CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Divergence Detected in AMG solver- Species 0 (http://www.cfd-online.com/Forums/fluent/78160-divergence-detected-amg-solver-species-0-a.html)

elmcmaster July 14, 2010 07:41

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

chaozhong.qin July 15, 2010 15:49

Hi,
Try this:

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

Good Luck

elmcmaster July 16, 2010 07:24

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

elmcmaster July 16, 2010 07:37

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

chaozhong.qin July 16, 2010 09:01

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.

elmcmaster July 16, 2010 09:45

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.

elmcmaster July 19, 2010 10:00

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

azadeh October 10, 2010 03:59

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

elmcmaster October 11, 2010 04:28

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

whtrs October 11, 2010 10:23

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

eegala April 12, 2011 02:08

error :divergence detected in AMG solver
 
Good post really. It had solved my problem

elmcmaster April 13, 2011 03:58

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.

Abhya March 10, 2013 10:22

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 ??

Kanarya April 17, 2013 07:31

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!
Quote:

Originally Posted by Abhya (Post 412937)
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 ??


vasava April 17, 2013 08:04

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.

vasava April 17, 2013 08:08

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.

Kanarya April 17, 2013 09:14

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!
Quote:

Originally Posted by vasava (Post 421215)
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.


Kanarya April 17, 2013 10:21

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!
Quote:

Originally Posted by vasava (Post 421215)
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.



All times are GMT -4. The time now is 18:48.