
[Sponsors] 
October 15, 2009, 12:38 
Help to reduce 3D computation time?

#1 
Member

Dear Foam Community,
Can someone give some insight on this matter? I am running a 3D simulation and the solver is taking forever to compute, so I attempted to resolve with GAMG solver but the times are not changing. Do I need to fix my blockMeshDict when choosing GAMG as a solver/preconditioner? I do not have clusters and am working from a 4 processor workstation. Sincerly, Lori Here is my FvSolutions: ____________________________________ solvers { p GAMG { preconditioner FDIC; mergeLevels 1; smoother GaussSeidel; agglomerator faceAreaPair; nCellsInCoarsestLevel 100; tolerance 1e07; relTol 0; }; U GAMG { preconditioner DILU; mergeLevels 1; smoother GaussSeidel; agglomerator faceAreaPair; nCellsInCoarsestLevel 100; tolerance 1e06; relTol 0; }; taufirst PBiCG { preconditioner DILU; tolerance 1e06; relTol 0; }; } PISO { momentumPredictor yes; nCorrectors 2; nNonOrthogonalCorrectors 1; pRefCell 0; pRefValue 0; } relaxationFactors { p 0.3; U 0.5; taufirst 0.3; } ______________________________________________ FvSchemes ______________________________________________ ddtSchemes { default CrankNicholson 1; } gradSchemes { default leastSquares; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default none; div(phi,U) Gauss upwind; div(phi,taufirst) Gauss upwind; div(tau) Gauss linear; } laplacianSchemes { default none; laplacian(etaPEff,U) Gauss linear corrected; laplacian(etaPEff+etaS,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(HbyA) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } _______________________________________________ 

October 16, 2009, 05:41 

#2 
Senior Member
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 8 
Hi.
"forever" is relative :) CFD simulations can take from a few seconds to days, months and even years to complete, so we need some figures here to see if yours "forever" is too long :) Well, some input could be, and I don't know if it's any news/use for you, but initial conditions and mesh severely affects how numerical solutions behave. If you haven't tried, and it makes sense in your case (depends what you're doing) you could try to initialize the domain with potentialFoam and maybe also take a look on any given mesh skewness. It seems that you are doing transient simulation, so maybe you could ease the simulation on by running with a reduced time step and then increase, if you have some violent startup effects in the flow. One could argue that your relaxation parameter for p is low, but for some simulations it's high. If you increase it, you might get quicker convergence  or divergence and numerical explosions (which I guess is the same thing :)) The tolerance on p is also strict, if you "only" run an engineering problem and not need scientific/academic precision. But, all suggestions may completely off for your case, but if you haven't dug into them, you might try to look into these. /Mads
__________________
Online free airfoilmesher for OpenFOAM here 

October 16, 2009, 05:51 

#3 
Member
Flavio Galeazzo
Join Date: Mar 2009
Location: Karlsruhe, Germany
Posts: 30
Rep Power: 8 
Hello Ith,
I agree with Mads, that "forever" is very relative. What can help us to estimate if your are having problems with you setup or if you have a problem that is too big to your computational resources is the following:  How big is your grid, and what type of elements are used  The solver you are using  The numerical scheme (you already give us that)  Your hardware configuration: type and number of CPUs and ammount of memory Regards, flga 

October 16, 2009, 10:50 

#4 
Member

Dear Mads and Flavio,
First off, thank you for taking the time to look at this with me. Forever is long, sorry, for 3D, it is taking about 3 to 6 weeks for a single run on a single processor to reach steady state. (2D took about 10 minutes to 3 hours). I did not know about potentiaFoam and can look into this, thanks and I will dig into some of the other suggestions. I was hoping GAMG would work better based on the OF Userguide suggestions but wondered if I was using this solver incorrectly or not. 1. I will attach the blockMesh where I use hex elements. 2. The physical solver is viscoelasticfluidFoam written by Jovani Favero. The numerical solver is GAMG with PBiCG, and PISO for Pressure and Velocity convergence. My first 3D runs with with the numerical solvers (attached below) which seems faster than GAMG? 4. Ubuntu Release 8.10 (intrepid) / Hardware Memory 3.2 GiB / 4 Processors: Intel Core2 Quad CPU Q9550@ 2.83GHz each. Let me know if i did not answer correctly, Thank you, Lori first 3D run solver (FvSolutions) info: __________________________________ solvers { p PCG { preconditioner DIC; tolerance 1e07; relTol 0; }; U PBiCG { preconditioner DILU; tolerance 1e06; relTol 0; }; taufirst PBiCG { preconditioner DILU; tolerance 1e06; relTol 0; }; } PISO { momentumPredictor yes; nCorrectors 2; nNonOrthogonalCorrectors 1; pRefCell 0; pRefValue 0; } relaxationFactors { p 0.3; U 0.5; taufirst 0.3; } _________________________________________ 3D blockMesh file: __________________________________________________ _____________ convertToMeters 0.0032; vertices ( (0 0 0) //0 (80 0 0) //1*** (0 1 0) //2 (80 1 0) //3*** (0 2.5 0)//4 (80 2.5 0)//5 (0 4 0) //6 (80 4 0) //7 (130 0 3.75)//8 (130 1 3.75) //9 (0 0 10) //10 (80 0 10)//11 (0 1 10) //12 (80 1 10)//13 (0 2.5 10)//14 (80 2.5 10)//15 (0 4 10) //16 (80 4 10) //17 (130 0 6.25) //18 (130 1 6.25) //19 (80 0 6.25) //20 (80 1 6.25) //21 (80 2.5 6.25)//22 (0 0 6.25) //23 (0 1 6.25) //24 (0 2.5 6.25) //25 (0 4 6.25) //26 (80 4 6.25) //27 //*** indent front face 09/20/09 (80 0 3.75) //28 (80 1 3.75) //29 (0 1 3.75) //30 (0 0 3.75) //31 (0 2.5 3.75) //32 (0 4 3.75) //33 (80 4 3.75) //34 (80 2.5 3.75) //35 ); blocks ( hex (23 20 21 24 10 11 13 12) (150 30 30) simpleGrading (0.002 0.3 1) hex (31 28 29 30 23 20 21 24) (150 30 20) simpleGrading (0.002 0.3 1) hex (0 1 3 2 31 28 29 30) (150 30 30) simpleGrading (0.002 0.3 1) hex (2 3 5 4 30 29 35 32) (150 30 30) simpleGrading (0.002 4 1) hex (30 29 35 32 24 21 22 25) (150 30 20) simpleGrading (0.002 4 1) hex (24 21 22 25 12 13 15 14) (150 30 30) simpleGrading (0.002 4 1) hex (4 5 7 6 32 35 34 33) (150 30 30) simpleGrading (0.002 0.3 1) hex (32 35 34 33 25 22 27 26) (150 30 20) simpleGrading (0.002 0.3 1) hex (25 22 27 26 14 15 17 16) (150 30 30) simpleGrading (0.002 0.3 1) hex (28 8 9 29 20 18 19 21) (90 30 20) simpleGrading (500 0.3 1) ); edges ( ); patches ( patch inlet ( (0 2 30 31) //0 (31 30 24 23) (23 24 12 10) //2 (2 4 32 30) (30 32 25 24) //4 (24 25 14 12) (4 6 33 32) //6 (32 33 26 25) (25 26 16 14) //8 ) wall fixedWalls ( (6 33 34 7) //top of wall R upstream (33 26 27 34) //top of wall M upstream (26 16 17 27) //top of wall L upstream (1 3 29 28) //contract R btm wall (3 5 35 29) //contract R mid wall (5 7 34 35) //contract R top wall (29 35 22 21) //contract M mid wall (35 34 27 22) //contract M top wall (20 21 13 11) //contract L btm wall (21 22 15 13) //contract L mid wall (22 27 17 15) //contract L top wall (29 21 19 9) //top of wall downstream ) patch outlet ( (8 9 19 18) //9 ) symmetryPlane simetry ( (0 1 28 31) //btm sym R upstream (31 28 20 23) //btm sym M upstream (23 20 11 10) //btm sym L upstream (28 8 18 20) //btm sym downstream ) wall frontAndBack ( (0 2 3 1) //btm frontface upstream (2 4 5 3) //mid frontface upstream (4 6 7 5) //top frontface upstream (28 29 9 8) //btm frontface downstream (10 12 13 11) //btm backface upstream (12 14 15 13) //mid backface upstream (14 16 17 15) //top backface upstream (20 21 19 18) //btm backface upstream ) ); mergePatchPairs ( ); // ************************************************** *********************** // Last edited by lth; October 16, 2009 at 12:14. 

October 19, 2009, 02:59 

#5 
Senior Member
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 8 
Hi Lori.
I am not familiar with the viscoelasticfluidFoam solver, but more than a month for a 1mio cellcase (if I am counting right) seems like a long time. Obvious, this also depends on the case you are trying to solve. Actually I'd guess that a viscoelastic case would exhibit quite rigid behaviour and quickly converge (?), but this does not seem to be the case here. I am sorry that I can't be of any help here. /Mads
__________________
Online free airfoilmesher for OpenFOAM here 

October 20, 2009, 03:10 

#6 
New Member
Matthew Philpott
Join Date: Aug 2009
Location: Belgium
Posts: 24
Rep Power: 8 
If you're running a solver over multiple CPU's, don't you have to break up the mesh into the number of CPU's and then solve each part using each CPU? I'm not sure if this applies to your situation or not. If you use the process manager (system manager or something, the one that shows CPU usage) in ubuntu does it show that all CPU's are being used during solving?
Have alook in the manual for decomposePar and mpirun under the heading, "running applications in paralell".
__________________
CAELinux 2009 + OF1.5 Ubuntu 9.04 x64 (jaunty jackalope) + OF1.6 

October 21, 2009, 12:13 

#7 
Member

Dear Mads,
These are dilute polymers so do not behaves as rigid bodies. They are highly nonlinear constitutive equations due to their convective stress terms. Thank you still for taking the time to look. Dear Bigred, Yes, I should look into using my computer as a parallel processor and have been running up to 4 separate cases on these processors to date. Good Point though. I am still believing that a multigrid method is the cheapest way to go from a computation time in any 3D viscoelastic case. I would like to be able to do both. Thank you, Lori 

October 23, 2009, 05:19 

#8 
Member
Flavio Galeazzo
Join Date: Mar 2009
Location: Karlsruhe, Germany
Posts: 30
Rep Power: 8 
Hello Ith,
Sorry for the late reply. I hope I can still help. You have a grid of 1+ million elements, it will take a bit time to converge in only one processor. As an example, my grids are larger (6 million, tetra), and running in 12 processors (3 x quad core) it takes 40 hours to converge using a solver base on the simpleFoam. You can take a look on the convergence behavior of the pressure correction, in my case is what takes the most of the time. I am using GAMG for the pressure, and more standard solvers for the other variables. My fvSolution is like this: solvers { p GAMG { tolerance 1e08; relTol 0.01; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 1200; agglomerator faceAreaPair; mergeLevels 1; }; U PBiCG { preconditioner DILU; tolerance 1e07; relTol 0.1; }; F PBiCG { preconditioner DILU; tolerance 1e07; relTol 0.1; }; k PBiCG { preconditioner DILU; tolerance 1e07; relTol 0.1; }; epsilon PBiCG { preconditioner DILU; tolerance 1e07; relTol 0.1; }; } SIMPLE { nNonOrthogonalCorrectors 1; } relaxationFactors { p 0.3; U 0.7; F 0.9; k 0.4; epsilon 0.4; } Regards, flga 

March 16, 2011, 10:06 

#9 
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12 
Hi flga,
Do you know what is the rule to set nCellsInCoarsestLevel? my case is an external incomoressible flow, using pisoFoam. 5m grids, 80 cpus (I am taking your advice to make each time step runs one sec) Thanks
__________________
~ Daniel WEI  NatHaz Modeling Laboratory Department of Civil & Environmental Engineering & Earth Sciences University of Notre Dame, USA Email  My Personal CFD Blog 

March 29, 2011, 04:05 

#10 
Member
Flavio Galeazzo
Join Date: Mar 2009
Location: Karlsruhe, Germany
Posts: 30
Rep Power: 8 
Hello lakeat,
I have learned (after posting my fvSolution file in this thread) that the number you specify in nCellsInCoarsestLevel is for each partition, and not for the whole domain as I have thought. So I am using nCellsInCoarsestLevel = 100 in my new simulations. 80 cpus for 5 million nodes seems adequate for me 

March 29, 2011, 09:20 

#11  
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12 
Quote:
Thanks, this is exactly what I am using
__________________
~ Daniel WEI  NatHaz Modeling Laboratory Department of Civil & Environmental Engineering & Earth Sciences University of Notre Dame, USA Email  My Personal CFD Blog 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Differences between serial and parallel runs  carsten  OpenFOAM Bugs  11  September 12, 2008 11:16 
Transient simulation not converging  skabilan  OpenFOAM Running, Solving & CFD  12  September 17, 2007 17:48 
Computation Time compared to OpenFOAM  Florian Fruth  CFX  4  June 29, 2007 10:18 
VOF  özgür  FLUENT  8  January 6, 2004 09:23 
Can periodic function reduce the time and cost?  Lam  FLUENT  3  December 8, 2003 13:24 