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

Post processing to tecplot

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

Like Tree1Likes
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Display Modes
Old   August 8, 2012, 17:54
Default Post processing to tecplot
  #1
New Member
 
Join Date: Jul 2012
Posts: 14
Rep Power: 5
danielec87 is on a distinguished road
Hi guys,
I am trying to post process my openFoam simulation, by using the istruction

-->foamToTecplot360

The problem is that I encounter the following error message:

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

Valid patchField types are :

52
(
advective
buoyantPressure
calculated
codedFixedValue
codedMixed
cyclic
cyclicAMI
cyclicSlip
directionMixed
empty
fan
fanPressure
fixedFluxPressure
fixedGradient
fixedInternalValue
fixedPressureCompressibleDensity
fixedValue
freestream
freestreamPressure
inletOutlet
inletOutletTotalTemperature
mapped
mappedField
mappedFixedInternalValue
mappedFixedPushedInternalValue
mixed
multiphaseFixedFluxPressure
nonuniformTransformCyclic
oscillatingFixedValue
outletInlet
outletMappedUniformInlet
partialSlip
phaseHydrostaticPressure
processor
processorCyclic
rotatingTotalPressure
sliced
slip
symmetryPlane
syringePressure
timeVaryingMappedFixedValue
totalPressure
totalTemperature
turbulentInlet
turbulentIntensityKineticEnergyInlet
uniformDensityHydrostaticPressure
uniformFixedValue
uniformTotalPressure
waveSurfacePressure
waveTransmissive
wedge
zeroGradient
)


file: /home1/dcappell/OpenFOAM/-2.1.1/run/tutorials/incompressible/simpleFoam/Hump_model_k_epsilon/0/nut::boundaryField::lowerWall from line 41 to line 42.

From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&)
in file /u/dcappell/OpenFOAM/OpenFOAM-2.1.1/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 135.

FOAM exiting
---------------------------------------------------------------------------------------------------------------------------
It seems that Tecplot is not compatible with turbulent wall functions...

Do you know how to fix this problem ?

Thank you very much !
danielec87 is offline   Reply With Quote

Old   August 9, 2012, 02:08
Default
  #2
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
The newest Tecplot versions have a native reader for OpenFOAM data, so there is no need for conversion with this tool.
Bernhard is offline   Reply With Quote

Old   August 9, 2012, 20:06
Default
  #3
New Member
 
Join Date: Jul 2012
Posts: 14
Rep Power: 5
danielec87 is on a distinguished road
Thank you for your answer, Bernard,
Could you be more specific, please ?

Which folder / file should I upload ?
danielec87 is offline   Reply With Quote

Old   August 9, 2012, 20:48
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,488
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!

@daniele: I don't know how exactly you've built your OpenFOAM build, but I've tested with OpenFOAM 2.1.1 a case that used said boundary condition and I had no problems. Nonetheless:
  • For using foamToTecplot360, try adding to the case's "system/controlDict" this line:
    Code:
    libs ("libincompressibleRASModels.so");
    This should forcefully load the missing BC.
  • As for using the latest Tecplot, probably you only have to open the folder of the case in Tecplot.
    The initial news about this is here: Tecplot 360 2011 R2 preview with OpenFOAM data loader available for evaluation
Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   August 10, 2012, 01:24
Default
  #5
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
As for using the latest Tecplot, probably you only have to open the folder of the case in Tecplot.
The initial news about this is here: Tecplot 360 2011 R2 preview with OpenFOAM data loader available for evaluation
It is enough to open the system/controlDict. Only be aware that you can open binary data, but not a binary stored mesh (you can use foamFormatConvert -constant -time :0 -noZero to convert this)
Bernhard is offline   Reply With Quote

Old   August 10, 2012, 13:16
Default
  #6
New Member
 
Join Date: Jul 2012
Posts: 14
Rep Power: 5
danielec87 is on a distinguished road
@ Bruno : your command -libs(...) - does not work. I have the following error:

"ill defined primitiveEntry"

@Bernhard: In controlDict you do not have any information about your solution...
danielec87 is offline   Reply With Quote

Old   August 10, 2012, 13:17
Default
  #7
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
Quote:
Originally Posted by danielec87 View Post
@Bernhard: In controlDict you do not have any information about your solution...
No, but like the .foam file for Paraview, Tepclot will find it from there.
Bernhard is offline   Reply With Quote

Old   August 10, 2012, 13:19
Default
  #8
New Member
 
Join Date: Jul 2012
Posts: 14
Rep Power: 5
danielec87 is on a distinguished road
Anyway, could you tell me how to plot the pressure coefficient over a curve wall (for instance an airfoil) in Paraview?
In this case I would avoid to use tecplot !
danielec87 is offline   Reply With Quote

Old   August 10, 2012, 13:29
Default
  #9
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,488
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
@daniele: Just in case I wasn't very clear, here is an example of a "system/controlDict":
Code:
/*--------------------------------*- 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      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     simpleFoam;

startFrom       latestTime;

startTime       0;

stopAt          endTime;

endTime         1000;

deltaT          1;

writeControl    timeStep;

writeInterval   50;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;

libs ("libincompressibleRASModels.so");
Notice there is a space between "libs" and "(".
danielec87 likes this.
wyldckat is offline   Reply With Quote

Old   August 10, 2012, 16:11
Default
  #10
New Member
 
Join Date: Jul 2012
Posts: 14
Rep Power: 5
danielec87 is on a distinguished road
Thank you...it works perfectly now !
danielec87 is offline   Reply With Quote

Reply

Tags
post processing tecplot

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
Ansys Post processing ano999 ANSYS 1 May 27, 2011 16:24
NO model vs post processing in coal combustion,CFX sakalido CFX 1 April 15, 2011 14:07
post processing for KIVA dirga Main CFD Forum 5 April 23, 2009 10:58
Tecplot for CFX post processing pantangi goud CFX 2 August 24, 2005 16:42
Post Processing in FEM Abhijit Tilak Main CFD Forum 0 April 26, 2004 11:59


All times are GMT -4. The time now is 16:09.