
[Sponsors] 
December 17, 2007, 11:39 
Hello,
When running turbFoa

#1 
Member
nicolas
Join Date: Mar 2009
Location: Glasgow
Posts: 42
Rep Power: 8 
Hello,
When running turbFoam, I get output from the DILUPBiCG solver: "DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 7.53093e07, No Iterations 4". But when running interFoam, i dont get any output from the momentum equations; the code looks similar. What governs the type of output? Thanks Nico 

December 17, 2007, 12:15 
Hi Nico,
i suppose you are

#2 
Member
Christian Winkler
Join Date: Mar 2009
Location: Mannheim, Germany
Posts: 63
Rep Power: 8 
Hi Nico,
i suppose you are running the dambreak testcase, where the momentum predictor in the fvSolution file is switched off. So only the pressure equation is solved. The correct velocity results from the pressurevelocity correction. You can change that in the PISO section: PISO { momentumPredictor yes; ... } regards Christian 

December 18, 2007, 08:50 
perfect, thank you very much

#3 
Member
nicolas
Join Date: Mar 2009
Location: Glasgow
Posts: 42
Rep Power: 8 
perfect, thank you very much


September 2, 2009, 00:01 

#4 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 420
Rep Power: 15 
Thanks to Caw for the answer, i was about to post the same question. I have some related questions:
1. What is the purpose of the momentum predictor? 2. Where I can find some theory about it? 3. With your clue we are able to see what are the residuals for the momentum equation, but, What parameters we have to change to set up the residuals limits in order to force the solver to go with the residuals below a given value (as is usual in commercial CFD codes)? Thanks in advance.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Postdoctoral Fellow Research Center for Computational Mechanics (CIMEC)  CONICET/FICHUNL T.E.: 543424511594 Ext. 1005 Güemes 3450  (3000) Santa Fe Santa Fe  Argentina http://www.cimec.org.ar 

September 2, 2009, 00:26 

#5  
Senior Member
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 9 
Quote:


September 2, 2009, 21:48 

#6 
Senior Member
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 9 
If the momentum predictor is switched off, the velocity fields will be gotten explicitly from the pressure equation, I guess, it is easier to implement parallel computation because only a pressure equation is solved. However, I think, if the momentum predictor is switched on, maybe we can get more efficiently during an unparellel simulation??


September 2, 2009, 23:16 

#7  
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12 
It's all about SIMPLE/PISO algorithm.
Quote:
Quote:
__________________
~ Daniel WEI  NatHaz Modeling Laboratory Department of Civil & Environmental Engineering & Earth Sciences University of Notre Dame, USA Email  My Personal CFD Blog 

September 7, 2009, 12:31 

#8 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 420
Rep Power: 15 
Thanks Daniel for your answers, it's a pleasure for me to interact with somebody in China (actually mi first time I guess). About answers 1 & 2 I'll read these thesis, I promise. And respect answer 3, you're right, I found the info in the pdf manuals. Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Postdoctoral Fellow Research Center for Computational Mechanics (CIMEC)  CONICET/FICHUNL T.E.: 543424511594 Ext. 1005 Güemes 3450  (3000) Santa Fe Santa Fe  Argentina http://www.cimec.org.ar 

September 23, 2009, 09:01 

#9 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 420
Rep Power: 15 
Daniel, I've been reading some thesis, specially the one from Jasak, it's awesone, none more clear about FVM and errors. Now I'm dealing with the interpretation of some lines of icoFoam solver, particularly with A and H operators. If we recall the annotated version from OpenFOAM Wiki:
Code:
//set up the linear algebra for the momentum equation. The flux // of U, phi, is treated explicity using the last known value of U. fvVectorMatrix UEqn ( fvm::ddt(U) + fvm::div(phi, U)  fvm::laplacian(nu, U) ); Code:
// solve using the last known value of p on the RHS. This gives us // a velocity field that is not divergence free, but approximately satisfies // momentum. See Eqn. 7.31 of Ferziger & Peric solve(UEqn == fvc::grad(p)); Code:
//  PISO loop take nCorr corrector steps for (int corr=0; corr<nCorr; corr++) { // from the last solution of velocity, extract the diag. term from the // matrix and store the reciprocal note that the matrix coefficients are // functions of U due to the nonlinearity of convection. volScalarField rUA = 1.0/UEqn.A(); Code:
// 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). Note that // since the pressure gradient is not included in the UEqn. above, this // gives us U without the pressure gradient. Also note that UEqn.H() is // a function of U. U = rUA*UEqn.H(); Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Postdoctoral Fellow Research Center for Computational Mechanics (CIMEC)  CONICET/FICHUNL T.E.: 543424511594 Ext. 1005 Güemes 3450  (3000) Santa Fe Santa Fe  Argentina http://www.cimec.org.ar 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Changing BC from Opening to Wall during Solving  Ahmad M. Kermani  CFX  0  December 17, 2008 22:20 
Solving the momentum equation  msg30  OpenFOAM Running, Solving & CFD  2  January 11, 2008 08:24 
Solving an additional equation  rene  OpenFOAM Running, Solving & CFD  2  May 12, 2005 03:36 
Implicit equation solving  Dr B.M. Smith (Smith)  OpenFOAM Running, Solving & CFD  2  December 10, 2004 06:36 
Differential equation solving  cfduser  Main CFD Forum  1  November 12, 2003 03:42 