I've recently been trying to v
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 thereabouts. 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 kepsilon 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? 
Andrew,
What is the depth o
Andrew,
What is the depth of your model the zdirection? 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 zdepth 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/(zdepth))/(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 * (zdepth)*pi*S). By S I mean your S. I hope this helps, Alessandro 
Additional resources:
http

Andrew,
I forgot to mention
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/(zdepth))/(1/2 * v^2 * S) CD = (Force)/(1/2 * V^2 * wettedArea)=(Drag)/(1/2 * v^2 * (zdepth)*pi*S). In other words OpenFOAM forces are really Force/density. Alessandro 
The current cylinder depth is
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? 
Andrew,
I think nu stands f
Andrew,
I think nu stands for kinematic viscosity. Alessandro 
Andrew,
Do you enforce the
Andrew,
Do you enforce the following boundary conditions? zconstant plane towards you (type empty) zconstant plane away from you (type empty) Since you problem is 2D, the pancake like elements far away from the cylinder should not matter too much as the badaspectratio 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 
Previously the Z planes toward
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 rerunning 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%. 
Still getting a Cd that's too
Still getting a Cd that's too high, approximately 0.75.

Sorry I meant the Cd is too sm
Sorry I meant the Cd is too small, not high.

"I've recently been trying to
"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? 
http://www.cfdonline.com/Open
http://www.cfdonline.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. 
Pack your case and post it her
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.

Hi Andrew,
To check force o
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 
Why don't you start off with a
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 
Srinath Madhavan, I'll pack up
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. 
Srinath, did you get a chance
Srinath, did you get a chance to look at the case I sent to you? I sent it to your gmail.

Yup, got it. Sorry I have not
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.

Also, what Frank suggests is v
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.cfdonline.com/OpenFOAM_D...tml?1152126462 [2] http://www.cfdonline.com/OpenFOAM_D...tml?1190761096 [3] http://www.cfdonline.com/OpenFOAM_D...tml?1197751034 
I just tried the cylinder with
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 7.69589e05 6.39884e21) Total viscous Force = (0.00678759 5.97422e05 2.00328e21) Total turbulent Force = (0 0 0) Total Force = (0.0197366 1.72167e05 4.39556e21) (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. 
All times are GMT 4. The time now is 00:20. 