
[Sponsors] 
January 10, 2014, 15:44 

#41 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,137
Blog Entries: 39
Rep Power: 110 
Hi Kumudu,
If you study this guide: http://linuxcommand.org/learning_the_shell.php  you should be able to figure it out on your own But the answer is simple:
Bruno
__________________


January 14, 2014, 17:28 

#42  
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 6 
Quote:
Thank you very much. Best regards, Kumudu 

January 27, 2014, 12:11 

#43  
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 6 
Quote:
I am back again after long time finishing all the exams. I have followed the steps you mentioned in the above. I still have maxZ face at the inlet and outlet faces. I use the "topoSet dict system/topoSetDict01 region water" and "createPatch overwrite region water" as you said. I am attaching the files and figures of the top view of the water region that shows maxZ at the inlet and outlet. Could you please tell me, what would be the reason that I still have these faces? Thanks in advance. Best regards, Kumudu Last edited by wyldckat; February 2, 2014 at 15:56. Reason: Added missing [/QUOTE] 

January 27, 2014, 12:30 

#44 
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 6 
Dear Bruno,
These are the steps I followed,if in case you need to check them, P { marginbottom: 0.08in; } runApplication blockMesh #define the cell set "refineCells" for the refinement and then refine runApplication topoSet dict system/topoSetDictRefine runApplication refineMesh overwrite dict #define the zones for the regions and split the mesh into regions runApplication topoSet dict system/topoSetDictRegions runApplication splitMeshRegions cellZones overwrite #define the faceSets for the inlet and outlet patches and create the patches runApplication topoSet dict system/topoSetDictFaceSet region water runApplication createPatch overwrite region water Please find the attached files. I couldn't attach them as a one Zip file. So, I am attaching them as 0,constant and system. Thanks in advance. Best regards, Kumudu 

February 2, 2014, 16:23 

#45 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,137
Blog Entries: 39
Rep Power: 110 
Hi Kumudu,
You have the boxes defined too tightly. Basically, if a box has a lower Z of 40 and a higher Z of 40, nothing can fit inside, because it's a plane and not a box Keep in mind that it's a "boxToFace", not a "planeToFace" (I don't think this one exists) Edit the file "system/water/topoSetDictFaceSet" and notice the changes I've made: Code:
zmaxP1 40; zmaxP2 40; zmaxP3 1.03; zmaxP1a 39.999; zmaxP1b 40.001; zmaxP2a 39.999; zmaxP2b 40.001; actions ( { name f_inlet; type faceSet; action new; source boxToFace; sourceInfo { box ($xminP1 $yminP1 $zmaxP1a)($xmaxP1 $ymaxP1 $zmaxP1b); } } { name f_outlet; type faceSet; action new; source boxToFace; sourceInfo { box ($xminP2 $yminP2 $zmaxP2a)($xmaxP2 $ymaxP2 $zmaxP2b); } } ); Code:
zmaxP1a 39.999999999999999999999999999999999999999; zmaxP1b 40.00000000000000000000000000000000001; zmaxP2a 38; zmaxP2b 42; Best regards, Bruno
__________________


February 3, 2014, 00:59 

#46  
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 6 
Quote:
Thank you very much. Now I understand what was wrong. I will make the corrections and let you know. Best regards, Kumudu 

February 3, 2014, 18:11 

#47 
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 6 

February 26, 2014, 12:29 
error occured in chtMultiRegionFoam

#48 
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 6 
Dear Bruno,
I have created a case which have four different materials (water,pipe,filling material, soil). I use blockMesh to create the domain and then use the topoSet to define the regions. This time I defined the inlet and outlet for the fluid region using the blockMeshDict. I have used several blocks with different grading in the mesh to catch the different length scales in my problem. I have attached the .jpg file of the regions. But when I run the file for 10s, it just run for 5s and gave the error massage: > FOAM FATAL ERROR: [1] Maximum number of iterations exceeded I have then changed the line "const int Foam::specieThermo<Thermo>::maxIter_ = 100;" in the opt/openfoam211/src/thermophysicalModels/specie/lnInclude$ gedit specieThermo.C into "const int Foam::specieThermo<Thermo>::maxIter_ = 5000;" But, it still gives me the same error. I have attached the case file. Could you please tell me how to fix this problem. Is this problem cause due to my mesh? Thanks in advance. Best regards, Kumudu 

February 26, 2014, 12:39 
error occured in chtMultiRegionFoam

#49 
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 6 
Dear Bruno,
here is part of the full error message: Code:
Solving for fluid region water diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.98619399, Final residual = 2.5437182e08, No Iterations 84 DILUPBiCG: Solving for Uy, Initial residual = 0.98967568, Final residual = 9.3487139e08, No Iterations 84 DILUPBiCG: Solving for Uz, Initial residual = 0.98334287, Final residual = 7.8463215e08, No Iterations 84 > FOAM FATAL ERROR: Maximum number of iterations exceeded From function specieThermo<Thermo>::T(scalar f, scalar T0, scalar (specieThermo<Thermo>::*F)(const scalar) const, scalar (specieThermo<Thermo>::*dFdT)(const scalar) const) const in file /home/opencfd/OpenFOAM/OpenFOAM2.1.0/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 69. FOAM parallel run aborting > FOAM FATAL ERROR: Maximum number of iterations exceeded From function specieThermo<Thermo>::T(scalar f, scalar T0, scalar (specieThermo<Thermo>::*F)(const scalar) const, scalar (specieThermo<Thermo>::*dFdT)(const scalar) const) const in file /home/opencfd/OpenFOAM/OpenFOAM2.1.0/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 69. FOAM parallel run aborting DILUPBiCG: Solving for h, Initial residual = 0.99994363, Final residual = 9.0410388e08, No Iterations 87 > FOAM FATAL ERROR: Maximum number of iterations exceeded From function specieThermo<Thermo>::T(scalar f, scalar T0, scalar (specieThermo<Thermo>::*F)(const scalar) const, scalar (specieThermo<Thermo>::*dFdT)(const scalar) const) const in file /home/opencfd/OpenFOAM/OpenFOAM2.1.0/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 69. FOAM parallel run aborting > FOAM FATAL ERROR: Maximum number of iterations exceeded From function specieThermo<Thermo>::T(scalar f, scalar T0, scalar (specieThermo<Thermo>::*F)(const scalar) const, scalar (specieThermo<Thermo>::*dFdT)(const scalar) const) const in file /home/opencfd/OpenFOAM/OpenFOAM2.1.0/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 69. Kumudu Last edited by wyldckat; March 2, 2014 at 15:25. Reason: Added [CODE][/CODE] 

March 2, 2014, 15:58 

#50 
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,137
Blog Entries: 39
Rep Power: 110 
Hi Kumudu,
So, this is basically several problems in a single case. Firstly, you're using chtMultiRegionFoam, which is a transient solver and which requires for the Courant number to stick to low values, usually around 0.5 at most. Since you turned off automatic deltaT adjustments: Code:
adjustTimeStep no; More specifically, this is what I'm talking about, which is the time iteration prior to the one that crashes: Code:
Time = 5 Solving for fluid region water diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.96712474, Final residual = 5.8988354e08, No Iterations 72 DILUPBiCG: Solving for Uy, Initial residual = 0.96904191, Final residual = 7.4006406e08, No Iterations 72 DILUPBiCG: Solving for Uz, Initial residual = 0.96440759, Final residual = 5.3647585e08, No Iterations 72 DILUPBiCG: Solving for h, Initial residual = 0.99601552, Final residual = 1.9933183e08, No Iterations 74 Min/max T:89820.961 1348.6201 GAMG: Solving for p_rgh, Initial residual = 0.99943473, Final residual = 0.0075440402, No Iterations 4 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (water): sum local = 96.789128, global = 1.0330402, cumulative = 0.38554559 GAMG: Solving for p_rgh, Initial residual = 0.53592312, Final residual = 0.00012831322, No Iterations 1000 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (water): sum local = 14.468018, global = 1.1572485, cumulative = 1.5427941 Solving for solid region soil DICPCG: Solving for T, Initial residual = 0.10794196, Final residual = 3.6911129e08, No Iterations 3 DICPCG: Solving for T, Initial residual = 4.0107831e08, Final residual = 4.0107831e08, No Iterations 0 Min/max T:min(T) [0 0 0 1 0 0 0] 277 max(T) [0 0 0 1 0 0 0] 295 Solving for solid region pipe DICPCG: Solving for T, Initial residual = 0.97059185, Final residual = 3.0475829e07, No Iterations 4 DICPCG: Solving for T, Initial residual = 7.2913056e09, Final residual = 7.2913056e09, No Iterations 0 Min/max T:min(T) [0 0 0 1 0 0 0] 50735.672 max(T) [0 0 0 1 0 0 0] 566.6835 Solving for solid region Borehole DICPCG: Solving for T, Initial residual = 0.63383353, Final residual = 1.8912943e07, No Iterations 6 DICPCG: Solving for T, Initial residual = 1.4856261e09, Final residual = 1.4856261e09, No Iterations 0 Min/max T:min(T) [0 0 0 1 0 0 0] 580.36232 max(T) [0 0 0 1 0 0 0] 302.58436 ExecutionTime = 5.93 s ClockTime = 6 s Region: water Courant Number mean: 330368.2 max: 2.799531e+08 Region: soil Diffusion Number mean: 4.3894482e05 max: 0.00056112935 Region: pipe Diffusion Number mean: 0.00012317156 max: 0.00054975752 Region: Borehole Diffusion Number mean: 0.00021248831 max: 0.0017169268 The actual reason for this? Run this command, after the mesh is completely done: Code:
checkMesh region water Code:
Min volume = 5.3733903e09. Max volume = 0.00014412465. Total volume = 0.021915648. Cell volumes OK. Remember the very first tutorial in the OpenFOAM User Guide: http://www.openfoam.org/docs/user/cavity.php It explains there how the Courant Number is calculated... which is directly related to the volume of a cell (unless you're simulating in 2D). And what cells is this in reference to? Here's the problem: U section of water pipe.jpg Click on the image and you'll see a very thin line of cells in the U part of the pipe. Those are the cells that are causing the problem. Unfortunately, this is probably not the only problem. You're using really long cells along the pipe, which can lead to problems in the near future. Why? Because meshes are extremely important for quality simulations+results. Here's a compilation of the interesting cases I've had the pleasure of analysing here on the forum: OpenFOAM: Interesting cases of bad meshes and bad initial conditions  innocent looking meshes resulted in solver crashes or at least lead to nonphysical results. There you should be able to see for yourself what bad cell proportions can lead to. Best regards, Bruno
__________________


March 3, 2014, 01:49 

#51  
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 6 
Quote:
Dear Bruno, Thank you very much. When I set the time step to 0.01 and remove the grading in the Zdirection by catching the Upart of the pipe with another block with dz=0.012, the error didn't appeared. Because,Courant Number was 0.3 at that part. Thanks again, Best regards, Kumudu 

March 7, 2014, 13:32 
changing the boundary conditions with time

#52 
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 6 
Dear Bruno,
I want to run the chtMultiRegionFoam with different inlet temperature and velocity magnitudes at different times. For example, lets say I want to change the inlet temperature of the fluid region hourly so that heat load to the system will change hourly. Also, after 12 hours of circulating the water in the pipe, I want to stop the circulation by setting the velocity equal to zero and recirculate it again after another 12 hours . Is there any way that I could set these conditions easily ? Also, I have another question regarding run the chtMultiRegionFoam in parallel. My server has 6 processors and I want to decompose the 4 regions (soil,water,...) into these 6 processors and run it. I changed the decomposeParDict as follows, Code:
numberOfSubdomains 6; // Keep owner and neighbour on same processor for faces in zones: // preserveFaceZones (heater solid1 solid3); method scotch; // method hierarchical; // method simple; // method manual; simpleCoeffs { n (2 2 2); delta 0.001; } hierarchicalCoeffs { n (1 1 1); delta 0.001; order xyz; } scotchCoeffs { processorWeights ( 1 1 1 1 1 1 ); //writeGraph true; //strategy "b"; } manualCoeffs { dataFile "decompositionData"; } //// Is the case distributed //distributed yes; //// Per slave (so nProcs1 entries) the directory above the case. //roots //( // "/tmp" // "/tmp" //); Code:
# Decompose for i in water soil pipe Borehole do decomposePar region $i > log.decomposePar.$i 2>&1 done # Run runParallel `getApplication` 6 # Reconstruct for i in water soil pipe Borehole do reconstructPar region $i > log.reconstructPar.$i 2>&1 done Thanks in advance. Best regards, Kumudu Last edited by wyldckat; April 5, 2014 at 15:35. Reason: Added [CODE][/CODE] for clarity 

March 20, 2014, 18:58 

#53 
Member
Lucas Mutti
Join Date: Aug 2013
Posts: 47
Rep Power: 7 
Hey guys,
Your discussion is very interesting. In fact, I just ran into a similar problem that I do not know how to solve. I am trying to model a 2D geometry as attached. As you can see I have one dome resting on top of a rectangle surrounded by walls. I am also trying to simulate a conjugate heat transfer problem but my problem is while using the topoSetDict. This is my topoSetDict file so far: 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 topoSetDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // // Useful website to help determine which geometry to use for the topoSetDict file // https://github.com/OpenFOAM/OpenFOAM...et/topoSetDict // OBS.: topoSetDict is in meters. actions ( // bottomWall { name bottomWall; type cellSet; action new; source boxToCell; sourceInfo { box (0 0.02 0 )(0.075 0 0.01); box (0.075 0 0.01)(0.125 2 0); box (0.125 2 0)(0.20 0 0.01); } } { name bottomWall; type cellZoneSet; action new; source setToCellZone; sourceInfo { set bottomWall; } } // leftWall { name leftWall; type cellSet; action new; source boxToCell; sourceInfo { box (0.02 0 0 )(0 0.10 0.01); } } { name leftWall; type cellZoneSet; action new; source setToCellZone; sourceInfo { set leftWall; } } // rightWall { name rightWall; type cellSet; action new; source boxToCell; sourceInfo { box (0.2 0 0 )(0.22 0.1 0.01); } } { name rightWall; type cellZoneSet; action new; source setToCellZone; sourceInfo { set rightWall; } } // air { name air; type cellSet; action new; source boxToCell; sourceInfo { // base box (0 0 0)(0.075 0.10 0.01); box (0.075 0.10 0.01)(0.125 0 0); box (0.125 0 0)(0.20 0.10 0.01); } } { name air; type cellZoneSet; action new; source setToCellZone; sourceInfo { set air; } } { name airdome; type cellSet; action new; source cylinderToCell; sourceInfo { p1 (0.10 0.10 0); p2 (0.10 0.10 0.01); radius 0.10; } } { name airdome; type cellZoneSet; action new; source cylinderToCell; sourceInfo { set airdome; } } ); // ************************************************************************* // Code:
Time = 0 mesh not changed. Created cellSet bottomWall Applying source boxToCell Adding cells with center within boxes 1((0.125 2 0) (0.2 0 0.01)) cellSet bottomWall now size 200 Created cellZoneSet bottomWall Applying source setToCellZone Adding all cells from cellSet bottomWall ... cellZoneSet bottomWall now size 200 Created cellSet leftWall Applying source boxToCell Adding cells with center within boxes 1((0.02 0 0) (0 0.1 0.01)) cellSet leftWall now size 200 Created cellZoneSet leftWall Applying source setToCellZone Adding all cells from cellSet leftWall ... cellZoneSet leftWall now size 200 Created cellSet rightWall Applying source boxToCell Adding cells with center within boxes 1((0.2 0 0) (0.22 0.1 0.01)) cellSet rightWall now size 200 Created cellZoneSet rightWall Applying source setToCellZone Adding all cells from cellSet rightWall ... cellZoneSet rightWall now size 200 Created cellSet air Applying source boxToCell Adding cells with center within boxes 1((0.125 0 0) (0.2 0.1 0.01)) cellSet air now size 200 Created cellZoneSet air Applying source setToCellZone Adding all cells from cellSet air ... cellZoneSet air now size 200 Created cellSet airdome Applying source cylinderToCell Adding cells with centre within cylinder, with p1 = (0.1 0.1 0), p2 = (0.1 0.1 0.01) and radius = 0.1 cellSet airdome now size 2088 Created cellZoneSet airdome Applying source cylinderToCell > FOAM FATAL IO ERROR: keyword p1 is undefined in dictionary "/home/meisu/OpenFOAM/meisu2.2.1/run/Research/ConjugateHeatTransfer/RayleighBenard/caseTwoDomeThreeWalls/system/topoSetDict.actions.sourceInfo" file: /home/meisu/OpenFOAM/meisu2.2.1/run/Research/ConjugateHeatTransfer/RayleighBenard/caseTwoDomeThreeWalls/system/topoSetDict.actions.sourceInfo from line 139 to line 139. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 402. FOAM exiting I greatly appreciate your attention, Lucas Last edited by wyldckat; April 5, 2014 at 15:41. Reason: Added [CODE][/CODE] and fixed link 

March 22, 2014, 04:16 

#54 
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 6 
Hi Lucas,
I am no expert in this area. But, I think the problem is with defining the topoSet region using cylinderToCell. "keyword p1 is undefined in dictionary "/home/meisu/OpenFOAM/meisu2.2.1/run/Research/ConjugateHeatTransfer/RayleighBenard/caseTwoDomeThreeWalls/system/topoSetDict.actions.sourceInfo" The above error indicates that the problem is with p1. I haven't use the cylinderToCell before. But, have a look at it again. Best regards, Kumudu Last edited by wyldckat; April 5, 2014 at 15:37. Reason: removed quote, to make it easier to read 

March 22, 2014, 13:08 

#55 
Member
Lucas Mutti
Join Date: Aug 2013
Posts: 47
Rep Power: 7 
Hey Kumudu,
Thanks for your response. I believe cylinderToCell might not be the best command so I am currently trying the zoneToCell approach. It turns out that I may execute the topoSetDict but unfortunately new domains are created (i.e. domain4, domain5, etc). I don't quite understand why. It is not a matter of unit for sure. Since I am dealing with half a circle it seems to me that the zoneToCell command is not properly covering all the regions. Also, I cannot identify the location of these domains so it is hard to to say where exactly the problem is. Would you be able to help me out with that? Thanks a lot, Lucas 

March 22, 2014, 13:29 

#56  
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 6 
Quote:
When I first create my regions, I got the same kind of problem. Like making excess domains. It is not due to type of the topoSet dictionary. You can view the excess domain by using paraview. Give the command, paraFoam  touch All. I am not sure. But you can find it in the Allrun file. Then view each domain by loading one by one. Then check your blockMesh dictionary. And change the cell size and run again the topoSet regions. You will find the error eventually. Best, Kumudu 

March 22, 2014, 14:48 

#57 
Member
Lucas Mutti
Join Date: Aug 2013
Posts: 47
Rep Power: 7 
Hey Kumudu,
Thanks for the input. Actually what I am trying to do is to break down my dome into a simpler geometry and trying to execute it. it seems that now I no longer have problems with the domains but instead this annoying message pops when I run the code. I have done some research but it is not clear what the problem is. What is the mystery behind this no finite volume options present? Cheers Code:
*** Reading solid mesh thermophysical properties for region rightWall Adding to thermos Selecting thermodynamics package { type heSolidThermo; mixture pureMixture; transport constIso; thermo hConst; equationOfState rhoConst; specie specie; energy sensibleEnthalpy; } Adding to radiations Selecting radiationModel opaqueSolid Selecting absorptionEmissionModel constantAbsorptionEmission Selecting scatterModel none Adding fvOptions No finite volume options present Region: leftAir Courant Number mean: 0 max: 0 Region: rightAir Courant Number mean: 0 max: 0 Region: midAir Courant Number mean: 0 max: 0 Region: boxairDome Courant Number mean: 0 max: 0 Region: leftairDome Courant Number mean: 0 max: 0 Region: leftbottomWall Diffusion Number mean: 9.29329e07 max: 1.22222e06 Region: midbottomWall Diffusion Number mean: 1.0967e06 max: 1.22222e06 Region: rightbottomWall Diffusion Number mean: 9.29329e07 max: 1.22222e06 Region: leftWall Diffusion Number mean: 1.37417e06 max: 2.44444e06 Region: rightWall Diffusion Number mean: 1.37417e06 max: 2.44444e06 deltaT = 45000 End Last edited by wyldckat; April 5, 2014 at 15:38. Reason: Added [CODE][/CODE] 

April 5, 2014, 16:09 

#58  
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,137
Blog Entries: 39
Rep Power: 110 
Greetings to all!
@Kumudu: Sorry for taking so long to answer you, but I haven't had the time to look into your questions sooner. Let's see... Quote:
But I think the easiest way would be to use a table based boundary condition. There was a couple of discussions on this topic sometime ago here: http://www.cfdonline.com/Forums/ope...lefilebc.html  and here: http://www.cfdonline.com/Forums/ope...ixedvalue.html Note: Be careful, because this feature of using data from a table means that it will interpolate between 2 time items on the list: http://www.openfoam.org/version2.1.0...conditions.php Example: Code:
uniformValue table ( ( 0 0.0) (100 10.0) ); Code:
inlet { type uniformFixedValue; uniformValue table ( ( 0 10.0) (3599.999 10.0) (3600 15.0) (7199.999 15.0) ); } Quote:
Code:
#!/bin/sh cd ${0%/*}  exit 1 # run from this directory # Source tutorial run functions . $WM_PROJECT_DIR/bin/tools/RunFunctions @Lucas: Quote:
When in doubt: run a similar tutorial case from OpenFOAM, to ascertain what's normal and what's not normal Best regards, Bruno
__________________


April 6, 2014, 02:19 

#59  
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 6 
Quote:
Dear Bruno, Many thanks for replying me. I will look into it carefully. Best regards, Kumudu 

July 28, 2016, 11:44 
Porting PlaneWall 2D for OF1606+

#60 
Member
Jaydeep
Join Date: Jun 2015
Posts: 33
Rep Power: 4 
Hello everyone,
I have been trying to port the classic PlaneWall 2D case for the latest OF release. I am attaching the zip for all files. The case runs well, but in the end it throws a ton of errors on ParaView and results are in my opinion unrealistic. Can somebody take a look at it and please let me know what all could be the probable causes ? Thanks! P.S. I use OF+ on windows, use native ParaView. Once the simulation is finished, you can open foam.foam file in PV for postprocessing. 

Tags 
fields chtmultiregionfoam 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Simulation of a single bubble with a VOFmethod  Suzzn  CFX  21  January 29, 2018 01:58 
Superlinear speedup in OpenFOAM 13  msrinath80  OpenFOAM Running, Solving & CFD  18  March 3, 2015 06:36 
LES simulation with Smagorinsky2 model  Zuixy  OpenFOAM Running, Solving & CFD  3  October 20, 2011 06:17 
Turbulence model in a simulation with wide spatial range of Reynolds numbers  Chander  CFX  33  September 28, 2011 08:48 
Experimental And Simulation Data for my model  Timothy Song  Siemens  0  January 12, 2009 06:23 