[gserban]

Hello everyone,

I am trying to add radiation to a conjugate heat transfer simulation (chtMultiRegionSimpleFoam solver) in OF 2.4.0.
Following the tutorials, I've defined my viewFactorsDict for the two fluid regions that I have have and executed faceAgglomerate command on them.

faceAgglomerate generated "finalAgglom" files in the constant directory for each region, so I guess that part went OK.

Folowing, I ran viewFactorsGen for both fluid regions, but for one of them it crashes with the following message:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.4.0-dcea1e13ff76
Exec : viewFactorsGen -region default_fluid
Date : Jan 08 2016
Time : 17:40:48
Host : "bx900-head"
PID : 10741
Case : /work1/serban/OpenFOAM/phone-rad
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh default_fluid for time = 0


Total number of coarse faces: 0
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigSegv::sigHandler(int) at ??:?
#2 ? in "/lib64/libc.so.6"
#3 ? at ??:?
#4 ? at ??:?
#5 __libc_start_main in "/lib64/libc.so.6"
#6 ? at ??:?
Segmentation fault (core dumped)

I am not sure what I did wrong ... the finalAgglom files looks sensible, so I am currently stuck.
Could someone give me a pointer in the right direction?

Thank you in advance,
Serban

[Rojj]

Hi Gserban,

did you manage to solve this problem? I am having the same issue.

Thanks

[gserban]

Hi Rojj,

Unfortunately not, still stuck at this stage

Serban

[derekm]

have you tried increasing the number of coarse faces for the patches in viewFactors.dict?

[Rojj]

The problem was probably related to maxDynListLength. I recompiled as suggested here.

It seems to work now

[MatteoQ]

Hi Rojj,

I am having the exact same error as posted by Gserban. FaceAgglomerate runs fine, but one region reports that "Total number of coarse faces= 0". I don't understand why.

I raised maxDynListLength up to 1e10, still that bloody region output that it has number of coarse faces = 0.


Did you just raise the number in maxDynListLength or did you do something else?

[Raza Javed]

Originally Posted by gserban

Hello everyone,

I am trying to add radiation to a conjugate heat transfer simulation (chtMultiRegionSimpleFoam solver) in OF 2.4.0.
Following the tutorials, I've defined my viewFactorsDict for the two fluid regions that I have have and executed faceAgglomerate command on them.

faceAgglomerate generated "finalAgglom" files in the constant directory for each region, so I guess that part went OK.

Folowing, I ran viewFactorsGen for both fluid regions, but for one of them it crashes with the following message:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.4.0-dcea1e13ff76
Exec : viewFactorsGen -region default_fluid
Date : Jan 08 2016
Time : 17:40:48
Host : "bx900-head"
PID : 10741
Case : /work1/serban/OpenFOAM/phone-rad
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh default_fluid for time = 0


Total number of coarse faces: 0
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigSegv::sigHandler(int) at ??:?
#2 ? in "/lib64/libc.so.6"
#3 ? at ??:?
#4 ? at ??:?
#5 __libc_start_main in "/lib64/libc.so.6"
#6 ? at ??:?
Segmentation fault (core dumped)

I am not sure what I did wrong ... the finalAgglom files looks sensible, so I am currently stuck.
Could someone give me a pointer in the right direction?

Thank you in advance,
Serban

Hi..


I have one question here regarding viewFactorsDict, how we can decide the values for 'nFacesInCoarsestLevel' and 'featureAngle'?


As I am new to radiation models, When I RUN faceAgglomerate and viewFactorsGen, i get the following error :

--> FOAM FATAL IO ERROR: 
cannot open file

file: /home/openfoam/run/radiation_box/constant/viewFactorsDict at line 0.

    From function regIOobject::readStream()
    in file db/regIOobject/regIOobjectRead.C at line 86.

FOAM exiting

And I am wondering that how can I get this file?


I shall be thankful if you can help me in this.


Thank you

[Rojj]

Originally Posted by Raza Javed

Hi..


I have one question here regarding viewFactorsDict, how we can decide the values for 'nFacesInCoarsestLevel' and 'featureAngle'?


As I am new to radiation models, When I RUN faceAgglomerate and viewFactorsGen, i get the following error :

--> FOAM FATAL IO ERROR: 
cannot open file

file: /home/openfoam/run/radiation_box/constant/viewFactorsDict at line 0.

    From function regIOobject::readStream()
    in file db/regIOobject/regIOobjectRead.C at line 86.

FOAM exiting

And I am wondering that how can I get this file?


I shall be thankful if you can help me in this.


Thank you

If you are looking for a sample dict file, I usually find very useful to look at the OF github repository directly. For example for viewFactorsDict I would search for

https://github.com/OpenFOAM/OpenFOAM...iewFactorsDict

Assuming you are on OF6

[me3840]

Originally Posted by MatteoQ

Hi Rojj,

I am having the exact same error as posted by Gserban. FaceAgglomerate runs fine, but one region reports that "Total number of coarse faces= 0". I don't understand why.

I raised maxDynListLength up to 1e10, still that bloody region output that it has number of coarse faces = 0.


Did you just raise the number in maxDynListLength or did you do something else?

I know this thread is old, but I wanted to post here as I also had the problem specified by MatteoQ. I did not get a segfault, but still got the message "Total number of coarse faces = 0". It turns out if you read the source code for viewFactorsGen.C, it loops over the boundary patches that are obtained by looking for a specific keyword:

const word viewFactorWall("viewFactorWall");

Which seems very peculiar until you read the header:

Description
    View factors are calculated based on a face agglomeration array
    (finalAgglom generated by faceAgglomerate utility).

    Each view factor between the agglomerated faces i and j (Fij) is calculated
    using a double integral of the sub-areas composing the agglomeration.

    The patches involved in the view factor calculation are taken from the
    boundary file and should be part on the group viewFactorWall. ie.:

    floor
    {
        type            wall;
        inGroups        2(wall viewFactorWall);
        nFaces          100;
        startFace       3100;
    }

So you need to add in the viewFactorWall group to any patch you wish view factors to be calculated on!

[B_R_Khan]

Originally Posted by MatteoQ

Hi Rojj,

I am having the exact same error as posted by Gserban. FaceAgglomerate runs fine, but one region reports that "Total number of coarse faces= 0". I don't understand why.

I raised maxDynListLength up to 1e10, still that bloody region output that it has number of coarse faces = 0.


Did you just raise the number in maxDynListLength or did you do something else?

I am having the exact problem

Edit: Ok just saw this problem is addressed in this thread
Thanks!