CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

swak4Foam - funkySetFields - not recognizing turbulent wall BC

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 6, 2011, 13:17
Default swak4Foam - funkySetFields - not recognizing turbulent wall BC
  #1
Member
 
Goncalo Pedro
Join Date: Nov 2009
Location: Victoria, British Columbia
Posts: 30
Rep Power: 9
gonpe is on a distinguished road
Hi All

Trying to run a funkySetFields (FSF) on the epsilon variable on one of the tutorials. The FSF utility is not finding the turbulent wall bc (in this case for epsilon). Any thoughts. Below is the output.

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 1.7.x-b32f406e2652
Exec   : funkySetFields -keepPatches -field epsilon -time 0 -expression 0.134799/(dist()+0.010000)
Date   : Jan 06 2011
Time   : 12:10:41
Host   : ubu1
PID    : 27303
Case   : pitzDaily
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Time = 0
 Using command-line options

 Putting "0.134799/(dist()+0.010000)" into field epsilon at t = "0" if condition "true" is true
 Keeping patches unaltered



--> FOAM FATAL IO ERROR:
Unknown patchField type epsilonWallFunction for patch type wall

Valid patchField types are :

42
(
advective
buoyantPressure
calculated
cyclic
directMapped
directionMixed
empty
fan
fixedFluxPressure
fixedGradient
fixedInternalValue
fixedPressureCompressibleDensity
fixedValue
freestream
freestreamPressure
inletOutlet
inletOutletTotalTemperature
mixed
oscillatingFixedValue
outletInlet
outletMappedUniformInlet
partialSlip
processor
rotatingTotalPressure
sliced
slip
symmetryPlane
syringePressure
timeVaryingMappedFixedValue
timeVaryingMappedTotalPressure
timeVaryingTotalPressure
timeVaryingUniformFixedValue
timeVaryingUniformInletOutlet
totalPressure
totalTemperature
turbulentInlet
turbulentIntensityKineticEnergyInlet
uniformDensityHydrostaticPressure
uniformFixedValue
waveTransmissive
wedge
zeroGradient
)


file: /projects/ubu1/09-40322-Makkah/ExternalFlow/Runs/pitzDaily/0/epsilon::boundaryField::upperWall from line 35 to line 36.

    From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&)
    in file /software/OpenFOAM/OpenFOAM-1.7.x/src/finiteVolume/lnInclude/newFvPatchField.C at line 110.

FOAM exiting
gonpe is offline   Reply With Quote

Old   January 10, 2011, 06:16
Default
  #2
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,971
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by gonpe View Post
Hi All

Trying to run a funkySetFields (FSF) on the epsilon variable on one of the tutorials. The FSF utility is not finding the turbulent wall bc (in this case for epsilon). Any thoughts. Below is the output.
That boundary condition is either located in libcompressibleRASModels.so or libincompressibleRASModels.so (depending on what kind of case this is) and FSF doesn't link these. The solution is to force the loading of that library. You do that by adding

libs ( "libcompressibleRASModels.so" );

to the system/controlDict (add an "in" in the right place if your case is incompressible).

If this works for you, then it would be nice if you added a remark to the regular FSF-Wiki-page so that future generations will profit from that knowledge

Bernhard
gschaider is offline   Reply With Quote

Old   January 10, 2011, 11:30
Default
  #3
Member
 
Goncalo Pedro
Join Date: Nov 2009
Location: Victoria, British Columbia
Posts: 30
Rep Power: 9
gonpe is on a distinguished road
That worked ... thanks for your help.

I will post to the Wiki.

Goncalo
gonpe is offline   Reply With Quote

Reply

Tags
swak4foam error

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
Look for applications to simulate a rough wall channel flow with turbulent model xiuying OpenFOAM Running, Solving & CFD 0 September 25, 2007 22:21
help with wall functions Nick Georgiadis Main CFD Forum 4 February 20, 2000 18:07
Wall function in adverse pressure gradients stephane baralon Main CFD Forum 11 September 2, 1999 04:05
CFD2000 and wall function for turbulent flows. jens Main CFD Forum 0 April 12, 1999 08:09
Wall functions Abhijit Tilak Main CFD Forum 6 February 5, 1999 02:16


All times are GMT -4. The time now is 03:49.