
[Sponsors] 
January 18, 2006, 10:05 
Hi,
does someone know how t

#1 
Member
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 9 
Hi,
does someone know how to solve "time step continuity errors" ?? Thanks a lot, Anja 

January 18, 2006, 10:23 
How big are they? They are rel

#2 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22 
How big are they? They are related to the pressure solver tolerance and you should be able to squeeze them by converging the pressure more tightly. If this doesn't work, you've probably messed up the boundary conditions.
Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

January 18, 2006, 10:36 
For example:
time step contin

#3 
Member
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 9 
For example:
time step continuity errors : sum local = 1.05535e08, global = 1.65393e14, cumulative = 9.944e11 What exactly do you mean by converging the pressure more tightly? Anja 

January 18, 2006, 10:41 
This does not worry me at all:

#4 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22 
This does not worry me at all: it says your global continuity error is 1e14, which is the double precision roundoff error, the sum local tells me that in the line above your pressure solver has converged to about 1e8; in other words, all is well.
Nothing to worry about here. Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

January 18, 2006, 10:49 
Okay then.
I was searching

#5 
Member
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 9 
Okay then.
I was searching a reason for the very long duration time of the calculation, which I have just launched. Every single time step takes around 10 minutes and before I didn't get an error message for this case. I try to calculate an incompressible, laminar flow through a sshaped tube. Anja 

January 19, 2006, 05:22 
Hi Anja,
It sounds to me as

#6 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22 
Hi Anja,
It sounds to me as if you need to tune the solver. For a steadystate laminar flow, I would use simpleFoam with the "laminar" turbulence model. You can then play around with underrelaxation factors, convergence parameters and discretisation to get a decent result. 10 mins per iteration is massively too much, unless you're trying to do a couple of million cells of a singleCPU machine. Is your mesh hexahedral or tetrahedral or mixed? How many cells, any problems reported by checkMesh? Do you have some fancy boundary conditions? Which solver are you using? Can you post the output from a single iteration (the one that takes 10 mins)  I'll have a look and see if there's somethign obvious I can suggest. Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

January 20, 2006, 07:59 
The mesh consists of 386106 he

#7 
Member
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 9 
The mesh consists of 386106 hexahedral cells.
Not one problem was reported by checkMesh. The boundary conditions are: wall; physicalType wall; p=zeroGradient; U=0 0 0 inlet;physicalType inlet; p=zeroGradient; U=4 0 0 outlet;physicalType outlet; p=0; U=zeroGradient I used icoFoam. Time = 0.0002 Mean and max Courant Numbers = 0.0186142 0.789515 BICCG: Solving for Ux, Initial residual = 0.403172, Final residual = 1.85342e06, No Iterations 3 BICCG: Solving for Uy, Initial residual = 0.334868, Final residual = 5.72366e07, No Iterations 3 BICCG: Solving for Uz, Initial residual = 0.30369, Final residual = 1.64811e06, No Iterations 3 ICCG: Solving for p, Initial residual = 0.0138496, Final residual = 9.63037e07, No Iterations 851 ICCG: Solving for p, Initial residual = 0.128861, Final residual = 9.18745e07, No Iterations 858 ICCG: Solving for p, Initial residual = 0.0693657, Final residual = 9.58556e07, No Iterations 849 time step continuity errors : sum local = 1.16673e07, global = 1.2324e10, cumulative = 8.26334e11 ICCG: Solving for p, Initial residual = 0.0237425, Final residual = 8.75212e07, No Iterations 855 ICCG: Solving for p, Initial residual = 0.164026, Final residual = 8.78886e07, No Iterations 856 ICCG: Solving for p, Initial residual = 0.0716675, Final residual = 9.91469e07, No Iterations 850 time step continuity errors : sum local = 2.52566e08, global = 1.38281e12, cumulative = 8.12506e11 ExecutionTime = 641.55 s It would be really great, if you could help me. Anja 

January 20, 2006, 08:23 
Hehe, a perfect candidate :)

#8 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22 
Hehe, a perfect candidate :)
The time of simulation is all spent in the pressure solver, which is doing way too many iterations (6 times 800). Secondly, it looks like the nonorthogonal pressure correctors are not converging and PISO is not too happy either. Try the following:  use the AMG solver on the pressure  try changing the discretisation of the pressure laplacian from Gauss linear corrected to Gauss linear limited  reduce the number of nonorthogonal correctors to 1  run checkMesh and report the nonorthogonality problems it reports (is the mesh really that bad?). This should be relatively easy to fix. Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

January 20, 2006, 09:10 
I can't find a tutorial using

#9 
Member
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 9 
I can't find a tutorial using the AMG solver.
What about: AMG 1e06 0 0 ?? And for the laplacian scheme: Gauss linear limited 1 ?? Concerning the checkMesh: Mesh nonorthogonality Max: 39.6288 average: 8.72216 Nonorthogonality check OK. 

January 20, 2006, 09:24 
Try:
Gauss linear limited 1

#10 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22 
Try:
Gauss linear limited 1; p AMG 1e06 0 100; (the last number is the number of equations on the top level) The mesh is good, looks like the CG is struggling a bit. I am really interested, please let me know if the AMG helps. Are you running on one CPU or in parallel? Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

January 20, 2006, 09:38 
Gauss linear limited 1;
s

#11 
Member
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 9 
Gauss linear limited 1;
solvers p AMG 1e06 0 100; U BICCG 1e05 0; PISO //momentumPredictor yes; nCorrectors 2; nNonOrthogonalCorrectors 0; //pRefCell 0; //pRefValue 0; //fluxGradp yes; (These // I also had before, but now it's only nCorrectors; nNonOrthogonalCorrectors) Here some excerpts: Time = 0.0003; ExecutionTime = 258.17 s Time = 0.0005; ExecutionTime = 378.72 s Time = 0.0008; ExecutionTime = 547.68 s What do you think? 

January 20, 2006, 14:16 
Better, huh? :)
How much w

#12 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22 
Better, huh? :)
How much work does the AMG do? I think you're in business now... Good luck, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

May 11, 2006, 07:50 
Hello!
I have had the same

#13 
Guest
Posts: n/a

Hello!
I have had the same problem as mentioned above, with many pressure itterations, but have had higher sum local and global values (about e4). The print out looks like the following for a time step: Time = 0.1 BICCG: Solving for Ux, Initial residual = 1, Final residual = 0.0164738, No Iterations 1 BICCG: Solving for Uy, Initial residual = 1, Final residual = 0.0138657, No Iterations 1 BICCG: Solving for Uz, Initial residual = 1, Final residual = 0.00943703, No Iterations 1 ICCG: Solving for p, Initial residual = 1, Final residual = 0.0871697, No Iterations 2223 time step continuity errors : sum local = 0.000278016, global = 1.48514e06, cumulative = 1.48514e06 BICCG: Solving for epsilon, Initial residual = 1, Final residual = 0.0117474, No Iterations 1 BICCG: Solving for k, Initial residual = 1, Final residual = 0.000467489, No Iterations 1 Creating alphaEff. BICCG: Solving for T, Initial residual = 1, Final residual = 0.0442807, No Iterations 43 ExecutionTime = 65.31 s Then I tried to modify it like it is said above and get the following print out (i.e. higher sum local and global values): Time = 0.1 BICCG: Solving for Ux, Initial residual = 1, Final residual = 0.0164738, No Iterations 1 BICCG: Solving for Uy, Initial residual = 1, Final residual = 0.0138657, No Iterations 1 BICCG: Solving for Uz, Initial residual = 1, Final residual = 0.00943703, No Iterations 1 AMG: Solving for p, Initial residual = 1, Final residual = 2.66915, No Iterations 501 AMG: Solving for p, Initial residual = 0.416487, Final residual = 0.342388, No Iterations 501 time step continuity errors : sum local = 0.0087574, global = 8.70409e05, cumulative = 8.70409e05 BICCG: Solving for epsilon, Initial residual = 1, Final residual = 0.011749, No Iterations 1 BICCG: Solving for k, Initial residual = 1, Final residual = 0.000470466, No Iterations 1 Creating alphaEff. BICCG: Solving for T, Initial residual = 1, Final residual = 0.0710206, No Iterations 43 BICCG: Solving for T, Initial residual = 0.0572284, Final residual = 0.00546826, No Iterations 29 ExecutionTime = 101.47 s I have also checked the mesh and the only thing wrong with it was that trere were 4 points that wasn't in use and put into an according file. But stil I have to many itterations for the pressure. Thankfull for help /Erik 

March 7, 2007, 08:37 
Hello.
I also have a problem

#14 
New Member
Holger Putz
Join Date: Mar 2009
Posts: 5
Rep Power: 9 
Hello.
I also have a problem with these continuity errors. I am running a modified simpleFoam case, where a liquid is streaming through a small cylinder into a bigger one, driven by the bodyforce and an inletvelocity. The time step continuity errors are rising, and after 10 iterations they are about 10^11. When I run the same case without the small inletcylinder, everything is fine and the error is about 10^9. also when I take the mesh with the small cylinder, but set g=0m/sē the error stays small. I have allready tried a lot of combinations for solvers, bc and relaxation factors. my mesh has about 1.2million cells. do you have any suggestions? hoping for your help, 

March 7, 2007, 08:45 
Yes. Check your boundary cond

#15 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22 
Yes. Check your boundary condition on that additional inlet. My guess is that you have specified both the pressure and the velocity at the boundary, which will give you a continuity error.
Let me know, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

March 7, 2007, 09:07 
Thank you for your quick reply

#16 
New Member
Holger Putz
Join Date: Mar 2009
Posts: 5
Rep Power: 9 
Thank you for your quick reply.
I have checked, but at the inlet (there is only one at the top of the smaller cylinder) I have only specified the velocity with 0.1m/s. pressure is fixed gradient because the bc is only inlet. Maybe there is a missunderstanding on my side. greetings, Holger 

March 7, 2007, 09:13 
Yup. Put zero gradient on the

#17 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22 
Yup. Put zero gradient on the pressure and the continuity error will go away. The fixed gradient b.c. gives you additional flux which is not accounted for in the continuity equation.
Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

March 7, 2007, 09:36 
I'm sorry. I meant zero gradie

#18 
New Member
Holger Putz
Join Date: Mar 2009
Posts: 5
Rep Power: 9 
I'm sorry. I meant zero gradient. the top of the small cylinder has p zero gradient.
what I am really wondering about is that everything works when I take away the small one and take the top of the big cylinder as an inlet. I have simulated several other geometries with this modified simpleFoam solver, but this is the only one where I get an error. 

March 8, 2007, 03:54 
I now created a inlet on the

#19 
New Member
Holger Putz
Join Date: Mar 2009
Posts: 5
Rep Power: 9 
I now created a inlet on the top of the big cylinder and took the small cylinder away. But these big continuity errors stay. and now, after the 6 iteration the simulation just stops. there is no errormessage, its just doing nothing. is there any connection between the number of cells included in the inlet and the continuity error?
ErrorLog: Create mesh for time = 0 Reading environmentalProperties Reading field p Reading field U Reading transportProperties Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting turbulence model laminar Starting time loop Time = 1 BICCG: Solving for Ux, Initial residual = 1, Final residual = 0.0191738, No Ite rations 2 BICCG: Solving for Uy, Initial residual = 1, Final residual = 0.0230878, No Ite rations 2 BICCG: Solving for Uz, Initial residual = 1, Final residual = 0.0119195, No Ite rations 2 AMG: Solving for p, Initial residual = 1, Final residual = 0.0210672, No Iterat ions 5 AMG: Solving for p, Initial residual = 0.151581, Final residual = 0.00186491, N o Iterations 2 AMG: Solving for p, Initial residual = 0.0159399, Final residual = 0.000486127, No Iterations 2 AMG: Solving for p, Initial residual = 0.00352732, Final residual = 0.000146953, No Iterations 2 time step continuity errors : sum local = 0.235539, global = 0.0450524, cumulative = 0.0450524 ExecutionTime = 78.6 s ClockTime = 78 s . . . . Time = 5 BICCG: Solving for Ux, Initial residual = 0.327544, Final residual = 0.00769073 BICCG: Solving for Uy, Initial residual = 0.378132, Final residual = 0.0157606, BICCG: Solving for Uz, Initial residual = 0.330114, Final residual = 0.0149679, AMG: Solving for p, Initial residual = 0.479773, Final residual = 0.0159471, No AMG: Solving for p, Initial residual = 0.846998, Final residual = 0.00354764, N AMG: Solving for p, Initial residual = 0.137398, Final residual = 0.00187623, N AMG: Solving for p, Initial residual = 0.0499261, Final residual = 0.00105473, time step continuity errors : sum local = 9.61023, global = 3.38102, cumulative ExecutionTime = 390.55 s ClockTime = 391 s Time = 6 BICCG: Solving for Ux, Initial residual = 0.284414, Final residual = 0.0203337, BICCG: Solving for Uy, Initial residual = 0.318962, Final residual = 0.0192187, BICCG: Solving for Uz, Initial residual = 0.315278, Final residual = 0.0149193, New Geometry greetings, Holger 

July 10, 2007, 14:17 
hi all,
a the title said ....

#20 
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 187
Rep Power: 9 
hi all,
a the title said .... I've got also a time step continuity errors ...following with > FOAM FATAL IO ERROR : IOstream::check(const char* operation) : error in IOstream for operation Ostream& operator<<(Ostream&, const Scalar&) From function IOstream::check(const char* operation) const in file db/IOstreams/IOstreams/IOcheck.C at line 54. well ... Foam is very talkative this evening. So, I checked my mesh, Nonorthogonality check OK. I changed my solver on the pressure to AMG (with same caracteristic as upper message) and then, ...It hasn't changed anything: Mean and max Courant Numbers = 0 0.0488421 Updating boundary gradient of U::outlet by Euler and normal schemes Saving oldtime boundary values of U::outlet Boundary gradient of U::outlet has already been updated Boundary gradient of U::outlet has already been updated BICCG: Solving for Ux, Initial residual = 1, Final residual = 2.872e07, No Iterations 1 BICCG: Solving for Uy, Initial residual = 1, Final residual = 2.87335e07, No Iterations 1 BICCG: Solving for Uz, Initial residual = 1, Final residual = 5.11098e07, No Iterations 1 AMG: Solving for p, Initial residual = 1, Final residual = 0.502698, No Iterations 501 time step continuity errors : sum local = 7.44298e06, global = 1.76024e08, cumulative = 1.76024e08 Updating boundary gradient of U::outlet by Euler and normal schemes AMG: Solving for p, Initial residual = 0.000116257, Final residual = 6.94937e05, No Iterations 501 time step continuity errors : sum local = 8.05415e06, global = 1.43586e11, cumulative = 1.7588e08 Updating boundary gradient of U::outlet by Euler and normal schemes PS: I created my mesh with BlockMesh, using only hexa and, CheckMesh found 4 tetra mesh, it's quite strange, isn't ? any ideas of what else I can check to solve this ...very small problem? thanks, Cedric 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
SimpleFoam and Time Step continuity errors  philippose  OpenFOAM Running, Solving & CFD  56  February 21, 2016 06:44 
Time step size and max iterations per time step  pUl  FLUENT  31  August 21, 2015 04:46 
SELECTING TIME STEP SIZE, NUMBER OF TIME STEP  NITUL KALITA  FLUENT  2  November 22, 2012 09:28 
Long time CHT transient simulation time step....  JP  CFX  0  May 9, 2008 03:36 
Relation of computational time step with real time  Salman  Main CFD Forum  2  August 3, 2005 14:13 