Hi!
I try to calculate a f
Hi!
I try to calculate a flow around some Naca 4 digit airfoils. In my calculation the lift is nearly right, but the drag is much too high. I'm comparing the calculated values with the book "theory of wing sections". Can you give me a reason or advice? I use a wall as boundary condition for a profil and the calculations are done with the standard k-epsilon turbulence model. Thank you Andreas |
Whats your y+?
Whats your y+?
|
Hi!
The y+ is something aro
Hi!
The y+ is something around 40. This is to high, right? Is there a way to calculate the y+ with OpenFOAM or how do I by hand? I did it with CFX this time. What turbulence model should I use? Thanks for the responce. Andreas |
Hi andreas
the y+ can be ca
Hi andreas
the y+ can be calculated with the checkYPlus command ( this is in utilities .) you can also calculate the lift and drag with the liftDrag command . i am also working with foils and am very curious to know the y+ range best for OpenFoam regards kumar |
If you use a low-Re turbulence
If you use a low-Re turbulence model a y+ = 1 is best.
If you use a high-Re turbulence model a 30 < y+ < 100 is preferred. If you have high streamwise pressure gradients and or weak seperation, a low-Re model will do better than the high-Re model. For aerofoils you should be using a low-Re model. Search the forum for a post by Hrv about what kinds are available. |
Hi!
Right now I'm useing th
Hi!
Right now I'm useing the standart k-epsilon-tubulence model. I know that it is thought for near wall problems, but I unable to get another model calculating. Could someone give me some advice? - Which schemes should I use? - Which model? - Which relaxations factor in simpleFoam? I'm calculating a Re=6 Mio and an speed of Ma 0.25. Thanks Andreas Sorry for my Englisch! |
Hi
sorry, I found answers o
Hi
sorry, I found answers of my question in older posts. 1. start by running potentialFoam, this is a good way of checking the BCs as well as generating a sensible starting U field. 2. start the simpleFoam run with very low under-relaxation on these fields, 0.05 or even lower. 3. after a few iterations this can be raised to a normal level Sorry, Andreas |
Andreas, I have only just seen
Andreas, I have only just seen this post. Your drag is too high because you have turbulent flow everywhere. The boundary layer is more than likely transitioning from laminar to turbulent flow. Hence your drag value would be incorrect for a RANS simulation that assumes turb flow throughout the domain.
Use XFOIL or if you can get a copy try MSES. Both codes are from Marc Drela and take into account boundary layer transition. regards Shaun.D |
Andreas-
Would you be willi
Andreas-
Would you be willing to send me a zipped file of your input parameters for your potential foam case? I've been trying to get an airfoil case running in potential foam, but have an error in my boundary conditions. I haven't been able to locate the error. Would you mind sending me your files so I can compare my BCs to yours? Thanks. -Doug |
Hi all
I am trying to solve
Hi all
I am trying to solve a laminar flow over an airfoil in a 2-D case with icoFoam as it is an incompressible flow. I am facing a problem with the Cd and Cl values. they are vey low with a reference area of 1 to the order of 1e-07. can some one help me? regarding the potentialFoam, I want to try it but need help in setting up the case as I can't understand it in my tutorials (it does not have reynold's number definition, and even if i change my end time, my solution stops after one second in the example of pitzDaily) thanks a lot |
Hello Mayank,
Could you giv
Hello Mayank,
Could you give more details about the particular foil that you are using, and the angle of attack you are simulating? Perhaps the lift-curve slope will be the quantity that interests you most for validation. Also, without turbulence, your drag coefficient may be very low, especially if it is a thin foil at a small angle of attack. About potentialFoam, I understand that this can be used to generate more realistic initial conditions for the Navier-Stokes solver, but be careful about the velocity at the trailing edge. I don't see how you can impose the Kutta-condition when solving the full Navier-Stokes equations for a case that is not at the angle of zero lift, and therefore with non-zero angle of attack the continuous solution will have infinite velocity at the trailing edge. If it were me, I would just start from uniform i.c.'s for this problem. Kind regards, Kevin |
Hi Kevin,
I m simulating a
Hi Kevin,
I m simulating a NACA 63A41 air foil at dynamic pressure fo 120 km/m/s and Reynold's Number of 1.67 million. I have to solve at various angles of attack but I first tried 0 degree and it is giving me errors in Cd and Cl. The problem is not only the low value of CD but also the low value of Cl. I am attaching my boundary conditions file alongwith controlDict here. If you could take a look. http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif U |
http://www.cfd-online.com/Ope
|
Dear Mayank,
If you are usi
Dear Mayank,
If you are using icoFoam, and your body resides entirely inside the flow domain, then you do not need to specify pressure. I had a glance at the new forces postProcessing tool, and the c++ is a little too heavy for me to comment on your choice of rho, I would check this and the reference length. But, as I was trying to get at in my earlier reply, if you are simulating an angle near the angle of zero-lift, you should have very small forces, right? The lift should be close to zero and the drag will be small anyway, cd~10e-(3-4), but you have no turbulent viscosity, so it can even be much smaller than that! Have you tried an angle that is larger so that you can compute the lift-curve slope? Regards, Kevin |
hi Kevin,
I had already tri
hi Kevin,
I had already tried with 0 pressure also but without any success. My drag forces are of the order of 10e-04 and cd is of 10e-07 with reference area of 1 but if i reduce the reference area by the order I get the Cd of the correct order but Cl is a order less. yes my airfoil is inside the whole domain. My cells near the airfoil (in the boundary layer) are smaller than the boundary layer thickness (0.1/Re^0.5) The only option I think left to try is make the upstream and downstream region very high or use another solver. I have already tried simpleFoam with turbulence off but no success there too. I am making a better mesh today and running the solver. Shall let you know if there is any improvement. The important thing is I am comparing these results with the actual wind-tunnel results. So the problem is in my CFD. I know this message is long but it has everything I believe relevant to my problem. Thanx a lot |
Quote:
|
Reynold number
Hai Guys, i'm a new member...please help me,, i want to know Reynold number for standart air flow for air conditioning of building ??
thanks for help :confused: |
Quote:
|
Problem with Drag force!
Quote:
I've been doing simulation on NACA 4 digits in Star-CCM+. I still got the problem as yours before. The lift force is ok, but the drag is higher than experimental data, especially, when increase the attack angle. Have you fixed your problem yet? then could you show me in very detail how to correct the drag force? I still confuse how to determine "y+", "testing grid independence". It should better for me if you can send me an email: trieuckgt@gmail.com Thanks you so much! |
Hi.
Any progress here? /Mads |
cd twice the theoretical value
Hello everybody,
I have the same problem as above: for an airfoil at Re 1.5*10^6, cl matches well with theoretical value, while cd is two times the wanted cd. I am using kOmegaSST as implemented in OF (and not with the lowRe variation), y+ is between 30 and 110 everywhere, with an average value of 70. The fvSchemes is as follows:
Is there anyone that has some ideas on what can be the cause of the problem? Something else I can try or I can check? Suggestions are welcome. Cheers mad |
Hi Mad
In general you will have a hard time not overpredicting drag and even more so if you have such high y+ as you have. Correct drag prediction is highly dependent on resolving the viscous effects in the boundary layer. You normally need a low-Re turbulence model (i.e. no wall functions) and a y+ of no more than 2. Cl is normally not a problem to predict correctly as it is mainly pressure driven. Actually 100% overprediction of drag is not unheard of, but you should be able to get down to "only" 10-20% overprediction of drag. This all is quite dependent of type of airfoil, angle of attack (HIGHLY - in the linear, substall, region you should be able to do fine), CFD package, turbulence model, 2D/3D, transition modelling, etc. /Mads |
Quote:
|
Yes for a highRe model y+ should be in that order of magnitude but I am not too surprised that you can't predict drag better than you observe with a highRe model. I would suggest finer mesh with a y+ around or below 2 and a lowRe model. komega-SST in lowRe mode is a good choice (when we're talking RANS simulation). I am not sure if there is a lowRe implementation of komega-SST in OpenFOAM though, then Launder-Sharma would be my second choice.
/Mads |
Hi Mads,
I succeeded in running two different cases:
Have you some suggestions on how to reduce pressure residual? My fvSolution is: Code:
p Code:
gradSchemes: faceMDLimited Gauss linear 0.5; mad |
Mad,
I have most experience with the k-omega-SST model so I do not know why you see such bad drag prediction from the L-S model, I know it is widely used for aerodynamics and I have also used it a few times, so I do not know what's wrong here. Remember that y+ is not the whole story, you also need to have enough cells within the boundary layer, i.e. the stretching should be kept reasonable and definitely below a factor of 1.15-1.2. In any case 500% error on the drag signifies that something isn't right. Previously I have made some sensitivity analysis of max(y+)@airfoil, and I normalized those results and put them below. You can see that one must be careful with y+ as it really can change results a lot. What I did was to systematically vary the size of the first cells at the wall and monitor the influence on the drag. I used CFX with steady simulation with k-omega-SST without transition. CFX has automatic wall functions but at these low y+ it is always in lowRe mode (I hope :-)). http://hvirvel.dk/pics/maxyplus.jpg Your solution parameters seems correct. Are you doing steady simulations? If so you might not need to solve to such a tough relative tolerance. It might help your solution to develop faster into fully developed flow if you set it to, say, 0.01 or even higher. At least that is how I understood it. /Mads [IMG]file:///C:/Users/mreck/AppData/Local/Temp/moz-screenshot.png[/IMG] |
Quote:
The mesh I generated has an aspect ratio as high as 150 close to the wall :eek:, so that's probably why the lowRe case is not working properly. According to this: http://geolab.larc.nasa.gov/APPS/YPlus/, I should have a first cell layer of 0.0000322 meter, that implies a cell number that is not admissible for me. Thus I probably remain on the high-Re model, knowing that the drag is overestimated. As for the relTol of my fvSolution, yes, I am running a steady simulation, but I read somewhere to keep the relTol tight to obtain better convergence and a stable simulation... Indeed, I succeded to have 2% on cl and 75% on cd. These values are not very far from the point I enter in the discussion yesterday, but at least now I know why and where I should move to improve my results. :cool: Really enlighten your job on y+-cd relationship! It has already been saved on my favourite folder. Thankyou, cheers, mad |
Mad,
An aspect ratio of 150 close to the wall is nothing :-) I assume that you are using hex-meshes and most modern solvers can handle aspect ratios way into 10,000 or even 100,000 and these figures are definitely common in airfoil flows. I am not entirely sure how OpenFOAM copes with high aspect ratio cells though. Your 75% off on drag is, as you mention, not too bad - I can't remember your particular airfoil, but the thicker it is the more difficult it also is to model. /Mads |
Wait wait wait...
you wrote Quote:
Indeed, my airfoil is thick. Thus, things are not as bad as I think. :rolleyes: Uhmmm... In any case, from this discussion I really learned a lot! That's is never useless! |
Well, maybe I wasn't making myself really clear :-) by [cell-] aspect ratio you would normally mean the ratio between cell-sides and by stretching I was referring to the factor you normally apply when successively increasing the cell-side-height when moving away from the airfoil. You probably know this page where you can read more about this expansion factor. I am not sure about reasonable expansion factors with blockMesh, but try different factors and look at your cell-count and checkMesh output.
Note: You should be able to model a 2D airfoil with around 250k cells, at least my sensitivity investigations seem to point towards this cell-count being reasonable together with a max(y+) of around 2. Also you might check for influence of exterior boundaries, how far away are your outer bounds? /Mads |
Ah, ok! Your stretching is my cell grading! I am using 1.1, that is under the limit you pointed out.
My mesh quality is quite good, there is no error from checkMesh. I have only certain cells that are a little bit too distorted in my opinion, but checkMesh does not complain about them. With the actual set-up, I have around 50k cells for the lowRe mesh, and around 10k for the highRe mesh. The domain is 15 chords far away, and it is of a circular shape, since I need to invesigate a wide range of AoA. Should I further increase it? I think it is a matter of refinement of results, and it cannot lower cd of so much I need for the lowRe case! mad |
My investigations on cl/cd sensitivity from proximity of outer boundaries show that there can be a substantial influence on the cd (not so much on cl). I am not able to explain that yet, and I would actually expect the impact being on the cl instead.
Anyways, 15 chords is (to my knowledge) definitely not enough. Try to double it and see if your result change, and then try to double it once more if it does. On the cell count: with only 10k cells there is no chance (or maybe only by chance :-)) that you will predict cd properly. Even with 50k cells I would wonder. I have also done mesh dependency study following the lines of Richardson extrapolation and found that these 250k-300k cells are a good, generic, cell count for airfoils in the Re=5mio order of magnitude regime. I saw heavy impact on both cl and cd when going to, say, 80k cells. /Mads |
Indeed cd changes moving the outer boundaries. I was able to reduce cd difference of 60% in regards of theoretical value, with boundaries placed 120 chords away. 240 chords did not bring any improvement. The 120 chords case y+ changed accordingly, reducing to 25 average. The strange thing is that cl difference increase... from 2% with 15 chords to 4% with 120 chords in comparison of expected value. That is with the highRe case and a 20k mesh.
To increase further the cell number, I should increase the cell number on the airfoil surface. But then I need to change the first cell layer thickness to keep my mesh quality good, and this is not fine according to my y+. I have not try the lowRe approach. 250K cells are definitely too much for my objectives! So, I think I have a good setup now. Go back to python to write a polar plot script. Thanks again! mad |
Okay, sounds good. Thank you for an interesting discussion :-)
Happy foaming, Mads |
Hey All,
I am some hard time with Convergence I have a windtunnel set up with a Blade My pressure is not going below 0.001 and it is oscillating and so is my Cl and Cd they are oscillating between the same few values residual control 0.25 for p and 0.7 for U and the rest i initialised with potential FOAM with turbulence off then turbulence on, then first order schemes, then second order. still there is oscillation i dunno why, if some one has an explanation please give when i use Code:
p but when i use Code:
p I need them to converge as i will be the mapping the data around the blade to a C-Grid for a transient simulation. - So any tips or ideas in getting the residual of P below 0.001 and make it stop oscillating my schemes are Code:
gradSchemes Hasan K.J |
Greetings to all!
@Hasan: Quote:
Code:
checkMesh -allTopology -allGeometry Bruno |
Hey Bruno,
Here is the Mesh check stats Code:
Mesh stats Hasan K.J |
Quote:
The simplified way to look at this is to imagine that the cell in question is as if it were extremely small (near zero) or that it is very contorted. What this equates to is a distortion in the mesh, that leads to non-physical values, because the numbers are stretched more than they should... Have a look into this blog post of mine, to see the effects bad meshes can have on results: OpenFOAM: Interesting cases of bad meshes and bad initial conditions |
But, I made the mesh in salome
and the distance of the first cell was what it had to be even though it was that small, to have a Y+ of 0.5-1, so is there any way to maintain the Y+ and the results Thanks, Hasan K.J |
After the checkMesh command, run this command:
Code:
foamToVTK -cellSet underdeterminedCells
|
All times are GMT -4. The time now is 00:23. |