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

singularity?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 21, 2012, 20:25
Default singularity?
  #1
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 190
Blog Entries: 1
Rep Power: 8
mihaipruna is on a distinguished road
I am trying to model a simple pipe with total pressure at inlet and fixed 0 pressure at outlet. Tried various things, last one being a filleting of the edges.
Please see images. Flat face facing you is inlet,curved faces are wall and there is symmetry on the Z=0 plane.
I pasted the BCs,o refer to this post:
internal flow BCs: pressure driven versus velocity driven
I am attaching screenshots. I already tried smaller relaxation factors. still got huge values.


FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object nut;
}
dimensions [0 2 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
rightZmax
{
type freestream;
freestreamValue uniform 0;
}
leftZmin
{
type symmetryPlane;
}
inletXmin
{
type freestream;
freestreamValue uniform 0;
}
outletXmax
{
type calculated;
value uniform 0;
}
topYmax
{
type freestream;
freestreamValue uniform 0;
}
bottomYmin
{
type freestream;
freestreamValue uniform 0;
}
Sductface1
{
type nutkWallFunction;
value uniform 0;
}
Sductface2
{
type nutkWallFunction;
value uniform 0;
}
SDuctInlet
{
type calculated;
value uniform 0;
}
SDuctOutlet
{
type calculated;
value uniform 0;
}
Sductface5
{
type nutkWallFunction;
value uniform 0;
}
Sductface6
{
type nutkWallFunction;
value uniform 0;
}
Sductface7
{
type nutkWallFunction;
value uniform 0;
}
Sductface8
{
type nutkWallFunction;
value uniform 0;
}
}






FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object k;
}
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0.240000;
boundaryField
{
outletXmax
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
inletXmin
{
type freestream;
freestreamValue uniform 0.240000;
}
bottomYmin
{
type freestream;
freestreamValue uniform 0.240000;
}
topYmax
{
type freestream;
freestreamValue uniform 0.240000;
}
leftZmin
{
type symmetryPlane;
}
rightZmax
{
type freestream;
freestreamValue uniform 0.240000;
}
Sductface1
{
type kqRWallFunction;
value $internalField;
}
Sductface2
{
type kqRWallFunction;
value $internalField;
}
SDuctInlet
{
type fixedValue;
value uniform 0.240000;
}
SDuctOutlet
{
type zeroGradient;
}
Sductface5
{
type kqRWallFunction;
value $internalField;
}
Sductface6
{
type kqRWallFunction;
value $internalField;
}
Sductface7
{
type kqRWallFunction;
value $internalField;
}
Sductface8
{
type kqRWallFunction;
value $internalField;
}
}





FoamFile
{
version 2.0;
format ascii;
class volVectorField;
location "0";
object U;
}
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0.000000 0.000000 0.000000);
boundaryField
{
inletXmin
{
type freestream;
freestreamValue uniform (0.000000 0.000000 0.000000);
}
outletXmax
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
bottomYmin
{
type freestream;
freestreamValue uniform (0.000000 0.000000 0.000000);
}
topYmax
{
type freestream;
freestreamValue uniform (0.000000 0.000000 0.000000);
}
rightZmax
{
type freestream;
freestreamValue uniform (0.000000 0.000000 0.000000);
}
leftZmin
{
type symmetryPlane;
}
Sductface1
{
type fixedValue;
value uniform (0 0 0);
}
Sductface2
{
type fixedValue;
value uniform (0 0 0);
}
SDuctInlet
{
type zeroGradient;
}
SDuctOutlet
{
type zeroGradient;
}
Sductface5
{
type fixedValue;
value uniform (0 0 0);
}
Sductface6
{
type fixedValue;
value uniform (0 0 0);
}
Sductface7
{
type fixedValue;
value uniform (0 0 0);
}
Sductface8
{
type fixedValue;
value uniform (0 0 0);
}
}


FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object omega;
}
dimensions [0 0 -1 0 0 0 0];
internalField uniform 1.780000;
boundaryField
{
inletXmin
{
type freestream;
freestreamValue uniform 1.780000;
}
outletXmax
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
bottomYmin
{
type freestream;
freestreamValue uniform 1.780000;
}
topYmax
{
type freestream;
freestreamValue uniform 1.780000;
}
leftZmin
{
type symmetryPlane;
}
rightZmax
{
type freestream;
freestreamValue uniform 1.780000;
}
Sductface1
{
type omegaWallFunction;
value $internalField;
}
Sductface2
{
type omegaWallFunction;
value $internalField;
}
SDuctInlet
{
type fixedValue;
value uniform 1.780000;
}
SDuctOutlet
{
type zeroGradient;
}
Sductface5
{
type omegaWallFunction;
value $internalField;
}
Sductface6
{
type omegaWallFunction;
value $internalField;
}
Sductface7
{
type omegaWallFunction;
value $internalField;
}
Sductface8
{
type omegaWallFunction;
value $internalField;
}
}




FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0.000000;
boundaryField
{
inletXmin
{
type freestreamPressure;
freestreamValue 0.000000;
}
outletXmax
{
type fixedValue;
value $internalField;
}
bottomYmin
{
type freestreamPressure;
freestreamValue 0.000000;
}
topYmax
{
type freestreamPressure;
freestreamValue 0.000000;
}
leftZmin
{
type symmetryPlane;
}
rightZmax
{
type freestreamPressure;
freestreamValue 0.000000;
}
Sductface1
{
type zeroGradient;
}
Sductface2
{
type zeroGradient;
}
SDuctInlet
{
type totalPressure;
gamma 1.4;
p0 uniform 100000.000000;
}
SDuctOutlet
{
type fixedValue;
value uniform 0.000000;
}
Sductface5
{
type zeroGradient;
}
Sductface6
{
type zeroGradient;
}
Sductface7
{
type zeroGradient;
}
Sductface8
{
type zeroGradient;
}
}



FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
solvers
{
p
{
solver GAMG;
tolerance 1e-7;
relTol 0.1;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration on;
agglomerator faceAreaPair;
nCellsInCoarsestLevel 10;
mergeLevels 1;
}
U
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}
k
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}
omega
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}
}
SIMPLE
{
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
residualControl
{
p 1e-5;
U 1e-5;
k 1e-5;
omega 1e-5;
}
}
potentialFlow
{
nNonOrthogonalCorrectors 10;
pRefCell 0;
pRefValue 0;
}
relaxationFactors
{
p 0.3;
U 0.7;
k 0.7;
omega 0.7;
}
cache
{
grad(U);
}
Attached Images
File Type: png sductissue.png (37.0 KB, 23 views)
File Type: png sductissuedgese.png (46.9 KB, 21 views)
__________________
Mihai Pruna's Bio
mihaipruna is offline   Reply With Quote

Old   April 22, 2012, 02:34
Default
  #2
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
At a first sight, there could be something wrong in a group of cells (the red area). What discretization schemes are you using? If you have problematic cells, turn limiters on to see if the situation improves.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats.
OpenQBMM - An open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   April 23, 2012, 14:17
Default
  #3
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 190
Blog Entries: 1
Rep Power: 8
mihaipruna is on a distinguished road
well, this is what i have in my fv schemes, copied from the motorbike tutorial.
will this work for internal flows as well? My solution seems to blow up only when I try to specify inlet pressure.

FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}
ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
default none;
div(phi,U) Gauss linearUpwindV grad(U);
div(phi,k) Gauss upwind;
div(phi,omega) Gauss upwind;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
fluxRequired
{
default no;
p;
}
__________________
Mihai Pruna's Bio
mihaipruna is offline   Reply With Quote

Old   April 23, 2012, 15:49
Default
  #4
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
Yes, but it might help to put a limiter on the gradients too:

Code:
gradSchemes
{
     default         cellLimited Gauss linear 1;
}
Also, check your mesh to see if there are very skewed cells (checkMesh will tell you).
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats.
OpenQBMM - An open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   April 23, 2012, 16:36
Default
  #5
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 190
Blog Entries: 1
Rep Power: 8
mihaipruna is on a distinguished road
Thanks for the suggestions. checkmesh returned all clear.
hmm, my numbers are too big too....been focused on the numerics didn't bother to check Bernoulli. 100000 deltap/rho gives supersonic velocity...and I was using simpleFoam....gonna try with 10000 instead.
__________________
Mihai Pruna's Bio
mihaipruna is offline   Reply With Quote

Old   April 24, 2012, 17:18
Default
  #6
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 190
Blog Entries: 1
Rep Power: 8
mihaipruna is on a distinguished road
thanks Alberto, the cell limiter helped prevent the values from attaining huge values.
However, I discovered another issue with my patches, which I fixed and I am hoping the simulation will run properly without limiters.
__________________
Mihai Pruna's Bio
mihaipruna is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
IcoFoam parallel woes msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58
solution singularity litonx OpenFOAM Running, Solving & CFD 1 February 21, 2007 02:32
Problems with sonicTurbFoam tangd OpenFOAM Running, Solving & CFD 0 May 29, 2006 09:07
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07
Volume Meshing & Face Meshing? singularity of grid ken FLUENT 0 September 4, 2003 11:08


All times are GMT -4. The time now is 09:57.