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

Low Reynolds number question

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

Like Tree4Likes
  • 4 Post By kalle

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 10, 2013, 10:49
Default Low Reynolds number question
  #1
Senior Member
 
Join Date: Jul 2013
Posts: 124
Rep Power: 12
wildfire230 is on a distinguished road
Does anyone know why using small Reynolds numbers ( < 5 ) requires continuously smaller time steps? Even with the cavity tutorial, using Reynolds numbers less than one requires very small time steps to prevent the Courant number from exploding. There is probably something fundamental I'm missing. Is icoFoam not the best choice for low Reynolds numbers?

Thanks for your help.
wildfire230 is offline   Reply With Quote

Old   August 10, 2013, 13:13
Default
  #2
Member
 
Glenn Carlson, PE, PhD (ret)
Join Date: Oct 2012
Location: US
Posts: 49
Rep Power: 13
gcengineer is on a distinguished road
Sorry. I'm not sure what you mean by "small Reynolds numbers."

Do you mean the velocity of the wall is low? Or are you referring to the behavior of turbulence models close to a wall?

Of course, very fine meshes can require small time steps to avoid large Courant numbers, but it doesn't sound like this is what you are referring to.
gcengineer is offline   Reply With Quote

Old   August 10, 2013, 13:20
Default
  #3
Senior Member
 
Join Date: Jul 2013
Posts: 124
Rep Power: 12
wildfire230 is on a distinguished road
Hi, thanks for you reply. I mean Reynolds numbers less than 5. I run into this problem with every mesh while using icoFoam, even the cavity tutorial. For example, in the cavity tutorial, the only thing I am changing is the Reynolds number, not the grid size or the velocity. I am controlling the Reynolds number by changing the kinematic viscosity. As far as I am aware, you only need to decrease the time step if you decrease the grid size in the direction of the velocity, or increase the velocity in the direction of the grid. However, when I start decreasing the Reynolds number below 5 or below 1, etc... I have to significantly decrease the time step in order to preserve stability.
wildfire230 is offline   Reply With Quote

Old   August 10, 2013, 13:57
Default
  #4
Member
 
Glenn Carlson, PE, PhD (ret)
Join Date: Oct 2012
Location: US
Posts: 49
Rep Power: 13
gcengineer is on a distinguished road
Sorry again.

How are you calculating Reynolds number? Re = UD/nu, where U is velocity of moving wall and nu is kinematic viscosity? What are you using for D? The length of a side of the cavity? Something else?

Are you modeling turbulence? If so, what model are you using?

Also, what version of OpenFOAM are you using?
gcengineer is offline   Reply With Quote

Old   August 10, 2013, 14:25
Default
  #5
Senior Member
 
Join Date: Jul 2013
Posts: 124
Rep Power: 12
wildfire230 is on a distinguished road
I'm calculating the Reynolds number as you said, Re = U * d / nu, where U = 1, d = 0.1. Thus my Re = 0.1 / nu. Just as they do in the cavity tutorial. I'm not modelling turbulence, as icoFoam is a laminar solver, and I'm using OpenFOAM 2.2.0. Everything is fine for Reynolds numbers from say 5 to 100, but with Reynolds numbers less than 5 or 1, I have to decrease the time step to preserve stability. I should also note that I am not using implicit schemes.
wildfire230 is offline   Reply With Quote

Old   December 12, 2013, 09:47
Default
  #6
New Member
 
Otto S.
Join Date: Oct 2013
Location: Germany
Posts: 2
Rep Power: 0
Otto S. is on a distinguished road
Dear wildfire230,

I have a similar problem: With increasing viscosity I have to lower the time steps. Do you found a solution for this problem?
Otto S. is offline   Reply With Quote

Old   December 13, 2013, 01:55
Default
  #7
Senior Member
 
Karl-Johan Nogenmyr
Join Date: Mar 2009
Location: Linköping
Posts: 279
Rep Power: 21
kalle is on a distinguished road
Ferziger and Peric discusses this. In 2nd edition you'll find it in section 6.3.1. When diffusion starts to dominate over convection, you have another instability to cater for than the one set by the Courant number. You'll trigger the instability by refining mesh, or increasing viscosity. And if your solver only sets time step according to Courant number, you'll trigger it when the Courant number allows you to take large time steps.

deltaT < 1 / ( 2*Gamma/(rho*dx*dx) + u/dx )

Courant number is only the last term above. (Gamma is diffusion coefficient (viscosity))
tfuwa, lev, SHUBHAM9595 and 1 others like this.
kalle is offline   Reply With Quote

Old   December 13, 2013, 04:34
Default
  #8
New Member
 
Otto S.
Join Date: Oct 2013
Location: Germany
Posts: 2
Rep Power: 0
Otto S. is on a distinguished road
Hey kalle,

thank you for your answer! This is the explanation I was looking for.
Otto S. is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
plotting drag coefficient in low reynolds number flow past cylinder atmcfd FLUENT 0 January 2, 2010 08:34
low reynolds number K-epsilon model amar STAR-CD 2 March 23, 2009 07:24
Low Reynolds number airfoil. Pablo Cornejo FLUENT 14 October 19, 2005 09:41
DNS -low Reynolds number Airfoils Pat Main CFD Forum 2 January 21, 2005 14:17
Low Reynolds number for airfoil Richard Main CFD Forum 1 March 20, 2000 07:24


All times are GMT -4. The time now is 14:59.