hexagon logo
Register Sign in
  • State Not Answered
  • Replies 7 replies
  • Subscribers 5 subscribers
  • Views 106 views
  • Users 0 members are here
Options
Related

Node merging for bodies of two differents parts.

kenny.fernando.conto
I made the model by parts due to each part has different mechanical properties. I would like to marge the common faces nodes but, unfortunately, MSC Apex can not realise that procedure if the bodies created belong to different parts. How can I solve it? if that is not possible, What is the best method to mesh the geometry and that the common faces nodes being merged?
  • 0
    Currently it's not possible to merge the nodes directly. This is due to the way the Apex solver works with its Computational Parts. In a future release you will be able to have common nodes between Parts.
     
    Right now to connect the Parts you can use the tools in the Interactions palette: Mesh Dependent Tie (previously called Edge Tie) or Mesh Independent Tie (previously called Glue), depending on how you want to handle the connection.
     
    Screen Shot 04-16-20 at 08.25 AM
    Screen Shot 04-16-20 at 08.19 AM
  • 0
    Dear Darrel,
     
    Thank you for your reply. We need to do a continuous solid for our purposes (coupling with elastodynamic BEM). Thus, mesh independent tie is not valid for us. With the mesh dependent tie we cannot do the interaction between two solids, if I am not wring.
    Previously in Patran, if I remember properly, we were solving this issue by making that the geometric interaction surface of two solids in contact is the same. Then, when the mesh seed is applied on that face, it works in the same way for both solids. We you automatically mesh that two solids, the FE nodes appearing at that interaction surface are shared by the two solids. Can we perform a similar action in Apex?
    Another option is to have a single partitioned solid. In this case, how we can set different properties for the different partitions?
    Thank you very much
  • 0
    No, your Patran method won't work in Apex. For a partitioned solid, you can assign properties to individual cells by using the pick filter:
     
    Screen Shot 04-16-20 at 02.01 PM
    Screen Shot 04-16-20 at 02.02 PM
    I hope this helps.
     
  • 0
    Thank you so much. That was useful in order to solve my problem.
  • 0
    @darrel.sinclair (MSC Software)
     
    the above explained method for connecting two solid body mesh is applicable for 1D mesh as well?
    Looking for 1D mesh(Curve mesh) to connect.
    Also how to assign the Geometrc properties to this elements.
    for example:- if Circular BEam , then how to assign the Area.
    MAterial properties etc.
     
    Will wait for your response.
  • 0
    No. For 1D meshes, if they're in the same Part they will automatically be connected. If they are in different Parts you need to specifically create connections: a good option for this is to use Auto Connect Vertices in the Custom Tools menus:
    Screen Shot 04-21-21 at 10.15 AM
    Creating section properties for your beams is done using the Beams tool:
    Screen Shot 04-21-21 at 10.21 AM
    Assigning material properties can be done from the Materials tool:
    Screen Shot 04-21-21 at 10.22 AM
    You can find full descriptions of all of these in the Apex help.
  • 0
    in relation to the original question, did you consider uniting the two component solids into a single solid body (Geometry Edit Tools > Boolean > Merge), then partitioning the two joined parts using a separate surface that defines the interface (Geometry Edit Tools > Split Tool > Split using offset face > Offset Distance 0.0 > Split Behaviour = Partition). It's a work around, but you will end up with a continuous mesh, with element faces lying on your intended boundary surface. Cheers. Andrew
© 2025 Hexagon AB and/or its subsidiaries. Privacy Policy | Cloud Services Agreement