|
[Sponsors] |
customized reactingFoam: DecomposePar fatal error |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
July 31, 2015, 16:49 |
customized reactingFoam: DecomposePar fatal error
|
#1 |
New Member
Jacopo
Join Date: Mar 2013
Location: Italy
Posts: 18
Rep Power: 13 |
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? |
|
August 10, 2015, 10:26 |
|
#2 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Quick questions:
|
|
September 7, 2015, 12:25 |
|
#3 |
New Member
Jacopo
Join Date: Mar 2013
Location: Italy
Posts: 18
Rep Power: 13 |
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; } } // ************************************************** *********************** // |
|
September 7, 2015, 19:25 |
|
#4 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
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:
__________________
|
|
September 8, 2015, 10:21 |
|
#5 |
New Member
Jacopo
Join Date: Mar 2013
Location: Italy
Posts: 18
Rep Power: 13 |
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. |
|
September 12, 2015, 17:40 |
|
#6 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
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 |
|
September 13, 2015, 05:30 |
|
#7 |
Senior Member
|
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. |
|
September 5, 2016, 07:37 |
|
#8 | |
New Member
lawching
Join Date: May 2016
Posts: 1
Rep Power: 0 |
Quote:
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 |
||
April 18, 2017, 05:46 |
|
#9 |
Member
Fynn
Join Date: Feb 2016
Posts: 48
Rep Power: 10 |
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 |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[OpenFOAM] an error in Calculator's equation | immortality | ParaView | 12 | June 29, 2021 01:10 |
Problem running perturbUCyl | sen.1986 | OpenFOAM | 17 | June 4, 2019 06:56 |
error compiling modified applications | yvyan | OpenFOAM Programming & Development | 21 | March 1, 2016 05:53 |
[OpenFOAM.org] Compile OF 2.3 on Mac OS X .... the patch | gschaider | OpenFOAM Installation | 225 | August 25, 2015 20:43 |
Errors in UDF | shashank312 | Fluent UDF and Scheme Programming | 6 | May 30, 2013 21:30 |