Divergence Detected in AMG solver- Species 0
 

Hi all,

I am using fluent 12, I am simualting flow and water gas shift reaction through a packed bed reactor. I am also using compiled UDFs for custom reaction rates and zone specific diffusivities.

For testing I run the simulation on my windows 7 PC first, initially with reactions off and product species equations off, to get a converged coldflow result before enabling reactions and product equations, then iterate to get a steady converged soloution, before going on to do various unsteady calculations.

Using this same case file, and a Text journal, i intend to do exactly the same procedure but more in depth on my universities Parallel computer, which is Itanium 64 architecture, however, even though there are no problems on the Windows computer, the output text file from the console indicates that even before the first iteration is copleted, that there is:

Divergence in the AMG solver- species-0

Then it just hangs


I have tried reducing the under relaxation factors for the species, though the error still remains.

Any suggestions would be most welcome.

Thanks

Also, when i cange the pressure velocity coupling from simple to coupled its no longer says anything about divergence error, however the porous regions, which have fixed values of velocity set to 0, then dont obey the fixed values rule, it appears as though its an empty cylinder

Michael

Hi,
Try this:

In multigrid solver, change the method for species0 to F cycle, with stabilization.

Good Luck

Ok But...
 

Hi Steven,

Thanks for your reply.

I did try what you said with the f-cycle and bcgstab method, but it then said there was divergence in species 3(species 1 and 2 eqs are turned off), so i did the same for species 3, but then it said there was divergence in temperature/energy, so i did the same for it, though when i did that it just gave out this error:

Error: > (greater-than): invalid argument [2]: wrong type [not a number]
Error Object: 1.#qnan

I have no real idea what this is about except that it might be something to do with the UDF i am using for having different regions of diffusivity.

Any ideas?

Thanks

Michael

Steven, i also unloaded the UDF library, but the error:


Error: > (greater-than): invalid argument [2]: wrong type [not a number]
Error Object: 1.#qnan

Still occurs, so it mustnt have anything to do with the UDF

Hi,

If the source/sink term is very big due to the chemical reaction in your species transport equation. You should use the implicit formualtion for it to stabilize your calculation.

Yes, ok
 

Ok Steven I will try that, though the reaction rate is specified as a volumetric reaction, occuring only in the porous zones, I.e. The catalyst particles
the rate equation is defined through a compiled udf. The rate is only of the order of 2e-2 kgmol/m3s and is only moldy exothermic.

But yes, I will try the implicit method as you suggested, then get back to you, thanks again.

I will also try a bit more in depth Reading of the solver user and theory section.

Got it sorted!!!
 

Yo Steven, i got it sorted, the error with the Temp was caused by the residual being too small for single precision solver, run in double precision

Set F-cycle with stabalisation for the species and then it works fine


Thanks for your assistance

thanks
 

thank you very much Michael. you really help me:)

cheers azedeh, glad the soloutions to my problems could be of help to someone

hi

I have ever meet this kind of problem。
At begining, I stop the calculation of all specie equations and energy euqation， after some iterations，turn on those equations。And no divergence detected anymore. good luck to you!

depan

error :divergence detected in AMG solver
 

Good post really. It had solved my problem

Great!
 

Great stuff, its good to know im not the only one having trouble, and that if we talk about it there may be ways to solve it.

hey thread owner and all ppl replied thanks a lot .. it helped me too ... Changing the multigrid options to "F cycle" and BCG STAB .. does remove the erro but in the residual for the "H2O" i get this - "1.#QNBe+00" for all iterations
What does that mean ??

heat tranfer between phases
 

hi,

I am simulating coal combustion with E-E model (gas-solid). when I am calculating without heat tranfer between phases it works fine but with gunn model it gives problem like 'temperature limited 5000'.
do you have any idea?

thanks in advance!

The UDFs that work for a serial calculation does not necessarily work for parallel calculations. And while you use a cluster or a multi-core computer for parallel calculations the method used to partition the mesh also plays significant role in how the calculation takes place.

I recommend you to do all your calculations in the cluster. Also make sure that you modify your UDF in order to make it compatible for parallel process.

Also some macros in UDFs rely on the initial values of variables. To avoid this you could initialize your case (hybrid initialization is a smart choice), hook the UDF and then continue calculations.

thanks for the answer!But I am using 12.1 version and I am not using parallel option now. so I think in this version there is no option like hybrid in init.

do you have any other advise!

thanks again!

hi,

are you working on gasification?
can you can tell me what is the Cp,thermal conductivity,molecular weight, standard state enthalpy and entropy properties for coal. I know that it differs for every type of coal but Can you give me a referance for that?

thanks in advance!

Hello guys,
i am having similar problem, I am working on combustion of CH4 in an ion transport membrane, when i tried the cold cases, it converged but as soon as i activated the volumetric, there is divergence, i have errors like:

temperature limited to 1.000000e+000 in 4 cells on zone 2 in domain 1
temperature limited to 1.000000e+000 in 4 cells on zone 2 in domain 1
temperature limited to 5.000000e+003 in 2759 cells on zone 2 in domain 1
temperature limited to 1.000000e+000 in 832 cells on zone 3 in domain 1
temperature limited to 5.000000e+003 in 1161 cells on zone 3 in domain 1

absolute pressure limited to 1.0000+000 in 448 cells on zone 2
absolute pressure limited to 1.0000+000 in 291 cells on zone 3
absolute pressure limited to 5.0000+010 in 1 cells on zone 3

Error: Floating point error: invalid number

Error Object: ()

kindly help me out, i still have a long way to go in my thesis

Hi I am using the chemkin for getting the autoignition for nheptane mixture:
for mixture heptane/N2/O2/AR: 0.562/58/30/10 mole fraction ratio

But unable to do it by any method .. I set the initial T=766K and Presuree= 14.1 bar

1. I tried the laminar rate- it showing error : flat Temp profile
2. If I check ISAT i gett some error about tbadhi