|
[Sponsors] |
Problem in reading fvOptions for chtMultiRegionFoam |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
December 1, 2018, 20:44 |
Problem in reading fvOptions for chtMultiRegionFoam
|
#1 |
New Member
Kyriakos Paso
Join Date: Nov 2018
Posts: 20
Rep Power: 7 |
Hello.
I have a domain that i want to split it in air region and solid region. I did it with topoSet and splitMeshRegion -cellzones -overwrite. Inside the air region i've got a porous medium, which i define it in another topoSetDict (cellToZone) without splitMeshRegions. I imported the source term of the porous media by using fvOptions, but when i run the chtMultiRegionFoam, i got the message shown in the image. Why doesn'i it read the porous zone? 47213061_304556510170052_5963947696954802176_n.png |
|
December 2, 2018, 01:12 |
|
#2 |
Member
Hussam
Join Date: Aug 2017
Location: Germany
Posts: 32
Rep Power: 8 |
Hey Kyriakos,
Can you upload your fvOptions, topoSetDict, and the cellZones located in constant/air/polyMesh. Obviously you have a cellZone called "inside".. May be you didn't change the name in topoSetDict. Cheers! |
|
December 2, 2018, 11:01 |
Problem in reading fvOptions for chtMultiRegionFoam
|
#3 |
New Member
Kyriakos Paso
Join Date: Nov 2018
Posts: 20
Rep Power: 7 |
Hello tobiasS.
I forgot to write that the inside cellZone is my solid. I attach the fvOptions, toposetDict1 which splits the domain in the air and the inside(solid), and the topoSetDIct where I define my porous media cellZone. I also attach the cellZones located in constant/air/polyMesh. |
|
December 2, 2018, 11:20 |
|
#4 |
Member
Hussam
Join Date: Aug 2017
Location: Germany
Posts: 32
Rep Power: 8 |
Hey Kyriakos,
For some reason topoSet didn't create "porousBlockage".Would you check the log file of the topoSet process, or share it also here? |
|
December 2, 2018, 11:44 |
|
#5 |
New Member
Kyriakos Paso
Join Date: Nov 2018
Posts: 20
Rep Power: 7 |
Hey tobiasS.
Where can I find the log file? In addition, when i open the paraFoam, the porousBlockage zone has been created. |
|
December 2, 2018, 11:56 |
|
#6 |
Member
Hussam
Join Date: Aug 2017
Location: Germany
Posts: 32
Rep Power: 8 |
The file isn't generated automatically.. But normally I send the information of such processes to log file like:
topoSet -dict topoSetDict1 > topoSet.log 2>&1 & Then you can read the file topoSet. log anytime you want. I don't know how it's possible that paraview sees a cellZone called "porousBlockage" in the region "air" although the cellZone file don't say so. But here is a question: did you use the option "- region air" in your topoSet process? If not, the region will be created in the old constant/polyMesh.. You can check the constant/polyMesh/cellZones to proof that. |
|
December 2, 2018, 11:58 |
|
#7 |
Member
Hussam
Join Date: Aug 2017
Location: Germany
Posts: 32
Rep Power: 8 |
P. S. If you will use "- region air" option you have to place your topoSetDict in system/air instead of system
|
|
December 2, 2018, 12:07 |
|
#8 |
New Member
Kyriakos Paso
Join Date: Nov 2018
Posts: 20
Rep Power: 7 |
Yes, I have tried to place it in system/air, and in system, but the problem remains.
Moreover, the fvOptions is placed in constant/air |
|
December 2, 2018, 12:27 |
|
#9 |
New Member
Kyriakos Paso
Join Date: Nov 2018
Posts: 20
Rep Power: 7 |
Yes you are right. In the constant/polyMesh/cellZones the porousBlockage it is created. But I run it through topoSet -dict system/air/topoSetDict.
How should i run it? |
|
December 2, 2018, 14:41 |
|
#10 |
Member
Hussam
Join Date: Aug 2017
Location: Germany
Posts: 32
Rep Power: 8 |
topoSet - region air > topoSet.log 2>&1 &
|
|
December 2, 2018, 14:48 |
|
#11 |
Member
Hussam
Join Date: Aug 2017
Location: Germany
Posts: 32
Rep Power: 8 |
In this case openfoam will search for the dict in system/air so you don't need to specify system/air.. Only the name of the file placed in system/air is enough.
There is an alternative solution: you can delete your constant/polyMesh or move it to another name like constant/polyMesh.old and then move the constant/air/polyMesh to constant/polyMesh.. So you don't need to use the "-region". In this case you need only to move the polyMesh back to system/air/polyMesh after successfully creating the cellZone. |
|
December 2, 2018, 18:37 |
|
#12 |
New Member
Kyriakos Paso
Join Date: Nov 2018
Posts: 20
Rep Power: 7 |
I tried the second way, and everything is okey.
Thank you very much tobiasS, you helped me a lot! |
|
December 3, 2018, 04:17 |
|
#13 |
Member
Hussam
Join Date: Aug 2017
Location: Germany
Posts: 32
Rep Power: 8 |
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[SOWFA] NREL SOWFA ABLTerrainSolver tutorial problem | cico0815 | OpenFOAM Community Contributions | 36 | February 3, 2022 11:54 |
decomposePar problem: Cell 0contains face labels out of range | vaina74 | OpenFOAM Pre-Processing | 37 | July 20, 2020 05:38 |
[Other] How to create an MRF zone ? | aminem | OpenFOAM Meshing & Mesh Conversion | 2 | December 8, 2014 10:45 |
cgns grid problem | praveen | SU2 | 20 | March 10, 2014 14:09 |
problem with reading the .dat file,error object:#f | Paulina | FLUENT | 6 | November 7, 2006 15:49 |