|February 1, 2011, 04:00||
Navier-Stokes Equation and icoFoam
Join Date: Feb 2011
Posts: 5Rep Power: 6
I was wondering if anyone could help me answer a question related to the implementation of the icoFoam solver. According to the code presented here, the momentum equation as stated in the icoFoam solver is:
fvm::ddt(U) + fvm::div(phi, U) - fvm::laplacian(nu, U) == -fvc::grad(p).
I do not get where the term "fvm::div(phi,U)" is coming from, as the classic incompressible laminar equations typically have this term as "U.div(U)". How is the flux, phi, defined for this solver?
Also, I looked at Dr. Jasak's explanation beginning in section 3.8 of his Ph.D. thesis, and there he writes "div(UU)". How is that related to the normal definition of "U.div(U)". Is one of the U's an implied scalar?
Many thanks to all who help! I am just an undergrad, so much of this is beyond my knowledge and current understanding.
|February 1, 2011, 05:02||
Join Date: Feb 2010
Location: Stanford University
Posts: 230Rep Power: 9
phi is the projection of the velocity field on the face of your cells. It is defined as :
surfaceScalarField phi = linearInterpolation(U) & mesh.Sf()
|February 2, 2011, 04:14||
Join Date: Mar 2009
Location: Besigheim, Germany
Posts: 134Rep Power: 8
in case you need a non-code reference you can find it in Hrvoje Jasak's thesis as well. The equation is on page 80 no (3.17)
|February 2, 2011, 21:24||
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 418Rep Power: 15
dU/dt + U&grad(U) = -grad(p)+nu*laplacian(U)
Where & implies dot product.
Written in this form this equation is vectorial but has tensorial terms behind it, the term grad(U) is a gradient of a vector, a tensor. Then U&grad(U) is done, which is a vector again. To do things easier we can decompose this equation in three scalar components:
du/dt + U*grad(u) = -dp/dx+nu*laplacian(u)
dv/dt + U*grad(v) = -dp/dy+nu*laplacian(v)
dw/dt + U*grad(w) = -dp/dz+nu*laplacian(w)
div(U tensorial U)
which can be transformed in
U & grad(U)
The form used in icoFoam resembles the first one, but in order to avoid the non-linearity arose from (U tensorial U) data from a previous time-step is used to assemble. Following equation in Hrv thesis p. 144, line 2, you have F=phi=U^0&S_f, and U_f=U_f^n. You are using U data from time-step 0 (past) and n (actual).
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Research Center for Computational Mechanics (CIMEC) - CONICET/FICH-UNL
T.E.: 54-342-4511594 Ext. 1005
Güemes 3450 - (3000) Santa Fe
Santa Fe - Argentina
|Thread||Thread Starter||Forum||Replies||Last Post|
|interFoam vs icoFoam on a single-phase case||nuovodna||OpenFOAM Running, Solving & CFD||1||May 1, 2014 09:37|
|OpenFOAM wonbt solve the momentum U equation||sek||OpenFOAM Running, Solving & CFD||5||March 6, 2008 17:27|
|Equation discretisation in icoFoam||kar||OpenFOAM Running, Solving & CFD||3||February 10, 2008 07:34|
|Pressure Correction Equation||morteza||OpenFOAM Running, Solving & CFD||2||September 4, 2007 06:16|
|IcoFOAM and Navier Stokes||juanduque||OpenFOAM Running, Solving & CFD||0||May 8, 2007 10:43|