# Take derivative of mean velocity in paraFoam

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

 January 30, 2014, 02:28 Take derivative of mean velocity in paraFoam #1 Member   Huynh Phong Thanh Join Date: Aug 2013 Location: Ho Chi Minh City Posts: 54 Rep Power: 4 I run LES simulation with pisoFoam and it's finish. And now, I would like to calculate derivative of mean velocity in parafoam also paraview. it means umean. I computed umean by fieldAverage in OpenFOAM and now I want to compute derivative above. Anyone can help me how to get it in parafoam? Thanks your help.

 January 30, 2014, 04:30 #2 Senior Member   Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 13 Why not using the FOAM framework for this with utilities foamCalc and foamCalcEx?

January 30, 2014, 05:04
#3
Member

Huynh Phong Thanh
Join Date: Aug 2013
Location: Ho Chi Minh City
Posts: 54
Rep Power: 4
Quote:
 Originally Posted by Bernhard Why not using the FOAM framework for this with utilities foamCalc and foamCalcEx?
Hi Bernhard,

I see in command foamCalc has div function.But is the laplacian, which is div(grad(umean)).
and about first derivative of umean?

I use OpenFOAm 2.1.1, I don't see foamCalcEx as you said. Could you show me clearly?

Thank you,
Thanh

 January 30, 2014, 05:43 #4 Member   Huynh Phong Thanh Join Date: Aug 2013 Location: Ho Chi Minh City Posts: 54 Rep Power: 4 Hi Bernhard, I saw your code extended of foamCalcEx on google. Thank you so much your code. Best regards, Thanh.

 January 30, 2014, 12:07 #5 Member   Huynh Phong Thanh Join Date: Aug 2013 Location: Ho Chi Minh City Posts: 54 Rep Power: 4 When I used command foamCalc or foamCalcEx to calculate div(U) and grad(U) but I meet error. Can anyone check help me? Code: Selecting calcType div /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.1.1-221db2718bbb Exec : foamCalc div U Date : Jan 30 2014 Time : 23:03:37 Host : "compeng" PID : 7276 Case : /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Time = 0 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.01 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.02 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.03 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.04 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.05 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.06 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.07 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.08 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.09 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.1 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.10001 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.11 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.12 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. Time = 0.13 Reading U Calculating divU --> FOAM Warning : --> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes" file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. End

 February 1, 2014, 09:48 #6 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 9,523 Blog Entries: 36 Rep Power: 97 Greetings to all! To answer the original question: there is a filter named "Compute Derivatives", but it doesn't seem to be able to calculate the laplacian. edit: In the Python Calculator, it does seem possible to use the "laplacian" function: http://www.paraview.org/Wiki/ParaVie...hon_Calculator As for the latest post: the "div(U)" entry is missing from the file "system/fvSchemes". You can find several examples for such an entry by running this command: Code: find $FOAM_TUTORIALS -name "fvSchemes" | xargs grep "div(U)" If you have a look into the file "compressible/rhoPimpleFoam/ras/cavity/system/fvSchemes" on the tutorials folder, you'll see this block of code: Code: divSchemes { default none; div(phi,U) Gauss limitedLinearV 1; div(phid,p) Gauss limitedLinear 1; div(phi,K) Gauss linear; div(phi,h) Gauss limitedLinear 1; div(phi,k) Gauss limitedLinear 1; div(phi,epsilon) Gauss limitedLinear 1; div(phi,R) Gauss limitedLinear 1; div(phi,omega) Gauss limitedLinear 1; div((rho*R)) Gauss linear; div(R) Gauss linear; div(U) Gauss linear; div((muEff*dev2(T(grad(U))))) Gauss linear; } If you look carefully, you'll see the line that starts with "div(U)". You need to add that line to the file "system/fvSchemes" in your case, inside the same block "divSchemes". Best regards, Bruno __________________ OpenFOAM: FAQ | Getting started Forum: How to get help and to post code/output What am I doing/planning: blog/wiki Read this before sending me PM ___ I'll be at OFW11 in Portugal Last edited by wyldckat; February 1, 2014 at 17:55. Reason: see "edit:"  February 2, 2014, 12:42 #7 Member Huynh Phong Thanh Join Date: Aug 2013 Location: Ho Chi Minh City Posts: 54 Rep Power: 4 Hi Bruno, I thank you so much about this guide, I can calculate div(U) but grad(U) can not compute. In fvscheme has defined grad(U): 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; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default backward; } d2dt2Schemes { } gradSchemes { default Gauss linear; grad(nuTilda) cellLimited Gauss linear 1; grad(U) cellLimited Gauss linear 1; } divSchemes { default none; div(phi,U) Gauss LUST unlimitedGrad(U); //div(phi,U) Gauss linearUpwind unlimitedGrad(U); //div(phi,k) Gauss limitedLinear 1; //div(phi,k) Gauss upwind; div(phi,k) Gauss SFCD; div(phi,nuTilda) Gauss limitedLinear 1; div(U) Gauss linear; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear limited 0.33; } interpolationSchemes { default linear; } snGradSchemes { default limited 0.33; } fluxRequired { default no; p; } // ************************************************************************* // And this is error. Code: Selecting calcType grad /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.1.1-221db2718bbb Exec : foamCalcEx grad U Date : Feb 02 2014 Time : 23:33:44 Host : "compeng" PID : 2674 Case : /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Time = 0 --> FOAM FATAL ERROR: Unable to process U No call to grad for fields of type volVectorField I really want to calculate and . I only have computed div(UMean) up to now. Could you show me my error?  February 2, 2014, 14:22 #8 Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 9,523 Blog Entries: 36 Rep Power: 97 Hi Huynh, foamCalcEx is missing the ability to handle "grad(U)" and "div(gradU)". I've finished doing a bug report and respective patch for this here: http://code.google.com/p/foamcalcex/issues/detail?id=2 Download the patch file "changes.patch" from that bug report and place the file inside the folder "foamCalcEx". Then run: Code: patch -p1 < changes.patch ./Allwmake Now go into your case folder and run: Code: foamCalcEx grad U foamCalcEx div gradU It will likely complain about the missing "div(gradU)", but I think you now know what to do WARNING: I have not checked if the results given are correct. I simply did what seemed logical in the source code... and the results seemed sane enough. Best regards, Bruno __________________ OpenFOAM: FAQ | Getting started Forum: How to get help and to post code/output What am I doing/planning: blog/wiki Read this before sending me PM ___ I'll be at OFW11 in Portugal Last edited by wyldckat; February 3, 2014 at 06:12. Reason: "I simply did you seemed logical" -> "I simply did what seemed logical"  February 3, 2014, 02:03 #9 Member Huynh Phong Thanh Join Date: Aug 2013 Location: Ho Chi Minh City Posts: 54 Rep Power: 4 Hi Bruno, It worked very good. I thank you so much. Best regards, Thanh. February 3, 2014, 04:54 #10 Senior Member Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 13 Quote:  Originally Posted by wyldckat WARNING: I have not checked if the results given are correct. I simply did you seemed logical in the source code... and the results seemed sane enough. That's why we didn't include it in the utility up till now, following the Gschaider-philosophy to implement what you need. Anton is working on including your patch. Thanh, can you let us know your experience with using this patch? February 3, 2014, 05:54 #11 Member Huynh Phong Thanh Join Date: Aug 2013 Location: Ho Chi Minh City Posts: 54 Rep Power: 4 Quote:  Originally Posted by Bernhard Thanh, can you let us know your experience with using this patch? Actually I am proving the variance of pressure equation: I have average of all these terms above by edit pisoFoam. I only prove left hand side equal to the right hand side of equation by using paraFoam, but gradient and laplacian of mean velocity does not have. So I must calculate it and using parafoam insert equation above. About the patch of Bruno, I only did following the guide of him. I added command div(U) and div(grad(U)) in fvscheme. Best regards, Thanh.  February 3, 2014, 06:04 #12 Senior Member Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 13 foamCalcEx was mainly designed for quick and dirty calculation of single operations. If you want to do whole expressions like this, I would recommend funkyDoCalc. wyldckat likes this. February 4, 2014, 06:46 #13 Member Huynh Phong Thanh Join Date: Aug 2013 Location: Ho Chi Minh City Posts: 54 Rep Power: 4 Quote:  Originally Posted by Bernhard foamCalcEx was mainly designed for quick and dirty calculation of single operations. If you want to do whole expressions like this, I would recommend funkyDoCalc. Thanks Bermhard. I will try funkyDoCalc.  April 26, 2016, 06:44 "grad(phi) undefined" error #14 New Member Join Date: Jul 2015 Posts: 4 Rep Power: 2 Hi guys! [EDIT]: Pffff my bad, lack of reading the error message properly.. It was referring to the multiRegion fvScheme file (in system/FluidRegion1), not the original file (system/fvScheme) which I had not defined at all yet. So, problem solved! I am quite new to OpenFOAM (so I hope this is a piece of cake for you guys ) and Im modifying the electrostaticsFoam into a multiRegion solver, but Im running into a similar problem as reported. Im trying to calculate the electric field (just as they do in the original electrostaticsFoam) during createField initialization. Compiling goes well, but when I run a case I get the following error: Code: $ electrostaticMultiRegionFoam /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 3.0.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 3.0.1-119cac7e8750 Exec : electrostaticMultiRegionFoam Date : Apr 26 2016 Time : 12:29:04 Host : "floris-SATELLITE-L850-184" PID : 5875 Case : /home/floris/OpenFOAM/floris-3.0.1/run/dischargeCase/electrostaticFoam/02_opposingConductorsMultiRegion nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create fluid mesh for region Fluid1 for time = 0 Create solid mesh for region Solid1 for time = 0 Reading physicalProperties *** Reading fluid mesh thermophysical properties for region Fluid1 Adding to rho Adding to phi Calculating field magE --> FOAM FATAL IO ERROR: keyword grad(phi) is undefined in dictionary "/home/floris/OpenFOAM/floris-3.0.1/run/dischargeCase/electrostaticFoam/02_opposingConductorsMultiRegion/system/Fluid1/fvSchemes.gradSchemes" file: /home/floris/OpenFOAM/floris-3.0.1/run/dischargeCase/electrostaticFoam/02_opposingConductorsMultiRegion/system/Fluid1/fvSchemes.gradSchemes From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 442. FOAM exiting I am calculating the electric field magnitude magE in "createField.H" accordingly: Code: // Initialise fluid field pointer lists PtrList rhoFluid(fluidRegions.size()); PtrList phiFluid(fluidRegions.size()); PtrList rhoFluxFluid(fluidRegions.size()); PtrList magEFluid(fluidRegions.size()); PtrList EFluid(fluidRegions.size()); PtrList kFluid(fluidRegions.size()); PtrList epsilon0Fluid(fluidRegions.size()); // Populate fluid field pointer lists forAll(fluidRegions, i) { Info<< "Reading physicalProperties\n" << endl; IOdictionary physicalProperties ( IOobject ( "physicalProperties", runTime.constant(), fluidRegions[i], IOobject::MUST_READ_IF_MODIFIED, IOobject::NO_WRITE ) ); dimensionedScalar epsilon0 ( physicalProperties.lookup("epsilon0") ); dimensionedScalar k ( physicalProperties.lookup("k") ); Info<< "*** Reading fluid mesh thermophysical properties for region " << fluidRegions[i].name() << nl << endl; Info<< " Adding to rho\n" << endl; rhoFluid.set ( i, new volScalarField ( IOobject ( "rho", runTime.timeName(), fluidRegions[i], IOobject::MUST_READ, IOobject::AUTO_WRITE ), fluidRegions[i] ) ); Info<< " Adding to phi\n" << endl; phiFluid.set ( i, new volScalarField ( IOobject ( "phi", runTime.timeName(), fluidRegions[i], IOobject::MUST_READ, IOobject::AUTO_WRITE ), fluidRegions[i] ) ); Info<< " Calculating field magE\n" << endl; magEFluid.set ( i, new volScalarField ( IOobject ( "magE", runTime.timeName(), fluidRegions[i], IOobject::NO_READ, IOobject::AUTO_WRITE ), mag(fvc::grad(phiFluid[i])) ) ); Info<< " Calculating field E\n" << endl; EFluid.set ( i, new volVectorField ( IOobject ( "E", runTime.timeName(), fluidRegions[i], IOobject::NO_READ, IOobject::AUTO_WRITE ), -fvc::grad(phiFluid[i]) ) ); Info<< " Calculating field rhoFlux\n" << endl; rhoFluxFluid.set ( i, new surfaceScalarField ( IOobject ( "rhoFlux", runTime.timeName(), fluidRegions[i], IOobject::NO_READ, IOobject::NO_WRITE ), -k*fluidRegions[i].magSf()*fvc::snGrad(phiFluid[i]) ) ); } I should have the grad operator defined properly in fvSchemes: Code: /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 3.0.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default Euler; } gradSchemes { default leastSquares; grad(phi) leastSquares; grad(phiFluid[i]) leastSquares; grad(phiFluid) leastSquares; } divSchemes { default none; div(rhoFlux,rho) Gauss upwind; } laplacianSchemes { default none; laplacian(phi) Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; snGrad(phi) corrected; } // ************************************************************************* // I have tried playing around with the fvSchemes input, but haven't found a solution yet. Anyone any idea what may go wrong here ? Thanks, Floris

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post houkensjtu OpenFOAM 4 October 8, 2012 04:41 wanna88 FLUENT 2 October 1, 2012 22:34 spk Main CFD Forum 3 July 9, 2010 08:42 Antech Main CFD Forum 0 April 25, 2006 02:15 chong chee nan FLUENT 0 December 29, 2001 06:13

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