CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

rhoSimplecFoam

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 8, 2015, 11:13
Question rhoSimplecFoam
  #1
Member
 
ufocfd
Join Date: Jun 2012
Posts: 53
Rep Power: 9
ufocfd is on a distinguished road
Hi guys, I'm trying to use rhoSimplecFoam from the OpenFOAM v2.1.x distribution (therein lies the problem).

It keeps crashing after a few iterations, with what seems to be a density spike, causing the epsilon equation to crash. When I view the solution from just before the crash, I see a high density cell just upstream of the aircraft. I'm imposing limits on the density (0.5min and 2.0max) within the fvSolution file.

Has anyone actually got rhoSimplecFoam (or rhoSimpleFoam for that matter) to work??? My testcase is an aircraft at 100m/sec and I'm using freestream boundaries. rhoSimpleFoam does not even get past the 1st iteration.

I think its likely something to do with the fvSchemes and fvSolution file settings... any help much appreciated. Thanks.
ufocfd is offline   Reply With Quote

Old   August 8, 2015, 13:04
Default
  #2
Member
 
ufocfd
Join Date: Jun 2012
Posts: 53
Rep Power: 9
ufocfd is on a distinguished road
...and it seems to have something to do with the location specified in pRefPoint:
pRefPoint (-15 35 35);
pRefValue 100000;
ufocfd is offline   Reply With Quote

Old   August 9, 2015, 14:34
Default
  #3
Member
 
ufocfd
Join Date: Jun 2012
Posts: 53
Rep Power: 9
ufocfd is on a distinguished road
Finally got rhoSimpleFoam working for an aircraft at 100m/sec.
Having consistent boundary conditions, and turbulence values,
seems to be the key factors, and not using pRefPoint also.
Got a nice convergence plot from rhoSimpleFoam below.
ufocfd is offline   Reply With Quote

Old   November 5, 2018, 06:24
Default
  #4
New Member
 
Join Date: Dec 2017
Posts: 2
Rep Power: 0
vale94 is on a distinguished road
Quote:
Originally Posted by ufocfd View Post
Finally got rhoSimpleFoam working for an aircraft at 100m/sec.
Having consistent boundary conditions, and turbulence values,
seems to be the key factors, and not using pRefPoint also.
Got a nice convergence plot from rhoSimpleFoam below.
Hi ufoCFD,
I know quite a lot time has passed, but do you still have the fvschemes and fvsolution to post? I'd like to know how you obtained such a beautiful convergence! Thank you
vale94 is offline   Reply With Quote

Old   November 5, 2018, 09:55
Default
  #5
Member
 
ufocfd
Join Date: Jun 2012
Posts: 53
Rep Power: 9
ufocfd is on a distinguished road
I will have a look for them...
ufocfd is offline   Reply With Quote

Old   November 5, 2018, 10:43
Default
  #6
Member
 
ufocfd
Join Date: Jun 2012
Posts: 53
Rep Power: 9
ufocfd is on a distinguished road
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
}

divSchemes
{
default none;

div(phi,U) Gauss upwind;
div((muEff*dev2(T(grad(U))))) Gauss linear;
div(phi,h) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,k) Gauss upwind;

div(phid,p) Gauss upwind;
div(phi,K) Gauss upwind;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
UD upwind phid;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
pCorr;
}

// ************************************************** *********************** //
ufocfd is offline   Reply With Quote

Old   November 5, 2018, 10:44
Default
  #7
Member
 
ufocfd
Join Date: Jun 2012
Posts: 53
Rep Power: 9
ufocfd is on a distinguished road
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
p
{
solver GAMG;
tolerance 1e-08;
relTol 0.1;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nFinestSweeps 2;
cacheAgglomeration true;
nCellsInCoarsestLevel 20;
agglomerator faceAreaPair;
mergeLevels 1;
}

"(U|h|k|epsilon)"
{
solver GAMG;
tolerance 1e-08;
relTol 0.1;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nFinestSweeps 2;
cacheAgglomeration true;
nCellsInCoarsestLevel 20;
agglomerator faceAreaPair;
mergeLevels 1;
}
}

SIMPLE
{
nNonOrthogonalCorrectors 0;
rhoMin rhoMin [1 -3 0 0 0] 0.5;
rhoMax rhoMax [1 -3 0 0 0] 2.0;
transonic no;
}

relaxationFactors
{
fields
{
p 0.3;
rho 0.1;
}
equations
{
// pEqn 0.3;
U 0.5;
h 0.5;
k 0.5;
epsilon 0.5;
}
}

// ************************************************** *********************** //
ufocfd is offline   Reply With Quote

Old   November 5, 2018, 10:47
Default
  #8
Member
 
ufocfd
Join Date: Jun 2012
Posts: 53
Rep Power: 9
ufocfd is on a distinguished road
Those (supplied) are the fvSchemes and fvSolution for the rhoSimple solver.
I have also done same for rhoSimplec solver if you need them.
Contact me on garcfd (at) gmail (dot) com if you need any help.
ufocfd is offline   Reply With Quote

Old   November 5, 2018, 16:13
Default
  #9
New Member
 
Join Date: Dec 2017
Posts: 2
Rep Power: 0
vale94 is on a distinguished road
Thank you very much!
vale94 is offline   Reply With Quote

Reply

Tags
openfoam2.1.x, rhosimplecfoam, rhosimplefoam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
rhoSimplecFoam with setFields sino75 OpenFOAM Pre-Processing 0 March 11, 2015 05:08
Big problem predicting adiabatic wall temperature (wing, mach 0.33, rhoSimplecFoam) fredo490 OpenFOAM Running, Solving & CFD 6 May 22, 2013 01:28
using GAMG in rhoSimplecFoam tutorial. why? Farshad_Noravesh OpenFOAM 0 November 21, 2012 02:38
rhoSimpleFoam versus rhoSimplecFoam jeff.freeman OpenFOAM Running, Solving & CFD 1 September 18, 2012 10:23
rhoSimplecFoam U-turn j-blindi OpenFOAM Running, Solving & CFD 6 October 29, 2011 18:21


All times are GMT -4. The time now is 21:57.