[decenu]

I am working on the multiphysics tutorial from SU2, specifically the static CHT simulation.

I am looking to recreate a very similar simulation, using a larger grid with more obstacles.

The issue I’m running into is creating the mesh as I don`t fully understand the structure.

The mesh I created uses a farfield, outer cylinder wall and inner cylinder wall. The mesh uses multiple zones but modelling it in GMSH seems tricky.

1. The tutorial defines a third zone called Core1 for the cylinders. I am struggling to understand what this mesh represents.

2. Is the cylinder thickness modelled as a surface?

I would be delighted if anyone could shed some light over how would one generate the mesh from said tutorial: https://su2code.github.io/tutorials/Static_CHT/

[bigfootedrockmidget]

1. The tutorial defines a third zone called Core1 for the cylinders. I am struggling to understand what this mesh represents.


The cylinder is hollow and we set the wall temperature of the inner circular boundary. This would be akin to a hollow tube with cooling water running through it. In this setup, the cooling water is not simulated, only the hollow tube. We simply assume that the water keeps the wall of the water channel at a constant temperature.



2. Is the cylinder thickness modeled as a surface?


Yes, all physical 2D zones are surfaces.


here is some further info:


https://su2code.github.io/docs_v7/Multizone/

[decenu]

Originally Posted by bigfootedrockmidget

1. The tutorial defines a third zone called Core1 for the cylinders. I am struggling to understand what this mesh represents.


The cylinder is hollow and we set the wall temperature of the inner circular boundary. This would be akin to a hollow tube with cooling water running through it. In this setup, the cooling water is not simulated, only the hollow tube. We simply assume that the water keeps the wall of the water channel at a constant temperature.



2. Is the cylinder thickness modeled as a surface?


Yes, all physical 2D zones are surfaces.


here is some further info:


https://su2code.github.io/docs_v7/Multizone/

Thank you very much for the quick reply. I ubderstand the actual physical model but what still confuses me is what is the actual difference when meshing between the "core" and "inner cylinder".

[Sprotte]

Hi,

there are four physical zones (sub-meshes, if you like) in the mesh, one for the fluid flow zone, three for the solid zones.

The boundaries in the fluid flow mesh are called farfield, cylinder_outer1, cylinder_outer2 and cylinder_outer3. The boundaries in solid zone mesh X are called cylinder_innerX, coreX. (The solid zones are annuli, the outer perimeter is called cylinder_inner, the inner perimeter is called core.)

The CHT coupling between the fluid zone and the solid zones is formed by exchanging data between cylinder_outerX and cylinder_innerX. At the cores, a temperature boundary condition is imposed.

For meshing it might be easiest, or actually the only way, to create meshes for each domain seperately and to concatenate them later on. The mesh file used for this tutorial is in text format, just check it out to see how it's done.

Does this help? :-)

[decenu]

Originally Posted by Sprotte

Hi,

there are four physical zones (sub-meshes, if you like) in the mesh, one for the fluid flow zone, three for the solid zones.

The boundaries in the fluid flow mesh are called farfield, cylinder_outer1, cylinder_outer2 and cylinder_outer3. The boundaries in solid zone mesh X are called cylinder_innerX, coreX. (The solid zones are annuli, the outer perimeter is called cylinder_inner, the inner perimeter is called core.)

The CHT coupling between the fluid zone and the solid zones is formed by exchanging data between cylinder_outerX and cylinder_innerX. At the cores, a temperature boundary condition is imposed.

For meshing it might be easiest, or actually the only way, to create meshes for each domain seperately and to concatenate them later on. The mesh file used for this tutorial is in text format, just check it out to see how it's done.

Does this help? :-)

Thank you for the advice. You have opened my eyes! It worked!!!!!

The answer to my question is exactly your suggestion i.e. concatenate the meshes together.

Still have a long way to go as for optimizing and everything but you might have saved a poor's student's week haha!

[Sprotte]

You're welcome :-)

Just out of curiosity, what are you working on?

[TKatt]

Just to add a little bit of resource/inspiration that might help with a few things:
1. video that covers general aspects of multizone simulations/setups https://www.youtube.com/watch?v=ez368rDYrFk (no guarantee that everything is still up to date, but e.g. the mesh concatenation definitely is)
2. A repository with a few gmsh meshes (also a few multizone ones, inidicated with e,g, '2zones' in the folder name). Take e.g. folder '18__3D-2Zone-pin-in-crossflow' for an easy setup. I pretty much only made structured meshes so setups might be easier for you but I generally create the interface boundary at the beginning that gets used for all relevant zones to have a single source of origin, all zone-specific stuff then comes later in the file https://github.com/TobiKattmann/Meshes/


Maybe this of use for you

[decenu]

Originally Posted by Sprotte

You're welcome :-)

Just out of curiosity, what are you working on?

Working on cfd simulations for Pin fin heat exchangers.

[decenu]

Originally Posted by TKatt

Just to add a little bit of resource/inspiration that might help with a few things:
1. video that covers general aspects of multizone simulations/setups https://www.youtube.com/watch?v=ez368rDYrFk (no guarantee that everything is still up to date, but e.g. the mesh concatenation definitely is)
2. A repository with a few gmsh meshes (also a few multizone ones, inidicated with e,g, '2zones' in the folder name). Take e.g. folder '18__3D-2Zone-pin-in-crossflow' for an easy setup. I pretty much only made structured meshes so setups might be easier for you but I generally create the interface boundary at the beginning that gets used for all relevant zones to have a single source of origin, all zone-specific stuff then comes later in the file https://github.com/TobiKattmann/Meshes/


Maybe this of use for you

Thank you this is very useful. I am actually trying something similar now using periodic conditions but with a different mesh than the tutorial one. For some reason it's not going past the 1st iteration diverging with a residual over the limit. Any idea why that might be?

[Sprotte]

Sounds like wrong settings or a corrupted mesh. We'd need to have a look on the output and/or config files

[decenu]

Originally Posted by Sprotte

Sounds like wrong settings or a corrupted mesh. We'd need to have a look on the output and/or config files

I'm attaching the config file here and a snip of the mesh, maybe you can have a look. The one thing that I can see different between my mesh and the tutorial is that I am using an unstructured grid and obviously a different array with more cylinders. Unfortunately, I can't seem to upload the mesh as it's too large. The markers that I am using are "Inlet" and "Outlet" for left- and right-hand sides, "cylinderx" (x = 1:15) for each cylinder surface and symmetry for the top and bottom sides which exclude the cylinders.

[decenu]

Originally Posted by decenu

I'm attaching the config file here and a snip of the mesh, maybe you can have a look. The one thing that I can see different between my mesh and the tutorial is that I am using an unstructured grid and obviously a different array with more cylinders. Unfortunately, I can't seem to upload the mesh as it's too large. The markers that I am using are "Inlet" and "Outlet" for left- and right-hand sides, "cylinderx" (x = 1:15) for each cylinder surface and symmetry for the top and bottom sides which exclude the cylinders.

In addition to this I have also tried replicating the exact tutorial by creating a similar unstructured mesh as in the picture attached (see below). Left and right sides are named Inlet/Outlet top and bottom are named symmetry and the cylinders surfaces are named cylinderx (x=1:3).

The config file for this is attached along with the resulting history excel file.

[bigfootedrockmidget]

Is this last case a fluid-domain simulation only? What is the mesh quality of the mesh? And the Reynolds number? The mesh also looks extremely fine close to the cylinder walls. For such simple meshes it can be very beneficial to use structured meshes instead of unstructured meshes.

[decenu]

Originally Posted by bigfootedrockmidget

Is this last case a fluid-domain simulation only? What is the mesh quality of the mesh? And the Reynolds number? The mesh also looks extremely fine close to the cylinder walls. For such simple meshes it can be very beneficial to use structured meshes instead of unstructured meshes.

Yes, it's fluid domain only, the mesh is very fine next to the cylinder walls having ~200 elements on the cylinder. The Reynolds number is somewhere around 70000.