
[Sponsors] 
October 14, 2013, 08:41 
InterDyMFoam takes for ever in parallel

#1 
Senior Member
musaddeque hossein
Join Date: Mar 2009
Posts: 309
Rep Power: 11 
Dear all:
I am running a parallel case for seismic data using interdymfoam. Seismic data can be erratic and not smooth such as sinusoidal data. The data may have several displacements in one direction and then suddenly switch and have displacements in another direction. I am running a case with approx 250 data points  which is not much. My mesh is 600x100. I have seen in this forum people suggesting that for 50,000 cells one processor is enough. In my case I have 6 processors. Yet it is taking over 12 hours. Initially I had 12 processors and it was taking more than 12 hours so I reduced the number of processors to 6. If I look at the log file, I see that each step takes a few iterations to solve. So can any one suggest ways I can speed up the process? I have reproduced the log file below and I am not quite sure I understand each and every line, but perhaps hidden in those lines are flags that are trying to tell me why it is taking so long? Any advice will be greatly appreciated, Thanks!! sinppet of the log file from when the analysis started: ** "CFSServer.26896" "CFSServer.26897" "CFSServer.26898" "CFSServer.26899" "CFSServer.26900" ) Pstream initialized with: floatTransfer : 0 nProcsSimpleSum : 0 commsType : nonBlocking polling iterations : 0 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring runtime modified files using timeStampMaster allowSystemOperations : Disallowing usersupplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Selecting dynamicFvMesh solidBodyMotionFvMesh Selecting solidbody motion function tabulated6DoFMotion Applying solid body motion to entire mesh Reading field p_rgh Reading field U Reading/calculating face flux field phi Reading transportProperties Selecting incompressible transport model Newtonian Selecting incompressible transport model Newtonian Selecting turbulence model type RASModel Selecting RAS turbulence model laminar Reading g Calculating field g.h No finite volume options present PIMPLE: Operating solver in PISO mode time step continuity errors : sum local = 0, global = 0, cumulative = 0 GAMGPCG: Solving for pcorr, Initial residual = 1, Final residual = 2.08439e10, No Iterations 1 time step continuity errors : sum local = 2.56957e07, global = 6.54836e13, cumulative = 6.54836e13 Courant Number mean: 1.21013e05 max: 4.18906e05 Starting time loop Reading surface description: leftwalls rightwalls Interface Courant Number mean: 0 max: 0 Courant Number mean: 1.18641e05 max: 4.10692e05 deltaT = 0.00116279 Time = 0.00116279 solidBodyMotionFunctions::tabulated6DoFMotion::tra nsformation(): Time = 0.00116279 transformation: ((0 0.0228556 0) (1 (0 0 0))) Execution time for mesh.update() = 0.07 s MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 0 Max(alpha1) = 1 MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 0 Max(alpha1) = 1 MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 0 Max(alpha1) = 1.00001 GAMG: Solving for p_rgh, Initial residual = 1, Final residual = 0.00989367, No Iterations 14 time step continuity errors : sum local = 0.000466452, global = 6.67992e16, cumulative = 6.54168e13 GAMGPCG: Solving for p_rgh, Initial residual = 0.0197322, Final residual = 1.38145e09, No Iterations 12 time step continuity errors : sum local = 1.4508e10, global = 5.7683e16, cumulative = 6.54745e13 ExecutionTime = 1.04 s ClockTime = 2 s Interface Courant Number mean: 0 max: 0 Courant Number mean: 5.34521 max: 44.9452 deltaT = 1.29336e05 Time = 0.00117572 solidBodyMotionFunctions::tabulated6DoFMotion::tra nsformation(): Time = 0.00117572 transformation: ((0 0.0231166 0) (1 (0 0 0))) Execution time for mesh.update() = 0.09 s MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 0 Max(alpha1) = 1.00001 MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 0 Max(alpha1) = 1.00001 MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 0 Max(alpha1) = 1.00001 GAMG: Solving for p_rgh, Initial residual = 0.929805, Final residual = 0.0088692, No Iterations 9 time step continuity errors : sum local = 1.62837e06, global = 5.29716e18, cumulative = 6.5474e13 GAMGPCG: Solving for p_rgh, Initial residual = 0.0549742, Final residual = 4.49069e10, No Iterations 9 time step continuity errors : sum local = 4.12279e13, global = 5.20441e18, cumulative = 6.54735e13 ExecutionTime = 1.71 s ClockTime = 2 s Interface Courant Number mean: 0.000239332 max: 0.550102 Courant Number mean: 0.0611436 max: 0.550102 deltaT = 1.17536e05 Time = 0.00118748 

October 14, 2013, 09:29 

#2 
Senior Member
Pablo Higuera
Join Date: Jan 2011
Location: Singapore
Posts: 385
Rep Power: 10 
Hi,
I may point the obvious, but your case takes a lot of time probably because your deltaT is very small. My best guess is that your earthquake signal induces very large velocities the first time step, yielding "Courant Number mean: 5.34521 max: 44.9452". You should try a smaller deltaT to minimize this initial effect. Furthermore, you may be experiencing the socalled spurious velocities afterwards as your maximum Courant number is located at the interface between both fluids. On top of that I will try to use 1 processor only. In my scaling testing using interFoam, I have a magic number of 100.000~150.000 cells/processor. These are actually my best wild guesses, as you provide very few details from your mesh and BCs. Best, Pablo 

October 14, 2013, 09:54 

#3 
Senior Member
Håkon Strandenes
Join Date: Dec 2011
Location: Norway
Posts: 111
Rep Power: 12 
Depending on your linear equation solver settings, OpenFOAM might scale well down to as little as 5 000  10 000 cells/process, but this require the correct case and much fine tuning.
Anyways, what Phicau pointed out regarding the Courant number is probably what you need to concentrate about. Decreasing the time step is often the only solution, but it might also be wise to investigate whether you can make any changes to the grid to reduce the Courant number. Perhaps it is a special region with high velocities that drives this number high? A small increase in the cell size here might help (but of course only as long as you capture the necessary physics involved). At last: The Courant number shall not vary with the number of processors in use, in that case something is seriously wrong. 

October 14, 2013, 11:11 

#4 
Senior Member
musaddeque hossein
Join Date: Mar 2009
Posts: 309
Rep Power: 11 
Gentlemen:
Thankyou for your response. I am looking at tanksloshing. The tank dimensions are 1mx1mx0.1m. Water depth is 0.6m. This is a two phase (water / air) problem. The CofG is located at the water air interface and centered along the length of the tank. So the left face of the tank is 0.5m away and the right face of the tank is also 0.5m away. Attached is the mesh and geometry information in the blockMeshDict file: vertices ( // SFINTAIRDISPLACEMENT.V2 (0.05 0.50 0.600) // Vertex back lower left corner = 0 (0.05 0.50 0.600) // Vertex back lower right corner= 1 (0.05 0.50 0.400) // Vertex back upper right corner= 2 (0.05 0.50 0.400) // Vertex back upper left corner = 3 (0.05 0.50 0.600) // Vertex front lower left corner = 4 (0.05 0.50 0.600) // Vertex front lower right corner= 5 (0.05 0.50 0.400) // Vertex front upper right corner= 6 (0.05 0.50 0.400) // Vertex front upper left corner = 7 ); blocks ( // block0 hex (0 1 2 3 4 5 6 7) (100 600 1) simpleGrading (1 1 1) ); //patches boundary ( lowerWall { type patch; faces ( (0 1 5 4) ); } rightWall { type patch; faces ( (1 2 6 5) ); } atmosphere { type patch; faces ( (2 3 7 6) ); } leftWall { type patch; faces ( (0 4 7 3) ); } frontAndBack { type Empty; faces ( (4 5 6 7) (0 3 2 1) ); } ); In the controlDict file, the parameters are as follows: application interDyMFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 48; deltaT 0.001; writeControl adjustableRunTime; writeInterval 0.05; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression compressed; timeFormat general; timePrecision 6; runTimeModifiable yes; adjustTimeStep yes; maxCo 0.5; maxAlphaCo 0.5; maxDeltaT 1; I have a question about the deltaT. Based on the mesh, my my deltaX=1m/100= 0.01 so If I want to have a courant number of 0.5, then deltaT=0.05*0.01/1= 0.0005. I have no idea about the velocity U. I am assuming U=1, hence the deltaT I am using. How would one obtain U to get a better estimate for deltaT? Thanks 

October 14, 2013, 11:20 

#5 
Senior Member
Pablo Higuera
Join Date: Jan 2011
Location: Singapore
Posts: 385
Rep Power: 10 
Beware, your mesh has 1:6 aspect ratio cells. Do you really need such detail in the Z direction with respect to the Y? Based on my experience for free surface flows you should go for something closer to 1:1, I personally like 1:2, and never beyond 1:5.
Even though checkMesh yields Mesh OK, you have to be very careful about it, as your results fully depend on it. Best, Pablo 

October 14, 2013, 12:09 

#6 
Senior Member
musaddeque hossein
Join Date: Mar 2009
Posts: 309
Rep Power: 11 
You bring up a very interesting point. I dont know any better. However, when I run the same with a sinusoidal input, the run completes (with 12 processors) in about 6 hours, with 4000 data input. So I did not change the mesh size assuming that it was not a mesh problem.
What is your thought on deltaT? 

October 16, 2013, 21:02 

#7  
Senior Member
musaddeque hossein
Join Date: Mar 2009
Posts: 309
Rep Power: 11 
Quote:
Interface Courant Number mean: 0.0124589 max: 0.372336 Courant Number mean: 0.0748294 max: 0.49897 deltaT = 4.49679e05 Time = 0.102739 solidBodyMotionFunctions::tabulated6DoFMotion::tra nsformation(): Time = 0.102739 transformation: ((0 0.232156 0) (1 (0 0 0))) Execution time for mesh.update() = 0.05 s MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 6.79989e32 Max(alpha1) = 1.00004 MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 6.79989e32 Max(alpha1) = 1.00004 MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 6.79989e32 Max(alpha1) = 1.00004 GAMG: Solving for p_rgh, Initial residual = 0.10069, Final residual = 0.00058348, No Iterations 2 time step continuity errors : sum local = 5.95014e07, global = 8.12922e17, cumulative = 5.6182e15 GAMGPCG: Solving for p_rgh, Initial residual = 0.0134842, Final residual = 1.1313e09, No Iterations 11 time step continuity errors : sum local = 1.15361e12, global = 8.15249e17, cumulative = 5.53667e15 ExecutionTime = 1788.55 s ClockTime = 1795 s Interface Courant Number mean: 0.0124613 max: 0.372751 Courant Number mean: 0.0749913 max: 0.499211 deltaT = 4.50107e05 Time = 0.102784 solidBodyMotionFunctions::tabulated6DoFMotion::tra nsformation(): Time = 0.102784 transformation: ((0 0.232022 0) (1 (0 0 0))) Execution time for mesh.update() = 0.05 s MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 6.79989e32 Max(alpha1) = 1.00004 MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 6.79989e32 Max(alpha1) = 1.00004 MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 6.79989e32 Max(alpha1) = 1.00004 GAMG: Solving for p_rgh, Initial residual = 0.0994884, Final residual = 0.000577669, No Iterations 2 time step continuity errors : sum local = 5.91006e07, global = 1.21072e16, cumulative = 5.65775e15 GAMGPCG: Solving for p_rgh, Initial residual = 0.0133797, Final residual = 1.82521e09, No Iterations 10 time step continuity errors : sum local = 1.92295e12, global = 1.20349e16, cumulative = 5.7781e15 ExecutionTime = 1788.96 s ClockTime = 1796 s Interface Courant Number mean: 0.0124672 max: 0.37248 Courant Number mean: 0.0750803 max: 0.499105 deltaT = 4.50536e05 Time = 0.102829 solidBodyMotionFunctions::tabulated6DoFMotion::tra nsformation(): Time = 0.102829 transformation: ((0 0.231887 0) (1 (0 0 0))) Execution time for mesh.update() = 0.05 s MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 6.79989e32 Max(alpha1) = 1.00004 MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 6.79989e32 Max(alpha1) = 1.00004 MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 6.79989e32 Max(alpha1) = 1.00004 GAMG: Solving for p_rgh, Initial residual = 0.0977454, Final residual = 0.000615333, No Iterations 2 time step continuity errors : sum local = 6.41009e07, global = 5.24555e17, cumulative = 5.72564e15 GAMGPCG: Solving for p_rgh, Initial residual = 0.0131217, Final residual = 1.93769e09, No Iterations 10 time step continuity errors : sum local = 2.04804e12, global = 5.23548e17, cumulative = 5.67328e15 ExecutionTime = 1789.37 s ClockTime = 1796 s Interface Courant Number mean: 0.0125151 max: 0.372502 Courant Number mean: 0.0751691 max: 0.498562 deltaT = 4.51831e05 Time = 0.102874 solidBodyMotionFunctions::tabulated6DoFMotion::tra nsformation(): Time = 0.102874 transformation: ((0 0.231751 0) (1 (0 0 0))) Execution time for mesh.update() = 0.05 s MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 6.79989e32 Max(alpha1) = 1.00004 MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 6.79989e32 Max(alpha1) = 1.00004 MULES: Solving for alpha1 Phase1 volume fraction = 0.6 Min(alpha1) = 6.79989e32 Max(alpha1) = 1.00004 GAMG: Solving for p_rgh, Initial residual = 0.0995661, Final residual = 0.000583261, No Iterations 2 time step continuity errors : sum local = 6.12205e07, global = 8.57513e17, cumulative = 5.58753e15 GAMGPCG: Solving for p_rgh, Initial residual = 0.0133902, Final residual = 1.45622e09, No Iterations 11 time step continuity errors : sum local = 1.52179e12, global = 8.59522e17, cumulative = 5.50158e15 ExecutionTime = 1789.79 s ClockTime = 1796 s Interface Courant Number mean: 0.0126211 max: 0.37309 Courant Number mean: 0.0754036 max: 0.498553 deltaT = 4.53134e05 Time = 0.102919 

October 18, 2013, 10:20 

#8 
Senior Member
musaddeque hossein
Join Date: Mar 2009
Posts: 309
Rep Power: 11 
can anyone tell me what the function of the maxalphaCo is in the setFieldsDirectory in OpenFoam sloshingtank2D case? I understand the maxCo applies to one of the phases  say water in the tank for example. But what does maxCo apply to? The verbiage of the setFieldsDict is appended below.
Thanks ** FoamFile { version 2.0; format ascii; class dictionary; location "system"; object setFieldsDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // defaultFieldValues // define the entire analysis space as phase zero or gas phase ( volScalarFieldValue alpha1 0 ); // now define a region in the gas phase that has the fluid. It extends from the origin to 100 meters // below the tank, and 100 meters in the x and y direction. // This is to ensure that the area you want is filled with the fluid. Phase value is 1 regions ( boxToCell { box ( 100 100 100 ) ( 100 100 0 ); fieldValues ( volScalarFieldValue alpha1 1 ); } ); // ************************************************** *********************** // 

October 24, 2013, 11:50 

#9  
Senior Member
musaddeque hossein
Join Date: Mar 2009
Posts: 309
Rep Power: 11 
Quote:


Tags 
interdymfoam, parallel processing, takes for ever, takes long time 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Parallel interDyMFoam cellLevel problem  tgvosk  OpenFOAM Running, Solving & CFD  5  February 19, 2014 03:24 
interDyMFoam, problems in mesh motion solutor run in parallel  DLC  OpenFOAM  11  December 11, 2012 03:20 
Problems in mesh motion solutor in parallel 4 interDyMFoam.  DLC  Main CFD Forum  0  November 21, 2009 17:17 
Problems in mesh motion solutor in parallel 4 interDyMFoam.  DLC  OpenFOAM  0  November 21, 2009 09:54 
Running interDyMFoam in parallel  sega  OpenFOAM Running, Solving & CFD  1  March 12, 2009 06:54 