Hi, recently I started using Femap.
I must create a geometry with a T shape using two perpendicular surfaces. Each surface has a thickness of 2mm, so i created the vertical surface at a 1mm from horizontal surface to avoid penetration.
Is possible to connect the two surfaces without use the Femap Connect options?
I tried to merge the vertical surface nodes with the related horizontal surface node, but i have penetration.
How i can connect the two surfaces without penetration?
Solved! Go to Solution.
You can use any of the following meshing approachs:
1.- Classic method: Stitched Midsurface Mesh
Simply extend the vertical surface till intersection with the horizontal one, and create a NonManifoldAdd geometry using command "Geometry > Surface > NonManifold Add". Mesh the Sheet body and you will have the T-joint meshed correctly. Yes, you have penetration, but it can be perfectly neglected: when you mesh with Shell elements is because you are telling that thickness of shell elements is small compared with the other dimensions of the element. If not, then better use SOLID CHEXA elements.
2.- GLUE EDGE-TO-SURFACE:
You can create the vertical surface at 1 mm from the horizontal surface and then define a GLUE edge-to-surface between Shell element edges (SOURCE Region) and shell element faces (TARGET region).
NX NASTRAN 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, but is recommended to use similar mesh density.
The following picture shows the way to define correctly a SOURCE EDGE REGION defined by curves and output by nodes:
A simplistic description of edge-to-surface glue is that the software creates pseudo-faces along the edges in the source region. It then connects these pseudo-faces to the shell or solid faces in the target region with stiff springs or weld like connections.
From the glue points on the EDGE SOURCE region the software projects a normal in the outward normal direction. In addition, the software searches a small distance in the inward normal direction in order to glue edges and surfaces that may interfere due to meshing irregularities.
A glue connection occurs when the following is satisfied:
For example, the green line below represents shell faces in a midsurface TARGET region, the blue line represents midsurface shell elements, and the red line represents an internally created pseudo-face along the edges in the SOURCE region. The pseudo-face can be visualized by extruding the element edge from -t/2 to +t/2 in the parent shell element normal direction.
3..- RBE2 RIGID Elements
Well, this should be the last resource, this is the method we used in the old times previous to NX NASTRAN V7.0 when the GLUE METHOD didn't exist. You can define RBE2 elements nodo-to-node to define a rigid joint, but is hard to explain why you have SUCH ARTIFICIAL big stress concentrations in the joint ...
In summary, if you have special interest to know what happens locally in the T-Joint (for install, you need to perform a fatigue analysis in the seam-weld) then forgot at all of using there GLUE or RBE2 elements, you will need to mesh locally the joint using the classic method of stitching shell midsurfaces or a more local approach using SOLID CHEXA elements, OK?.
Dear Blas_Molero thanks a lot for your answer.
I have found another solution:
when i do the horizontal surface mesh in Mesh;Geometry;Surface; i selct More Options;Offset;Surface To Bottom Face; in this way all thickness is directed downwards. So i can create the vertical surface with the edge on the horizontal one without penetration and merge the coincident nodes.
Anyway I will try to use your own solutions and compare results.
The drawback of your meshing approach is just the OFFSET, I want to warm you of the important limitations of using OFFSETs with Shell elements with the NX NASTRAN solver, look why:
Generally, you should use OFFSETS if you have a sufficiently fine mesh in the region where you want to define the offsets. If your mesh is more coarse, using rigid elements (RBAR, RBE2, etc..) to define offsets is generally more accurate.
NX Nastran doesn’t modify the mass properties of an offset element to reflect the existence of the offset. If you need the weight or mass properties of an offset element for your analysis, use the rigid element method to create the offset.
Offsets in the CBEAM and Shells CTRIA3 and CQUAD4 elements are not allowed in combination with nonlinear material, then one never knows what type of analysis is required to perform (a double-check with nonlinear analysis is always required!!), so is good to let the FE model correctly defined from just the beginning.
The results in linear and nonlinear buckling with offsets may be incorrect.
In summary, I hope you see clear my position about OFFSETS, I try to avoid them as much as possible!!. Definitely the classical approach is always the best ....
Thanks for the clarification.
I must do a modal analysis and a FRF analysis on a sandwitch pannel. So to study high frequencies the skin mesh is very fine.
What do you suggest me in this case?
To learn how to perform a FRF using FEMAP take a look to my blog in the following address: