Hi , My question is about th
My question is about the fact that the newly implemented fluent3DMeshToFoam does not write sets anymore. I need that in order to set some properties to sets with the setFieldByCellSet...
I see that it writes out cellZones, though. What is the difference between a cellZone and a cellSet and what would be the correct syntax for setting a value of some (scalar) field on that cellZone? I mean, to do the same thing as in setFieldsByCellSet.
I had the same problem with th
I had the same problem with the fluentMeshToFoam utility. I just compiled the old utility using the new OF-1.4.1.....now it writes sets again....
You can fairly easily convert
You can fairly easily convert a zone to a set and vice versa.
setsToZones will convert sets to zones.
cellSet with 'zoneToCell' converts a cellZone into a cellSet
Thank you Mattijs for your sug
Thank you Mattijs for your suggestions. Will look into it.
Can anyone explain what is the
Can anyone explain what is the conceptual difference between cellSets and cellZones? Why are they both necessary?
I might not be the most approp
I might not be the most appropriate person to answer the first part but for the second question, I guess that one does not need them both. Unless you want to use some "old" tools like the aforementioned setFiedlbyCellSet or foamToVTK that does not use Zones (or it did not use zones when I used it) but Sets.
The difference is historical i
The difference is historical in origin and maintained due to inertia. Ideally there should be only one very flexible element grouping construct.
Zones are supported by mesh topo change engines, sets are not. As Radu mentioned, sets are older and used in many utilities including cellSet, pointSet, faceSet, setSet, foamToVTK and a few more.
Thanks both of you for the exp
Thanks both of you for the explanations. Can you add something about regions? Are they different from zones or sets?
Regions are the seeds of a mul
Regions are the seeds of a multi-mesh system. They don't do much at present.
Hi , The fluent3DMeshToFoam
The fluent3DMeshToFoam does not write faceZones. I need that in order to use the MRF (impeller and zone MRF).
How can I get the faceZones?
Thanks a lot.
Hi, Danielle, You need first
You need first faceSets, using faceSets you can
make faceZones (setsToZones).
Thank you for your answer Paul
Thank you for your answer Paul,
I have tree zones. and I should have the zone_MRF in faceCells.
I make this steps:
1) flunet3DMeshToFoam . case3dMRF
2) in faceSetDict I make the name of zone zone_MRF and action new
3) faceSet . Test_zones
4) to create zone_MRFCells file I make in cellSetDict
5) cellSet . Test_zones
6)setsToZones . Test_zones
My first question is:
is that the right commandes to have a corresponding face of my zone_MRF is faceCells file ?
my second is:
what is the roole of flipMap?
I make -noFlipMap like option
Thank you for your precious help!
Hi, the steps are exactly:
the steps are exactly:
1) fluent3DMeshToFoam .. yourCase file.msh (you are in the folder yourCase)
2)copy the file cellSetDict from the case mixerVessel2D of MRFSimpleFoam to system of your case.
3)cellSet .. yourCase
4) copy the file faceSetDict_rotorFaces from the case mixerVessel2D of MRFSimpleFoam to system/faceSetDict of your case.
5)faceSet .. yourCase
6)copy the file faceSetDict_noBoundaryFaces from the case mixerVessel2D of MRFSimpleFoam to system/faceSetDict of your case.
7)faceSet .. yourCase
8)setsToZones .. yourCase -noFlipMap
dear everyone, when i do the s
dear everyone, when i do the step 1) as BANNARI ,i can not get the mesh .for the error message is :
-->FOAM FATAL ERROR : Do not understan characters:
from function fluentMeshToFoam::lexer
in file FluentMeshToFoam.L at line 703
how can i resolve it？
You must have some unrecognise
You must have some unrecognised character in the .msh file. Check fluentMeshToFoam.L to see what is accepted and what not.
Typpically this occurs when th
Typpically this occurs when the mesh was exported from a gambit running under windows.
Therefore: do a dos2unix on the mesh file before converting it with fluent3dmeshtofoam
Thanks a lot i resolve it by
Thanks a lot i resolve it by do a dos2unix
but when i finished all steps accordig to Rachid,and running my case there is FATAL EEROR!
cannot find MRFzone cellzone ,what is the problem?
i think it may be caused by th
i think it may be caused by the name "rotor" in the MRFsimplefoam tut.,for too much name "rotor",cellzone name is "rotor",boundary name also "rotor",set name still "rotor",could you please give me more about that tut？
Hi my case is running now,bu
my case is running now,but i am not quiet sure it is right,for just modify the cellzone name and some boudary name.i do not clearly understand the procedure of cellSet and faceSet.
1why should do faceset and cellset?
2what is the meannig of the both?
3when do these what changes?
4what is setTozone
by the way: 5 when i just wan
by the way:
5 when i just want to simulate the a rotated zone like impeller without interaction with station zone do i still need to do cellSet and faceSet?
6 in object MRFZones the definition of omega omega omega [0 0 -1 0 0 0 0] ,does that mean the dimension is revolution per second? or rad/s?
|All times are GMT -4. The time now is 03:50.|