CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Programming & Development (https://www.cfd-online.com/Forums/openfoam-programming-development/)
-   -   Why we subtract continuity Eqn into momentum Eqn instead of adding it? (https://www.cfd-online.com/Forums/openfoam-programming-development/152230-why-we-subtract-continuity-eqn-into-momentum-eqn-instead-adding.html)

sharonyue April 27, 2015 03:14
Why we subtract continuity Eqn into momentum Eqn instead of adding it?
 
Hey guys,

This piece of code is quite common in OpenFOAM；
Code:
fvm::ddt(alpha1, U1)  //mom eqn
        -fvm::Sp(fvc::ddt(alpha1),U1) //continuity eqn
          + fvm::div(alpha1, U1) //mom eqn
          - fvm::Sp(fvc::div(alpha1), U1) ////continuity eqn
Why dont we add continuity eqn?...like this:..

Code:
fvm::ddt(alpha1, U1)  //mom eqn
        +fvm::Sp(fvc::ddt(alpha1),U1) //continuity eqn
          + fvm::div(alpha1, U1) //mom eqn
          +fvm::Sp(fvc::div(alpha1), U1) ////continuity eqn
continuity is zero right?

kebsiali April 27, 2015 05:38
I dont really know
normally we seek diagnal dominance, so i would say so
but thats the contrary of what is done here ??????

sharonyue April 27, 2015 11:31
Yep...Wish someone who can explain this. lol

Cyp April 27, 2015 12:32
Quote:
Originally Posted by sharonyue (Post 543952)
Yep...Wish someone who can explain this. lol
Hi,


Actually, we subtract a momentum transfer term because the real equation (left hand side of NS) we want to solve is

\rho \frac{\partial \mathsf{U}}{\partial t} + \rho \mathsf{U} . \nabla \mathsf{U} = (...)

which is written in a non-conservative form. In FVM, however, we prefer conservative form,
\frac{\partial \rho \mathsf{U}}{\partial t} + \nabla. \left( \rho \mathsf{U} \mathsf{U} \right)= (...)

These two equations are not the same if the fluid is not incompressible or if there is phase change. You can notice that you can switch from non-conservative to conservative form with,
\rho \frac{\partial \mathsf{U}}{\partial t} + \rho \mathsf{U} . \nabla \mathsf{U} = \frac{\partial \rho \mathsf{U}}{\partial t} + \nabla. \left( \rho \mathsf{U} \mathsf{U} \right) - \left( \frac{\partial \rho }{\partial t} + \nabla. \left( \rho \mathsf{U} \right) \right)\mathsf{U}

So adding the continuity equation do not have any sense.

Cheers,

sharonyue April 28, 2015 02:21
Quote:
Originally Posted by Cyp (Post 543962)
Hi,


Actually, we subtract a momentum transfer term because the real equation (left hand side of NS) we want to solve is

\rho \frac{\partial \mathsf{U}}{\partial t} + \rho \mathsf{U} . \nabla \mathsf{U} = (...)

which is written in a non-conservative form. In FVM, however, we prefer conservative form,
\frac{\partial \rho \mathsf{U}}{\partial t} + \nabla. \left( \rho \mathsf{U} \mathsf{U} \right)= (...)

These two equations are not the same if the fluid is not incompressible or if there is phase change. You can notice that you can switch from non-conservative to conservative form with,
\rho \frac{\partial \mathsf{U}}{\partial t} + \rho \mathsf{U} . \nabla \mathsf{U} = \frac{\partial \rho \mathsf{U}}{\partial t} + \nabla. \left( \rho \mathsf{U} \mathsf{U} \right) - \left( \frac{\partial \rho }{\partial t} + \nabla. \left( \rho \mathsf{U} \right) \right)\mathsf{U}

So adding the continuity equation do not have any sense.

Cheers,
hey Cyprien,

Yeah, The problem is why we want to solve the first Eqn in your posts. The reason why I ask this kind of problem is that: "openfoam22x is solving non-conservative equations but 23x is solving conservative eqns."for two-fluid model.

So I think the thing deeper is :

1. Why we solve Eqn 2 instead of Eqn 1. I saw some posts that Hrv and Henry explain this, They just said the conservative eqn is stable and good. I dont know the reason.

2. Eqn 2 and Eqn 1 should predicts the same results rite? But sometimes it does not.


Best,

Cyp April 28, 2015 11:39
Hi Dongyue,

Eq 1 and Eq 2 are equivalent only if the continuity equation (equal to zero) is satisfy. I guess that since we deal with an operator-splitting scheme (first we solve the momentum, then the pressure, then the correction, then we iterate), the continuity equation is not fully respected, and that why we add to add this term, to avoid spurious momentum transfer due to an ill-evaluation of the continuity.


Cheers,

blais.bruno June 3, 2015 12:00
Quote:
Originally Posted by sharonyue (Post 544024)
hey Cyprien,

Yeah, The problem is why we want to solve the first Eqn in your posts. The reason why I ask this kind of problem is that: "openfoam22x is solving non-conservative equations but 23x is solving conservative eqns."for two-fluid model.

So I think the thing deeper is :

1. Why we solve Eqn 2 instead of Eqn 1. I saw some posts that Hrv and Henry explain this, They just said the conservative eqn is stable and good. I dont know the reason.

2. Eqn 2 and Eqn 1 should predicts the same results rite? But sometimes it does not.


Best,

Equation 1 and 2 are not equivalent numerically because they do not allow for the same Riemann invariant. If you take the example of a shockwave or any other type of discontinuity, as a Cauchy-Riemann classical problem, you find that the wave propagation / shock propagation/ discontinuity propagation will be at the wrong velocity if you do not formulate your problem using the conserved variables.

I am not familiar with these issues in the context of two phases flows, but for compressible flows this is an extremely critical issue and you always need to formulate the problem in conservative variables (rho, rho * u, rho * e). I believe that since these multiphase flows contain large amount of discontinuity in the phases (like air on top of water or whatever), a conservative formulation is a lot more appropriate if you want to obtain the right propagation of the interface.

There is a very very nice book by Euleterio Toro on hyperbolic systems that discusses these issues if I remember.

danny123 June 4, 2015 05:20
Hi,

I am confused with these statements. Sharonyue refers to the alpha1Eq, not the momentum equation. In interDymFoam, I have the following code:

Code:
        fvScalarMatrix alpha1Eqn
        (
            #ifdef LTSSOLVE
            fv::localEulerDdtScheme<scalar>(mesh, rDeltaT.name()).fvmDdt(alpha1)
            #else
            fv::EulerDdtScheme<scalar>(mesh).fvmDdt(alpha1)
            #endif
          + fv::gaussConvectionScheme<scalar>
            (
                mesh,
                phiCN,
                upwind<scalar>(mesh, phiCN)
            ).fvmDiv(phiCN, alpha1)
        );
which is the same, no?

I changed to:

Code:
        fvScalarMatrix alpha1Eqn
        (
            #ifdef LTSSOLVE
            fv::localEulerDdtScheme<scalar>(mesh, rDeltaT.name()).fvmDdt(alpha1)
            #else
            fv::EulerDdtScheme<scalar>(mesh).fvmDdt(alpha1)
            #endif
          + fv::gaussConvectionScheme<scalar>
            (
                mesh,
                phiCN,
                upwind<scalar>(mesh, phiCN)
            ).fvmDiv(phiCN, alpha1)
          - fvc::div(phi)*fvm::Sp(1,alpha1)
        );
It does not make a whole lot of difference in my case, but the idea is that there are large areas, where alpha1 does not change (only around the interface). In those domains I want interFoam to behave like a single phase solver, so any incosistency in mass conservation should not affect alpha1Eq (d alpha1/dt is 0 if there is no alpha change in space). If alpha1 is constant, the last 2 terms become equivalent. Because div(phi) has to be 0, the ultimate result should be identical. You basically eliminate solving alpha1Eq, where it is not needed (the equation system is overdetermined).

By the way, for compressible solvers, this code is wrong (div phi is not zero, but div rho phi.

Regards,

Daniel


All times are GMT -4. The time now is 14:00.