CFD Online Discussion Forums - compressibilty effect in alphaEqn.H

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)

- - compressibilty effect in alphaEqn.H (https://www.cfd-online.com/Forums/openfoam/92850-compressibilty-effect-alphaeqn-h.html)

nimasam

September 27, 2011 07:04

compressibilty effect in alphaEqn.H

i have two compressible flow , i would like to track interface between them
i can not use compressibleInterFoam , because the flow is self expanding due to pressure and temperature , and reaction conversion
now my question is related to VOF method for compressible flow

Code:

1-1) ddt (rho1*alpha1)  + div(rho1*alpha1*U1) = 0

1-2)ddt (rho2*alpha2)  + div(rho2*alpha2*U2) = 0



by simplifying  1-1 we have



ddt (alpha1) + div (alpha1*U1) =alpha1(ddt (rho1) + U & grad (rho1) ) /rho1



now we add and subtract div (rho1 U) in the LS of above equation, so



2) ddt (alpha1) + div (alpha1*U1) = alpha1*div(U1);



now we consider 

U = U1*alpha1* + U2*alpha2;

and

Ur = U1 - U2;

so

U1 = U + Ur*alpha2;

we rearange equation 2 to reach equation 3 :



3) ddt (alpha1) + div (alpha1*U)+div(Ur*alpha1*alpha2) = alpha1*div(U1);



the LS of above euqation is what solved with interFoam,

for interFoam which is for incompressible flows div(U1) is zero! 

so alpha1*div(U1) is the effect of compressibility of phase

now i have two ways in my mind

A) div(U1) = - (ddt(rho1) + u & grad (rho1))/rho1

or

B) div(U1) = div (U) + div(Ur*alpha2)

and none of them work wells,

A) the interface is moving but the alpha gets unbounded after several iteration

B) nothing happens, interface is fixed

any hint or idea how to consider compressibilty effect in alphaEqn ?

linch

May 16, 2012 12:05

Hi Nima,

I'm working on the same problem, but I have only thermal expansivity and no compressibility. First I wold like to ask, what is your status? Did you find a proper solution?

Second question, which form of the pressure correction equation do you have?

Generally I see two way to solve the VOF and the pressure correction equation (the similarity is that both of them have to ensure mass conservation): not conservative and conservative form, like I posted here

The conservative form converges poorly and as far as I know becomes unstable for density ratio between both phases.

The non-conservative converges much better, but then there is the question "how to obtain velocity divergence". This is exact the question you asked here.

Mathematically, the RHS of your simplified eqn. 1-1 is equal to:
$\frac{\alpha_1}{\rho_1} \left( \frac{\partial{\rho_1}}{\partial{t}} + \vec{U}_1 \cdot \nabla\rho_1 \right) = \frac{\alpha_1}{\rho_1} \frac{D\rho_1}{Dt}$

so I use

Code:

alpha1Su = alpha1/rho1*fvc::DDt(phi1,rho1)

for this term. It works somehow, but even if the mathematical formula is correct, such numerical implementation causes mass imbalance in the interfacial zone. May be you have an idea, how to implement this term consistently and reduce the mass imbalance?

nimasam

May 16, 2012 13:00

i calculate the source terms like below:

Code:

vDotP1 = fvc::ddt(rho1) + fvc::div(phi,rho1) - rho1*fvc:: div(phi);

vDotP2 = fvc::ddt(rho2) + fvc::div(phi,rho2)- rho2*fvc::div(phi);



vDotAlpha = (pos(alpha2)*(vDotP2/rho2) + pos(alpha1)*(vDotP1/rho1));

but now really i dont remember why i implement like this

linch

May 16, 2012 13:41

And you don't experience any problems with mass balance? I'll try your implementation, thanks a lot.

linch

May 16, 2012 13:49

in your implementation, vDotP1 is equal to fvc::DDt(phi,rho1), and vDotP2 to DDt(phi,rho2) respectively.

The third line looks like velocity divergence for entire flow, and not for a single phase, and this confuses me a little. Is your vDotAlpha an explicit source term for alpha1? Could you please tell me, how your MULES looks like?

nimasam

May 16, 2012 13:58

1 Attachment(s)

i think it was some how poor in continuity specially in cumulative continuity was some how high but golbal and local continuity error was around 1e-05

linch

May 16, 2012 14:17

Thanks again.

In you code I find this even more strage:

Code:

Sp[celli] -= vDotAlpha[celli]*alpha1[celli];

Su[celli] += vDotAlpha[celli]*alpha1[celli];

Though they have the same dimensions, their meaning is different. $Su = \alpha_1 (\nabla \cdot U_1)$ while $Sp = (\nabla \cdot U_1)$
Due to my logic

Code:

Sp[celli] -= vDotAlpha[celli];

Su[celli] += vDotAlpha[celli]*alpha1[celli];

would be the "right" pair. But implementation in compressibleInterFoam looks similar to yours. Hm, I still don't get it.

nimasam

May 16, 2012 15:06

look at here

linch

May 21, 2012 08:38

Hi Nima,

me again here :) Sry, we had a long weekend here in Germany. Back to the topic:

- I read again the thread you linked, but it is still not 100% clear for me, how can Sp and Su have the same form?

- In the compressibleInterFoam our EOS reads rho1 = rho10 + psi1*p, so we can recast DDt(rho1) into psi1*DDt(p). But since you have temperature & pressure dependency of the density, means your EOS reads rho=rho(p,T), you have to modify the pEqn. May I ask how did you do it? Where do you update the density and what is the RHS of your pressure correction eqn.?

- is your vDotAlpha the same as divU ?

Best,
Illya

nimasam

May 22, 2012 01:28

Hi Illya
psi is somehow (1/RT), so after temperature calculation, i update rho,
then i calculate source term in pEqn from rho not p!, so it became an explicit source term for pressure equation

linch

May 22, 2012 04:13

Hi Nima.

Explicit source term in pEqn means div(U), right? Do you have something like

Code:

// update density

// update vDotP1 & vDotP2



divU = alpha1*vDotP1/rho1 + alpha2*vDotP2/rho2;



fvScalarMatrix p_rghEqnIncomp

(

    divU

 + fvc::div(phi)

  - fvm::laplacian(rUAf, p_rgh)

);

linch

May 22, 2012 08:40

I've implemented the pressure correction like above, but the simple loop doesn't converge. Could you take a look and say, what do you think about it?

In expandableInterFoam.C:

Code:

        while (pimple.loop())

        {

            #include "updateSinglePhaseProperties.H" // rho1, rho2 updated here



            Drho1Dt   = fvc::ddt(rho1) + fvc::div(phi,rho1) - fvc::div(phi)*rho1;

            Drho2Dt   = fvc::ddt(rho2) + fvc::div(phi,rho2) - fvc::div(phi)*rho2;

            rho     == alpha1*rho1 + (scalar(1) - alpha1)*rho2;    // update rho-field (changes due to temperature transport)



            divU = (alpha1*Drho1Dt/rho1 + (scalar(1)-alpha1)*Drho2Dt/rho2);

            

            #include "UEqn.H"

            

            // --- Pressure corrector loop

            while (pimple.correct())

            {

                #include "pEqn.H"

            }

            



            #include "alphaEqnSubCycle.H" // rho, alpha1, phiAlpha updated here

            

            #include "updateFluxes.H" // rhoPhi1, rhoPhi, rhoCpPhi updated here

            

            #include "TEqn.H"

        }

        {

        /*************** continuity check ***************************/

            volScalarField rhoAlpha1 = rho1*alpha1;

            rhoAlpha1.oldTime() = rho1.oldTime()*alpha1.oldTime();

            

            volScalarField rhoAlpha2 = rho2*(scalar(1)-alpha1);

            rhoAlpha2.oldTime() = rho2.oldTime()*(scalar(1)-alpha1.oldTime());



            contErr   = fvc::ddt(rho)+fvc::div(rhoPhi);

            contErr1 = fvc::ddt(rhoAlpha1)+fvc::div(rhoPhi1);

        /***********************************************************/

        }

in pEqn.H:

Code:

    while (pimple.correctNonOrthogonal())

    {

        fvScalarMatrix p_rghEqn

        (

            fvm::laplacian(rAUf, p_rgh) 

            == 

            fvc::div(phi) + divU

        );



        p_rghEqn.setReference(pRefCell, getRefCellValue(p_rgh, pRefCell));



        p_rghEqn.solve(mesh.solver(p_rgh.select(pimple.finalInnerIter())));



        if (pimple.finalNonOrthogonalIter())

        {

            phi -= p_rghEqn.flux();

        }

    }

and in alphaEqn.H:

Code:

    for (int aCorr=0; aCorr<nAlphaCorr; aCorr++)

    {

        volScalarField dgdt

        (

            IOobject

            (

                "dgdt",

                runTime.timeName(),

                mesh

            ),

            (pos(scalar(1.0) - alpha1)*(Drho2Dt/rho2) - pos(alpha1)*(Drho1Dt/rho1))

        );

        

        divU = fvc::div(phi);



        alpha1Sp = dimensionedScalar("Sp",dimensionSet(0,0,-1,0,0,0,0),0);

        alpha1Su = divU*alpha1;

        



        forAll(dgdt, celli)

        {

            if (dgdt[celli] > 0.0 && alpha1[celli] > 0.0)

            {

                alpha1Sp[celli] -= dgdt[celli]*alpha1[celli];

                alpha1Su[celli] += dgdt[celli]*alpha1[celli];

            }

            else if (dgdt[celli] < 0.0 && alpha1[celli] < 1.0)

            {

                alpha1Sp[celli] += dgdt[celli]*(1.0 - alpha1[celli]);

            }

        }

        

        

        phiAlpha =

            fvc::flux

            (

                phi,

                alpha1,

                alphaScheme

            )

          + fvc::flux

            (

                -fvc::flux(-phir, scalar(1) - alpha1, alpharScheme),

                alpha1,

                alpharScheme

            );

        MULES::explicitSolve(geometricOneField(), alpha1, phi, phiAlpha, alpha1Sp, alpha1Su, 1, 0);

    }

For Drho1Dt & Drho2Dt I use Gauss linear div-schemes:

Code:

div(phi,rho1)               Gauss linear;

div(phi,rho2)               Gauss linear;

What are significant differences from your implementation? alphaEqn looks similar, Drho1Dt & Drho2Dt also (you called them vDotP1 & vDotP2 respectively). Equation solution order should not matter, if the solution is converged. The only possible difference I see is the pressure correction eqn. and the source term in it.

linch

May 22, 2012 09:03

update: I had a small typo, it converges. But the mass conservation is still poor. I get local error in the order of 1e+02 and not 1e-05

linch

May 24, 2012 07:40

Hi Nima,

is my procedure the same as yours, or do you have different pressure correction eqn.?

Best regards,
Illya

nimasam

May 24, 2012 10:16

hi dear Illya
sorry4 late answer, take a quick look on your code, it seems look a like, ofcourse i implemented it for PISO loop in OpenFOAM-1.6, however i suggest you play with algorithm
i prefer for example in each loop first update alpha1, then i have rhoPhi, then update rho from rhoEqn (rhoPhi), and so on ....
keep the structure of compressibleInterFoam

linch

May 24, 2012 11:18

Hi Nima,

thanks for the reply. On my opinion the order of equations doesn't really matter for me, since I have an outer (SIMPLE) loop over all equations till the solution converges. The reason to solve the alphaEqn after the pressure correction is following: alphaEqn needs volumetric fluxes "phi" coming from the momentum equation, so the fluxes of the alpha1-phase "phiAlpha" are consistent with the volumetric fluxes "phi" in this way.

What really wracks my brain is the mass imbalance. If I understood you write, you additionally solve the rhoEqn to ensure the continuity is satisfied I think this could be the solution of my problem.

I'm sorry to terrorize you with my endless questions :-), but I have a couple of them again:
1) Do you solve the rhoEqn twice, for each phase?
2) Do you solve the rhoEqn after the PISO loop, means at the end of your time step?

A lot of thanks and best regards,
Illya

nimasam

May 24, 2012 14:45

i solved rhoEqn once,
when I solve alphaEqn, rhoPhi is getting update,
then i calculate total rho from rhoPhi from continuity Eqn (look compressibleInterFoam)

linch

May 25, 2012 04:52

Thank you Nima,

apparently I'm to dumb to get it :)

1) solving the continuity eqn. for rho could ensure the overall continuity, but not the continuity of each phase

2) solving rhoEqn in between doesn't ensure the mass balance, because of the density update following in the end of the timestep

3) we also implicitly include conti in alphaEqn and pEqn, but in a non-conservative form, what means only if the source terms in these equations are derived consistently with other equations and their discretization, mass conservation can be achieved

4) I use the same source term as you. Your mass balance is good, my not. Why?

Do you use ideal gas law for the gas phase? Which EOS do you use for the liquid? How high are your temperature caused density variations beneath each phase (in %)? There must be a reasonable reason :)

Best regards,
Illya

nimasam

May 25, 2012 05:18

Quote:

Originally Posted by linch (Post 363052)

1) solving the continuity eqn. for rho could ensure the overall continuity, but not the continuity of each phase

you are right!

Quote:

2) solving rhoEqn in between doesn't ensure the mass balance, because of the density update following in the end of the timestep

why?
in each iteration, update rho total, based on continuity
in end of iteration update rho based on mixture equation ( i guess this help each phase mass conservation)

Quote:

3) we also implicitly include conti in alphaEqn and pEqn, but in a non-conservative form, what means only if the source terms in these equations are derived consistently with other equations and their discretization, mass conservation can be achieved

????

Quote:

4) I use the same source term as you. Your mass balance is good, my not. Why?

i really dont know :D

Quote:

Do you use ideal gas law for the gas phase? Which EOS do you use for the liquid? How high are your temperature caused density variations beneath each phase (in %)? There must be a reasonable reason :)

actually i had two phase one phase was air (perfect gas) and the other one was polyurethane foam which density changes based on temperature, chemical conversion and ...)

linch

May 25, 2012 05:28

3) I mean, the source terms in alphaEqn and pEqn are based on single phase continuity equations.

If you have already published your results, would you mind giving me the whole solver to examine it carefully?

linch

May 25, 2012 08:57

Hi Nima,

Update: I've added 2 rhoEqns, for rho1 and rho2 at the end of my time step. Now I force the continuity of each phase. The drawback is the the EOS is not exactly fulfilled in some interface cells, that caused problems earlier, but I can live with it, since the continuity is more important.

Thanks a lot for the discussion, it helped me a lot. If if you're interested, you can still give me your solver some day, and I could test it with my case. I have a high thermal expansivity of both phases and it may be interesting to know, if your solver still performs well. It must not be now, some day you wish.

Best wishes and a nice weeked!
Illya

kal1943335

February 20, 2018 16:30

Any references on your work?

Hi,
first need to thank both of you for the valuable discussion and I'm really sorry as I'm trying to refer your work 6 years ago. I'm trying to simulate high pressure gas atomization problem and molten metal is atomizing due to the high pressure gas. The gas inlet is a pressure boundary condition and pressure is in the range of 15-30 atm. However, I tried compressibleInterFoam in OF40 and it crashes with negative temperatures. I know it's due to the sudden expansion of the gas. I tried different solver conditions but still getting the same error. I assume it's a result of taking density as a function of pressure only.

I trying to workout the math to obtain the effect of rho(P,T), following the method described in "A pressure based compressible, two phase flow finite volume method for underwater explotions" by Miller et al. I'm still trying to understand the PEqn.H. However, seems like you to have made some progress on this.

Can you please give me some references of your work so that I can follow.

Thank you.
Kalpana

All times are GMT -4. The time now is 08:08.