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

Let's talk about foamyHexMesh

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

Like Tree2Likes
  • 1 Post By zordiack
  • 1 Post By l_r_mcglashan

Reply
 
LinkBack Thread Tools Display Modes
Old   September 24, 2014, 06:25
Default Let's talk about foamyHexMesh
  #1
Member
 
Pekka Pasanen
Join Date: Feb 2012
Location: Finland
Posts: 78
Rep Power: 7
zordiack is on a distinguished road
I just wanted to hear if anyone has been successfully using the new mesher? There hasn't been much buzz around it since the release of 2.3.0 and it's already October.

The biggest issue I'm having is the mesh quality after collapseFaces. It just isn't usable and even the tutorial meshes are bad. I mean for example the flange tutorial, compare the output of fresh tutorial run (image attached) with the image on the page http://www.openfoam.org/version2.3.0/foamyHexMesh.php. I don't think they quite match.

I'd like to hear about your experiences with foamyHexMesh and maybe get an "official" opinion about the issues.
Attached Images
File Type: jpg foamyflange.jpg (91.0 KB, 311 views)
cutter likes this.
zordiack is offline   Reply With Quote

Old   November 25, 2014, 06:22
Default
  #2
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 16
l_r_mcglashan will become famous soon enough
What is the actual mesh quality like from checkMesh?

Those look like it could be a polygon visualisation issue with paraview. If you instead view the patches those artefacts will disappear.
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   November 25, 2014, 06:25
Default
  #3
Member
 
Pekka Pasanen
Join Date: Feb 2012
Location: Finland
Posts: 78
Rep Power: 7
zordiack is on a distinguished road
It's not just an visualization issue. I calculated simple pipe flow with foamyHexMesh generated mesh and there were pressure anomalies along with the "gaps" in the mesh. I've also tried all visualization options paraview has to offer and the holes won't go away. You can check this by zooming inside the mesh or using cutting planes.
zordiack is offline   Reply With Quote

Old   November 25, 2014, 06:33
Default
  #4
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 16
l_r_mcglashan will become famous soon enough
You'll have to provide a full test case, and please post the output of checkMesh when complaining about meshes.
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   November 25, 2014, 07:56
Default
  #5
Member
 
Pekka Pasanen
Join Date: Feb 2012
Location: Finland
Posts: 78
Rep Power: 7
zordiack is on a distinguished road
Ok I need to back down from my latest claim. It doesn't seem to affect the CFD results as I ran it again now. I could swear it did after 2.3.0, but that's probably my error. Mesh can be generated with ./Allrun.

Anyway, here is the test case and checkMesh results for a simple pipe mesh. There are initial condition files in the directory 0.org for running the pipe case with simpleFoam.

https://dl.dropboxusercontent.com/u/...amytest.tar.gz

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.x-c5944c539043
Exec   : checkMesh -latestTime -allGeometry -allTopology
Date   : Nov 25 2014
Time   : 13:35:30
Host   : "frontlight"
PID    : 12990
Case   : /home/zordiack/OpenFOAM/zordiack-2.3.x/run/foamytest
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 202

Enabling all (cell, face, edge, point) topology checks.

Enabling all geometry checks.

Time = 202

Mesh stats
    points:           62811
    faces:            136648
    internal faces:   125148
    cells:            35833
    faces per cell:   7.306002847
    boundary patches: 3
    point zones:      5
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     14341
    prisms:        3
    wedges:        27
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     21462
    Breakdown of polyhedra by number of faces:
        faces   number of cells
            5   2
            6   459
            7   9468
            8   4070
            9   3511
           10   2180
           11   1059
           12   460
           13   170
           14   59
           15   17
           16   5
           17   2

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Topological cell zip-up check OK.
    Face-face connectivity OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
                   Patch    Faces   Points                  Surface topology Bounding box
                cylinder    10846    12484  ok (non-closed singly connected) (-0.05009437746 -0.05011496529 -2.236166981e-18) (0.0501163457 0.05008318806 0.5)
                   inlet      324      483  ok (non-closed singly connected) (-0.04995583898 -0.04998437827 0.5) (0.04999974697 0.04998514011 0.5)
                  outlet      330      495  ok (non-closed singly connected) (-0.04996418047 -0.04994094389 -4.987329993e-18) (0.04999983931 0.05002103416 4.770489559e-18)

Checking geometry...
    Overall domain bounding box (-0.05009437746 -0.05011496529 -4.987329993e-18) (0.0501163457 0.05008318806 0.5)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-7.495268535e-17 1.550779668e-16 -9.362460359e-18) OK.
    Max cell openness = 2.67711213e-16 OK.
    Max aspect ratio = 3.026979926 OK.
    Minimum face area = 1.85472645e-07. Maximum face area = 8.477292546e-05.  Face area magnitudes OK.
    Min volume = 6.113686583e-09. Max volume = 6.081426879e-07.  Total volume = 0.003926260336.  Cell volumes OK.
    Mesh non-orthogonality Max: 43.48830284 average: 6.064106049
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 2.077547245 OK.
    Coupled point location match (average 0) OK.
    Face tets OK.
    Min/max edge length = 1.369775303e-05 0.01306167326 OK.
   *There are 594 faces with concave angles between consecutive edges. Max concave angle = 72.72201769 degrees.
  <<Writing 594 faces with concave angles to set concaveFaces
    Face flatness (1 = flat, 0 = butterfly) : min = 0.8605772727  average = 0.998100246
    All face flatness OK.
    Cell determinant (wellposedness) : minimum: 1.356882461 average: 25.26420198
    Cell determinant check OK.
 ***Concave cells (using face planes) found, number of cells: 82
  <<Writing 82 concave cells to set concaveCells
    Face interpolation weight : minimum: 0.2505709292 average: 0.4521304918
    Face interpolation weight check OK.
    Face volume ratio : minimum: 0.1563647709 average: 0.7474324311
    Face volume ratio check OK.

Failed 1 mesh checks.

End
Now, if the meshing is actually working, how can the mesh be refined only in the wall-normal direction?
Attached Images
File Type: jpg clip.jpg (61.9 KB, 278 views)
zordiack is offline   Reply With Quote

Old   November 26, 2014, 06:49
Default
  #6
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 16
l_r_mcglashan will become famous soon enough
For pipes you could try foamyQuadMesh. You would just mesh a circle and then extrude it however you want.

If you look at one of the tutorials as a starting point:

https://github.com/OpenFOAM/OpenFOAM...llShapeControl

One thing you can do depending on how the surface of your pipe is defined is specify the cell size settings for the pipe (with appropriate values):

pipeSurface
{
type searchableSurfaceControl;
priority 1;
mode inside;
forceInitialPointInsertion on;

surfaceCellSizeFunction uniformValue;
uniformValueCoeffs
{
surfaceCellSizeCoeff 1;
}

cellSizeFunction linearDistance;
linearDistanceCoeffs
{
distanceCellSizeCoeff 1;
distanceCoeff 4;
}
}

To get only wall normal refinement the ends of your pipe will need to be in a separate surface to the cylindrical wall.
Romarius likes this.
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   November 26, 2014, 06:56
Default
  #7
Member
 
Pekka Pasanen
Join Date: Feb 2012
Location: Finland
Posts: 78
Rep Power: 7
zordiack is on a distinguished road
Wouldn't this refine the cells in all directions like in my example? What I'm looking for is refinement of the cells only in the wall normal direction, in the spirit of refineWallLayer or boundary layer addition in snappyHexMesh. Would this be possible using foamyHexMesh?
zordiack is offline   Reply With Quote

Old   December 4, 2014, 11:40
Default
  #8
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 754
Rep Power: 10
sharonyue is on a distinguished road
I just played with this foamHexMesh for fun. And this is a pic from the tutorial of flange: I think its okay, dont forget show the mesh on time step 102.

I didnot change anything, did u change your dict? and did you run collapseEdges? this will filter out the small faces.
I saw many small faces in your latest pic.
Attached Images
File Type: jpg 1.jpg (75.0 KB, 301 views)
sharonyue 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
Problems building foamyHexMesh: CGAL missing? laurent98 OpenFOAM Installation 19 February 17, 2017 07:26
foamyHexMesh boundary layers zordiack OpenFOAM Native Meshers: snappyHexMesh and Others 10 March 3, 2016 07:09
talk about the most suitable way to discretize diffusion term in UEqn bieshuxuhe OpenFOAM Programming & Development 1 April 16, 2014 10:10
foamyHexMesh error ethan oh OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 13, 2014 20:25
Talk more about CFX-4.2 SXF Main CFD Forum 1 May 15, 1999 10:02


All times are GMT -4. The time now is 15:42.