[msrinath80]

Hi all,

I have compared the pressure and viscous drag predicted by OpenFOAM with those from another reference which provides pressure drag, viscous drag, pressure lift, viscous lift and Strouhal number over a range of Reynolds numbers for both the circular (Re = 50 to 5000) and square (Re = 40 to 300) cylinders[1]. The differences are less than 0.75% as shown below:


Force coefficient OF 1.4 Ref. 1 % difference

Cd (total) 1.98002 1.98 0.00115

Cd (pressure) 1.68851 1.69 -0.08805

Cd (viscous) 0.29151 0.29 0.521



The only catch is that I had to use approx 6 million uniform cells to get to this answer which isn't very encouraging. The paper uses QUICK with non-uniform cells and gets this answer using just 4864 cells. I tried the case with these settings and found differences as high as 7%. Certainly I am doing something stupid here. Can anyone help?

My case is attached to this post. I would appreciate if someone could comment of the choice of discretization schemes that would yield a similar result with much fewer cells.

References:

[1] Franke, R., W. Rodi and B. Schonung, "Numerical calculation of laminar vortex-shedding flow past cylinders", Journal of Wind Engineering and Industrial Aerodynamics, v35, 237-257 (1990).

Attachments:

franke_et_al.tar.gz

[msrinath80]

I forgot to mention that the above results are for Re = 40 (square cylinder).

[mcp]

Hi,

I think I am facing a similar problem. I did some convergence testing on viscous wall shear stress acting on a cuboid in laminar flow. I also had to use more than 2 million elements to obtain reasonable results.

As Srinath Madhavan in the original post I would appreciate if someone could comment on the discretization schemes or any other reason that might cause this behavior.

Cheers,
Christian

[msrinath80]

Hello once again to all Foamers:

I have completed part 2 of the above LiftDrag validation and am pleased to report the results for unsteady time-periodic flow (Re = 100) from the same reference[1] as above.


Force coefficient OF 1.4.1 Ref. 1 ABS(% difference)

Cd (total [time avg]) 1.62667 1.61 1.035

Cd (pressure [time avg]) 1.56689 1.55 1.089

Cd (viscous [time avg]) 0.059774 0.06 0.3766

Cl (total max) + 0.2674 + 0.27 0.9629

Cl (total min) - 0.26739 - 0.27 0.9667

Cl (pressure max) + 0.23434 + 0.24 2.358

Cl (pressure min) - 0.23435 - 0.24 2.354

Cl (viscous max) + 0.03488 + 0.03 16.267

Cl (viscous min) - 0.03488 - 0.03 16.267

Strouhal number 0.15894 0.154 3.207






Notes:

I believe that there is a chance that that 16% difference in Cl (viscous max and min) is due to lack of precision in the values printed in the reference. The fact that the reference also lists the same Cl (viscous max and min) value (i.e plus or minus 0.03) for Re = 70 reaffirms the above plausibility.

The fundamental vortex shedding frequency was obtained by performing a FFT on the transverse velocity time signal at a point downstream of the cylinder (using the probes functionality in OpenFOAM). The Strouhal number was of course estimated by multiplying this frequency with the characteristic length scale (i.e. cylinder diameter) and dividing the result by the characteristic velocity scale (i.e. average velocity at inlet). As expected, the Strouhal number obtained from a FFT of Lift coefficient data was found to be the same as that obtained from the transverse velocity data.

For anyone interested, the GNU/Octave code to perform an FFT is also attached to this post[2].

As always, any comments/suggestions/criticisms are appreciated :-)


References:

[1] Franke, R., W. Rodi and B. Schonung, "Numerical calculation of laminar vortex-shedding flow past cylinders", Journal of Wind Engineering and Industrial Aerodynamics, v35, 237-257 (1990).


Attachments:

[1] franke_et_al_re_100.tar.bz2

[2] octave_fft_routine.tar.bz2

[msrinath80]

Addendum: I used a time-step size of 0.00006 seconds and the 'backward' scheme. The maximum Courant number never exceeded 0.25. At least 10 full cycles were used for time-averaging all relevant data. The initial transients were of course discarded before this was done. The domain was discretized using 556784 cells. Once again, the original reference used only 6688 cells to get these results.

[msrinath80]

Any comments anyone?

[mgz1985]

hi srinath,

sorry to be posting my query here. I wanted to know if some-one has verified the liftDrag codes with the wind-tunnel datas for an airfoil. I have tried every thing I knew with OpenFOAM-1.5 forces function but I get wrong results for Cl although Cd is perfect. (icoFoam because it is incompressible flow)

the error is in reference length I guess because even if i change the reference length, it does not affect my results.

can u suggest me something new to try?

[msrinath80]

Are you sure, you're doing the calculation right? Remember to divide by the distance in the third direction (even if your case is 2D). See [1] for more details.

Also, it would help if you post the grid you use, the Reynolds number you are trying to simulate and the percentage difference in Cd and Cl that you are observing presently.

References:

[1] http://www.cfd-online.com/OpenFOAM_D...es/1/2726.html

[mgz1985]

I dont understand what u mean by saying divide by the length in the third direction.

Anyways, my chord length is 600mm and span is 1200mm, so i guess my Aref is 0.72 and Lref is 0.6.

My reynolds number is 1.67 million, so using the BL thickness layer, my minimum cell thickness becomes 7.9e-05 (I used 0.1/sqrt(Re)

can u tell me if these values are correct?time step i m using is 3e-0 to stabilize the courant number.

regarding the blockMeshDict it is in my office. i shall put it here on wednesday as I m not going tomorrow.

You culd still tell if these values are correct or not.

Thank a lot

[mgz1985]

my time step is 3e-08

velocity is 14.7m/s

and i m attaching my blockMesh file with this. I used a rectangular box.

blockMeshDict

[msrinath80]

Why are you using icoFoam for Re = 1670000? Do you want to resolve the turbulence as opposed to modeling it?

[mgz1985]

i m using icoFoam because the flow is incompressible Mach<0.3.

I have tried using simpleFoam with the k-epsilon model but it did not help improve the results and even spalart-allmaras model. and yes also, when i use simpleFoam, my pressure field is absurd

The turbulence modelling is not as important as the validation of the co-efficients.

The latest thing i m trying is to use the latestTime in the controlDict file instead of endTime. currently my simulations are running with this modification.

yes one more thing, i forgot to mention the wind-tunnel values

Cd=0.016, Cl=2.6

thanks a lot

[mgz1985]

HI srinath,

I have received my values for the running case but it did not help either. Cl=0.091..,Cd=0.023

I am again running some new cases. I have changed my nNonorthogonalcorrectors to 4. The news is that the difference between the co-effieicients is of the order of 2.

I am also running a turbulence steady state model and can tell you the results tomorrow but it is not showing me any hope.

As this is my first case in OpenFOAM, I would like to if there is any mistake in my settings of files? Because if the settings are correct I would like to start playing with the different schemes in solution?

Thanks for your patience

[msrinath80]

Please post your case here.

[l_r_mcglashan]

I need to get the forces on a wall, so have been using these benchmark cases to see what mesh I'll need for my real geometry.
I'm quite curious about the need for so many cells. Did you try having a higher grading nearer the square cylinder?
Also are you happy with the boundary condition of symmetry?

[l_r_mcglashan]

Today I did a quick run for a circular cylinder with a flow of Re=1.

The mesh is:





and the drag coefficient appears to be starting to oscillate as the pressure residuals decrease

[msrinath80]

Did you try having a higher grading nearer the square cylinder?

A very good question indeed. The answer is Yes. In fact that was the first thing I tried. However, whenever I exceeded an aspect ratio of 1:5, the amount of time required to complete a certain number of time steps increased (when compared to a uniformly graded mesh) as well. Nevertheless, on the best (i.e. well adapted) mesh which is very well refined all around the cylinder and downstream of the cylinder, I could not get accurate answers for the lift/drag coefficients (i.e. the % difference was greater than 5%).



Also are you happy with the boundary condition of symmetry?

My feelings are irrelevant :-) The original numerical reference with which I was comparing used symmetry B/Cs, so I had no choice!



Today I did a quick run for a circular cylinder with a flow of Re=1.

Give it more iterations. It should stabilize soon enough. Also I would try and monitor the pressure and/or velocity at certain points inside the domain to see if they stabilize with increasing iterations.

[lakeat]

I'm interested in this too.

Hi srinath, can you have a look at my problem,
http://www.cfd-online.com/OpenFOAM_D...es/1/1678.html

Is it the same problem with you?

Regards, \Daniel

[msrinath80]

I don't see any problem. No offense, but in fact, I fail to even comprehend your post.

In my experience, OpenFOAM seems to be giving *very* accurate answers for the dimensionless force coefficients if you provide it with a very nicely refined mesh in regions of strong gradients in pressure/velocity. Keep the Courant number around 0.25 and you have a very ideal problem setup from the view point of accuracy.

[naveen]

hi msrinath80,

myself Naveen working on flow around a circular cylinder using OpenFOAM 1.4.1 and 1.5 versions past 1 month. I am getting pressure and velocity contours correctly in both the versions.I am facing difficult to get the vortex shedding frequency in OpenFOAM.

Can you please suggest me how to get the strouhal number and vortex shedding frequency in OpenFOAM.

Flow conditions:

Reynolds number---------> 150 (based on cylinder diameter)
velocity------------------------>1 m/s
viscosity---------------------->1 (based on cylinder diameter)
diameter of cylinder--------> 2 m

can you please give me a suggestion how to get these values.

waiting for your response

Regards,

Naveen