CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Pre-Processing

viewFactorsGen crashes

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By Rojj

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 8, 2016, 15:09
Default viewFactorsGen crashes
  #1
New Member
 
Serban Georgescu
Join Date: Sep 2011
Posts: 2
Rep Power: 0
gserban is on a distinguished road
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
Attached Files
File Type: zip finalAgglom.zip (5.6 KB, 12 views)
File Type: zip viewFactorsDict.zip (549 Bytes, 15 views)
gserban is offline   Reply With Quote

Old   April 1, 2016, 13:07
Default
  #2
Member
 
Ruggiero Guida
Join Date: Apr 2013
Location: World
Posts: 41
Rep Power: 9
Rojj is on a distinguished road
Hi Gserban,

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

Thanks
Rojj is offline   Reply With Quote

Old   April 2, 2016, 01:18
Default
  #3
New Member
 
Serban Georgescu
Join Date: Sep 2011
Posts: 2
Rep Power: 0
gserban is on a distinguished road
Hi Rojj,

Unfortunately not, still stuck at this stage

Serban
gserban is offline   Reply With Quote

Old   April 2, 2016, 02:12
Default
  #4
Senior Member
 
Derek Mitchell
Join Date: Mar 2014
Location: UK, Reading
Posts: 163
Rep Power: 9
derekm is on a distinguished road
have you tried increasing the number of coarse faces for the patches in viewFactors.dict?
__________________
A CHEERING BAND OF FRIENDLY ELVES CARRY THE CONQUERING ADVENTURER OFF INTO THE SUNSET
derekm is offline   Reply With Quote

Old   April 2, 2016, 06:08
Default
  #5
Member
 
Ruggiero Guida
Join Date: Apr 2013
Location: World
Posts: 41
Rep Power: 9
Rojj is on a distinguished road
The problem was probably related to maxDynListLength. I recompiled as suggested here.

It seems to work now
MatteoQ likes this.
Rojj is offline   Reply With Quote

Old   June 26, 2019, 10:37
Default
  #6
New Member
 
Matteo Quirino
Join Date: Feb 2019
Posts: 4
Rep Power: 3
MatteoQ is on a distinguished road
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?
MatteoQ is offline   Reply With Quote

Old   August 6, 2019, 06:02
Default
  #7
Senior Member
 
Raza Javed
Join Date: Apr 2019
Location: Germany
Posts: 183
Rep Power: 3
Raza Javed is on a distinguished road
Quote:
Originally Posted by gserban View Post
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 :


Code:
--> 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
Raza Javed is offline   Reply With Quote

Old   August 6, 2019, 12:26
Default
  #8
Member
 
Ruggiero Guida
Join Date: Apr 2013
Location: World
Posts: 41
Rep Power: 9
Rojj is on a distinguished road
Quote:
Originally Posted by Raza Javed View Post
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 :


Code:
--> 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
Rojj is offline   Reply With Quote

Old   June 23, 2020, 21:27
Default
  #9
Senior Member
 
Join Date: Nov 2010
Location: USA
Posts: 1,228
Rep Power: 20
me3840 is on a distinguished road
Quote:
Originally Posted by MatteoQ View Post
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:

Code:
const word viewFactorWall("viewFactorWall");

Which seems very peculiar until you read the header:


Code:
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!
me3840 is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
potentialFoam & simpleFoam crashes after snappyhexmesh [parallel execution] pilot320 OpenFOAM Running, Solving & CFD 10 November 12, 2015 16:56
reactingFoam crashes mysteriously jose_rodrig OpenFOAM Running, Solving & CFD 9 August 4, 2015 10:18
Simulation crashes early, crashes hard... MtnRunBeachBum OpenFOAM Running, Solving & CFD 6 April 22, 2015 09:27
HELP!!! viewFactorsGen is not calculating view factors!! zfaraday OpenFOAM Pre-Processing 0 September 15, 2014 08:55
flo-efd v11.0.0 crashes YoavF FloEFD, FloWorks & FloTHERM 3 June 21, 2012 12:37


All times are GMT -4. The time now is 06:49.