[baran_foam]

Greeting all,
I want to create separate zone for polyMesh for chtMultiRegionFoam solver of complex geometry exported from gambit meshing software ...so using co-ordinate point in topoSet is not a good option.
So can you suggest how can i do this thing....I have no idea about this...


Regards,
baran

[wyldckat]

Hi Baran,

I saw the private message you sent me and came to this thread.

You'll need to provide more details, because your question is too generic Keep in mind that people here on the forum are not able to see what you're seeing.

If you follow the instructions given here --> http://www.cfd-online.com/Forums/ope...-get-help.html <-- it will make it a lot easier to help you.

Best regards,
Bruno

[baran_foam]

Greeting all,
I am trying to solve a case of cavity surrounded by two layer of insulation. Inside the cavity coiled heating element is placed for heat source which is shown in the attachments. This mesh is generated in gambit meshing software and then imported in openFoam by the command "fluentMeshToFoam".
AS geometry is complex..only heating element is shown for better understanding
https://www.dropbox.com/s/m8u1hn84gq08oeq/he.JPG?dl=0
https://www.dropbox.com/s/a15p16t949vot1c/he1.JPG?dl=0
So for this case using topoSet or any other option how to separate this zone for chtMultiRegionFoam case. But specifying co-ordinate points zone separation is not possible for this as it is given in tutorial.
What are the other way to solve this issue.. I have no idea about this thing. Can anyone have any idea regarding this problem??

Regards,
baran

[nimasam]

Dear baran

still, your information is some how vague
you can define your zones in gambit and import it in OpenFOAM with:

fluentMeshToFoam -writeZones

if you want to split this zone then you should use following command

splitMeshRegions -cellZones

[baran_foam]

Greeting all,
@ nimasam ...thanks for your reply......It works for me ......But there is another issue i want to specify.....

I create a geometry and do meshing in gambit meshing software...After that i specify some number of disconnected volume under one volume such as "heating_element_volume" under which four disconnected volume is there...but when i was importing geometry in openFoam , for disconnected volume ... it is just reading one volume under this volume name...rest are created separately as per as there region name...
Like in "heating_element_volume" volume one is imported by the openFoam under this name... rest are created as Region2, Region3, Region4...

Do you have any idea about this issue...?


Thanks & regards,
baran

[vasava]

Here is what I do to setup a case for chtMultiRegion*.* solvers.

1. Make mesh with matching interface in Ansys Meshing.
2. Import mesh to Fluent
3. Fuse interfaces. This will create 'interior'. Rename the 'interior' so that it is easily identified in openfoam.
4. Save fluent case. (Remember to un-check the binary option)
5. Import the case and split mesh using fluentMeshToFoam and splitMeshRegions respectively.

These steps should give you n distinct regions for chtMultiRegion*.* solvers.

[manuc]

Dear all,

As suggested in this thread:
1. Generated geometry in Ansys WB ( all bodies frozen) and tool bodies preserved after boolean
2. Grouped the bodies as a part to ensure interface mesh matching.

3.in ANSYS Mesh I found no interfaces. Meshed all bodies.
Named collection of solid bodies as solid (using volume selection and doing named selection)
Named remaining body as fluid

4. Imported it in fluent no option for coupling , but a surface and its shadow (wall type0 available)
Exported case file.
5. IN OPENFOAM used command
fluentMeshToFoam *.cas-writeZonesIt generated files in polymesh
6.USed
splitMeshRegions -cellZones -overwriteIt created fluid and solid folders in '0/'
In addition have folders called domain.
I dont understand why these addition folders are present

I have attached my constant and 0 folder herewith. (BC conditions not correct.)
https://drive.google.com/open?id=0B6...3FUQWJTRUJRam8

[vasava]

Your case has 2D mesh and openFoam does not support 2D meshes. To create a 2D case in openFoam you need a mesh with some thickness (atleast 1 element).

You can try again and let us know if it worked.

[manuc]

Dear Vasava

I tried it for 3d geo aswell. It still creates more domains. I my case I had 5 cylinders as solids. I named the cylendertogether as cyl. in ANSYS. In openfoam it creates a domain with name cyl and 4 domains with name domain 1,2,4,5 .

I think that the cylinder group sint made into a single domain.

Isnt it possible to groups those (5 cylinders in presnt case but it can go high to 250) into a single domain

Bye the way the mesh I hgeneratedfor 2D case earlier when imported in openfoam was itlsef projected in z direction and front and back planes BC was alloted by itself (by mfluentMeshtoFOAm). So I think its not an issue with geo being 2d ealrier, But still to ensure I tried it with 3D geo

[vasava]

Can you post your 3D mesh, I can have a look.

[manuc]

Dear Vasava

Please find the mesh here
https://drive.google.com/open?id=0B6...lZIU29DRk84bE0

[vasava]

Originally Posted by manuc

I dont understand why these addition folders are present.

These folders are generated by splitMeshRegions command. As the name suggests, the command splits meshes in to multiple regions that are separated by interfaces.

For conjugate heat transfer this is necessary because unlike fluent, openFoam CHT solvers treats each sub-domain individually. I assume you know how Conjugate Heat transfer cases are set in openFoam.

If you want multiple domain to appear as one (just like fluent) you can try this trick (there is no guarantee but worth a try).

1. In Ansys meshing select the domains and use name selection to name the group as 'cyl'. This is just like selecting multiple walls and naming them as walls. Instead of walls here you select domains.
2. Export mesh and continue.

[manuc]

This named selection is what I tried..when converted using split regions it assigns the name to a single cylinder and names the other cylinder as region *..it doesn't keep the group name

[vasava]

Try renaming all the solids to 'cyl'.

Also, what CAD program are you using to generate geometry?

[manuc]

I use ansys design modeller