[rsa]

Hi,

I am wondering if anyone can tell me what is the equivalent of topoSet in foam-extend 4.0

in OF using topoSet, I can set "zones" in the mesh with assigned names where latter I can search for those zones by name in a modified solver. Basically, what I want to do is to define a volScalarField variable in the createField and then initialize it to a certain value for the zone(s) generated by topoSet and zero every where else. I know how to do this using topoSet in OF but as I noticed there is no topoSet in fe40.
I found setField which if I put "myVar" the variable I want to initialize in the 0-directory then it will return a non-uniform field using setField but I could not read the "myVar" into "myVar" that I defined in createFields.H

Thanks.

[DenysW]

I found the same problem, but in my case due to wanting to use topoSet ahead of createBaffles to general zero-thickness baffles on internal boundaries between blocks.

Exporting to Fluent using foamMeshToFluent in openFoam 1706 followed by fluent3DMeshToFoam in foam-extend 4.0 worked for the mesh. Then there was some minor messing around with boundary conditions to use ones foam-extend recognised/liked. Then it ran.

[aeronerd]

This is an old thread, but I am still struggling to establish face zones to create a GGI interface in FE4.1

I even tried to make the zones in OF, and then bring the zone definition files over and FE4.1 didn't recognize them...

I'm starting with a salome mesh (which runs), but can't establish cyclicGGI boundaries to get things going.

I can't find a manual or wiki entry that describes GGI either. I feel I could figure it out with even a little official information

[aeronerd]

To answer my own question for the sake of helping others, a function external to setSet in FE4.1 called "setsToZones" did what I needed.

generate sets through FE4.1's setSet, and then convert them to face zones with setsToZones -noFlipMap.

That was about 2 hours of my life :/

[Wolfram]

Hi aeronerd,

I did not get exactly how you used the setSet utility.

Right now I am facing the same Issue:
Created the mesh with salome but I am not able to assign cellSet to use them as MRFZone

Could you please give me a hint?

Best wishes

[aeronerd]

I first created a cellSet using the function setSet. You then quit the setSet prompt and run the command line function called "setsToZones" which will convert all your established cellSets to cellZones.

[Wolfram]

Originally Posted by aeronerd

I first created a cellSet using the function setSet. You then quit the setSet prompt and run the command line function called "setsToZones" which will convert all your established cellSets to cellZones.

yap, understood. In my mesh, since it is meshed with Salome, I have two regions. In OpenFoamv2012 I used "checkMesh" in order to assign the two regions and afterwards I use the setSet functionality.
I am stuck in assigning these two regions in order to use them in setSet

[aeronerd]

I am in fact doing MRF with a dual region mesh made in salome right now

I don't think this is the best way to do it....... but I linked the region boundaries with a cyclicAMI boundary, and just set the rotating region cell zone as the MRF rotating zone.

It's running, but I think the cyclicAMI boundary between rotating and stationary regions is entirely unnecessary for a smarter person.

[Wolfram]

Originally Posted by aeronerd

I am in fact doing MRF with a dual region mesh made in salome right now

I don't think this is the best way to do it....... but I linked the region boundaries with a cyclicAMI boundary, and just set the rotating region cell zone as the MRF rotating zone.

It's running, but I think the cyclicAMI boundary between rotating and stationary regions is entirely unnecessary for a smarter person.

First of all, many thanks for your help so far! Meanwhile I found a solution for my purpose ...

1. create the mesh in separate directories. For example /rotor/ and /stator/
2. merge the mesh with "mergeMeshes"
3. split the regions and let OpenFoam "create" the cell-zones in the merged mesh with "splitMeshRegions" -makeCellZones -overwrite"
4. use the setSet functionality and set for example the region0 to the rotor region with "cellSet rotor new setToCell region0"

Maybe this is not elegant but it works for me ...


How does this "dual region mesh" work with salome?

Best wishes