k-omega SST simulation of turbulent flow around a circular cylinder
I have been analyzing the performance of the k-epsilon and k-omega SST turbulence models using a test case of a 2D circular cylinder. The numerical model was set up for Re = 3900 in order to compare the results with experimental data. As comparison parameter the drag coefficient Cd was calculated which according to experiments should be at around 0.99 for Re = 3900. The results significantly deviate from this value, especially for the k-omega SST model. With OpenFoam, an average value of about 1.6 was calculated using k-omega SST. The following boundary conditions were used for the model:
At the wall
k = 0 (and kqRWallFunction)
omega = 10*6*nu/(0.075*y^2) (and omegaWallFunction)
nut = 0 (and nutWallFunction)
At the inlet
k = 3/2*(U*I)^2
omega = Cmu^(-0.25)*k^(0.5)/L
nut = calculated uniform 0
internalField at timestep 0
k = 3/2*(U*I)^2
omega = Cmu^(-0.25)*k^(0.5)/L
nut = 0
The calculation resulted in an average yPlus value of around 2 with the maximum just over 4. Both mesh refinement and a test case without the use of wall functions did not help to significantly improve the results. Further, a second test case, which made use of the k-epsilon model, seemed to improve the results significantly using the exact same boundary conditions as before which leads to the following values for epsilon:
At the wall
epsilon = 0 (and epsilonWallFunction)
At the inlet and internalField at timestep 0
Here, Cd averaged about 0.9. I find this rather surprising, as the literature suggests that the k-omega SST model should perform better for this particular case (or at least just as good).
Has anyone experienced similar difficulties or can tell me if there is a mistake in the boundary conditions? I would like to use k-omega SST for future calculations and need to make sure it is set up correctly. Any suggestions for a possible source of error is much appreciated.
Thanks a lot,
I havenít received an answer to my post yet and am still facing the same problems with my model. I ran some further tests and by now am fairly certain that my solution is neither mesh dependent nor does the use of wall function significantly change the results. Maybe I should post my question a bit more general. I am interested what boundary conditions are typically used at the inlet and walls when making use of the k-omega SST model. Is there an alternative approach to the boundary conditions I have listed in my fist post? I would very much appreciate any input on this.
Thanks a lot, Dan
I had a similar problem but with a different geometry. For the yplus value you reported you should not use wall functions, if you want to use WFs you should have 30<yplus<300 (if i well recall). If you still want to use that mesh, you should use a near wall treatment (do not use wall functions in your BCs) and an appropriate low-re turbulence model.
In my personal experience, I found that is extremely tricky to get good results.
Hope this helps,
i have the same problem with the komegasst model. I have a Re-number of 5000 and komegast isnt working, with and without bcs. I tested the kepsilon model with the same case and it is working, but the problem is, that kepsilon can not compute seperation that good.
Perhaps there is a bug in the komegasst-model?
Thank you very much for the answers. I have spent some more time with this particular problem and suspect that one of the problems is that the Reynolds number is in the transitional regime between fully laminar and fully turbulent boundary flow. This means that while the flow is turbulent in the regions behind the cylinder, the boundary around the cylinder itself is still laminar (the wall has a damping effect on the development of turbulence). Only for high Reynolds flow the near wall regions start becoming turbulent as well. For k-omega SST calculations with Reynolds numbers in the transitional regime this means that a turbulence model is used near the wall to predict a behavior that in practice is actually laminar, which might be one source of error. I have started to use the k-omega SST model for high Reynolds flows, but have found that it is very difficult to get satisfactory results here as well.
There are some discussions about transitional turbulence models, but so far I think they are not implemented in openfoam. Let's see what the gurus have to say. In any case I think kwsst will give you way much better results than kepsilon (if you manage to get it working for your case), just pay attention to your y+. Also try to change to a low-re model (near wall treatment),
I like SpalartAllmaras, but is often used for high speed external aerodynamics. Another thing, I would rather prefer to use a small value for epsilon (1-08) instead of 0, there is a discussion of this somewhere in the forum.
Let us know if you get your simulations working. Have a nice day,
There are blended wall functions in OpenFOAM. omegaWallFunction (as recommended by Menter) and the spalding wall functions for nut. Both should give good results for any y+ value. However, I also believe that the k-w SST & the k-w can be run as low-re turbulence models without any additional damping functions for the near wall region (these are normally required for the k-e models). Wilcox discusses this in his book, Turbulence Modelling for CFD. However, the y+ isn't the only important element. You should make sure you have enough layers off the wall to properly resolve your boundary layer, otherwise you will be wasting your time. I wouldn't recommend anything less than 10 (for a cylinder, you could easily get away with 20-30).
I find interesting what was written about setting epsilon equal to 1-08. In my experience I have found that I seem to get better results when setting k equal to zeroGradient at the wall. Of course the turbulent kinetic energy should theoretically be equal to zero right at the wall (just like epsilon), but I suspect that the boundary conditions for k, epsilon and omega are in fact applied to the first cell center in OpenFOAM, rather than to the wall itself (unlike for the velocity for example). According to Pope, k is equal to zero right at the wall, but constant (and not equal to zero) in the log-law region adjacent to the wall. If in fact they are applied to the first cell center in OpenFOAM it would mean that the boundary condition k=0 for the walls, as I had previously suggested, would therefore not be correct. Does anybody know how the boundary conditions for k, omega and epsilon are treated in OpenFOAM? By the way: Mesh refinement (and therefore reduction of yPlus) did not significantly improve my results.
omegaWallFunction blended wall function
Regarding to the omega blended wall function (omegaWallFunction) for low-re, how should I setup my case?. I guess I have to impose the omegaWallFunction in the viscous walls. But what about k and nut?. Should I use kqrwallfuntion and nutwallfunction on the viscous walls as well? or should I assign to k and nut a fixedValue (1e-10) or a zeroGradient?.
Finally, I wonder if this model will suffer of some kind of stability problems when using simplefoam?. From my previous experience, I had terrible convergence problems using k-e with simplefoam, so I ran all my simulations using pisofoam.
You can find some info here about low Re wall function: http://www.cfd-online.com/Forums/ope...tml#post265758
My understanding is this: fluctuation reaches to their peak around y+~15~25, so once you put the first cell center in the viscous layer, the k value is small if its y+<5, so setting wall condition of k as fixedvalue to a very small value still make sense.
flow over a circular cylinder.. @ Re=1000
i m very new to in CFD area...
i have worked on flow over a single cylinder, two clinder in tandem and tow cylinder in side by side @ diff Re with diff ... i got good results....
but when i started working for Re=1000 .. for single cylinder...
i didnt get gud result.... :confused:
i have use used mesh wid y~min <1 to Y+max<5.. wid Kw-sst model...
Cd wich i m getting is 1.4 and as per journals and different thesis, i went through, Cd should be 1~ or < 1.
i hv tried wid 0.5% turbulence @ inlet and hydraulic dia equal to dia of cylinder.... and @ outlet 0, 0.5 and 0.7 back flow turbulence and same hyd dia...
but still... :confused:
y+ is not only the important factor. Placing first cell in viscous sub-layer will give you the Y+ around 1, but it does not mean you have properly resolved the boundary layer. You should ensure 15-40 layers in boundary layer with at-least 3-5 cells in viscous sub-layer.
Use second order scheme.
If flow is transitional then use the transition model and use the appropriate mesh resolution. In this case your stream wise meshing is also important. Resolving the normal and stream-wise in the immediate vicinity will give you the correct values of Cd.
Hope it help you.
fow past circular cylinder...
hello Far sir,
thnx 4 showing interest..
sir i m using 2nd order scheme..
and i hv also tried wid 45 layers of boundary... wid 1st row height 0.007D and 1.1 increment..
but still i dint get result.. :(
dis time y+min was <.4....
Can you show us your mesh and share info like the domain size, total no of nodes etc
flow past a circular cylinder.. @Re=1000
Hello.. Far sir..
Here is detail of d mesh which i m using... @Re1000
* No of nodal grid point on cylinder=100
* Domain size: 16DX35D, D=1cm
* No of nodes=12298
* No of cells=19800
* with boundary layer: * 1st row: .004D
* Growth factor: 1.05
* No of rows: 45
and while solving (wid 2nd order) BC which i m giving:
*velocity inlet: u=1m/sec with turbulent intensity (I)= 0.6% and turbulent length scale(l)= 0.07D
*pressure outlet: gauge pr=0 with back flow turbulent intensity = 0.7% and turbulent length scale(l)= 0.007
*upper and lower boundary as symmetry.
Hi Far and Others,
I am using kepsilon turbulence model, I ran the case many time with different mesh. unfortunately I dint touch system and solution folder, but non of my case shows good results.
Now I have changed the turbulence model in to kwsst,
Grad - fourth;
div - p - Gauss linear,
k - upwind
omega - upwind
and rest of them are Gauss linear,
I am using GAMG Solver and GaussSeidel - smoother for p, remaining all smoothSolver.
first layer is 3 mm
growth factor is 1.05 and 15 layers.
the total mesh size is 3.1 millions
I have noticed moment, there is no change in that.
actual torque should be 70 Nm but the simulation shows 57Nm.
as well the pressure raise is much less tan the experimental result.
my geometry is an axial flow fan passage
my questions are:
is there any way to check the origin of my geometry ( I am suspecting this),
the torque from simulation is it right?
the out show :
force ( x y z) viscous (x y z)
moment (x y z) viscous (x y z)
here is the moment is torque of the fan?
please help me to get clear
Thanks a lot,
|All times are GMT -4. The time now is 22:30.|