CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > SU2

CHT Mesh generation using GMSH

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 4, 2022, 05:33
Default CHT Mesh generation using GMSH
  #1
New Member
 
Robert
Join Date: Nov 2022
Posts: 12
Rep Power: 2
decenu is on a distinguished road
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 Iím 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/
decenu is offline   Reply With Quote

Old   November 4, 2022, 07:42
Default
  #2
Senior Member
 
bigfoot
Join Date: Dec 2011
Location: Netherlands
Posts: 338
Rep Power: 15
bigfootedrockmidget is on a distinguished road
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/
bigfootedrockmidget is offline   Reply With Quote

Old   November 4, 2022, 08:32
Default
  #3
New Member
 
Robert
Join Date: Nov 2022
Posts: 12
Rep Power: 2
decenu is on a distinguished road
Quote:
Originally Posted by bigfootedrockmidget View Post
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".
decenu is offline   Reply With Quote

Old   November 4, 2022, 11:02
Default
  #4
Member
 
Ole Burghardt
Join Date: Mar 2016
Location: Kiel, Germany
Posts: 60
Rep Power: 9
Sprotte is on a distinguished road
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? :-)
Sprotte is offline   Reply With Quote

Old   November 4, 2022, 18:06
Default
  #5
New Member
 
Robert
Join Date: Nov 2022
Posts: 12
Rep Power: 2
decenu is on a distinguished road
Quote:
Originally Posted by Sprotte View Post
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!
decenu is offline   Reply With Quote

Old   November 5, 2022, 11:13
Default
  #6
Member
 
Ole Burghardt
Join Date: Mar 2016
Location: Kiel, Germany
Posts: 60
Rep Power: 9
Sprotte is on a distinguished road
You're welcome :-)

Just out of curiosity, what are you working on?
Sprotte is offline   Reply With Quote

Old   November 6, 2022, 12:57
Default
  #7
Member
 
na
Join Date: Jul 2018
Posts: 78
Rep Power: 7
TKatt is on a distinguished road
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
TKatt is offline   Reply With Quote

Old   November 11, 2022, 05:33
Default
  #8
New Member
 
Robert
Join Date: Nov 2022
Posts: 12
Rep Power: 2
decenu is on a distinguished road
Quote:
Originally Posted by Sprotte View Post
You're welcome :-)

Just out of curiosity, what are you working on?
Working on cfd simulations for Pin fin heat exchangers.
decenu is offline   Reply With Quote

Old   November 12, 2022, 17:12
Default
  #9
New Member
 
Robert
Join Date: Nov 2022
Posts: 12
Rep Power: 2
decenu is on a distinguished road
Quote:
Originally Posted by TKatt View Post
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?
decenu is offline   Reply With Quote

Old   November 13, 2022, 04:28
Default
  #10
Member
 
Ole Burghardt
Join Date: Mar 2016
Location: Kiel, Germany
Posts: 60
Rep Power: 9
Sprotte is on a distinguished road
Sounds like wrong settings or a corrupted mesh. We'd need to have a look on the output and/or config files
Sprotte is offline   Reply With Quote

Old   November 13, 2022, 06:33
Default
  #11
New Member
 
Robert
Join Date: Nov 2022
Posts: 12
Rep Power: 2
decenu is on a distinguished road
Quote:
Originally Posted by Sprotte View Post
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.
Attached Images
File Type: jpg Screenshot 2022-11-13 113024.jpg (191.0 KB, 18 views)
Attached Files
File Type: zip period_pins.zip (2.5 KB, 1 views)
decenu is offline   Reply With Quote

Old   November 13, 2022, 06:43
Default
  #12
New Member
 
Robert
Join Date: Nov 2022
Posts: 12
Rep Power: 2
decenu is on a distinguished road
Quote:
Originally Posted by decenu View Post
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.
Attached Images
File Type: jpg Screenshot 2022-11-13 113644.jpg (78.4 KB, 11 views)
Attached Files
File Type: zip period_pins_3Pin.zip (9.3 KB, 2 views)
decenu is offline   Reply With Quote

Old   November 14, 2022, 02:33
Default
  #13
Senior Member
 
bigfoot
Join Date: Dec 2011
Location: Netherlands
Posts: 338
Rep Power: 15
bigfootedrockmidget is on a distinguished road
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.
bigfootedrockmidget is offline   Reply With Quote

Old   November 14, 2022, 06:23
Default
  #14
New Member
 
Robert
Join Date: Nov 2022
Posts: 12
Rep Power: 2
decenu is on a distinguished road
Quote:
Originally Posted by bigfootedrockmidget View Post
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.
decenu is offline   Reply With Quote

Reply

Tags
cht modelling, gmsh, gmsh cylinder, mesh, su2

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[snappyHexMesh] non uniform mesh near the stl object vava10 OpenFOAM Meshing & Mesh Conversion 0 January 31, 2021 14:41
how to set periodic boundary conditions Ganesh FLUENT 15 November 18, 2020 06:09
decomposePar problem: Cell 0contains face labels out of range vaina74 OpenFOAM Pre-Processing 37 July 20, 2020 05:38
[snappyHexMesh] No layers in a small gap bobburnquist OpenFOAM Meshing & Mesh Conversion 6 August 26, 2015 09:38
[Gmsh] gmshToFoam problem: not the same mesh in Gmsh vs. paraview zhernadi OpenFOAM Meshing & Mesh Conversion 8 July 7, 2011 02:28


All times are GMT -4. The time now is 21:53.