Hello In compressible liqu
 

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

> why the need for pressre tim
 

> 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.

Is the implementation same as
 

Is the implementation same as artificial compressibility method ?

Certainly not, it's real compr
 

Certainly not, it's real compressibility, there is nothing artificial about the compressibility in the compressible codes in OpenFOAM.

does the term 'dp/dt' vanish a
 

does the term 'dp/dt' vanish after reaching certain tolerance level ? what is this method for solving compressible flow called?

For steady-state flows all tim
 

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.

I am solving transient flows a
 

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

> Is the pressure correction e
 

> 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.

I've got an old report on this
 

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

For the analysis of compressib
 

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

Eliptic pressure equation base
 

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.

why is that the convergence pr
 

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

> why is that the convergence
 

> 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.

Incompressible flows would rep
 

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

> could the equation still be
 

> 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.

I am still running openFoam 1.
 

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

There are no convergence probl
 

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.

I actually ran lot of cases wi
 

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

Hi Guys I would like an opi
 

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

The subject of segregated vs p
 

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.