Showing results for 
Search instead for 
Did you mean: 

3D Mesh weld


I'm trying to simulate an arm for bending. The arm has an I beam cross section but it is created by stitch welding two C beams togheter. The stiffness is controlled by the length and the spacing of the welds.The two C beams are seperate 3D meshes.


What is the best way to simulate these stitch welds? I would like to keep the FE model as a 3D mesh because of other bodies connected to the end of the arm. 


Please see attachments for further reference. Thanks in advance. 


Re: 3D Mesh weld

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom


Based in your picture you can use a few meshing strategies here:




RBE2 elements:

You can ignore the weld and capture its mission, ie, defining a rigid joint: for this purpose you can use rigid RBE2 elements between both parts, just between the two regions where the welding is performed. You need to divide both beam profiles to isolate the welding regions, and then use commands under 1-D CONNECTIONS to define a "many-to-many connections", ie, a node-to-node connection. You need to select multiple source nodes and multiple target nodes, then NX AdvSim will pairs source and target nodes to create a connection mesh using RBE2. Select the method by Proximity, then the software will pairs locations by finding the shortest distance between the source and the target.


As a general guideline, the source and target selections should contain the same number of nodes or points. This ensures that each source node or point will be paired with a target node or point. If the source and target selections are unequal, the software pairs source and target locations using the specified Method of connection and ignores the remainder. If you select multiple source and target nodes using one of the selecting methods, you get the most predictable results if the source and target selections have a similar distribution and pattern of nodes.


GLUE face-to-face

Yes, in fact, GLUE can be used to define a local rigid "weld-like" joint between bodies of an assembly, this is defined in the SIM environment. This option to glue elements together is available in NX Nastran solver during solution. Glue is a simple and effective method to join meshes which are dissimilar. It correctly transfers displacement and loads resulting in an accurate strain and stress condition at the interface. The grid points on glued edges and surfaces do not need to be coincident. Glue creates stiff springs or a weld like connection to prevent relative motion in all directions The key is to define correctly the "distance" between SOURCE & TARGET regions, enter the maximum separation between surfaces.


Surface-to-surface glue can be defined on the faces of the following elements.

  • Shell elements CTRIA3, CTRIA6, CTRIAR, CQUAD4, CQUAD8, and CQUADR.

  • Solid elements CHEXA, CPENTA, CPYRAM, and CTETRA.

The software creates a glue element if:

  • Any of the source element normals intersect with an element in the target region.

  • The distance between the two faces is equal to or less than the search distance which you specify for the glue pair on the BGSET entry.

Surface-to-surface glue definitions are supported in all solution sequences except for SOL 144–146, and 701.



Well, you always can treat the seam weld like an assembly, creating a 3-D solid geometry of the seam weld and mesh using 3-D solid elements, either HEX or TETRA. The connection could be using the above method GLUE FACE-TO-FACE, or merging nodes in the FEM environment using the Mesh Mating Condition to connect individual 3D meshes together at a specified interface.


Well, as you see you have many options. The best one depends of what you need to know best:

  • If your main concern is to know what happens in the seam weld locally based in stress results, then meshing explicitly the seam weld using HEX elements should be your method.
  • If your target is to know the general stiffness of the beam profile or the buckling behaviour of the assembly, then GLUE FACE-TO-FACE is easy to implement and fast to solve.
  • RBE2 elements should be your last resource: it generates locally important stress concentration -as consequence of the nature of the rigid elements- that are difficult to explain in an stress report ...

Good luck!!.

Best regards,


Blas Molero Hidalgo, Ingeniero Industrial, Director
Blog Femap-NX Nastran: