[yaqb]

Hi All!

I have a small issue witch I cannot understand - I am trying to decompose my case based on my own solver and I receive the fatal error massage

request for volScalarField T from objectRegistry region0 failed
available objects of type volScalarField are

6
(
CO2
k
IDefault
C4H6
alphaSgs
H2O
)

There must be an issue with IDefault BC, when I remove this file the decomposition takes place but without this valuable component responsible for radiative heat combustion.
The simulation runs fine without decomposition.
Do you have ideas, hints or anything what can help me to understand what does the decomposition solver wants from me?

[wyldckat]

Quick questions:

1. When you remove what specific file?
2. Can you please provide more details on what did you implement that requires a T file that does not yet exist?

Please keep in mind that we cannot see what you're seeing, so I'm not even sure what else to ask you to provide! Other than giving us a good description of what exactly you did different from the standard OpenFOAM solvers and tutorial cases.

[yaqb]

Hello wyldcat!

Thank you for you answer.
I still have not figured out what is the problem. I have made some changes in reactingFoam solver, implementing solid-fluid interaction but and it works.
The problem comes when I try to run it in parallel - than when i run decomposePar it pop up an error.
I figured out when I delete the IDefault file I can decompose the case but than I cannot run it- this is a crucial part of the solver.

I think the problem is not in the changes I made in the solver, because I have not yet even start to initiate it - rather I mix something with the BC.

Here is the IDefault file

boundaryField
{

".*"
{
type greyDiffusiveRadiation;
T T;
emissivityMode lookup;
emissivity uniform 1.0;
value uniform 0;
}
"(region0_to.*)"
{
type greyDiffusiveRadiation;
T T;
emissivityMode solidThermo;
value uniform 0;
}
}

// ************************************************** *********************** //

[wyldckat]

Hi yaqb,

Unfortunately I can't figure out what the exact problem is, because I don't know how to reproduce the same error you're getting. Please provide more details:

1. Which OpenFOAM or foam-extend version are you using?
2. What tutorial case can be used for replicating the same error you're getting?
3. What is the exact error message you're getting?
4. What were the changes you made to reactingFoam?

Best regards,Bruno

[yaqb]

Well I am using OpenFoam 2.1.1. The only thing I had changed is the pyrolysis model which I added.It is done in a simillar way to fireFoam solver. The core part stayed the same.
I came to idea that there is a problem within IDefault BC, since it is refering to Temperature field. Here is the full error message.

--> FOAM FATAL ERROR:

request for volScalarField T from objectRegistry region0 failed
available objects of type volScalarField are

7
(
CO2
k
IDefault
C4H6
mut
alphaSgs
H2O
)


From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/jakub/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 131.

FOAM aborting

I think I am missing just some small detail, or do not fully understand how does the decomposition is performed.

[wyldckat]

Hi yaqb,

OK, this is very strange... are you able to run the tutorial "combustion/fireFoam/les/smallPoolFire3D"? Because that tutorial is configured to run in parallel and if it works, then something might be broken in your case.

Best regards,
Bruno

[alexeym]

Hi,

My $0.02, since temperature field is created in thermo class (which in turn is created by reactingFoam in createField.H, there is really no T volScalarField during parallel decomposition of the case, yet decomposePar tries to evaluate boundary conditions.

To avoid the error, you can first call foundObject (http://foam.sourceforge.net/docs/cpp...85a5590fbebd84) method to check if volume field is available. If it is found, you call lookupObject and proceed as usual, if it is not found, well, it is up to you to decide what to do in this case.

[luoqinggd]

Originally Posted by alexeym

Hi,

My $0.02, since temperature field is created in thermo class (which in turn is created by reactingFoam in createField.H, there is really no T volScalarField during parallel decomposition of the case, yet decomposePar tries to evaluate boundary conditions.

To avoid the error, you can first call foundObject (http://foam.sourceforge.net/docs/cpp...85a5590fbebd84) method to check if volume field is available. If it is found, you call lookupObject and proceed as usual, if it is not found, well, it is up to you to decide what to do in this case.

Hi Alexey,

Thanks very much for your solution.

However, I still don't know how to call foundObject to avoid this problem. Can you finger out more?

not only decomposePar tries to evaluate boundary conditions, but also paraFoam. So I can run my case in single processor, but cannot in multi processor.
After I got results from single processor running, my paraFoam cannot read part of the field results.

Best regards,

Mark Luo

[PanPeter]

Hi,

This thread is a little old but I might still explain a work around to a similar case I had:
For a modified solver with a modified boundary condition, both decomposePar and paraFoam would crash with a similar error message.

Is it right that you added T as a new variable to be computed at the interface?
Both decomposePar and paraFoam execute the boundary condition, which demand a field for T and look for it in the objectRegistry. If it isn't defined there because T is added to the objectRegistry by the solver (and not by the boundary condition), your error is triggered.

To solve this, I looked into the boundary implementation and found the respective constructors called by decomposePar and paraFoam. If these constructors access the objectRegistry and demand a field for T, I first check if T is defined in the objectRegistry (what alexeym suggested). If that was not the case, I was simply not executing the initialization of the boundary and got away with it

Hope that helps,
Fynn