
[Sponsors] 
July 17, 2005, 13:44 
Dear OpenFoam friends,
i am

#1 
New Member
Klaus Wittig
Join Date: Mar 2009
Posts: 20
Rep Power: 10 
Dear OpenFoam friends,
i am just beginning to use foam for certain cases were i already know the answer. First i had a try with the NACA profil 23012 at an angle of attack of 0 and 12 degree at 90 m/s. Chord length is 0.24 m. I did run this before with duns. I used sonicTurbFoam first but in both cases (0 and 12 deg) the initial boundary layer is extremly thick even in the regions where the flow accelerates. And the flow separates immediatelly. After a while the calculation gets instable and produces "NAN"s. Why is the boundary layer unusual thick? I checked the materialdata and could not find an error. Then i used icoFoam with better results. The boundary layer is about as thick as i guess is right. But also after a while the calculation crashes. Is there anybody who could look at my example? Or can anybody assist me? Some more questions comming into my mind:  is there a way that foam calculates the appropriate timestep instead of defining it? Based on the Max Courant Number it seems likely.  Is there an easy way to watch the convergence (of U or p etc.)? For example a file which can be used by gnuplot etc? The format of the default output is not well suited for gnuplot. Best regards, Klaus P.S. i try to attach scetches and the input. Please untar it in the "sonicTurbFoam" folder. It should run out of the box. 

July 18, 2005, 05:32 
 automatic time stepping: hav

#2 
Super Moderator
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 18 
 automatic time stepping: have a look at
setInitialDeltaT.H and setDeltaT.H which adjust the timestep based on max Co number (see e.g. the interFoam solver)  convergence: the foamLog utility will extract all the nessecary information out of the log file. Is in simple column format which gnuplot or xmgrace can use. 

July 24, 2005, 15:44 
Hi Mattijs,
thanks for the

#3 
New Member
Klaus Wittig
Join Date: Mar 2009
Posts: 20
Rep Power: 10 
Hi Mattijs,
thanks for the hints. In the meantime i finished my pre/post processor and i discovered the reason of the big boundary layer (LaunderSharmaKE instead kEpsilon model). But there is now a bigger problem which i could not solve so far. See the attached picture (bunzip2 result.jpg.bz2). There you see the totaltemperature calculated (tt=u*u*/2. /cpg + t) with cpg=1000. as in the thermophysicalProperties file defined. The total temperature should not change, at least not so much in such big areas (up to 3 K). First i defined a uniform temperature (i guess U ist the static temperature) even at the profil faces. But then i assigned the value of the total temperature at the profilfaces, because there the static temperature should be equal to the totaltemperature (U==0). But that did not change the results anyway.  What on earth is going wrong? See the listings below. Made i any bad assumptions? I checked the results with buoyantFoam, rhoTurbFoam and sonicTurbFoam. They are all the same. I would have expected a slightly different result with buoyantFoam because of the heat transfer.  is element to element heattransfer regarded by all this solvers? Best regards, Klaus P.S. the boundary listing: 6 ( in { type patch; nFaces 56; startFace 7214; } out { type patch; nFaces 60; startFace 7270; } /* s1 s2 are the 2D meridiancuts */ s1 { type empty; nFaces 3676; startFace 7330; } s2 { type empty; nFaces 3676; startFace 11006; } profil { type wall; nFaces 78; startFace 14682; } /* wall connects inlet (in) and outlet (out) */ wall { type patch; nFaces 82; startFace 14760; } ) U: dimensions [0 1 1 0 0 0 0]; internalField uniform (90 0 0); boundaryField { in { type fixedValue; value uniform (90 0 0); } out { type zeroGradient; } s1 { type empty; } s2 { type empty; } profil { type fixedValue; value uniform (0 0 0); } wall { type fixedValue; value uniform (90 0 0); } } T: dimensions [0 0 0 1 0 0 0]; internalField uniform 288; boundaryField { in { type fixedValue; value uniform 288; } out { type zeroGradient; } s1 { type empty; } s2 { type empty; } profil { type fixedValue; value uniform 292.3759; } wall { type zeroGradient; } } p: dimensions [1 1 2 0 0 0 0]; internalField uniform 100000; boundaryField { in { type fixedValue; value uniform 100000; } out { type fixedValue; value uniform 100000; } s1 { type empty; } s2 { type empty; } profil { type zeroGradient; } wall { type zeroGradient; } } 

July 25, 2005, 05:56 
This is a subsonic case but yo

#4 
Super Moderator
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 18 
This is a subsonic case but you seem to specify all boundary values (U,p,T) at the inlet. Isn't this overspecified?


July 25, 2005, 14:51 
Hi Mattijs,
actually i defi

#5 
New Member
Klaus Wittig
Join Date: Mar 2009
Posts: 20
Rep Power: 10 
Hi Mattijs,
actually i defined p at inlet and outlet with 100000 Pa. But even without the definition of p in the inlet there is no other result. So in the inlet there is specified U,T and in the outlet p. But the result is practically the same. Also total pressure is not uniqe in the flow field. I would understand if a drop would occur in the boundary layer but i see an increase for example in the stagnation area (pic). Any ideas? Best, Klaus 

July 25, 2005, 15:06 
Not immediately. Looks like a

#6 
Super Moderator
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 18 
Not immediately. Looks like a boundary condition problem.


August 1, 2005, 16:54 
Meanwhile i spent another coup

#7 
New Member
Klaus Wittig
Join Date: Mar 2009
Posts: 20
Rep Power: 10 
Meanwhile i spent another couple of hours this weekend and found the parameter
which caused the trouble. Its the kEpsilon turbulence model. After i changed to LRR the results developed in the right direction. To finish this topic i summarize what i found. In the pictures you see the cp distribution and the y+ values along the airfoil for a coarse mesh and a fine mesh, compared to measurements and the results calculated with duns. Below the lift and drag coefficients of this calcs are listed: ca: lift coefficient cw: drag coefficient cp: pressure coefficient (pp_inlet)/q_inlet ca cw naca23012_12deg_coarse_kEpsilon 1.117340 0.277036 naca23012_12deg_fine_kEpsilon 1.083124 0.293196 naca23012_12deg_coarse_LRR 1.181551 0.071775 flow starts to separate naca23012_12deg_fine_LRR 1.358733 0.061862 flow starts to separate duns.cfd (QOmega turbulence mod.) 1.439210 0.030384 measured rough surface 1.23 0.0315 flow starts to separate measured smooth surface 1.41 0.0128 

August 1, 2005, 17:07 
Try the LaunderGibson model ra

#8 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
Try the LaunderGibson model rather than LRR, it has much better nearwall treatment. Also you might find it useful to try alternatives to the standard kepsilon, e.g. the RNG or even better the realisable form.


August 21, 2005, 08:01 
Meanwhile i used the LaunderGi

#9 
New Member
Klaus Wittig
Join Date: Mar 2009
Posts: 20
Rep Power: 10 
Meanwhile i used the LaunderGibson model and others. I used this case
and a case with less angle of attac (8.8 deg). But the results are not any better. Also i calculated results for the profil RAE 2822 at M 0.73 which is well documented in the ISAAC users guide. The problem with the Reynolds Stress model is always a very instable boundary layer with a fluctuating pressure distribution in the rear part of the profil. And with the kepsilon model(s) even the pressure distribution is far from matching the measurements. Also total temperature and pressure are not reasonable as shown in the previous mails. I am not a cfd guy and i wonder how big the influence of the turbulece model can be. So far i used only duns with the qomega model. And it was quite easy to reproduce the measurements for the models in question. Is it possible that the problems are only linked to the turbulence models? Have you seen a comparable situation before? regards, Klaus Wittig 

August 21, 2005, 09:55 
There may still be issues with

#10 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
There may still be issues with your farfield BCs and yes the choice of turbulence model will have a large influence on the results particularly in the boundary layer. The models included with OpenFOAM are not particularly suitable to this kind of flow, although they should produce reasonable results, and if you already know that the qomega model works well for your cases perhaps you should implement that model in OpenFOAM.


December 14, 2005, 11:10 
Just a question for Klaus; Wha

#11 
New Member
Lars Edvardsen
Join Date: Mar 2009
Posts: 3
Rep Power: 10 
Just a question for Klaus; What program did you use for making your 2D model / mesh?
Best Regards Lars Edvardsen 

December 15, 2005, 18:04 
You can use Gambit that is a u

#12 
Member
Muzio Grilli
Join Date: Mar 2009
Posts: 36
Rep Power: 10 
You can use Gambit that is a utility that goes with Fluent or Ansa that is much better than Gambit but it is less easy to learn


January 14, 2006, 10:13 
Lars,
by chance i had seen yo

#13 
New Member
Klaus Wittig
Join Date: Mar 2009
Posts: 20
Rep Power: 10 

January 17, 2006, 05:14 
I am new to this list, so plea

#14 
New Member
Holger Bauer
Join Date: Mar 2009
Posts: 1
Rep Power: 0 
I am new to this list, so please forgive me if this was already answered.
From looking at the results of your pictures above that you obtained with the kepsilon TM it looks to me that the implementation of the kepsilon model does not have the corrections for the socalled stagnation point anomaly. This is an overprediction of turbulent kinetic energy around stagnation points. There are papers of Durbin and others who suggest fixes for this. 

May 15, 2006, 23:36 
How are you getting the data i

#15 
New Member
Jonathan Gerald Pelham
Join Date: Mar 2009
Posts: 9
Rep Power: 10 
How are you getting the data into grace?
when i've tried it to just didn't accept it 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Mach number  Singh  Main CFD Forum  0  July 2, 2008 09:51 
urgent "inlet vilocity profil"  machrouki  FLUENT  0  April 6, 2007 18:24 
error reading profil  Ralf Schmidt  FLUENT  0  November 9, 2006 08:42 
save transient temperature profil  isaac  FLUENT  1  May 26, 2004 04:06 
MACH=25 HAVE YOU TRIED ?  Tomawak  FLUENT  1  December 19, 2000 15:53 