# Compressible Flow Solvers

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

 April 28, 2005, 15:33 Hello In compressible liqu #1 Member   Join Date: Mar 2009 Posts: 43 Rep Power: 10 Sponsored Links Hello 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

 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 steady-state flows all tim #6 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 15 For steady-state flows all time derivatives will vanish but not for transient flows. If you are solving steady-state flows you might be better of using one of the steady-state 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 E-mail 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 pseudo-compressibility 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 non-segragated method in the openfoam? How hard work is necessary to do it? In other words, what is necessary to implement a non-segragated method in openfoam? Are the solvers implemented in openfoam able to solve the matrix generated in a non-segragated method? About wiki-openfoam: 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 point-coupled vs block-coupled 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 Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post dinonettis OpenFOAM Post-Processing 7 October 6, 2011 05:51 James Main CFD Forum 5 January 19, 2009 06:15 ag Main CFD Forum 2 September 27, 2005 06:18 Tom Brown Main CFD Forum 7 December 29, 2000 14:41 Manu Main CFD Forum 2 October 31, 2000 03:11