
[Sponsors] 
July 10, 2006, 07:58 
I've select rhoSimpleFoam as a

#1 
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 779
Rep Power: 18 
I've select rhoSimpleFoam as a starting point for using openFOAM for standard industrial applications  steadystate, k/eps, moderate compressibility  thus my apologies for posting with presumably banal questions.
Backtracking from my original geometry, I am now using blockMesh to create a very simple test case. I assume that encountered stability problems arise from incorrect configuration, but I am uncertain as to what I should be changing. The test geometry is a simple square duct (50mmx50mm) with a ubend. The inlet is L/D = 1, the bend is R/D = 1, and the outlet is L/D = 10. I've used surfaceNormalFixedValue for the inlet velocity and fixedValue (1.1e5) for the outlet pressure. With U=15m/s, I obtain a physically reasonable result (relaxation parameters 0.3/0.7). At a slightly higher inlet velocity (U=20m/s), the solution seems to diverge rapidly regardless of the relaxation parameters (lowest tried was 0.05/0.3). I really cannot figure out if the difficulty arises from the physics (outlet too close) or from incorrect specification of the BCs and/or schemes. Ideally the inlet would be specified as an integral massflux, which would also alleviate the divergence problem, but I cannot imagine that this is the sole factor here. If anyone has a few minutes to look at the problem and see what is going awry, I would be greatly appreciate it. I could also offer the problem for a potential rhoSimpleFoam tutorial. Thanks, /mark 

July 18, 2006, 08:09 
As a followup to my own post.

#2 
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 779
Rep Power: 18 
As a followup to my own post.
Thanks to Joern Beilke for suggesting initialization with potentialFoam and providing some settings for fvSolution that had worked for him. Initializing with potentialFoam did help for lower (fixedValue) inlet velocities, but problems persist at higher flow rates. Underrelaxing rho (0.1) and p (approx. 0.05) seemed to delay the divergence problem, but not prevent it. With help of "computeMassFlux.H" (found on the forum), the mass flow can be seen to steadily increase. The obvious explanation would be that increases in the density at the inlet result in a correspondingly increased mass flow at the outlet (via adjustPhi). Using my own "integralInlet" boundary condition to force a fixed inlet mass flow, the solver runs reasonably stably for moderate Mach numbers. I am still, however, puzzled about the pressure correction. In the pEqn.h we have the following lines: AU = UEqn().A(); ... pEqn( fvm::laplacian(rho/AU, p) == fvc::div(phi) ); I can't figure out where the density corrections are hidden  cf. Eq. 10.12 Ferziger & Peric. Or am I missing something quite obvious? /mark 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
RhoSimpleFoam  maritozzo  OpenFOAM Running, Solving & CFD  1  April 30, 2010 18:18 
★ HELP! startup problem, help me  Conan  FLUENT  4  October 16, 2009 15:21 
Paraview cannot startup  gnom  OpenFOAM Paraview & paraFoam  6  October 14, 2009 00:30 
Stability problems with kepsilon in external aero  edreed  OpenFOAM Running, Solving & CFD  21  July 16, 2008 15:00 
RhoSimpleFoam  luca  OpenFOAM Running, Solving & CFD  0  August 22, 2005 12:26 