# LiftDrag validation Part 1 steady

 Register Blogs Members List Search Today's Posts Mark Forums Read

 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: 703 Rep Power: 14 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

 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: 703 Rep Power: 14 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: 703 Rep Power: 14 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

 August 20, 2008, 17:45 Addendum: I used a time-step s #5 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 14 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.

 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: 703 Rep Power: 14 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: 10 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?

 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: 703 Rep Power: 14 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

 August 25, 2008, 13:35 I dont understand what u mean #9 Senior Member   mayank gupta Join Date: Mar 2009 Posts: 110 Rep Power: 10 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

 August 26, 2008, 06:59 my time step is 3e-08 veloc #10 Senior Member   mayank gupta Join Date: Mar 2009 Posts: 110 Rep Power: 10 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

 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: 703 Rep Power: 14 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: 10 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

 August 28, 2008, 07:13 HI srinath, I have received #13 Senior Member   mayank gupta Join Date: Mar 2009 Posts: 110 Rep Power: 10 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

 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: 703 Rep Power: 14 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: 16 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: 16 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: 703 Rep Power: 14 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: Beijing, China Posts: 689 Blog Entries: 9 Rep Power: 14 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 __________________ ~ Daniel WEI ------------- Boeing Research & Technology - China Beijing, China Email

 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: 703 Rep Power: 14 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: 10 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 Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post hoochie OpenFOAM Post-Processing 29 September 19, 2014 03:38 nuovodna OpenFOAM Running, Solving & CFD 45 September 2, 2009 17:56 ryan_m OpenFOAM Running, Solving & CFD 2 August 24, 2009 21:26 marco OpenFOAM Post-Processing 10 March 6, 2009 10:51 fabian_korn OpenFOAM Post-Processing 1 September 22, 2008 02:34

All times are GMT -4. The time now is 00:37.