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

STL file

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 13, 2012, 09:28
Default STL file
  #1
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi,

I have problem with newly created STL files.

I use OF-2.1.x.
I have created an STL file with ICEMCFD version 13.
But SHM doesn't see any patch:

Adding patches for surface regions
----------------------------------

Patch Type Region
----- ---- ------
Added patches in = 0 s

Has someone encountered same kind of problem recently.

Best regards,

Stephane
openfoam_user is offline   Reply With Quote

Old   January 15, 2012, 09:53
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Stephane,

OK, there are several reasons why this might have happened:
  • The STL file might not be in a visible place in the initial bounding box mesh.
  • The resolution of the bounding mesh might be insufficient to have enough lines crossing the STL geometry.
  • The names used in "snappyHexMeshDict" might not relate directly to the STL file.
  • Which "snappyHexMeshDict" file are you using as reference? If it was from OpenFOAM 1.7 or older, I think those aren't compatible with the new definitions on and above 2.0.
  • Is the STL file in binary or ASCII format?
  • Just in case... Did you try this with OpenFOAM 2.0.x as well?

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   January 16, 2012, 05:19
Default
  #3
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi Bruno,

None of your proposals solve my problem.

It is strange because when I use the surfaceFeatureExtract command to extract the edges sHM see the edges (and do the refinement). But sHM still doesn't any patch so it can't delete any cells inside or outside.

Best regards,

Stephane.
openfoam_user is offline   Reply With Quote

Old   January 16, 2012, 06:24
Default
  #4
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
Hi Bruno,

If I write as below sHM see the patch:

geometry
{
flange.stl
{
type triSurfaceMesh;
name flange;
}
};

But if I write as below sHM doesn't see any patch:

geometry
{
flange.stl
{
type triSurfaceMesh;
regions
{
FLANGE// Named region in the STL file
{
name flange;// User-defined patch name
}
}
}
};

Why ?

Regards,

Stephane.
openfoam_user is offline   Reply With Quote

Old   January 16, 2012, 16:14
Default
  #5
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Stephane,

I thought it might be something like that. Older versions of OpenFOAM (<2.0.0) allowed that kind of renaming. But with >= 2.0.0, snappyHexMesh considers a more hierarchical name assignment. If I'm not mistaken, you should write "flange_FLANGE" or "flange.FLANGE". Let me check the examples... no, wait, that's only when the naming procedure is done automatically, as shown in the examples:
  • "mesh/snappyHexMesh/flange"
  • "incompressible/simpleFoam/motorBike"
But tutorial "multiphase/interPhaseChangeFoam/cavitatingBullet" does support the naming procedure you are using!


OK, the base example present in the source code at "applications/utilities/mesh/generation/snappyHexMesh/" clearly indicates:
Code:
    sphere.stl
    {
        type triSurfaceMesh;

        //tolerance   1E-5;   // optional:non-default tolerance on intersections
        //maxTreeDepth 10;    // optional:depth of octree. Decrease only in case
                              // of memory limitations.

        // Per region the patchname. If not provided will be <name>_<region>.
        regions
        {
            secondSolid
            {
                name mySecondPatch;
            }
        }
    }
Mmm... upon re-reading your last post, the comments are too much on top of the word itself:
Quote:
FLANGE//
There is no space between the name and the comment marker!

Best regards,
Bruno
wyldckat 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
2.0.x on Mac OSX niklas OpenFOAM Installation on Windows, Mac and other Unsupported Platforms 74 March 28, 2012 16:46
OpenFOAM Install Script ljsh OpenFOAM Installation 82 October 12, 2009 11:47
Compiling OpenFOAM13 on AMD64 with Redhat Enterprise mbeaudoin OpenFOAM Installation 20 June 17, 2008 06:43
DecomposePar links against liblamso0 with OpenMPI jens_klostermann OpenFOAM Bugs 11 June 28, 2007 17:51
PHI file structure Eugene Phoenics 9 November 2, 2001 23:00


All times are GMT -4. The time now is 17:16.