I'm having problem creating tetrahedral mesh on my model. More precisely meshing two parts with matched surface i get following message:
Tet Mesh Solid
1 Solid(s) Selected...
Unable to link mesh locations between Surfaces 4501 and 7165. Surfaces must be on same solid or must be coincident.
233 Node(s) Merged.
Elements do not form a closed outer surface. There are free edges.
2 independent surfaces located. 0 voids.
MESHING SOLID 108 ______________________________________________________
-- SURFACE MESH 2 Triangles
-- SURFACE MESH QUALITY
MINIMUM ANGLE _____________________
25.0 > A > 15.0 1 Elements
0.5 > A > 0.0 1 Elements
Worst Angle = 0. Element 77281 (92752 92753 92755)
Shortest Edge = 0. Element 77281 (92752 92753 92755)
Longest Edge = 3. Element 77282 (92419 92753 92752)
>>> ERROR: ERR 5621
>>> ERROR: FACE 1 WITH VERTICES : 2 3 4
>>> ERROR: SMALL INRADIUS : 0.000000000000000E+000
Surfaces must be on same solid or must be coincident and they are coincidental, but mesh is only generated on one solid. I used Mesh Size on Solid with Assembly/Multi-Solid Sizing to achieve surface match.
What can cause this problem and is there some way to avoid it?
Just a little digression, what I'm actually trying to achieve is something similar to:
but with this method i get poor element quality, so i made triangular prisms to control elements in volume of solid.
Geometry after removing volume of prism.
Every help or advice is greatly appreciated. Thanks in advance.
The TET mesher runs OK if both surfaces are not only coincident, but have exactly the same geometry. I means that both surfaces should have the similar curves, length, size, etc..
Try to mesh the surfaces of the solids with 2-D PLOT-ONLY seed mesh, if your 2-D mesh is successful then the 3-D TET mesh will be OK.
Or post your FEMAP model here and we will take a look to it.
Thank you for your response Blas.
I always prepare surfaces so that they have same geometry.
I found that there are several issues that can cause the problem i described.
The easiest scenario is when you have completely identical surfaces, points and lines mach perfectly,mesher can't create mesh and reports that there are nodes that causes errors. Solution for this is just to create one or two slices across surfaces and it will help mesher to generate mesh.
Second scenario (that caused me a lot of headache) is caused while using Solid Remove. Edge on surface is divided in two places instead of one or it isn't divided at all. So now instead of just two break points on two coincident edge lines it ends up with more points. Distance between those points is around 3.5E-7.
Through whole model i use same order to get my geometry, and i get this problem only few times.
For this i used Move by Point and moved points that desen't mach and then return them all on same coordinate, but Move by Point doesen't always work on solids.
Do you know some of conditions in with Move by Point doesn't work on solid and is there some other method to deal with those points, because order of E-7 very small or there is some other tolerance and distance between those points is outside of tolerance for generating mesh.
A command I use a lot with success is SOLID CLEANUP > ADVANCED activating the option to remove small edges, this is a great command, and I use it when the standard GEOMETRY > SOLID > SOLID CLEANUP command do not remove small edges or sliver surfaces. Play with the small edge tolerance and you will see a great improvement, this is a little jewel hidden between commands available in FEMAP since many years, but really powerful.
In general I don't use MOVE BY POINT command a lot, depends of the problem type, better post your FEMAP model here to see the best approach to follow, OK?.
Also, is very important you run the newest version of FEMAP V11.2.1, you have a lot of enhancements in geometry manipulation, we are the ENVY of most CAD systems!!.
there is an another method to repair this problem. You can make combined surfaces and combined curves from problematic surfaces and curves. So you don't need to repair solids, and surfaces will match to mesh sizing.
I completely overlooked Solid Cleanup. In past i only used Solid Cleanup to remove redundant geometry and sliver surfaces, but i will definitely check those advanced options.
I think that this is just what I needed, because my problems originates of very complex geometry. Just for reference, part of a model I'm working on (400x200x115m).
Thank you Blas, I appreciate your help.
Peter, I use a lot as well the MESHING TOOLBOX Combined/Composite Curves & Combined/Boundary Surfaces commands, but I see a problem here: if later I want to perform any geometry operation with solid (say GEOMETRY > SOLID > SLICE) then the solid body is difficult to edit, or at least the resulting geometry is not predictible. Then always I let the Combined commands under MESHING TOOLBOX for the very last step, when no more geometry editing is required.
Milan, I am happy you discover the SOLID CLEANUP >ADVANCED, I like it a lot because any change in the geometry is not radical, is like "natural" editing!.