Using Femap 11.3.1
See solid body with the 2 smaller holes in figure 1. I am tet meshing this solid. I wish to create 2 layers of small elements around the hole and the rest of the mesh can be much coarser. In figure 2, you can see that I created concentric circles that represent the 2 layers.
I used the command: Slice > With Curve > Match Faces across slice. I then select the main solid to be cut and I select the concentric curves to use as cutting tools. The geometry that results is perfect: the main solid body now has a hole with two concentric pipes running through it.
Figure 3 shows 1 of the "pipe solids" highlighted in yellow as an example.
However, the meshing does not obey the 'match face across slice' as can be seen in figure 4. I set a small mesh size on the pipe solids and a larger mesh on the main solid. The meshes do not match at the interface. This seems like a bug in the slice command since I specifically asked to match across slice.
How can I accomplish my goal? I have also tried slicing using "Geometry > Solid > Embed Face" and I get the same results (i.e. unmatched mesh).
Solved! Go to Solution.
You need to select simultaneosly the 3 solids in order to run OK the "Adjacement Surface Matching" feature of the "MESH > MESH CONTROL > SIZE ON SOLIDS" command.
Blas - Thank you. But how can I have different sizes on the different solids if I use your solution? It will override individual sizing.
I want small elements where I need them ->pipes and larger elements where I can -> main block. Femap should enforce same size at interface and then transition to coarser elements automatically.
Is this not possible in Femap?
The meshing approach is basic in FEMAP: go from global to local, first in solids, next in surfaces and finally in curves!!. I have recreated a simply problem, each solid has a different color.
I have applied a global element size =5.0 to all solids using command MESH > MESH CONTROL > SIZE ON SOLIDS, using a Max angle tolerance = 15 (default is 25):
The result is the following:
And here you are the resulting TET mesh: a regular mesh, not mesh transition used.
But if you want to have refined mesh in the inner solids then DELETE TET MESH and use command MESH > MESH CONTROL > SIZE ON SURFACES and using METHOD=BY SOLID select all surfaces of the inner solids (pipes) using -for instance- and Element Size=2.5 mm
The result is the following, make sure that all curves have the same element size as well, use locally command MESH > MESH CONTROL > SIZE ALONG CURVE as required, OK?.
Next TET mesh the solids, make sure to activate MERGE NODES option:
The result is a refined mesh in the inner solids ....
But if you want to have a quality mesh & accurate stress results with minimum model size I suggest to forgot at all using TET meshing and play with HEX MESHING + MESH TRANSITION using command MESH > MESH EDTING > INTERACTIVE, then you will arrive to examples like in the following picture: next you can combine TET with HEX mis¡xing mesh elements using GLUE SURFACE-TO-SURFACE, is a great feature in NX NASTRAN solver:
To learn more take a look to my blog in the following address: