[Clau.77]

Hey guys!


I m having trouble adding layers in my multi region case.


The way I tried it:
1. snappyHexMesh with addLayers false
2. Then copy the polyMesh folder of the region where I want layers into the constant folder
3. set addLayers in snappy to true and the other two to false


That works so far, when I open Paraview, I can see the region with the layers. Put when I copy the polyMesh folder back to its constant/region/ position and then take a look at the mesh with all regions, the layers are gone.



So, did I miss a step? Or is there another way to add layers?
When I try to addLayers the "normal" way (without copying the polyMesh folders from one place to another), snappy always tells me that there are no layers to generate...


I m getting really frustrated with this, I would appreciate some tipps

[Yann]

Hi Claudia,

If I am not mistaken, you are using OpenFOAM foundation version right?

Maybe have a look at the "mergeFaces" parameter which has been introduced since OpenFOAM-7 : https://github.com/OpenFOAM/OpenFOAM...c2d75980212a63

Foundation and ESI/OpenCFD versions have different ways to deal with layer addition in multiregion cases.
I am more used to OpenCFD version so I never used "mergeFaces" but I think this is worth trying.

Cheers,
Yann

[Clau.77]

Hey Yann,


thank you for the tipp


Yes, i am using OF-8. I looked up the mergeFaces option, but I am not sure how it can help me.


I tried mergeFaces=true on the whole mesh, but there where this no layers to generate.

So I tried again to copy the polyMesh folder from the region to the constant folder, added the layers and the copied everything back to place but the mergeFaces option does not make a difference. So I tried to use splitMeshRegion -cellZonesOnly -overwrite before and after the addLayers step but when I use it after adding the layers I have problems with mssing entries in the nSurfaceLayers file.


Would you suggest a different workflow?
And just out of curriosity, how does it work when using OpenCFD?

[Yann]

Hi Claudia,

Have a look at this tutorial, it seems it uses the mergeFaces parameter : https://github.com/OpenFOAM/OpenFOAM...eHeatExchanger

In OpenCFD versions, there is the "locationsInMesh" parameter used to define the cellZones corresponding to the different regions in your mesh. It automatically creates interfaces while meshing (ie. region1_to_region2) and you can use these interfaces in addLayersControls.

Yann

[Clau.77]

That tutorial helped a lot, I finally managed to get the layers that I wanted


Thank you so much for your help, Yann!

[ofWorld]

Hi Yann,

I am trying to mesh a complex vessel geometry. I have two regions to mesh: one is the blood flow region and the other is the thin vessel wall.

The parameter "locationsInMesh" works well to mesh them at the same time. The problem is that the command, "splitMeshRegions -cellZones -overwrite", does not separate the vessel wall from the background mesh. In other words, I got only two mesh folders in the end, with one folder having the fluid domain and the other one having the vessel wall & background.

Looking forward to hearing from you.
Many thanks,
Guanqi

[Yann]

Hello Guanqi,

First thing coming to mind would be an issue with your STL files.
Did you make sure there is no hole in the vessel wall in your STL file?

How is your mesh setup? Do you have closed surfaces for both the blood flow region and the vessel region?

Are you able to share files or screenshots of your STL files and background mesh?

[ofWorld]

Hi Yann,

Thank you very much for your quick reply!

In the attached two geometries, the "insideDomain.stl" represents the domain of blood flow, and the "outsideDomain.stl" stands for the vessel shell.

I double checked the geometry, and have re-ran the meshing process before I replied this message. My stl files are too big as an attachment, please let me know if you need the original copies.

Best,
Guanqi

[Yann]

To check if something is wrong with your STL file, you can either:

• Run the surfaceCheck utility on your STL files and see if the surface is closed
• Use the leak detection feature of snappy: https://doc.openfoam.com/2306/tools/...onsOutsideMesh (have a look at the "New leakage detection" feature in the release notes here: https://www.openfoam.com/news/main-n...pre-processing)