3-way surface intersection & fixing edges of surfaces.

JamesHJamesH
Hello I am a new user figuring things out.

What is the most convenient way to deal with this work flow?

A 3-way intersection between surfaces, they need to be different components to have different materials, so I import them seperately. I copy mesh parameters and mesh them together, the meshes visually line up, but the result is they are not connected?




i found I can merge nodes by proximity, is that the only method?

Comments

  • SebastianmaklarySebastianmaklary
    You can also use constraint equations for tying nodes together but that is a very manual process.
  • disladisla
    Hi @JamesH ,
    -For simple stiffeners you could also try to use manual mesh generation by extrusion.
    -*Tie should also work here.
    Regards
  • FatmacFatmac
    Have u tried merging nodes?? keep the surfaces as different compounds so u can have them as different materials but use merge nodes to tie them together - if they are not exactly coincident then try slow increasing
    the merge tolerance till they merge. If u upload the file I will happily have a quick look
  • JamesHJamesH
    yes I am aware of merge nodes, this does seem to work, provided the number of nodes along edges are very closely matched.
    Is there a way to select edges before meshing, to inform the mesher that these need to be joined, or at least have the same number of nodes/spacing, so that I can reliably merge nodes after the meshing?

    I'm wanting to run FEA on a yacht, with a large number of different sized panels, bulkheads and stiffeners all connected.

    for now I am just practising on this simple panel with a stiffener to get a good workflow before I attempt the larger yacht structure.

    I have attached an STP file.
  • polymathicpolymathic
    This is highly relevant to me, professionally, and for mine is the Number 1 limitation in the open source/accessibly priced meshing world.

    Ansys has shared topology. Altair Hypermesh has seam welds. The best I’ve found in FOSS world is that Gmsh can take compulsory nodes as an input to a mesh command, so you can mesh part A first and give the coincident edge nodes in the mesh command for part B then merge at zero distance. Gets a bit icky where element edges are far from parallel.

    Doing the merging by hand or using tie is ok… until you have a chassis of hundreds of parts and you need to iteratively design.
  • SergioSergio
    Hi @polymathic I have tried to mesh your part in Salome, and looks like the surfaces have some errors, such as the edges of some faces are not shared or coincidents with the adjacents, very different to what I see when I model with standard CAD tools like Solidedge/Solidworks or FreeCAD. Your model looks made in Rhino, is there a way to improve those details?
  • VictorVictor
    Gmsh is probably best for this. It's hard to work out the command to do it properly but I think a key is this: 
    SetFactory("OpenCASCADE");
BooleanFragments{ Surface{:}; }{ Delete; };
    That merges adjacent edges of surfaces at the geometry level before meshing, then they end up still merged in the mesh. Unfortunately, it also makes duplicate surfaces for some reason. I'm not sure if that's an issue with the STEP file or not?




  • polymathicpolymathic
    @Sergio, I'm not the OP, should be @JamesH tagged so he is notified.

    I was just commenting on the method I have tested to get around the problem for myself.
  • disladisla
    edited December 2025
    Hi,

    I recall some years ago Sergio found the way to create a compound part in GMESH before meshing so the mesh was conformal in between the different parts.
    Maybe it could work here.

    https://mecway.com/forum/discussion/comment/3956#Comment_3956

    EDITED: Sorry my browser didn't update last posts. I think it is the same solution proposed by Victor. Seems it generates some surfaces dublicated isn't it.


  • JamesHJamesH
    Thanks all for the responses.
    Yes I work in Rhino, which is less anal about tolerances than other CAD software, though you I can dial up the tolerance before export.

    Above was just a simple example, I am wanting to do FEA on entire yacht structures where this problem repeats across hundreds of components. So my workflow which I find to be working is to do the meshing in Rhino, then using a Rhino Python script to write the rhino mesh direct to a new .liml file.

    A big advantage for me, as all the structures are composite and element orientation is critical. Is that I can control the element orientation inside rhino through UV mapping, so its all written to the liml file :D

    And being a daily Rhino user for years, its much quicker for me to orient UV maps, perform mesh cleanup, refinement, merge nodes etc. before export, than it is to do inside the Mecway UI.

    so far so good...
Sign In or Register to comment.

Howdy, Stranger!

It looks like you're new here. If you want to get involved, click one of these buttons!

Sign In Register