# Navier-Stokes Equation and icoFoam

 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 1, 2011, 04:00 Navier-Stokes Equation and icoFoam #1 New Member   Nick Mai Join Date: Feb 2011 Posts: 5 Rep Power: 7 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 #2 Senior Member   Cyprien Join Date: Feb 2010 Location: Stanford University Posts: 251 Rep Power: 10 Hi nickmai! phi is the projection of the velocity field on the face of your cells. It is defined as : Code: `surfaceScalarField phi = linearInterpolation(U) & mesh.Sf()` It has the dimension of m^3/s (velocity * surface). It is created in createField.H either with the previous snippet or by calling: Code: `#include "createPhi.H"` Best regards, Cyp

 February 2, 2011, 04:14 #3 Senior Member   Kathrin Kissling Join Date: Mar 2009 Location: Besigheim, Germany Posts: 134 Rep Power: 9 Hey, 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) Best Kathrin Woj3x likes this.

February 2, 2011, 21:24
#4
Senior Member

Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 430
Rep Power: 16
Quote:
 Originally Posted by nickmai123 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?

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:

where U=(u,v,w)

Quote:
 Originally Posted by nickmai123 I 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?.
Second term of equations or convective acceleration is really

div(U tensorial U)

which can be transformed in

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).

Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Research Scientist
Research Center for Computational Methods (CIMEC) - CONICET/UNL
Tel: 54-342-4511594 Int. 7032
Colectora Ruta Nac. 168 / Paraje El Pozo
(3000) Santa Fe - Argentina.
http://www.cimec.org.ar

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post nuovodna OpenFOAM Running, Solving & CFD 1 May 1, 2014 09:37 sek OpenFOAM Running, Solving & CFD 5 March 6, 2008 17:27 kar OpenFOAM Running, Solving & CFD 3 February 10, 2008 07:34 morteza OpenFOAM Running, Solving & CFD 2 September 4, 2007 06:16 juanduque OpenFOAM Running, Solving & CFD 0 May 8, 2007 10:43

All times are GMT -4. The time now is 11:42.