
[Sponsors] 
June 25, 2013, 08:12 
How to add AttachDetachFvMesh to layeredEngineMesh solver?

#1 
New Member
RJ HO
Join Date: Dec 2012
Posts: 21
Rep Power: 5 
Hi Foamers,
I'm looking to compile the engineMesh > layeredEngineMesh with dynamicMesh > attachDetach. I have tried to combine both files but I realize that layeredEngineMesh runs on move() while attachDetach runs on update(). How do I put them together? Regards RJ 

June 25, 2013, 12:46 

#2 
Senior Member
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18 
If you can download a copy of OpenFOAM 1.6ext, its engine library includes a class called layerAR that does what you want. I can confirm that this class works in 2.0.x through 2.2.x, with the caveat that you have to change some of the calls to polyTopoChanger. I did it a while ago and don't have access to the machine with the installation now, but its similar to the change I had to make to get attachDetach to work:
http://www.openfoam.org/mantisbt/view.php?id=786 Good luck! 

June 26, 2013, 05:46 

#3 
New Member
RJ HO
Join Date: Dec 2012
Posts: 21
Rep Power: 5 
i take that as you are talking about mapPolyMesh function calling morphing.
And why is changeMesh() has to change to changeMesh(True) for it to work. Kinda lost there. Can you point out which line do I need to change in my mapPoly. 

June 26, 2013, 12:19 

#4 
Senior Member
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18 
I can't find the 1.6ext file as the project isn't being actively hosted (at least that I can find). From what I remember, polyTopoChanger runs through all the topoChanges and executes them. The reason the new argument is used is that we are actually calling a different function that ends up calling the old changeMesh(). Search the online code database for changeMesh and you will see that there is one for polyTopoChanger and polyTopoChange. We want the first one (I think, again its been a while).


June 28, 2013, 02:00 

#5 
New Member
RJ HO
Join Date: Dec 2012
Posts: 21
Rep Power: 5 
Got it! changes to polyTopoChanger is not neccessary but instead layerAR.C only.
Adapted engineTopoChanger and layerAR to 2.2.x The only files require changing is return true to return topoChange.valid(), changeMesh() to changeMesh(true), allpoints to points in layerAR.C. That's all i think that the simulation seems to work fine from 180 to 180 with compiled with new moveEngineMesh with adapted engineTopoChanger. Gonna try including solvers next! 

June 29, 2013, 08:59 

#6 
New Member
RJ HO
Join Date: Dec 2012
Posts: 21
Rep Power: 5 
Does anyone happen to know how to compile engineTopoChanger class in OpenFoam 2.2.x?
The adapted compilation worked in my laptop. I tried to do the same with my desktop and the case that's running in my laptop in transferred together. Apparently, inside my newEngineTopoChangerMesh.C says something like the below and my solver with the adapted engineTopoChanger selector refuse to start. Is there something I have to do to make my solver work? // Enclose the creation of the engineGeometry to ensure it is // deleted before the engineTopoChangerMesh is created otherwise the dictionary // is entered in the database twice Valid engineTopoChangerMesh types are : 2 ( myLayerAR layerAR ) From function engineTopoChangerMesh::New(const IOobject&) in file engineTopoChangerMesh/engineTopoChangerMesh/newEngineTopoChangerMesh.C at line 67. FOAM exiting 

July 4, 2013, 08:01 
Solver Crashed!

#7 
New Member
RJ HO
Join Date: Dec 2012
Posts: 21
Rep Power: 5 
Simulation on diesel spray combustion on a hypothetical engine cylinder with customized sprayEngineFoam with adapted engineTopoChanger with layer addition and removal crashed. The dynamic mesh work fine I suppose as I tested with adapted moveDyMEngineMesh from 180 to 180 and ran checkMesh through it. Mesh seems to be O.K at each time interval. However, sprayEngineFoam crash at somewhere 58 CAD. I checked the mesh at that point over and over again. It looked the same like any other mesh motion before. Nothing different.
As for image; It's just a simple cylinder created with blockMesh by selecting the centre point twice. I'm pretty sure it works at I have test with sprayEngineFoam with engineMesh layered. But it crashed after having engineMesh replaced with adapted engineTopoChanger from 1.6ext. Again, the engineTopoChanger performed as expected and tested with adapted moveDyMEngineMesh. It's just the solver seem to prefer engineMesh over engineTopoChangerMesh? Lol =D P.S. I'm using OpenFOAM 2.2.X because of its sprayFoam Class and had to adapt 1.6ext for it's engineTopoChanger class. Error Log. Code:
Solving cloud sprayCloud Cloud: sprayCloud Current number of parcels = 0 Current mass in system = 0 Linear momentum = (0 0 0) Linear momentum = 0 Linear kinetic energy = 0 Rotational kinetic energy = 0 model1: number of parcels added = 23324 mass introduced = 1.40018e05 Parcels absorbed into film = 0 New film detached parcels = 0 Parcel fate (number, mass)  escape = 0, 0  stick = 0, 0 Temperature min/max = 0, 0 Mass transfer phase change = 1.40018e05 D10, D32, Dmax (mu) = 0, 0, 0 Liquid penetration 95% mass (m) = 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.01057, Final residual = 2.62337e06, No Iterations 6 DILUPBiCG: Solving for Uy, Initial residual = 0.0107857, Final residual = 3.26699e06, No Iterations 4 DILUPBiCG: Solving for Uz, Initial residual = 0.0111489, Final residual = 7.23998e06, No Iterations 5 DILUPBiCG: Solving for C7H16, Initial residual = 0.000128444, Final residual = 2.77758e06, No Iterations 1 DILUPBiCG: Solving for O2, Initial residual = 0.00023513, Final residual = 5.40333e06, No Iterations 1 DILUPBiCG: Solving for CO2, Initial residual = 0.00024192, Final residual = 5.66135e06, No Iterations 1 DILUPBiCG: Solving for H2O, Initial residual = 0.00024192, Final residual = 5.66135e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.000348675, Final residual = 8.54449e06, No Iterations 1 T gas min/max = 373, 1227.9 DICPCG: Solving for p, Initial residual = 0.946616, Final residual = 0.0387792, No Iterations 1 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0.00308543, global = 0.00281121, cumulative = 0.0187543 DICPCG: Solving for p, Initial residual = 0.122943, Final residual = 4.33585e07, No Iterations 7 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 6.68342e08, global = 1.00723e08, cumulative = 0.0187544 DILUPBiCG: Solving for epsilon, Initial residual = 0.184601, Final residual = 6.73394e06, No Iterations 5 DILUPBiCG: Solving for k, Initial residual = 0.14352, Final residual = 3.70806e06, No Iterations 5 Mean pressure:1.21075e+06 Mean temperature:1000.98 Mean u':7.30158 ExecutionTime = 2586.16 s ClockTime = 2589 s Courant Number mean: 0.0383579 max: 9.37156 deltaT = 2.27587e08 Crank angle = 58.2433 CAdeg deltaZ = 9.29923e08 Piston at:0.0553827 pistonLayerID: 0 Piston layering mode virtualPistonPosition = 0.0573819, deckHeight = 0.072 clearance: 0.0166174 Piston speed = 4.08602 m/s Total cylinder volume at CA 58.243256 = sum(V) [0 3 0 0 0 0 0] 7.00003e05 Solving cloud sprayCloud Cloud: sprayCloud Current number of parcels = 0 Current mass in system = 0 Linear momentum = (0 0 0) Linear momentum = 0 Linear kinetic energy = 0 Rotational kinetic energy = 0 model1: number of parcels added = 23324 mass introduced = 1.40018e05 Parcels absorbed into film = 0 New film detached parcels = 0 Parcel fate (number, mass)  escape = 0, 0  stick = 0, 0 Temperature min/max = 0, 0 Mass transfer phase change = 1.40018e05 D10, D32, Dmax (mu) = 0, 0, 0 Liquid penetration 95% mass (m) = 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.00465004, Final residual = 6.67201e07, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.00464643, Final residual = 5.90659e06, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.00637995, Final residual = 3.58223e08, No Iterations 1 #0 Foam::error::printStack(Foam::Ostream&) in "/home/rj/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/home/rj/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64linuxgnu/libc.so.6" #3 Foam::chemistryModel<Foam::psiChemistryModel, Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::solve(double, double) in "/home/rj/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/lib/libchemistryModel.so" #4 Foam::combustionModels::PaSR<Foam::combustionModels::psiChemistryCombustion>::correct() in "/home/rj/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/lib/libcombustionModels.so" #5 in "/home/rj/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/bin/mySprayEngineFoam" #6 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #7 in "/home/rj/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/bin/mySprayEngineFoam" Floating point exception (core dumped) Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { rho { solver PCG; preconditioner DIC; tolerance 1e05; relTol 0.1; } rhoFinal { $rho; tolerance 1e05; relTol 0; } "(Uh)" { solver PBiCG; preconditioner DILU; tolerance 1e05; relTol 0.1; } p { solver PCG; preconditioner DIC; tolerance 1e06; relTol 0.1; } pFinal { $p; tolerance 1e06; relTol 0; } "(Uh)Final" { $U; tolerance 1e05; relTol 0; } "(kepsilon)" { $U; } "(kepsilon)Final" { $UFinal; } "(YiO2N2H2O)" { $UFinal; } cellMotionUz { solver PCG; preconditioner DIC; tolerance 1e08; relTol 0; } } PIMPLE { transonic no; nCorrectors 2; nNonOrthogonalCorrectors 0; momentumPredictor yes; } relaxationFactors { fields { ".*Final" 1; } equations { ".*Final" 1; } } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.0   \\ / 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 Gauss linear; grad(p) Gauss linear; } divSchemes (added div(meshPhi,p) Gauss upwind; and div(phid,p) Gauss upwind; The rest is pretty much the same) { default none; div(phi,U) Gauss upwind; div(phid,p) Gauss upwind; div(phi,h) Gauss upwind; div(meshPhi,p) Gauss upwind; div(phi,K) Gauss linear; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(U) Gauss linear; div((muEff*dev2(T(grad(U))))) Gauss linear; div(phi,Yi_h) Gauss upwind; } laplacianSchemes { default Gauss linear orthogonal; laplacian(muEff,U) Gauss linear orthogonal; laplacian(mut,U) Gauss linear orthogonal; laplacian(DkEff,k) Gauss linear orthogonal; laplacian(DepsilonEff,epsilon) Gauss linear orthogonal; laplacian(DREff,R) Gauss linear orthogonal; laplacian((rho*(1A(U))),p) Gauss linear orthogonal; laplacian(alphaEff,h) Gauss linear orthogonal; } interpolationSchemes { default linear; } snGradSchemes { default orthogonal; } fluxRequired { default no; p ; } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.2.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application mySprayEngineFoam; startFrom latestTime; startTime 180; stopAt endTime; endTime 180; deltaT 0.05; writeControl adjustableRunTime; writeInterval 1; purgeWrite 0; writeFormat binary; writePrecision 6; writeCompression uncompressed; timeFormat general; timePrecision 6; adjustTimeStep yes; maxCo 0.25; runTimeModifiable yes; // ************************************************************************* // 

July 4, 2013, 12:42 

#8 
Senior Member
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18 
Your max temperature looks like it might be close to autoignition. What is the global equivalience ratio at crash time (or are there any combustible gases in the mixture at all?)


July 5, 2013, 00:31 

#9 
New Member
RJ HO
Join Date: Dec 2012
Posts: 21
Rep Power: 5 
yep! Combustion at 58 CAD is at its end. Injection starts at 23 CAD and peak at 4.5 CAD with 2504K with 15% oxygen (which is pretty accurate in my opinion after calculating the adiabatic flame temperature)
Now I tried running the simulation at 2X finer mesh at 10X smaller time steps to see what happen. Unfortunately, it has been running for 22 hours straight and i'm just at 15CAD. Btw, can anyone here able to explain how come the temperature simulated by sprayEngineFoam with engineMesh reaches peak at 3500K while similar set up with engineTopoChangerMesh (layer additon and removal) gives peak combustion temperature at 2500K which is more accurate? Is it possible that mesh layering and mesh addition and removal able to cause such a big difference? I think sprayEngineFoam with engineMesh is defective. Because with mesh layering the mesh cell at TDC is ridiculously "flat" after cramping 62mm stroke with 62 cell at BDC to 2mm at TDC. The timestep that close to TDC is in a factor of 10^9. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Creating New Solver: For particleladen compressible jets  sankarv  OpenFOAM Running, Solving & CFD  17  December 3, 2014 20:41 
how to modify a solver to add a disturbance  goodkid  OpenFOAM  2  June 25, 2011 04:35 
Working directory via command line  Luiz  CFX  4  March 6, 2011 21:02 
why the solver reject it? Anyone with experience?  bearcat  CFX  6  April 28, 2008 14:08 
Error during Solver  cfd guy  CFX  4  May 8, 2001 06:04 