[alundilong]

This might be silly question, but it confused me a lot..
these snippet code comes from buoyantSimpleFoam of OpenFOAM-2.1.1
3 tmp<fvVectorMatrix> UEqn
4 (
5 fvm::div(phi, U)
6 + turbulence->divDevRhoReff(U)
7 );
8
9 UEqn().relax();
10
11 if (simple.momentumPredictor())
12 {
13 solve
14 (
15 UEqn()
16 ==
17 fvc::reconstruct
18 (
19 (
20 - ghf*fvc::snGrad(rho)
21 - fvc::snGrad(p_rgh)
22 )*mesh.magSf()
23 )
24 );
25 }
shouldn't be this?
3 tmp<fvVectorMatrix> UEqn
4 (
5 fvm::div(phi, U)
6 + turbulence->divDevRhoReff(U)
7 );
8
9 UEqn().relax();
10
11 if (simple.momentumPredictor())
12 {
13 solve
14 (
15 UEqn()
16 ==
17 fvc::reconstruct
18 (
19 (
20 - ghf*fvc::snGrad(rho)
21 - fvc::snGrad(p_rgh)
22 )*mesh.magSf()
23 )
24 + rho*g
25 );
25 }

[akidess]

No, the gravity term is hidden in between the usage of p_rgh and ghf*snGrad(rho). There is a thread on the forum with the derivation.

[mturcios777]

For bouyancy driven flows that is why we use p_rgh instead of p. If prgh = p + rho*g*h, then when we do grad p in the NS equations we get grad(p) and rho*g. I don't do a lot of buoyancy driven flow so I'm not 100% on the notation.

[alundilong]

thanks for your reply.
I derived, but may not correctly, so I did not see the term of rho*gravity.
How can I find that thread? some keywords are quite helpful.

[alundilong]

Originally Posted by mturcios777

For bouyancy driven flows that is why we use p_rgh instead of p. If prgh = p + rho*g*h, then when we do grad p in the NS equations we get grad(p) and rho*g. I don't do a lot of buoyancy driven flow so I'm not 100% on the notation.

Thanks! I got the idea. I mistakenly took grad(rho*g*h) = grad(rho)*g*h without caring rho*g*grad(h), which equals to rho*g. Shame on me!

[akidess]

Originally Posted by alundilong

thanks for your reply.
I derived, but may not correctly, so I did not see the term of rho*gravity.
How can I find that thread? some keywords are quite helpful.

I think it was this one:
http://www.cfd-online.com/Forums/ope...tml#post323761

[m.Chrsitiano]

Hello!

I'm new to OpenFOAM, I started using about 1 month ago. And I have created and account here just now. So i didn't know if it was better to create a new topic or just replay an old one since my doubt is related to this topic.

So, I'm working on a simulation with the twoLiquidMixingFoam solver. And just like the UEqn.H posted here before, there is this: * mesh.magSf().
I would like to know what it is, what does it for? What this meaning?

Besides this, I want to learn the mathematical modelling form OpenFOAM, for example, in twoLiquidMixingFoam, what is the equations that the solver use to run? If someone could me introduce to a book or anything that may help me to understand the math from this software I would be very thankful.

Best regards!