 0.23 to 4.2. Quite expected as long as max(y+)<2, Cl does not vary much (about 0.5%) but when max(y+) get above 2 I get a difference of 5-10%. Also as expected.
For Cd, the value changes around 2-3% when max(y+) varies below 2 and by 20% when max(y+) goes up to 4.

It seems that max(y+)<2 is okay. Nothing new here, I know, but I just did the check with CFX and the SST model.

/Mads
__________________
Online free airfoil-mesher for OpenFOAM here
MadsR is offline   Reply With Quote

Reply

Tags
2-d, airfoil, cfx, drag, validation

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
Drag prediction martingariepy FLUENT 2 March 25, 2009 20:02
where to find AIAA CFD Drag Prediction Workshop? zaidun Main CFD Forum 4 April 11, 2006 23:35
S-A Turbulence Model and drag prediction Alan FLUENT 0 November 15, 2005 18:48
drag prediction in FLUENT Hua FLUENT 0 November 4, 2002 00:16
Drag prediction benchmarks Althea Main CFD Forum 12 October 18, 1999 12:57


All times are GMT -4. The time now is 20:16.