# Attempting to validate force code with 2D cylinder

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

 December 13, 2007, 19:17 I've recently been trying to v #1 Member   Andrew Burns Join Date: Mar 2009 Posts: 36 Rep Power: 8 I've recently been trying to verify the force outputs of the 'ssimpleFoam' solver I got from another thread on this forum, it's essentially the simpleFoam solver which computes and outputs forces in 3 axes to a file during the simulation. The problem is a 0.5m diameter 2D cylinder in a flow field of 10m/sec and an nu of 0.05, am I correct in calculating a reynolds number of 100 for this situation? Re = (10*0.5)/0.05 Taken from a pdf I downloaded off the Nasa technical report server I have a graph of experimental Cd values for infinite cylinders Vs. Re. For a cylinder of Re 100 in steady translation through a viscous fluid I should be getting a Cd of between 1.3 and 1.5 or there-abouts. At an Re of 100 flow around the cylinder should be laminar, however I ran a laminar simulation with ssimpleFoam and ended up with a drag of only roughly 15N for this cylinder. Using the equation: Cd = Drag/0.5*rho*v^2*S Where: S = 0.5m rho = 1.225 Kg/m^3 Drag = 15N Cd = 0.49 Which is far far too low. I turned on turbulence with a k-epsilon model from this point and ran another 2000 iterations. I noticed a very slow oscillation in the Fx force, I've attached a plot of Fx vs iteration as an example but you can't really see the oscillation as its not really severe. http://i76.photobucket.com/albums/j2..._iteration.png The mesh was made in gmsh so it's unstructured. I tried to tighten up the mesh close into the surface of the cylinder and it's fairly detailed so I don't think it's a mesh problem but I can't be certain. Here are pics of the mesh as you zoom in. http://i76.photobucket.com/albums/j2...whole_mesh.png http://i76.photobucket.com/albums/j2...mesh_close.png http://i76.photobucket.com/albums/j2...ltra_close.png The average final value of drag from the turbulent model solution was about 23.5N, which using the above equation for Cd still only gives a Cd of 0.767 which is far too low. Does anyone have any ideas as to why my Cd are so far under what they should be? Other than nu in transport properties are there any other ways to specify the fluid properties like density that I'm missing?

 December 13, 2007, 21:05 Andrew, What is the depth o #2 Member   Alessandro Spadoni Join Date: Mar 2009 Location: Atlanta, GA Posts: 65 Rep Power: 8 Andrew, What is the depth of your model the z-direction? If it is large, it can introduce error in your force estimates. This is due to a really large aspect ratio of the cells closed to your cylinder, and the procedure used to compute forces. (If you do a search for liftDrag, you will find a thread where Dr. Jasak mentions this). Try making you z-depth something like 1% - 10% of the diameter of your cylinder. If the solver outputs forces then your drag will be: Cd = (Force per unit span)/(1/2 * rho V^2 * chord )=(Drag/(z-depth))/(1/2 * rho * v^2 * S). I mean your S, which I assume is the diameter of your cylinder. Alternatively, you can compute CD as: CD = (Force)/(1/2 * rho V^2 * wettedArea)=(Drag)/(1/2 * rho * v^2 * (z-depth)*pi*S). By S I mean your S. I hope this helps, Alessandro

 December 13, 2007, 21:07 Additional resources: http #3 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 699 Rep Power: 12

 December 13, 2007, 21:10 Andrew, I forgot to mention #4 Member   Alessandro Spadoni Join Date: Mar 2009 Location: Atlanta, GA Posts: 65 Rep Power: 8 Andrew, I forgot to mention the following: nu = mu / rho so your value of viscosity already includes information about density. This means that: Cd = (Force per unit span)/(1/2 V^2 * chord )=(Drag/(z-depth))/(1/2 * v^2 * S) CD = (Force)/(1/2 * V^2 * wettedArea)=(Drag)/(1/2 * v^2 * (z-depth)*pi*S). In other words OpenFOAM forces are really Force/density. Alessandro

 December 13, 2007, 21:12 The current cylinder depth is #5 Member   Andrew Burns Join Date: Mar 2009 Posts: 36 Rep Power: 8 The current cylinder depth is 100% cylinder diameter, so yes the aspect ratio is fairly far off close into the cylinder. However yesterday I accidently tried running with a mesh thickness 1% of the cylinder diameter and I could not get convergence, in fact the solution pressure would explode after only a few iterations, I think this is because while the prisms up close to the cylinder were fine, the ones out at the boundaries of the solution were flat as pancakes. I will try 10% diameter depth and see how that goes however. One thing I am still confused with is how OpenFoam deals with dynamic and kinematic viscosities. Just for reference, which of the two is nu in transport properties?

 December 13, 2007, 21:15 Andrew, I think nu stands f #6 Member   Alessandro Spadoni Join Date: Mar 2009 Location: Atlanta, GA Posts: 65 Rep Power: 8 Andrew, I think nu stands for kinematic viscosity. Alessandro

 December 13, 2007, 21:20 Andrew, Do you enforce the #7 Member   Alessandro Spadoni Join Date: Mar 2009 Location: Atlanta, GA Posts: 65 Rep Power: 8 Andrew, Do you enforce the following boundary conditions? z-constant plane towards you (type empty) z-constant plane away from you (type empty) Since you problem is 2-D, the pancake like elements far away from the cylinder should not matter too much as the bad-aspect-ratio side is being neglected (if you set them to type empty). Not super sure about this last statement. But make sure you make your frontBack planes as type empty. Alessandro

 December 13, 2007, 21:32 Previously the Z planes toward #8 Member   Andrew Burns Join Date: Mar 2009 Posts: 36 Rep Power: 8 Previously the Z planes towards and away from me were set as symmetryplane. I've now set them to empty and I reduced the height of my mesh to 10% of the cylinder diameter and I'm re-running the solution, which appears to be running correctly. If it does work and my answer is different again I may try reducing the cell heights to 1%.

 December 13, 2007, 23:02 Still getting a Cd that's too #9 Member   Andrew Burns Join Date: Mar 2009 Posts: 36 Rep Power: 8 Still getting a Cd that's too high, approximately 0.75.

 December 13, 2007, 23:03 Sorry I meant the Cd is too sm #10 Member   Andrew Burns Join Date: Mar 2009 Posts: 36 Rep Power: 8 Sorry I meant the Cd is too small, not high.

 December 14, 2007, 00:22 "I've recently been trying to #11 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 699 Rep Power: 12 "I've recently been trying to verify the force outputs of the 'ssimpleFoam' solver I got from another thread on this forum, it's essentially the simpleFoam solver which computes and outputs forces in 3 axes to a file during the simulation. " Which thread are you referring to?

 December 14, 2007, 01:06 http://www.cfd-online.com/Open #12 Member   Andrew Burns Join Date: Mar 2009 Posts: 36 Rep Power: 8 http://www.cfd-online.com/OpenFOAM_D...es/1/5067.html About half way down that page. I used the same mesh and increased Re to approx 500000 and ended up with a Cd of around 0.9, when it should be around 0.3. I don't think the separation point is being accurately simulated, which would explain why I'm getting low Cd's for detached cases and high Cd's for attached cases.

 December 14, 2007, 02:15 Pack your case and post it her #13 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 699 Rep Power: 12 Pack your case and post it here or email it to me. I will look into it. My email address is available in my profile.

 December 14, 2007, 02:39 Hi Andrew, To check force o #14 Senior Member   Vincent RIVOLA Join Date: Mar 2009 Location: France Posts: 277 Rep Power: 9 Hi Andrew, To check force outputs, I wouldn't try the cylinder case with a Re of 100. If I remember well, this is about the starting point for vortex sheding, which might explain the oscillations you noticed. Do you have results to compare with for other Re numbers? Then, I'm not sure it's right but I would computed Cd as: Cd = Drag/(0.5*v^2*(domaineDepth*D)) with D being the diameter of the cylinder and domainDepth the depth of your domain (1%, 10% of D) Hope this helps a little, Vincent

 December 14, 2007, 05:20 Why don't you start off with a #15 Senior Member   Frank Bos Join Date: Mar 2009 Location: The Netherlands Posts: 338 Rep Power: 9 Why don't you start off with a static 2D cylinder at Re=200 using icoFoam. Just laminar vortex shedding which is well documented and you can test if your forces are calculated correctly. Frank __________________ Frank Bos

 December 14, 2007, 06:55 Srinath Madhavan, I'll pack up #16 Member   Andrew Burns Join Date: Mar 2009 Posts: 36 Rep Power: 8 Srinath Madhavan, I'll pack up the case and send it to you tomorrow when I'm back at work, thanks for the help. Currently I'm trying the simplefoam case because the only solver I have that outputs forces is ssimplefoam, I haven't yet compiled liftdrag into my version of openfoam.

 December 17, 2007, 17:47 Srinath, did you get a chance #17 Member   Andrew Burns Join Date: Mar 2009 Posts: 36 Rep Power: 8 Srinath, did you get a chance to look at the case I sent to you? I sent it to your gmail.

 December 17, 2007, 18:03 Yup, got it. Sorry I have not #18 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 699 Rep Power: 12 Yup, got it. Sorry I have not had a chance to look at it. I am at work right now. I'll give it a looksie once I'm at home. By the way I noticed that your Re is far from the laminar regime. I almost certainly can tell you to expect discrepancies when comparing dimensionless force coefficients (such as lift/drag) with experiments or DNS data. As you can see, there are folks still working on validating the liftDrag tool for turbulent flows. However, the one regime where I can be confident that you will get good agreement with exp. data is the laminar steady or even unsteady regime. I am willing to try out your case for that Re if you are interested.

 December 17, 2007, 18:07 Also, what Frank suggests is v #19 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 699 Rep Power: 12 Also, what Frank suggests is very logical. I would also recommend that you start off with low Re, validate your Cd/Cl calculation and then progress to higher Re. Frank has performed comprehensive tests on a circular cylinder[1]. Be sure to check that thread for pointers. Other things worth investigating are: a) Use of a convective outlet B/C. See [2]. b) Use of a Fixed mean value pressure outlet B/C. See [3]. References: [1] http://www.cfd-online.com/OpenFOAM_D...tml?1152126462 [2] http://www.cfd-online.com/OpenFOAM_D...tml?1190761096 [3] http://www.cfd-online.com/OpenFOAM_D...tml?1197751034

 December 17, 2007, 20:17 I just tried the cylinder with #20 Member   Andrew Burns Join Date: Mar 2009 Posts: 36 Rep Power: 8 I just tried the cylinder with an Re = 50, this Reynolds number should be too low for vortex shedding so a steady state solution should do, Cd should be around 1.5. I'm getting a Cd of 0.68 after 1500 iterations, pressure has converged to 1*10^-3 and the force is fairly stable, slightly decreasing. The force readout is: Total pressure Force = (0.012949 7.69589e-05 6.39884e-21) Total viscous Force = (0.00678759 -5.97422e-05 -2.00328e-21) Total turbulent Force = (0 0 0) Total Force = (0.0197366 1.72167e-05 4.39556e-21) (note I'm running a laminar only solution). One thing to note is viscous force is about half that of pressure force, could it be that the mesh close to the surface of the cylinder is not fine enough to accurately capture the effects of viscous force? I thought that at such a low Re viscous forces would account for a large percentage of drag.

 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 student Main CFD Forum 1 December 13, 2008 17:59 Kai Yan Main CFD Forum 0 July 16, 2008 07:07 Abhi Main CFD Forum 3 July 14, 2006 01:49 pradeep PANTANGI CD-adapco 5 September 14, 2004 14:25 Bin Li Main CFD Forum 5 October 10, 2003 16:37

All times are GMT -4. The time now is 10:54.