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

Low Reynolds Number help new to openfoam

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

Like Tree2Likes
  • 2 Post By eugene

Reply
 
LinkBack Thread Tools Display Modes
Old   July 21, 2006, 10:28
Default Hi, I have never used openf
  #1
New Member
 
Bryan Godbolt
Join Date: Mar 2009
Location: London, Ontario, Canada
Posts: 14
Rep Power: 8
soup is on a distinguished road
Hi,

I have never used openfoam before. I want to simulate a deformable body on a microscopic scale. This means I need to solve incompressible viscous flow at low reynolds number in an infinite space.

Can someone point me in the right direction as to what solver I should be looking at or any other tips ? I'm also fairly new to fluid dynamics so if something i've said doesn't make sense I am happy to clarify.

Thanks,

Bryan
soup is offline   Reply With Quote

Old   July 21, 2006, 12:32
Default Perhaps icoFoam or simpleFoam.
  #2
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
Perhaps icoFoam or simpleFoam. But if you want to study deformations, I think you might need to look into DynFoam or some such. Have you searched the forum for similar cases?
msrinath80 is offline   Reply With Quote

Old   July 21, 2006, 12:36
Default Thank you for your reply. I
  #3
New Member
 
Bryan Godbolt
Join Date: Mar 2009
Location: London, Ontario, Canada
Posts: 14
Rep Power: 8
soup is on a distinguished road
Thank you for your reply.

I have searched the forum and the internet for information on low reynolds number simulation in openFoam and I haven't been able to find anything saying whether current solvers in openFoam are capable of this.

How can I find out whether icoFoam or simpleFoam will work?
soup is offline   Reply With Quote

Old   July 21, 2006, 12:39
Default If the flow is laminar, icoFoa
  #4
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
If the flow is laminar, icoFoam or one its moving mesh capable variants (search the forum, there are a good number of folks working on moving mesh) will do just fine. If you're referring to low-Re turbulence models, there is info out here[1].

[1] http://www.opencfd.co.uk/openfoam/tu...tml#turbulence
msrinath80 is offline   Reply With Quote

Old   July 23, 2006, 21:08
Default Just to clarify with laminar f
  #5
New Member
 
Bryan Godbolt
Join Date: Mar 2009
Location: London, Ontario, Canada
Posts: 14
Rep Power: 8
soup is on a distinguished road
Just to clarify with laminar flow icoFoam will work even at very low reynolds number?
soup is offline   Reply With Quote

Old   July 24, 2006, 10:34
Default Totally. It should in principl
  #6
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
Totally. It should in principle at least. Or maybe is there a stokes solver around in OpenFOAM?
msrinath80 is offline   Reply With Quote

Old   July 24, 2006, 11:25
Default If the Re number is really rea
  #7
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
If the Re number is really really low, just remove the convection term, + fvm::div(phi, U), from icoFoam's Ueqn and recompile. Instant Stokes flow.
jferrari and Nucleophobe like this.
eugene is offline   Reply With Quote

Old   August 2, 2006, 10:32
Default The re number that i want to s
  #8
New Member
 
Bryan Godbolt
Join Date: Mar 2009
Location: London, Ontario, Canada
Posts: 14
Rep Power: 8
soup is on a distinguished road
The re number that i want to simulate is very low. I tried the idea of removing fvm::div(phi, U) from icoFoam and recompiling but I now get this error when I run icoFoam:

--> FOAM FATAL IO ERROR : Unknown symmetric matrix solver BICCG

Valid symmetric matrix solvers are :

4
(
ICCG
GaussSeidel
DCG
AMG
)


file: /home/bryan/OpenFOAM/bryan-1.2/run/tutorials/potentialFoam/lowrecylinder/system/ fvSolution::U at line 28.

From function lduMatrix::solver::New(const fvMesh&, Istream&)
in file matrices/lduMatrix/lduMatrixSolver.C at line 100.

FOAM exiting

I have not changed the fvSolution file and if I put the line back in and recompile if works fine once again.

Does anyone have any ideas as to what may be wrong? I am not very familiar with c++ so I may be missing something obvious that is done by this line.

Are there any other ways of acheiving creeping flow in openFoam?
soup is offline   Reply With Quote

Old   August 2, 2006, 10:37
Default Yes. OpenFOAM knows whether th
  #9
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Yes. OpenFOAM knows whether the matrix you have assembled is symmetric or assymetric. For symmetric matrices it will use symmetric matrix solvers, which are prettier, faster etc. than assymetric solvers.

When your equation contains the convection term, you will have an assymetric matrix, which requires an assymetric solver, e.g. BiCCG. When you remove it, the matrix will be symmetric and you need to use a symmetric solver, for example ICCG - this is exactly what the error message says.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak 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
Reynolds number Fede CFX 4 November 6, 2006 12:51
Reynolds number Joseph FLUENT 0 January 30, 2006 16:40
Reynolds number??? Joseph FLUENT 0 January 30, 2006 16:33
Help with Reynolds number: Re Isa Main CFD Forum 2 December 4, 2003 10:47
Reynolds number Mult Main CFD Forum 1 April 12, 2002 11:02


All times are GMT -4. The time now is 02:19.