Meshing of sheet metal assemblies

Hi Guys,

I am totally new with Mecway and not very familiar with FEM. I would like to do static calculations on big welded sheet metal and four cornered shafts. (See some example attached). I want to get a volume mesh on it without special preparing of the model for the calculation. Netgen cannot generated a mesh on it, and Gmsh does completely crash the windows system.
Does anybody know if there is a possibility to mesh such geometries?

Thanks for feedback and regards, Roland


  • Is possible to mesh but considering the part composed by several bodies. Is better to modify the geometry into only one solid body.

    1890 x 936 - 200K
  • Hi Andrea,

    thanks very much! The mesh looks really good for what I want to do. Can you please tell me how you managed to mesh it?

    Regards, Roland
  • In your CAD package open the file and export every component as a single body step file (I did it with FreeCad), then import all in Mecway and mesh separately. Then you must join the parts (meshes) with bonded contacts.

    For this kind of geometry I would mesh it as surface elements with mostly quads and then extrude to create hexas, two or three along the thikness.


    2017-11-27 19_38_07-assembly.liml - Mecway.png
    1362 x 726 - 92K
    2017-11-27 19_38_26-assembly.liml - Mecway.png
    1362 x 726 - 145K
  • Some parts intersect each other which is probably why it's not meshing. To see where, make a surface mesh (which works), and use the cutting plane slider to look inside. No doubt, converting it to a single solid body in CAD as Andreas suggested will correct this.
    surface mesh.png
    1366 x 738 - 87K
  • Thanks again! Your comments are quite helpful. Is it possible to use bonded contacts for parts that are intersecting each over are just have a line contact?
    I tried to contact two intersecting bodies in a simple model, but it did not work.
    Also by merging the parts into one solid netgen doesn ´t work. Is there any possibility to get Gmsh working?
  • Is it possible to use bonded contacts for parts that are intersecting each over are just have a line contact?
    I´m not sure, try changing the tolerance zone

    I tried to contact two intersecting bodies in a simple model, but it did not work.
    Maybe this answer the first one. But why not just fix the CAD to get the right geometry?

    Also by merging the parts into one solid netgen doesn ´t work. Is there any possibility to get Gmsh working?
    I was able to merge the bodies in Salome 8.3 (Fuse is the boolean option) and then create a conformal mesh, but again, in my opinion this mesh is not accurate, you need more elements in thikness and with tets the model will be excesively big.

    2017-11-27 21_47_40-SALOME 8.3.0 - [Study1].png
    1362 x 726 - 337K
    2017-11-27 21_53_04-Mecway.png
    1362 x 726 - 144K
  • By the way, you could try to export the fused geometry as step in Salome, and then try to mesh it in Mecway to get an associated cad/mesh model.
  • For linear analysis, bonded contact can be on intersecting parts. Not sure what you mean by a "line contact" - I don't think two solid meshes can intersect at only a line - they would have some volume in common if they intersect. A limitation is that the slave nodes have to be able to be projected onto the master faces. As long as the master surface is flat, that shouldn't be a problem.

    For nonlinear analysis, you have to use TIE which is OK for small intersections and you need to set the tolerance value as Sergio said.
  • On my experience welded component are modelled as a multibody parts for convenience to put them into a drawing but for FEM I modified the assembly into a single part to save time and to avoid to build contacts. I sometimes model the fillet joint as a single part to exptapolate not the stress but the forces at the interface with the parent material. Is a hard job and is necessary to evaluate if there is a convenience of that. For groove joints I prefer single body.
  • Really thanks for your answers!
    To do fast calculations on concepts of such welded assemblies it would be great to get automatic mesh without manual preparation. I now got the assembly meshed after merging the bodies together. Now I will trie to get the complete structrure meshed.
    What is your experience on Netgen and Gmsh?
  • Modify of the model is normal routine for FEA. For example think at your assembly where a plate has a line contact with C profile. Is it real or it will be filled with weld?

  • About Netgen, normally I get better results (meshes) with it than Gmsh.
  • Hi Guys again!

    Thanks for your advises. I tried out some things the last nights, and killed my illusion to get the mesh simple on the assembly.
    I tried out Salome and worked with explode, fuse and partion (its a bigger one than the step data above), but I did not get a mesh on the optimized solid with Salome or Mecway. There must be still a lot of failures in.

    Another way would be to mesh the parts singular in Mecway. When I have for example to plates welded that are not in a 90° angel, I make the goemetry a bit bigger than in reality to get an intersection. But I could not fit them together in a proper way with "merge". Its almost impossible to create the geometry with all contacts plane to each other, to bring them together with "bonded contact".
    Is there ananother way to bring the meshes of different parts that are intersecting in Mecway together?

  • For this kind of geometries If they are perfectly modeled in the cad, then it should be able to merge it on the same cad program. As you say, sometimes you need to force the intersection to make the fusion to work. If you cannot do it in the cad, surely in Salome would not allow neither, is not magic. Anyway is not a problem to work with TIE to join the meshes in case you cannot make as one continuous body. Feel free to upload or sent me the model maybe we could find the problem.
  • Hi Sergio,

    really nice! Maybe a strange question, but where can I find the TIE function in Mecway?
  • Is called bonded contact
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!