
[Sponsors] 
April 28, 2005, 15:33 
Hello
In compressible liqu

#1 
Member
Join Date: Mar 2009
Posts: 43
Rep Power: 10 
Sponsored Links
In compressible liquid/gas flows, the pEqn reads : ( fvm::ddt(psi,p)+fvc::div(phi)+fvm::div(phid,p,".." )fvm::laplacian(..,p) ) where as in an incompressible code pEqn is given as, ( fvm::laplacian(1/A, p)==fvc::div(phi) ) I tried to look into pressure correction methodologies for compressible flows, but was not able to figure out the reason of this implementation procedure (why the need for pressre time derivative) . Can someone help me out with this ? Thanks Vatant 

Sponsored Links 
April 28, 2005, 15:39 
> why the need for pressre tim

#2 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
> why the need for pressre time derivative
Because in compressible flow there is a rate of change of density and hence pressure, or vice versa depending on how you look at it. 

April 28, 2005, 15:40 
Is the implementation same as

#3 
Member
Join Date: Mar 2009
Posts: 43
Rep Power: 10 
Is the implementation same as artificial compressibility method ?


April 28, 2005, 15:43 
Certainly not, it's real compr

#4 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
Certainly not, it's real compressibility, there is nothing artificial about the compressibility in the compressible codes in OpenFOAM.


April 28, 2005, 15:51 
does the term 'dp/dt' vanish a

#5 
Member
Join Date: Mar 2009
Posts: 43
Rep Power: 10 
does the term 'dp/dt' vanish after reaching certain tolerance level ? what is this method for solving compressible flow called?


April 28, 2005, 15:56 
For steadystate flows all tim

#6 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
For steadystate flows all time derivatives will vanish but not for transient flows. If you are solving steadystate flows you might be better of using one of the steadystate solvers.


April 28, 2005, 16:10 
I am solving transient flows a

#7 
Member
Join Date: Mar 2009
Posts: 43
Rep Power: 10 
I am solving transient flows and was wondering if rho and p relations are not explicity given (unlike ideal gas relation), how does this pressure correction method works?
Is the pressure correction equation derived from combination of continuity and momentum equation ? If i want to search in literature about this method, could you tell me whats this compressible solver schemes called? Vatant 

April 28, 2005, 16:17 
> Is the pressure correction e

#8 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
> Is the pressure correction equation derived from combination of continuity and momentum equation ?
Yes in the same manner as for incompressible PISO. I guess it would be called compressible PISO but I am not sure I didn't implement it from a paper I derived it from first principles and implemented it. However I am sure other people have implemented the same and named and published it. 

April 28, 2005, 16:25 
I've got an old report on this

#9 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,802
Rep Power: 24 
I've got an old report on this which contains the derivation of the pressure equation for compressible flow  send me an Email if you want it.
Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

April 28, 2005, 16:38 
For the analysis of compressib

#10 
Member
Join Date: Mar 2009
Posts: 43
Rep Power: 10 
For the analysis of compressible flows, it is possible that some regions of the flow domain
such as in the boundary layers have low speeds and thus are incompressible. This low velocities result in numerical disorders..due to eigenvalue mismatch.. So, if we have an first principle formulation, would we require any kind of preconditioning for handling low speed regions? or by any means numerical stability is inherently guaranteed... Vatant 

April 28, 2005, 16:46 
Eliptic pressure equation base

#11 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
Eliptic pressure equation based compressible flow solvers do not suffer from problems handling low speed regions like density based solvers which is why we choose them. We are able to solve subsonic, transonic and supersonic flows with or without boundary layers without difficulty.


April 28, 2005, 17:08 
why is that the convergence pr

#12 
Member
Join Date: Mar 2009
Posts: 43
Rep Power: 10 
why is that the convergence problem be easily handled with elliptic systems ?
The derived pEqn from continuity and momentum eqn was of the form d/dt(p) + laplacian(..,p)+div(phi)...=0 , is it a completely elliptic version (with the time derivative terms) ? Vatant 

April 28, 2005, 17:13 
> why is that the convergence

#13 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
> why is that the convergence problem be easily handled with elliptic systems ?
This is well known and explained in books on the subject. The pressure equation may take several forms depending on how the compressibility effects are handled. At least it is a Poisson's equation but it may also include a "convection" term as in sonicFoam. 

April 28, 2005, 17:25 
Incompressible flows would rep

#14 
Member
Join Date: Mar 2009
Posts: 43
Rep Power: 10 
Incompressible flows would represent elliptic, solving laplacian (p) == div (phi)..
In the sonicFoam, the pEqn has the extra time derivative term with compressiblity effect, ddt(psi,p)+ div (phid,p,..)laplacian(rho/A,p)=0 could the equation still be called a poisson ? Since, the time derivative appears (with compressiblity), im not sure how this works. Vatant 

April 28, 2005, 17:35 
> could the equation still be

#15 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
> could the equation still be called a poisson ?
No it isn't a Poisson's equation with the implicit "convection" term but it might be called one if that part is explicit as it is in our new compressible flow solver, it depends on your definition of Poisson's equation. I guess with an explicit "convection" term but implicit compressibility term it would be a linear combination of a Poisson's equation and a Helmholtz equation; I am not sure if that kind of equation has a special name. 

April 28, 2005, 18:03 
I am still running openFoam 1.

#16 
Member
Join Date: Mar 2009
Posts: 43
Rep Power: 10 
I am still running openFoam 1.0 which has implicit convection solves..you think i might have any problem in convergence since convection is not done explicit taking it away from elliptic ?
Does a combination of poisson's and helmholtz equation in behavior result close to poisson ? Since that the flow needs show elliptic behavior for better convergence. Vatant 

April 28, 2005, 18:31 
There are no convergence probl

#17 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
There are no convergence problems with the compressible codes in OpenFOAM, the equations are what they are, the pressure equation is implemented implicitly and it doesn't matter what the name of this type of equation is, it is what it is.


April 28, 2005, 18:44 
I actually ran lot of cases wi

#18 
Member
Join Date: Mar 2009
Posts: 43
Rep Power: 10 
I actually ran lot of cases with OpenFoam compressible codes with different flow velocities and the convergence was good . I did experience some problems in injector flows with sharp corners...
Hence I was interested in the numerical essence of the implementation. With good convergence available with OpenFoam, I shall study some acoustics due to compressiblity effects at high speed flows with low speed regions in the domain. Vatant 

June 8, 2005, 14:23 
Hi Guys
I would like an opi

#19 
Member
Wladimyr Mattos da Costa Dourado
Join Date: Mar 2009
Location: Sao Jose dos Campos, SP, Brazil
Posts: 36
Rep Power: 10 
Hi Guys
I would like an opinion about the following subject. We would like to implement a pseudocompressibility solver or some kind of preconditioned method based solver in the OpenFoam. In my knowledge, the non segregated methods is one of the best way to do that. Is possible to implement some nonsegragated method in the openfoam? How hard work is necessary to do it? In other words, what is necessary to implement a nonsegragated method in openfoam? Are the solvers implemented in openfoam able to solve the matrix generated in a nonsegragated method? About wikiopenfoam: Which is better to use for these type of discussions: this site or wiki site? Is wiki site as up to dated such much this site? Many Tanks in advance! Wladimyr 

June 8, 2005, 14:37 
The subject of segregated vs p

#20 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 15 
The subject of segregated vs pointcoupled vs blockcoupled compressible solvers has already been discussed on this site, you might find it useful to search for and read those threads.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Yplus in compressible solvers  dinonettis  OpenFOAM PostProcessing  7  October 6, 2011 05:51 
Incompressible vs compressible solvers  James  Main CFD Forum  5  January 19, 2009 06:15 
NSincompressible and compressible flow solvers  ag  Main CFD Forum  2  September 27, 2005 06:18 
External Flowcompressible flow solverlift/drag  Tom Brown  Main CFD Forum  7  December 29, 2000 14:41 
MHD flow solvers  Manu  Main CFD Forum  2  October 31, 2000 03:11 
Sponsored Links 