CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Native Meshers: snappyHexMesh and Others

bad trailing edge boundary layer with snappyHexMesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 15, 2011, 08:42
Default bad trailing edge boundary layer with snappyHexMesh
  #1
New Member
 
Florian Becker
Join Date: Apr 2010
Posts: 12
Rep Power: 0
draufunddran is on a distinguished road
Hallo,

i want to make a mesh around a naca-0012 with snappyHexMesh, but when i add boundarylayer i get this at the trailing edge of the airfoil.



all the boundarylayer are coming together at one line. this is giving me a not wanted result when i run pimpleFoam.

Is there any Option to turn this behaviour off?


greeting draufunddran
draufunddran is offline   Reply With Quote

Old   March 3, 2012, 22:34
Default featureAngle
  #2
New Member
 
Travis
Join Date: Oct 2011
Location: seattle
Posts: 7
Rep Power: 5
seadmiral is on a distinguished road
I know this is an old post, but I ran across it (and others) today with the same problem.

My solution was to play with featureAngle in the addLayersControls parameters of snappyHexMesh. I decreased this angle to 30 degrees and the resulting boundary layer mesh no longer extended all the way to the TE.
seadmiral is offline   Reply With Quote

Old   July 9, 2013, 05:20
Default
  #3
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
Like the previous poster, I ran across this old post and thought I'd post a reply as well.

I've found that replacing a sharp trailing edge feature with one with a small radius leads to a much better mesh snap and layer addition.

Of course, the feature angle mentioned previously is also a key parameter.
Artur is offline   Reply With Quote

Old   September 20, 2013, 09:36
Default
  #4
New Member
 
PaoloFariselli
Join Date: Aug 2013
Location: Milan, Italy
Posts: 28
Rep Power: 3
Paolo.F is on a distinguished road
Hallo everyone,
I'm also having some problems meshing a NACA0010...I've tried to work with the FeatureAngle and i've also replaced the sharp edge with a small radius, but it isn't still ok...any other idea?!

Anyway, I've tryed to start a simulation with simpleFoam...everything works fine till the end, but when i try to watch the results with paraView I get this error message:

Code:
FOAM FATAL IO ERROR: 
size 0 is not equal to the given value of 166400

file: /home/paolo/TESI/Lungo/soluzioni/ultimo/3/U.boundaryField.NACA from line 1551485 to line 1551486.

    From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.1/src/OpenFOAM/lnInclude/Field.C at line 236.

FOAM exiting
It seems that the problem is in the boundary file; I can see that I have 8 Boundary conditions, and that two of them are on the NACA. The last one ha 0 faces but I don't know how to handle the problem...

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "3/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

8
(
    inlet
    {
        type            patch;
        nFaces          4000;
        startFace       4647766;
    }
    outlet
    {
        type            patch;
        nFaces          4000;
        startFace       4651766;
    }
    left
    {
        type            symmetryPlane;
        inGroups        1(symmetryPlane);
        nFaces          10298;
        startFace       4655766;
    }
    right
    {
        type            symmetryPlane;
        inGroups        1(symmetryPlane);
        nFaces          10298;
        startFace       4666064;
    }
    top
    {
        type            symmetryPlane;
        inGroups        1(symmetryPlane);
        nFaces          3200;
        startFace       4676362;
    }
    bottom
    {
        type            wall;
        nFaces          3200;
        startFace       4679562;
    }
    NACA
    {
        type            wall;
        nFaces          166400;
        startFace       4682762;
    }
    NACA
    {
        type            wall;
        nFaces          0;
        startFace       4849162;
    }
)

// ************************************************************************* //
Can anyone help me?
thanks!
Paolo

Last edited by wyldckat; September 23, 2013 at 17:15. Reason: Added [CODE][/CODE]
Paolo.F is offline   Reply With Quote

Old   September 22, 2013, 03:52
Default
  #5
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
Try removing the empty boundary condition, either by manually editing the boundary file or by running the following:
Code:
createPatch -overwrite
See if that helps with removing the error message...
Artur is offline   Reply With Quote

Old   September 23, 2013, 06:24
Default
  #6
New Member
 
PaoloFariselli
Join Date: Aug 2013
Location: Milan, Italy
Posts: 28
Rep Power: 3
Paolo.F is on a distinguished road
Hi Artur,
thanks a lot for you reply!

Do you mean I should edit the boudary file before starting the simulation?

At the moment I have 2 simulations running:

One with the boundary file edited, and the other one non-edited ( i'll chenge it at the end)

I hope I can see something in a few hours...
Paolo

Last edited by Paolo.F; September 23, 2013 at 10:34.
Paolo.F is offline   Reply With Quote

Old   September 23, 2013, 15:50
Default
  #7
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 226
Rep Power: 6
Artur is on a distinguished road
I think it would be best to do this right after the meshing process as having two BC's for the same patch might make the solver do some hard to predict thing, I imagine.
Artur is offline   Reply With Quote

Old   September 25, 2013, 04:13
Default
  #8
New Member
 
PaoloFariselli
Join Date: Aug 2013
Location: Milan, Italy
Posts: 28
Rep Power: 3
Paolo.F is on a distinguished road
Hi Artur!
Thanks for your hints!!! I've just finished my simulation and it worked properly!
Now I just need to refine the mesh to get better results...

regards,
Paolo
Paolo.F is offline   Reply With Quote

Old   October 1, 2013, 17:13
Default
  #9
Member
 
Miro
Join Date: Jan 2013
Location: Europe
Posts: 51
Rep Power: 4
miro2000 is on a distinguished road
Regarding trailing edge boundary layer, from my experience It's difficult to obtain better results. I found It's helpful to introduce some refinement in the trailing edge.
One can do that via surface refinement or via volume refinement. I've used surfaceref. but vol version is easier to implement but it creates more cells, so if your mesh is small and not already very refined, that's a place to start.
Let my know if you get stuck
miro2000 is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Turbulent Boundary Layer on a Flat Plate Hoshang Garda FLUENT 1 November 27, 2013 11:24
[GAMBIT] 3D boundary layer and meshing problem in GAMBIT 2.4.6 prashanthreddyh ANSYS Meshing & Geometry 1 December 20, 2011 01:35
direction of boundary layer in gambit Ilu FLUENT 7 October 16, 2008 03:20
CREATION OF BOUNDARY LAYER Jibran Haider FLUENT 3 August 1, 2008 00:33
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55


All times are GMT -4. The time now is 14:42.