|
[Sponsors] |
[Gmsh] Gmsh: "Physical Volume" of a NACA airfoil? |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
October 8, 2014, 11:32 |
Gmsh: "Physical Volume" of a NACA airfoil?
|
#1 |
Member
Join Date: Mar 2014
Location: Austrian abroad in Germany
Posts: 48
Rep Power: 12 |
I am trying to mesh a NACA airfoil that can be later on imported into OpenFOAM. I searched for information about that on the internet. That's what I found so far:
https://community.dur.ac.uk/g.l.ingr...torial2012.pdf On page 5 the tutorial says that one have to define a "Physical Volume". The attached file shows what I have so far. Gmsh shows up two volumes (yellow points). One inside the Airfoil (Volume 1) and the other one outside the airfoil (Volume 2). Which volume do I have to select!? |
|
October 8, 2014, 11:54 |
|
#2 |
Senior Member
|
Hi,
cause you need to mesh volume around airfoil (as you need to know flow around the airfoil), you have to select volume outside the airfoil. |
|
October 8, 2014, 15:44 |
|
#3 |
Member
Join Date: Mar 2014
Location: Austrian abroad in Germany
Posts: 48
Rep Power: 12 |
Ok, that sounds logical. Thank you. I combined the two surfaces into one surface (see attached file). When I press "3" nothing happens!? What's wrong here?
|
|
October 9, 2014, 03:25 |
|
#4 |
Senior Member
|
Hi,
what's the version of your Gmsh? 2.8.5 was able to produce the mesh. Though with certain nuances:
|
|
October 10, 2014, 04:34 |
|
#5 |
Member
Join Date: Mar 2014
Location: Austrian abroad in Germany
Posts: 48
Rep Power: 12 |
I am using Gmsh Version 2.8.3 (Ubuntu 14.04). Sometimes meshing works but I can't zoom in or out. Gmsh stops responding or freezes frequently. I will try the latest stable version 2.8.5.
Why is Gmsh meshing inside the airfoil..!? |
|
October 10, 2014, 11:34 |
|
#6 | ||
Senior Member
|
Hi,
Quote:
Quote:
1. Define points - you've done it. 2. Define lines connecting points - you've done it. 3. Define surfaces (in you case those will be several plane surfaces - outer boundaries and couple of ruled surfaces - surface of the airfoil) - you've started doing it... 4. Define geometric volumes using bounding surfaces defined during step 3 - well, you've decided to go straightly to defining physical surfaces and volumes. 5. Finally I define physical groups of surfaces (future patches) and physical volume (only one but still we need to define it). I guess, in case of your file, Gmsh is trying to guess volumes those it needs to mesh. Sometimes Gmsh does it successfully, sometimes - not (for example it decides to mesh additional plane). |
|||
October 10, 2014, 15:13 |
|
#7 |
Member
Join Date: Mar 2014
Location: Austrian abroad in Germany
Posts: 48
Rep Power: 12 |
Thank you for your help. I have attached my newest version. I tried to follow your instructions:
1. Points 2. Lines (Splines, Line Loop, Rotate Line) 3. Surfaces That seems to work now. And I tried Gmsh 2.8.5., too. This version seems to work better. I have one more question: How can I adjust these settings? |
|
October 12, 2014, 06:53 |
|
#8 |
Senior Member
|
Hi,
to generate structured meshes, you need to utilize transfinite lines (and then surfaces, and volumes) - http://www.geuz.org/gmsh/doc/texinfo...ructured-grids. Though to use transfinite algorithm you have to modify mesh file. Gmsh can use this algorithm for surfaces with 4 corners and volumes with 6 corners. So you have to divide the area around the airfoil as shown on attached figure, as usual define points, lines, surfaces and volumes and then first define lines as transfinite: Code:
Transfinite Line {line entity numbers} = <number of points on the line>; Code:
Transfinite Surface "*"; Recombine Surface "*"; Transfinite Volume "*"; Maybe you'll need to move point A to the left to reduce non-orthogonality of the mesh around point F. |
|
October 13, 2014, 08:35 |
|
#9 |
Member
Join Date: Mar 2014
Location: Austrian abroad in Germany
Posts: 48
Rep Power: 12 |
Ok, so my plan is as follows: I will start with an unstructured grid (easily meshed, rapid generation, quick progress etc...). So I can go on learning OpenFOAM. When I got my first results I will try to create a structured grid.
I have attached the newest version of my .geo file. Before I go on converting the mesh to OpenFOAM can someone please double check my .geo file? @ alexeym: Thank you so much for your support! |
|
October 13, 2014, 09:10 |
|
#10 |
Senior Member
|
Gmsh 2.8.5 has generated quite descent mesh, here's checkMesh output:
Code:
Checking geometry... Overall domain bounding box (-5 -5 0) (6 5 1) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) Boundary openness (-4.10252e-18 2.52463e-18 -9.75447e-16) OK. Max cell openness = 2.09221e-16 OK. Max aspect ratio = 846.979 OK. Minimum face area = 3.26324e-06. Maximum face area = 0.278444. Face area magnitudes OK. Min volume = 3.26324e-06. Max volume = 0.0251815. Total volume = 109.898. Cell volumes OK. Mesh non-orthogonality Max: 34.1439 average: 7.41136 Non-orthogonality check OK. Face pyramids OK. Max skewness = 0.491911 OK. Coupled point location match (average 0) OK. Mesh OK. Code:
Mesh 3; Save "NACA2415AngleOfAttack12.msh"; |
|
October 13, 2014, 10:36 |
|
#11 |
Member
Join Date: Mar 2014
Location: Austrian abroad in Germany
Posts: 48
Rep Power: 12 |
||
October 13, 2014, 11:43 |
|
#12 |
Senior Member
|
Hi,
I'm also cause my Gmsh doesn't complain about Save (even installed 2.8.3 to check). |
|
October 13, 2014, 16:33 |
|
#13 |
Member
Join Date: Mar 2014
Location: Austrian abroad in Germany
Posts: 48
Rep Power: 12 |
Sorry, my fault
Edit: I wrote a GNU Octave script to create the geo file and the reason for the error was that I forgot to add a new line: Code:
... fprintf(fileID,'Mesh 3;\r\n'); fprintf(fileID,'Save "%s";\r\n',filenameMsh) |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[Gmsh] Meshing 3D volume from STL/STEP Files (Gmsh) | jgross | OpenFOAM Meshing & Mesh Conversion | 6 | July 15, 2022 05:11 |
multiphase turbulance case floating error | harsha_kulkarni | OpenFOAM Running, Solving & CFD | 3 | February 18, 2016 05:06 |
Problem of simulating of small droplet with radius of 2mm | liguifan | OpenFOAM Running, Solving & CFD | 5 | June 3, 2014 02:53 |
Problem with restart solution in shape_optimization.py | robyTKD | SU2 Shape Design | 21 | May 29, 2013 09:26 |
[blockMesh] non-orthogonal faces and incorrect orientation? | nennbs | OpenFOAM Meshing & Mesh Conversion | 7 | April 17, 2013 05:42 |