|
[Sponsors] |
November 12, 2014, 01:35 |
|
#81 | |
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 12 |
Quote:
|
||
November 12, 2014, 04:58 |
|
#82 | |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 52 |
Quote:
boundary conditions
decompose the mesh
your error
what should you do first now
__________________
Keep foaming, Tobias Holzmann |
||
November 12, 2014, 05:30 |
|
#83 | |
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 12 |
Quote:
|
||
November 12, 2014, 06:00 |
|
#85 | |
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 12 |
Quote:
Output from decomposePar, used subdomain division (2 4 1) , I think this is slightly better compared to previouse one here http://www.cfd-online.com/Forums/ope...tml#post518507 .please comment Code:
Processor 0 Number of cells = 828661 Number of faces shared with processor 1 = 9078 Number of faces shared with processor 2 = 28421 Number of faces shared with processor 3 = 11335 Number of processor patches = 3 Number of processor faces = 48834 Number of boundary faces = 85632 Processor 1 Number of cells = 828661 Number of faces shared with processor 0 = 9078 Number of faces shared with processor 3 = 17113 Number of processor patches = 2 Number of processor faces = 26191 Number of boundary faces = 81355 Processor 2 Number of cells = 828661 Number of faces shared with processor 0 = 28421 Number of faces shared with processor 3 = 15007 Number of faces shared with processor 4 = 27368 Number of faces shared with processor 5 = 1229 Number of processor patches = 4 Number of processor faces = 72025 Number of boundary faces = 57213 Processor 3 Number of cells = 828661 Number of faces shared with processor 0 = 11335 Number of faces shared with processor 1 = 17113 Number of faces shared with processor 2 = 15007 Number of faces shared with processor 5 = 13092 Number of processor patches = 4 Number of processor faces = 56547 Number of boundary faces = 69703 Processor 4 Number of cells = 828661 Number of faces shared with processor 2 = 27368 Number of faces shared with processor 5 = 20564 Number of faces shared with processor 6 = 9942 Number of processor patches = 3 Number of processor faces = 57874 Number of boundary faces = 57452 Processor 5 Number of cells = 828661 Number of faces shared with processor 2 = 1229 Number of faces shared with processor 3 = 13092 Number of faces shared with processor 4 = 20564 Number of faces shared with processor 6 = 1159 Number of faces shared with processor 7 = 14195 Number of processor patches = 5 Number of processor faces = 50239 Number of boundary faces = 67825 Processor 6 Number of cells = 828661 Number of faces shared with processor 4 = 9942 Number of faces shared with processor 5 = 1159 Number of faces shared with processor 7 = 20886 Number of processor patches = 3 Number of processor faces = 31987 Number of boundary faces = 81669 Processor 7 Number of cells = 828661 Number of faces shared with processor 5 = 14195 Number of faces shared with processor 6 = 20886 Number of processor patches = 2 Number of processor faces = 35081 Number of boundary faces = 88809 Number of processor faces = 189389 Max number of cells = 828661 (0% above average 828661) Max number of processor patches = 5 (53.8462% above average 3.25) Max number of faces between processors = 72025 (52.1208% above average 47347.2) |
||
November 12, 2014, 09:02 |
|
#86 |
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 23 |
@ jetFire: What was the range of pressure and temperature in the last time after which the simulation crashes?
|
|
November 12, 2014, 09:04 |
|
#87 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27 |
I always try just a few times. Decompose -> benchmark -> Decompose differently -> benchmark. Then, I choose the fastes one.
__________________
The skeleton ran out of shampoo in the shower. |
|
November 13, 2014, 00:39 |
|
#88 |
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 12 |
@vasava
You can find the output for the last time step here. http://www.cfd-online.com/Forums/ope...tml#post518635 |
|
November 13, 2014, 04:48 |
|
#90 |
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 12 |
I had read few threads about the same error, few people felt this error was due to the mesh refinement.Coarsening the mesh may solve the problem but not sure. I have increased nCellsInCoarsest level to 400 and trying with constTransport model , not using sutherland
|
|
November 13, 2014, 05:05 |
|
#91 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27 |
You are mixing several things Jetfire.
1) He does not mean the residual of the pressure solver but the actual physical values of pressure in your domain. You need to have a look at paraView. 2) Setting nCellsInCoarsest is a solver setting that has nothing to do with "coarsening the mesh". It just sounds somehow similar.
__________________
The skeleton ran out of shampoo in the shower. |
|
November 13, 2014, 05:20 |
|
#92 |
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 12 |
Ok, I will let you know soon
|
|
November 14, 2014, 07:30 |
|
#93 |
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 23 |
This may sound obvious but from what i have read I feel that the error is coming from the Sutherland Coefficient part. If I am not wrong Sutherland viscosity has limitations with operating pressure and temperature. If they are outside the limits perhaps openfoam would have difficulties guessing the right material properties. Thats is the reason why I ask for those values.
Anyway, If I were you I would first try with normal viscosity and little lower rotational speed and see if everything works. Doing this will let me know if there is any additional issues with mesh, convergence and stability. Also its might help me predict the initial turbulence parameter better (just incase). Although openfoam handles the difference in meshes at cyclicAMI but you must do your part as well to make them as identical or almost identical. At 300000 RPM this is already a complicated and heavy computing case (high turbulence and large mesh that you need). Last edited by vasava; November 14, 2014 at 07:31. Reason: typo |
|
November 17, 2014, 00:25 |
|
#94 |
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 12 |
Hi guys,
After 2-3 days of the simulation running with different thermophysical model( constTransport).I end up getting this error . Code:
PIMPLE: iteration 4 DILUPBiCG: Solving for Ux, Initial residual = 4.698848279e-06, Final residual = 1.728346388e-10, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.0004148947624, Final residual = 1.605476696e-08, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.0004124625538, Final residual = 1.720494925e-08, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.001073898534, Final residual = 4.419787961e-07, No Iterations 1 GAMG: Solving for p, Initial residual = 0.0001402588605, Final residual = 4.530336629e-12, No Iterations 1 GAMG: Solving for p, Initial residual = 1.270429705e-09, Final residual = 1.270429705e-09, No Iterations 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 1.21975605e-05, global = -1.193260374e-05, cumulative = -0.03947889224 rho max/min : 2.5 0.1 GAMG: Solving for p, Initial residual = 9.809918063e-05, Final residual = 3.149546253e-12, No Iterations 1 GAMG: Solving for p, Initial residual = 8.907323553e-10, Final residual = 8.907323553e-10, No Iterations 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 1.219755365e-05, global = -1.193260374e-05, cumulative = -0.03949082484 rho max/min : 2.5 0.1 DILUPBiCG: Solving for omega, Initial residual = 5.101593458e-07, Final residual = 2.047378385e-11, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 4.414193461e-06, Final residual = 7.768684524e-10, No Iterations 1 PIMPLE: iteration 5 DILUPBiCG: Solving for Ux, Initial residual = 3.853220256e-06, Final residual = 1.380582769e-10, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.0003599162519, Final residual = 1.39347785e-08, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.0003569465205, Final residual = 1.390306585e-08, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.001096976628, Final residual = 4.135438555e-07, No Iterations 1 [3] [3] [3] --> FOAM FATAL ERROR: [3] Maximum number of iterations exceeded [3] [3] From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const [3] in file /home/eatin/OpenFOAM/OpenFOAM-2.3.0/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76. [3] FOAM parallel run aborting [3] [3] #0 Foam::error::printStack(Foam::Ostream&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [3] #1 Foam::error::abort() in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" [3] #2 Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy>::T(double, double, double, double (Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy>::*)(double, double) const, double (Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy>::*)(double, double) const, double (Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy>::*)(double) const) const in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so" [3] #3 Foam::hePsiThermo<Foam::psiThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so" [3] #4 Foam::hePsiThermo<Foam::psiThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::correct() in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so" [3] #5 [3] in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam" [3] #6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" [3] #7 [3] in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam" -------------------------------------------------------------------------- mpirun has exited due to process rank 3 with PID 28754 on node EAT-Standalone exiting improperly. There are two reasons this could occur: 1. this process did not call "init" before exiting, but others in the job did. This can cause a job to hang indefinitely while it waits for all processes to call "init". By rule, if one process calls "init", then ALL processes must call "init" prior to termination. 2. this process called "init", but exited without calling "finalize". By rule, all processes that call "init" MUST call "finalize" prior to exiting or it will be considered an "abnormal termination" This may have caused other processes in the application to be terminated by signals sent by mpirun (as reported here). --------------------------------------------------------------------------
|
|
November 17, 2014, 01:12 |
|
#95 |
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 12 |
I was able to run the simulation upto 1.9375e-07 after which it should the error posted above. Based on some threads I have read it may be better to use zeroGradient conditon for pressure and temperature at outlet.
As vasava asked for the pressure and temperature range Temperature: 221 - 408 k pressure: 1.84e+04 - 2.92e+05 Please Check the pictures attached. |
|
November 17, 2014, 04:03 |
|
#97 |
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 12 |
||
November 17, 2014, 06:22 |
|
#98 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 52 |
Never compare CFX, FLUENT settings with OpenFOAM settings.
Fluent and CFX always have some settings you do not see. I had a discussion about that with Bernhard and please never think that if you apply the fluent/cfx conditions to openfoam that this is sufficient and the calculation should work. Maybe your settings in CFX are also very bad and non physical. Fluent/CFX is more robust for wrong user input and in most of all cases it will give you some result. If you want to use foam in a good way, you have to know how things are working and what BC are correct, how many you can/have to set to make the equations solvable. Therefor you should have a knowledge at:
Most of these things should always be available for all who make CFD simulations but I know a few people which do not know anything about it and they still do it and get results with fluent and cfx. I dont want to say that these toolboxes are bad but much more user friendly (especially in user input things, stability etc.). Thats the reason why a lot of people think foam is not able to solve complex things because the solver crashes all the time etc. But the problem is: they dont know why!
__________________
Keep foaming, Tobias Holzmann |
|
November 21, 2014, 01:20 |
|
#99 |
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 12 |
Hi ,
I tried running the simulation with the constTransport thermophysical model few changes to boundary condition zeroGradient instead of inletOutlet at the outlet for pressure and temperature for velocity inlet i have used pressureInletVelocity and at outlet flowRateInletVelocity Even with these I get the same error as posted before. As I am approaching my project deadline I have to start writing the report , maybe there is a problem with the mesh/ Boundary conditions or this is a too complex simulation as it has 3 interfaces and compressor rotates at 300000 rpm that OpenFOAM can handle as of now. So I am stopping the simulation and closing the project. It was really nice of you guys @Tobi @RodriguezFatz @vasava for trying to help me out in each and every step of the simulation and taking your time to explain the concepts involved in the simulation. I thank all of you for your kind support and I will surely acknowledge your efforts in my report Thank you!! |
|
November 29, 2014, 05:52 |
|
#100 |
Member
Christian
Join Date: Apr 2014
Posts: 74
Rep Power: 12 |
Dear all,
thank you for the interesting topic, I learned more on rhoPimpleDyMFoam here than by searchign the entire forum! I have some doubts of the BCs I see in the last attachment: jetfire basically places, for p,U,T, inlet fixed values (or mass flow rate) and inletOutlet at outlet. Would not be better to provide values for both inlet and outlet, maybe leaving inletOutlet only for T? As I have a similar case for which I know the input pressure, the outlet pressure (atmospheric p), the atmospheric temperate at outlet and the inlet velocity, should I use something like this: -inlet: U fixed Value (or flowRateInletVelocity), p totalPressure, T inletOutlet -outlet: U inletOutlet, p fixedValue 101325 Pa, T 293K ? I got also floating point errors similar to the one had by jetfire at page 3 (foamHePsiThermo), should I use the constant transport properties? My rpm velocities are much lower so I should not have the turbulence problems that jetfire had rotating at 300k rpm! |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Study of the EEqn.H in rhoPimpleDyMFoam. | Horacio Aguerre | OpenFOAM Programming & Development | 11 | August 19, 2022 03:47 |
Developing a rhoPimpleDyMFoam solver | bvieira | OpenFOAM Programming & Development | 20 | October 9, 2014 13:12 |
rhoPimpleDymFoam | jvd.mechanic | OpenFOAM Running, Solving & CFD | 0 | June 15, 2014 06:20 |
Divergence in rhoPimpleDyMFoam | bvieira | OpenFOAM Running, Solving & CFD | 1 | July 19, 2012 03:22 |