
[Sponsors] 
October 17, 2007, 14:44 
Hi all,
I have compared the

#1 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12 
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 nonuniform 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 vortexshedding flow past cylinders", Journal of Wind Engineering and Industrial Aerodynamics, v35, 237257 (1990). Attachments: franke_et_al.tar.gz 

October 17, 2007, 14:51 
I forgot to mention that the a

#2 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12 
I forgot to mention that the above results are for Re = 40 (square cylinder).


October 18, 2007, 06:29 
Hi,
I think I am facing a s

#3 
New Member
Christian
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1
Rep Power: 0 
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 

August 20, 2008, 17:31 
Hello once again to all Foamer

#4 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12 
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 timeperiodic 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 vortexshedding flow past cylinders", Journal of Wind Engineering and Industrial Aerodynamics, v35, 237257 (1990). Attachments: [1] franke_et_al_re_100.tar.bz2 [2] octave_fft_routine.tar.bz2 

August 20, 2008, 17:45 
Addendum: I used a timestep s

#5 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12 
Addendum: I used a timestep 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 timeaveraging 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.


August 24, 2008, 16:22 
Any comments anyone?

#6 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12 
Any comments anyone?


August 25, 2008, 01:39 
hi srinath,
sorry to be pos

#7 
Senior Member
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 8 
hi srinath,
sorry to be posting my query here. I wanted to know if someone has verified the liftDrag codes with the windtunnel datas for an airfoil. I have tried every thing I knew with OpenFOAM1.5 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? 

August 25, 2008, 12:32 
Are you sure, you're doing the

#8 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12 
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.cfdonline.com/OpenFOAM_D...es/1/2726.html 

August 25, 2008, 13:35 
I dont understand what u mean

#9 
Senior Member
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 8 
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 7.9e05 (I used 0.1/sqrt(Re) can u tell me if these values are correct?time step i m using is 3e0 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 

August 26, 2008, 06:59 
my time step is 3e08
veloc

#10 
Senior Member
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 8 
my time step is 3e08
velocity is 14.7m/s and i m attaching my blockMesh file with this. I used a rectangular box. blockMeshDict 

August 26, 2008, 18:23 
Why are you using icoFoam for

#11 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12 
Why are you using icoFoam for Re = 1670000? Do you want to resolve the turbulence as opposed to modeling it?


August 27, 2008, 01:49 
i m using icoFoam because the

#12 
Senior Member
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 8 
i m using icoFoam because the flow is incompressible Mach<0.3.
I have tried using simpleFoam with the kepsilon model but it did not help improve the results and even spalartallmaras 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 coefficients. 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 windtunnel values Cd=0.016, Cl=2.6 thanks a lot 

August 28, 2008, 07:13 
HI srinath,
I have received

#13 
Senior Member
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 8 
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 coeffieicients 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 

August 28, 2008, 18:34 
Please post your case here.

#14 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12 
Please post your case here.


October 1, 2008, 10:02 
I need to get the forces on a

#15 
Senior Member
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 14 
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?
__________________
Laurence R. McGlashan :: Website 

October 1, 2008, 10:17 
Today I did a quick run for a

#16 
Senior Member
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 14 
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
__________________
Laurence R. McGlashan :: Website 

October 1, 2008, 16:14 
Did you try having a higher gr

#17 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12 
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. 

October 9, 2008, 23:00 
I'm interested in this too.

#18 
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12 
I'm interested in this too.
Hi srinath, can you have a look at my problem, http://www.cfdonline.com/OpenFOAM_D...es/1/1678.html Is it the same problem with you? Regards, \Daniel
__________________
~ Daniel WEI  NatHaz Modeling Laboratory Department of Civil & Environmental Engineering & Earth Sciences University of Notre Dame, USA Email  My Personal CFD Blog 

October 10, 2008, 09:45 
I don't see any problem. No of

#19 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12 
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. 

May 21, 2010, 05:49 
LiftDrag validation Part 1 steady

#20 
Senior Member
NAVEEN.K.M
Join Date: Mar 2009
Location: Bangalore, Karnataka, india
Posts: 114
Rep Power: 8 
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 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Question to liftDrag  hoochie  OpenFOAM PostProcessing  29  September 19, 2014 03:38 
LiftDrag tool  nuovodna  OpenFOAM Running, Solving & CFD  45  September 2, 2009 17:56 
LiftDrag for 141  ryan_m  OpenFOAM Running, Solving & CFD  2  August 24, 2009 21:26 
Liftdrag calculation  marco  OpenFOAM PostProcessing  10  March 6, 2009 10:51 
LiftDrag coefficient in LES  fabian_korn  OpenFOAM PostProcessing  1  September 22, 2008 02:34 