
[Sponsors] 
June 30, 2005, 22:06 
I am very new to openFoam (jus

#1 
New Member
Paul Lees
Join Date: Mar 2009
Posts: 4
Rep Power: 10 
I am very new to openFoam (just installed it) but before I dive into it I would like to know if it can do what I would like to do. Can you simulate a fan via the use of rotating reference where all non moving parts are bodies of revolution about the fan?
Is it also possible to use multiple stationary and rotating reference frames? Thanks in Advance. 

July 1, 2005, 05:13 
No, there is no presupplied s

#2 
Super Moderator
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 18 
No, there is no presupplied solver that can do what you want.
(however OpenFOAM was created to implement these kinds of problems easily and efficiently so you might want to try implementing it yourself) 

July 1, 2005, 05:51 
Any code can easily be changed

#3 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
Any code can easily be changed to operate in a rotating reference frame, e.g. for simpleFoam the momentum equation would be:
UEqn ( fvm::div(phi, U)  fvm::Sp(fvc::div(phi), U) + turbulence>divR(U) + (2*Omega ^ U) // Coriolis force + Fcent ); where e.g. dimensionedVector Omega ( "Omega", dimensionSet(0, 0, 1, 0, 0), vector(0, 0, 2*M_PI*1200/60) ); // Calculate the centrifugal force volVectorField Fcent = (Omega ^ (Omega ^ mesh.C())); MRF is a lot more tricky and I will implement it as soon as it is important enough for someone to be prepared to sponsor the work. 

July 1, 2005, 11:23 
Thanks for the info, I am not

#4 
New Member
Paul Lees
Join Date: Mar 2009
Posts: 4
Rep Power: 10 
Thanks for the info, I am not really at the level to start writing any code but I will be sure to watch and see what becomes avaiable. This type of method is vital for the design of many fluid handling devices so I hope it gets implemented soon.


July 1, 2005, 11:40 
That all depends on someone pa

#5 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
That all depends on someone paying for the work. I have been approached several times to implement MRF but so far no one has been willing to pay for my time to do it.


July 1, 2005, 12:17 
Even the SRF is very widely us

#6 
New Member
Paul Lees
Join Date: Mar 2009
Posts: 4
Rep Power: 10 
Even the SRF is very widely used though and would be an nice addition. Lets hope you can find someone in a position to put up the money.


July 1, 2005, 12:35 
SRF is trivial and can be impl

#7 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
SRF is trivial and can be implemented in any solver by anyone using OpenFoam simply by including the source terms I posted above into the momentum equation. I don't think there is any need to us to include this as a standard feature in all solvers as the number of users needing it is not large enough to warrant the overhead and it can be added by them so easily.


July 1, 2005, 12:57 
Well maybe when I am feeling a

#8 
New Member
Paul Lees
Join Date: Mar 2009
Posts: 4
Rep Power: 10 
Well maybe when I am feeling adventerous I will give it a go.


December 22, 2005, 10:40 
HI Henry,
I am implementing

#9 
Member
olivier Petit
Join Date: Mar 2009
Location: Göteborg, Sweden
Posts: 67
Rep Power: 10 
HI Henry,
I am implementing MRF method. the velocity at cell P (in absolute frame) is related to the velocities at its neighboring cells. So In order to convert the velocity in cell N ( which is the neighbor of P, P is adjacent to the interface and N is in the rotating frame). I use a volVectorField F=Diag()*omega ^ mesh.C(), after that if cellI is not in the interface F[cellI]=0. my questions is: 1what you think about this Idea? 2when I add this term in the momentum equation as: U = rUA*(UEqn.H()F) or by add it like source term. I had the non realistic physical results. what you think about that ? If you have some suggestions, I'm very interested to know them. thank you 

May 22, 2009, 17:58 

#10 
New Member
Sam Lee
Join Date: Mar 2009
Location: Shanghai, P.R.China
Posts: 4
Rep Power: 10 
Hi, Henry and foamers:
I am trying to use openfoam to simulate wind field in hurricane. one question would be how the coriolis force of earth is added in openfoam. by looking your message in this thread, it seems what I need to do is only finding out the omega vector of earth's rotation. however, I am trying to understand why you add a term fvm::Sp(fvc::div(phi), U) in U equation. does this have something to do with the coriolis force and Fcent you added in U equation? thanks 

January 22, 2011, 18:12 
answer is now in openfoamwiki

#11 
New Member
Brian Fiedler
Join Date: Jul 2009
Location: Norman, Oklahoma USA
Posts: 5
Rep Power: 10 
This is new, and may have the information that you need:
http://openfoamwiki.net/index.php/Ho...Make_a_Tornado 

January 11, 2012, 06:58 
tangential force calculation

#12  
Member
Stefano
Join Date: Jul 2009
Posts: 34
Rep Power: 10 
Hi guys! I have only one question about what is written below. How would you calculate the tangential force if the rotation "Omega" is not constant? Thank you Quote:


April 20, 2012, 07:28 

#13 
Member
Kim Yusik
Join Date: Dec 2009
Posts: 39
Rep Power: 9 
Does anyone can tell me why either multile or single reference frame (MRF, SRF) are not implemented in the transient solver? such as pisoFoam or pimlpeFoam?. is there any practical or physical reason? Please do shed some lights on my ignorance.
Yusik 

April 29, 2013, 05:18 

#14 
New Member
afluent
Join Date: Apr 2013
Posts: 6
Rep Power: 6 
Hello
i want to simulate a T channel in single rotating reference frame. i studied user guide and tutorial . according to them i should choose 2D option in solver ( DefineSolver2D) not axisymmetric or axisymmetric swirl . but when i just choose 2D after that in defining boundary condition for fluid when i choose moving reference frame, it doesn't ask for rotational speed? i would be grateful if anyone could help me. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Rotating reference frame  David Banks  FLUENT  0  August 13, 2007 06:52 
Rotating Reference frame  Ketan  FLUENT  0  May 25, 2007 11:58 
Rotating Reference Frame for a Fan  carlo_fabrizi  OpenFOAM Running, Solving & CFD  0  June 1, 2006 14:02 
Rotating reference frame  hsieh  OpenFOAM Running, Solving & CFD  2  April 5, 2006 15:05 
rotating reference frame  Jason  FLUENT  0  January 18, 2005 14:00 