CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Attempting to validate force code with 2D cylinder

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 13, 2007, 19:17
Default I've recently been trying to v
  #1
Member
 
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 8
andrewburns is on a distinguished road
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?
andrewburns is offline   Reply With Quote

Old   December 13, 2007, 21:05
Default Andrew, What is the depth o
  #2
Member
 
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 8
gtg627e is on a distinguished road
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
gtg627e is offline   Reply With Quote

Old   December 13, 2007, 21:07
Default 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
msrinath80 is on a distinguished road
Additional resources:

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

[2] http://www.cfd-online.com/OpenFOAM_D...es/1/2320.html

[3] http://www.cfd-online.com/OpenFOAM_D...es/1/1678.html
msrinath80 is offline   Reply With Quote

Old   December 13, 2007, 21:10
Default Andrew, I forgot to mention
  #4
Member
 
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 8
gtg627e is on a distinguished road
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
gtg627e is offline   Reply With Quote

Old   December 13, 2007, 21:12
Default The current cylinder depth is
  #5
Member
 
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 8
andrewburns is on a distinguished road
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?
andrewburns is offline   Reply With Quote

Old   December 13, 2007, 21:15
Default Andrew, I think nu stands f
  #6
Member
 
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 8
gtg627e is on a distinguished road
Andrew,

I think nu stands for kinematic viscosity.

Alessandro
gtg627e is offline   Reply With Quote

Old   December 13, 2007, 21:20
Default Andrew, Do you enforce the
  #7
Member
 
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 8
gtg627e is on a distinguished road
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
gtg627e is offline   Reply With Quote

Old   December 13, 2007, 21:32
Default Previously the Z planes toward
  #8
Member
 
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 8
andrewburns is on a distinguished road
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%.
andrewburns is offline   Reply With Quote

Old   December 13, 2007, 23:02
Default Still getting a Cd that's too
  #9
Member
 
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 8
andrewburns is on a distinguished road
Still getting a Cd that's too high, approximately 0.75.
andrewburns is offline   Reply With Quote

Old   December 13, 2007, 23:03
Default Sorry I meant the Cd is too sm
  #10
Member
 
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 8
andrewburns is on a distinguished road
Sorry I meant the Cd is too small, not high.
andrewburns is offline   Reply With Quote

Old   December 14, 2007, 00:22
Default "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
msrinath80 is on a distinguished road
"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?
msrinath80 is offline   Reply With Quote

Old   December 14, 2007, 01:06
Default http://www.cfd-online.com/Open
  #12
Member
 
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 8
andrewburns is on a distinguished road
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.
andrewburns is offline   Reply With Quote

Old   December 14, 2007, 02:15
Default 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
msrinath80 is on a distinguished road
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.
msrinath80 is offline   Reply With Quote

Old   December 14, 2007, 02:39
Default Hi Andrew, To check force o
  #14
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 277
Rep Power: 9
vinz is on a distinguished road
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
vinz is offline   Reply With Quote

Old   December 14, 2007, 05:20
Default 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
lr103476 is on a distinguished road
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
lr103476 is offline   Reply With Quote

Old   December 14, 2007, 06:55
Default Srinath Madhavan, I'll pack up
  #16
Member
 
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 8
andrewburns is on a distinguished road
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.
andrewburns is offline   Reply With Quote

Old   December 17, 2007, 17:47
Default Srinath, did you get a chance
  #17
Member
 
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 8
andrewburns is on a distinguished road
Srinath, did you get a chance to look at the case I sent to you? I sent it to your gmail.
andrewburns is offline   Reply With Quote

Old   December 17, 2007, 18:03
Default 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
msrinath80 is on a distinguished road
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.
msrinath80 is offline   Reply With Quote

Old   December 17, 2007, 18:07
Default 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
msrinath80 is on a distinguished road
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
msrinath80 is offline   Reply With Quote

Old   December 17, 2007, 20:17
Default I just tried the cylinder with
  #20
Member
 
Andrew Burns
Join Date: Mar 2009
Posts: 36
Rep Power: 8
andrewburns is on a distinguished road
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.
andrewburns is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
drag force in flow over a cylinder student Main CFD Forum 1 December 13, 2008 17:59
Urgently Need the code of Lift force and VM force Kai Yan Main CFD Forum 0 July 16, 2008 07:07
Code for flow over a cylinder Abhi Main CFD Forum 3 July 14, 2006 01:49
Error attempting to open X display pradeep PANTANGI CD-adapco 5 September 14, 2004 14:25
the question about validate code Bin Li Main CFD Forum 5 October 10, 2003 16:37


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