open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi,

working on a river mesh by differencing the river bed and the floodplain, i'd like to know if there is a better and smarter way to detect and correct flattened triangles with sharps angles than to delete them one by one manually... They are concentrated on riverbed's boundaries and most of the time difficult to select.

Thank you in advance!
Max.

Hi Max,

The best way to get rid of very slim elements is to not generate them in the first place.

The process of mesh generation in Blue Kenue is meant to be parametric. That is to say that you should adjust the input to the mesher and let it do the "heavy lifting" rather than focus on manual editing. IMHO the advantages of this approach is that it is repeatable. That way when you need to modify certain areas of your mesh further on in a project you simply change the input to the mesher rather than having to redo a bunch of manual edits.

I suggest you start by adjusting the density criteria.

If you're still having problems, post your t3m file here so I can have a look at it.

Hope this helps... Martin

Hi Martin,

Thank you for your answer, it helps me reconsidering the mesh approach.

As a beginner with Telemac, i use BlueKenue in order to generate the mesh, selafin files, and Fudaa for the initial and boundary conditions. I still find some difficulties in adjusting the mesh. I have for example one flat triangle that generate a problem while simulating the project with Telemac:

" INBIEF (BIEF) : MACHINE NON VECTORIELLE (SELON VOS DONNEES)
GEOELT: ELEMENT 40048 : DETERMINANT NEGATIF "

I corrected it by editing the node position manually. I would like to know if it's possible to tackle this differently (maybe directly in Fudaa?) in order to avoid coming and going between Blue Kenue and Fudaa. Please find, the concerned triangle and my t3m file.





Your comments are very welcome as it's my first project with Telemac and working alone on it doesn't help me much. I don't know what i don't know ^^.

Thank's,
Max.

Hi Max,

A couple of comments about your t3m file.

1. In a number of locations you supply constraints in the form of "soft lines" that are superimposed on or are VERY close to the outline and/or the edge of your submesh. This should be avoided.

2. You have a number of constraints that are fully within the outline polygon of your submesh. These have no affect on the mesher since the elements in the area covered by a submesh are considered fixed. These will not cause problems but do add confusion when debugging the result mesh.

3. One of the density objects "Crete_amont_5m" is a simple open line and will have no affect on the mesher.

4. The ends of your submesh are very close to the outline. It is best to have the edges of the submesh either pierce the outline or be well within it. (at least 1 element width)

Hopefully the following bit of info will help you understand what is going on.

In the meshing process, the very first step performed is the resampling of the supplied outline. A current limitation of the mesher is that this resampling only uses information from the density object. (ie. geometry from hard & softlines, points, submesh nodes etc. are not taken into consideration when generating outline nodes) We hope to fix this in a future release but for now, it's something that we must live with.

Lastly, nn some areas of your mesh the element sizes are less than 1m.
I suggest you shift your source data to resolve truncation of coordinate data problems you will certainly see.
See post #5626 in the topic "Flat triangle in mesh generated with BlueKenue" for more info.

Hope this helps...
Cheers... Martin