[LordKelvin]

Hello Foamers,

I've been struggling with the classic turbulent flow past a cylinder over the last weeks.
Case is solved with pisoFoam and k-omega SST model.
The case is taken from a master's thesis for which results are totally fine : at Re=10k vortex shedding shows St=0.205. Such a Reynolds is reached with a very low inlet velocity (V_\infty=0.02[m/s]) and a quite large cylinder (D=0.5[m]).
However, my geometry being different, i simply used the transformPoints -scale '( ....)' utility to map the mesh to the correct dimensions. For sure, other parameters are different in order to have the same (or close) Reynolds and turbulent Reynolds numbers. Velocity is 10[m/s] and D=0.015[m]

The simulation converges, but results are quite far from expectations : frequency of von Karman vortex shedding is close to twice as low as it should be, and the discrepancy gets bigger as i increase the inlet velocity (and linked turbulence quantities accordingly).
Moreover, when plotting the drag coefficient, though in the reference case it is coherent and close to unity, it reaches crazy values (around 40) for the mapped case.
Though, the mean velocity profiles are self-similar, so the issue does not come from a wrong Re.

Has anyone ever encountered this issue ? If so, what could be wrong in my work.
Thanks a lot for helping

[SUBHANKAR]

Hi all

I too am solving the same problem. But i am encountering a different problem.
I am solving flow past a cylinder problem using pisoFoam. When i run the solver i get the following message:

subhankar@subhankar-Lenovo-G50-70:~/OpenFOAM/subhankar-3.0.1/run/tutorials/incompressible/pisoFoam/new$ pisoFoam
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 3.0.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 3.0.1-d8a290b55d28
Exec : pisoFoam
Date : Oct 14 2016
Time : 04:43:29
Host : "subhankar-Lenovo-G50-70"
PID : 9975
Case : /home/subhankar/OpenFOAM/subhankar-3.0.1/run/tutorials/incompressible/pisoFoam/new
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


PISO: Operating solver in PISO mode

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type laminar
No MRF models present

No finite volume options present


Starting time loop

forces forces:
Not including porosity effects

forceCoeffs forceCoeffs:
Not including porosity effects

Time = 0.5

Courant Number mean: 9.9323e-07 max: 0.00404131
...

Though it is running but i can't plot anything.No data is stored in my log document. Also i couldn't understand the line"No finite volume options present". Can anyone explain where i could have gone wrong?

Thanks and regards
Subhankar

[fredicenci]

Hi,

Did you change you files of forces and coefficients? seems like you forgot.

I am also trying to simulate this flow (Re = 10000) around a circular cylinder. My Cd and Cl are quite good but strouhal that should be around 0.2 is 0.13... I am starting to think that PisoFoam is the one messing with strouhal...

Did you solve your simulation? if yes, could you please share the files?


Thanks, good luck!

[fredicenci]

Hello all,

I am performing a simulation in a 2d cylinder using PISO and k-omega SST. I am getting good results for lift and drag, close to experimental results, however the frequency is bad. THe St should be around 0.2 but i am getting 0.13. I saw that it could be the relaxation factors that i used and PISO doesnt use, however if i remove them the st goes to 0.25 and lift and drag coefficients go up... Following is the link with my files..

https://www.dropbox.com/s/yqvex3mcld...er.tar.gz?dl=0

does anyone knows where i am messing up?

THanks a lot

[piu58]

Dear Fredi,

I looked at your simulation. Your Re number is 10000, so the expected drag coefficient is in the area between 1.05 (Sighard Hoerner, 1965) and 1.16 (Hermann Schlichting, 1951). You got around 1.03 which is in that range.

You use RANS for determination of viscosity. This method is applicable to predict total forces like drag and lift coefficients at not too high Re numbers. It is of lesser value if you need to know what happens in the boundary layer.

The Strouhal number results from a flow separation in the boundary layer. To get an idea of it you should use a more advanced turbulence model. Unfortunately, the most common LES models tend to introduce to much energy in the vortices. This leads to a prediction of forces which is too high. In other words: It is very hard to predict the lift/drag coefficients and the Strouhal number with one model.

~

I saw that you use first order schemes. This is not recommended because they are too diffusive. The problems rise with the turbulence, and Re = 10000 in not a unproblematic case.

~

You should assure that your results are confident, which is a task by it's own. There is no error control in CFD, so you have to assure that your results are acceptable with all means you have.
Whether the computed drag coefficient is 1.0 or 1.1 is not most important. A deviation from the experimental results is even probable, because the simulation assumes an infinite smooth surface, what is different from reality.
It would be much more of interest whether the changes calculated values with the Re number are as expected. I recommend the results from Schlichting for that which cover a very wide range of Re numbers, including the drag crisis.

[fredicenci]

Fist of all thanks for take your time and help me out. I really appreciate this.

1- According to this threat: Relaxation Factors for Transient solvers

I must not have relaxation factors in PISO. So I removed them.


2 -Yes, I am not trying to reach all the values of experimental results, i am just trying to perform a simulation right, and there was a disagreement between two works that I was following.
First the PhD theses from Rosetti 2015, where using Refresco code and the same turbulence model he found the values attached, which are high compared from experimental.

Second a paper, Stringer (2014), where using OF 1.7.1 he found much better results. Pictures attached.

Conclusion: Removing the relaxation factor my results seems to go in Rosetti's direction and I was wondering why. I guess it is because of the OF version, but i am still not sure.

Thanks for the tip about the numerical schemes.. what would you recommend? https://cfd.direct/openfoam/user-gui...s/#x20-1130159 .. leastSquare,Gauss linearUpwind grad(), and which Laplacian scheame?

Thanks for you time =)

[piu58]

The flow past a cylinder is a often used model geometry. The results differs widely, the two articles you mentioned are not the only results.

I looked at both.

The Stringer works shows a drag coefficient which gets lower with Re. This is not what the experiments give: A more or less constant value around 1 between 400 and 100000, and then a sharp decreasing down to 0.3 at Re ~ 300000 followed by a continuous increasing. You find experimental values at page 121 in the work of Rosetti. Rosetti's results show a decreasing drag coefficient form Re=10000 to 1 Mio, similar to Stinger.

Both results do not verify the experimental results. You may find some other articles which come to similar numerical values. Conclusion: The numeric used is not suitable for this question. I don't see any value in imitating one of the calculation procedures.

I found only one work which predicts the drag crisis more or less correct:
Boterill, Morvan, Owen: Investigation into the numerical modelling of the drag crisis for circular cylinders (2009). And even here the numerical results needs to be "corrected" in some way (correction for inlet turbulence, which I did not understand to full extend).

The most important question is, what do you want to get from your simulation. Then you have to look for the numerical tools which may be able to give you that kind of answer. Studies of uncertainties and numerical "effects" (=errors) are a large part of such a simulation.

[fredicenci]

Yes, i totally agree with you. I know that using URANS and k-omega SST it is not gonna predict correctly the drag, lift, pressure and etc. The paper from Boterill, Morvan, Owen (2009) they used LES.

My goal here is to learn how to perform correctly the simulation.

My concern is how Stringer got a Cl_rms value of close 0.4 using OF v1.7.1 and I using OF v4.1 get 1.2. I am close to Rosetti's value of 1.1. All of us is using K-omega SST.

So I was thinking that my values should be closer to Stringer' because it is the same software. This leads me to think that I have something wrong in my setup..

But as you look at my files and think that it is fine I will follow like this and see how the simulation goes. Look the results for my medium mesh at the pictures, they are without relaxation factors.

Thanks for looking after that so much.

[piu58]

The first thing I recommend for change are the schemes. I am sure that Stringer did not use first order schemes.

My (personal tinted) recommendation:

Use Gauss limitedLinear 1: The "1" means no limit = maximum accuracy. If you get problems with stability, reduce the 1 by 0.7 ... 0.5. If you need lower values something is wrong with your mesh.

[albet]

Hello,

I have a 3D case of water flow around the cylinder in Re=2e5. Can RANS be an applicable model for this simulation or I have to use LES model?
I tried the same case (Re =2e5) in 2D with RANS, but the Strouhal number is incorrect!
Could you please let me know your idea about it.

Kind regards,
Amir

[albet]

Hello again,
Could anybody help me with replying to above post?
Thanks,

[fredicenci]

Originally Posted by albet

Hello,

I have a 3D case of water flow around the cylinder in Re=2e5. Can RANS be an applicable model for this simulation or I have to use LES model?
I tried the same case (Re =2e5) in 2D with RANS, but the Strouhal number is incorrect!
Could you please let me know your idea about it.

Kind regards,
Amir

I know that 2D cases you will not get write results because of tridimensional fluid structures. However, I am not sure if URANS will get it on 3D cases... You probably should search for publications about it. Do you have computational power to run LES? if yes, you should try it.