
[Sponsors] 
Two fundamental questions about icoFoam while updating the velocities and pressure 

LinkBack  Thread Tools  Search this Thread  Display Modes 
May 27, 2007, 01:02 
(1) In typical CFD literature,

#1 
Member
roy fokker
Join Date: Mar 2009
Posts: 44
Rep Power: 15 
(1) In typical CFD literature, after the pressure correction equation is solved, the velocity is updated by adding the initial tentative velocity U* solved from the UEqn == fvc::grad(p*), here p* is the initial pressure and the velocity correction U' from the pressure correction rUA*fvc::grad(p'),i.e. U=U*+U'(a)
However from icoFoam code, it seems that the velocity is updated using: U = rUA*UEqn.H()rUA*fvc::grad(p')(b) the difference between (a) and (b) is rUA*grad(p*), which is the gradient of initial pressure gradient, is there any reference for this difference? (2) I didn't find the code for updating the pressure field which, in typical CFD literature, is p=p*+p', it seems that icoFoam is using the pressure correction value as the pressure value: p=p'? I wonder if I have made my question clear, am I misunderstanding some basic concepts? Thanks a lot! 

May 27, 2007, 04:00 
This is pretty basic stuff  h

#2 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,881
Rep Power: 31 
This is pretty basic stuff  have a look at my Thesis:
 we solve for the pressure and not pressure correction  the derivation of the pressure laplacian is given in detail in the Thesis. Enjoy, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

May 27, 2007, 04:43 
Thanks, actually I already rea

#3 
Member
roy fokker
Join Date: Mar 2009
Posts: 44
Rep Power: 15 
Thanks, actually I already read your thesis section 3.8.1, and I know that the pressure laplacian correction is from Eqn 3.141, because I read the wiki page:
http://openfoamwiki.net/index.php/IcoFoam it says: ... // take a Jacobi pass and update U. See Hrv Jasak's thesis eqn. 3.137 and Henrik Rusche's thesis, eqn. 2.43 // UEqn.H is the righthand side of the UEqn minus the product of (the offdiagonal terms and U). // See Eqn. 7.37 of Ferziger and Peric. U = rUA*UEqn.H(); Ferziger's 7.37,7.39 is a pressure correction p' Do you mean that your equation 3.137, 3.141 is the pressure p and not p'? And therefore the PISO loop is different (or slightly different) from the procedure by Ferziger? I know this is quite fundamental, thanks for your reply. 

May 31, 2007, 09:40 
Roy,
You are right that the

#4 
Member
David P. Schmidt
Join Date: Mar 2009
Posts: 71
Rep Power: 15 
Roy,
You are right that the icoFoam implementation differs slightly from Feriger and Peric. The reference to Eqn. 7.37 in the Wiki comments is also misleading (mea culpa). So the pressure Equation is Eqn. 7.35 from Ferziger and Peric; e.g. it is for the whole pressure, not just the correction to the estimated pressure field. If this explanation makes sense, and you think you could improve the Wiki text, feel free to correct it. David 

May 31, 2007, 15:58 
Thanks, in fact I plan to make

#5 
Member
roy fokker
Join Date: Mar 2009
Posts: 44
Rep Power: 15 
Thanks, in fact I plan to make a step by step explanation of the icoFoam with PISO, the wiki page seems too simple an explanation for beginners. So far I still have some problem about one line:
adjustPhi(phi, U, p); 

May 31, 2007, 16:41 
Consider a case which has zero

#6 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,881
Rep Power: 31 
Consider a case which has zero gradient boundary condition on the pressure all the way around, like a pipe wit zero gradient outlet. In such a case, the pressure equation will not guarantee global continuity.
At the same time, if the mass flux in is not identical to mass flux out, the pressure equation (= continuity condition) will not have a solution. adjustPhi will look for cases where p has got no fixed boundary condition and adjust total outflow from the domain after the momentum predictor to match the total inflow. Standard practice, slightly unusual packing :) Enjoy, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

April 12, 2016, 16:05 
Another very basic question

#7 
New Member
Join Date: Nov 2010
Posts: 10
Rep Power: 13 
Hey FOAMers
I've been wondering for a while why the simple algorithm is implemented in that way. What are the advantages or disadvantages of both formulations? Is it about avoiding to implement Rhie & Chow??? Are there side effects or is it simply simpler () to do it the Jasak way??? Thanks a lot in advance!!! 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
velocities and pressure  Palani Velladurai  Main CFD Forum  2  March 16, 2007 10:22 
A fundamental problem about the UcorrectBoundaryConditions in icoFoam  dbxmcf  OpenFOAM Running, Solving & CFD  0  February 26, 2007 22:16 
A fundamental problem about Pressure equation of the potentialFoam solver  dbxmcf  OpenFOAM Running, Solving & CFD  0  October 6, 2006 11:32 
2 Fundamental CFD Questions regarding convergence  Jon  Main CFD Forum  0  September 24, 2005 20:47 
fundamental questions  Jim Kim  Main CFD Forum  1  March 25, 2005 10:30 