viscous layer on surface inside partition

Hello,

I am having quite a bit of difficulty with the viscous layer feature.

In order to model both solid and fluid regions, such as with openfoam, my understanding is that I need to build models with different regions using partitions.

In my partition, I need a viscous layer against the internal boundary face of the mesh.  Is this possible?  Does the viscous layer feature only work for faces that are on the outside boundary of the mesh domain?  All the examples I can find only show viscous layers on the outside faces.

Thank you,

Hello,

you are right, viscous layers can't be created on internal faces of a model. A possible workaround is following:
1) Create a geom model using partition.
2) Mesh the solid part with viscous layers separately from the fluid part. Create a group (group on geometry) of 2d mesh elements laying on the boundary faces between the fluid and solid parts.
3) Mesh the fluid part. To mesh the boundary faces use "Use existing 2D elements" algorithm with Source Faces = <a group of 2d elements> and option "To copy mesh"=True. Thus two meshes will be united.

St.Michael

Saying "to mesh separately" I mean creating a mesh for a solid part and another mesh for a fluid part.

Thank you, I will try that!

Here is a script making what I meant. It creates viscous layers on internal faces of 3 boxes.

St.Michael

Thank you, I will look into the approach used in the python script.

I have also looked into Hexotic as a solution for this issue.  It looks Hexotic has the capabilities to add boundary layers on internal surfaces between domains.  However, that capability is in a very new stand-alone version, but not available as a plug in with Salome (yet?).  It appears to require a surface mesh first, therefore I would have to make a surface mesh in Salome, export, mesh in Hexotic, then convert that mesh for the solver I'm using (openfoam).

Any idea how to get a mesh from Salome to work with a .mesh or .meshb format, that is required by Hexotic?  I am unable to find much info on conversion from unv or med to .mesh...

Hello

.mesh format is very simple and is described in Hexotic User Manual. So it's not so hard to write a python script that would write 2D mesh computed by SALOME into a .mesh file.

Another solution is to catch an input tmp file SALOME generates for Hexotic before it is removed. I would open such a file in emacs and then store it in a safe place.

St.Michael

Hello Chaz,

have you been able to mesh boundary layers in your internal faces? Which way did you solve your problem?

Hi

In v7.4.0 it's possible to make viscous layers on any face. To get viscous layers on an internal face it's necessary to use an option allowing to specify faces WITH viscous layers.

St.Michael

Hi all, I think I have a similar problem to the one discussed in this thread, but I am still not able to solve it.

I am trying to mesh a domain partitioned by means of a plane, and I am trying to generate a viscous layer mesh on the surface interfacing the two partition solids.

Unfortunately, there is no way I can make this work. Regardless if I try with GUI or TUI. I always run into an error which reads

"NETGEN_2D3D_2" failed on "Solid_1". Error: Invalid input mesh. NgException at Volume meshing: Stop meshing since surface mesh not consistent

Some edges multiple times in surface mesh

I am attaching a TUI script which reproduces the issue on a simple cube geometry.

Is there any one who can help me solving the problem, or who can point me out to a thread in which this problem is discussed?

Thank you very much for the help!

    Andrea

Hi Andrea,

I am sure there is a bug in NETGEN-1D2D3D. As a workaround use NETGEN-3D + NETGEN-1D2D instead of NETGEN-1D2D3D .

St.Michael

Hi Michael,

thank you VERY much for the suggestion, and for the quick answer. I just tried it and it finally works!

     Andrea

Previously Saint Michael wrote:

Hi Andrea,

I am sure there is a bug in NETGEN-1D2D3D. As a workaround use NETGEN-3D + NETGEN-1D2D instead of NETGEN-1D2D3D .

St.Michael

 

Hi there,

i have a similar case as dicussed above in SALOME 9.2 (The later versions dont start on my ubuntu)

Here i dont get any viscous layers on the internal face (see attached file)

no errors, if i use outer boundaryies it works,

could you have a look at that?

pretty please

best regards

Franz

Hi

I managed to get the desired mesh by defining a sub-mesh with Viscous Layers hypothesis on each of faces.

St.Michael

Hello

I am trying to mesh an object with viscous layers next to a wall (this will be the entrance for a porous media volume). I have tried some of the suggested solutions above and have had no luck. does anyone have any  suggestions? 

I continuously get this error for NETGEN 3D: OCC exception. gp_VectorWithNullMagnitude: 

I've added the python dump below