I have prepred Porous material structure using voronoi Tesselation method. Now I have to perform FEA using FEMAP software. but when I try to do mesh there are error, it says mesh aborted.
Could you please someone help me out with this problem. In the attachemnt please see the error message prompted during the meshing.
Looking for ward to hear from someone soon.
FEMAP is very powerful performing TET meshing, but miracles ... first you need to have a valid 3-D solid, check the geometry quality using GEOMETRY > SOLID > CLEANUP command:
Even if th solid is not a proper 3-D solid (i.e.,the volume is not closed, only surfaces) you can create a valid 3-D solid mesh using command MESH > GEOMETRY > SOLID FROM ELEMENTS, in this case you need to mesh the surfaces with 2-D planar elements enclosing the volume instead of a solid. The key is to avoid gaps between 2-D elements, you need to have a fully closed 2-D mesh, then ask for free-edges.
Another option in case of complex 3-D solid geometry is to use command MESH > GEOMETRY PREPARATION, this command makes magic: it uses a combination of automatic curve/surface splitting, creation of Combined Curves/Boundary Surfaces, and feature suppression to likely improve mesh quality. In addition, this command will “prepare” some parts to a degree which will allow FEMAP to successfully mesh the part. I suggest to use "default" parameters.
Thank you very much sir for the answer.
Well, I tried both the technque still error occuring, the model I have is porous structure. it is in solid form.
could you please tell me how can I proceed.
Just to be sure it is in solid form, if you use Tools -> Mass Properties -> Solid Properties, Femap must report a volume for the solid for it to regard the solid as a proper solid.
Also, using the Meshing ToolBox and the Toggle entity Locator icon, the solid must have no Free Edges.
Lastly, due to the obviously complex geometry, you should make sure the mesh merge tolerance (Tools -> Parameters) is smaller than the shortest geometric feature in your solid.
And you probably should try a very fine mesh size compared to the small geometry features in your solid.
The error is probably happening because some of your geometry features will be too small compared to the chosen mesh size.
The smallest element edge is 1/100th of the longest element edge. Presumably you have set a mesh size of about 0.05. Femap reported the smallest edge as 0.000356. This is very small compared to your mesh size, and usually means you have some tiny features, which may or may not be suppressed.
Please advise what mesh size you set and how you did it.
Please advise what merge tolerance you have set.
Please advise the approximate shortest curve length is in your solid (using the Meshing Toolbox entity locator).
Please advise the approximate smallest surface area in your model also using the Meshing Toolbox entity locator.
There is a high chance that you have suppressed curves or surfaces as a by-product of having tiny curves and using default settings for mesh sizing a solid. These suppressed curves may represent a problem.
Please highlight supressed curves and surfaces via the Feature Suppression section of the Meshing Toolbox.
If Femap cannot succesfully form a closed domain of merged surface elements (a surface mesh of your solid must have no free edges), then it will fail to create a solid mesh,
If you have numerous tiny features, these are probably causing your mesh to fail.
Mesh -> Geometry Preparation might help you out automatically, but if you have numerous tiny surfaces and curves in that solid, you may need to use Meshing Toolbox -> Combined Curves and Combined Surfaces so the mesher is not attempting to put "big" mesh onto microscopic features.
Femap is very precise, but if asked to perform a mesh that is unreasonable it will fail. for example if the mesh size is coarse for geometry that has undercuts and "void cracks", then it may attempt to produce elements which are inside out - and fail.
If you want to mesh to small features in a complex geometry, I suggest a maximum mesh size of only 5 to 10 times the smallest feature. If you don't want to mesh every tiny feature, you need to turn tiny detailss into larger ones, or have them "ignored" using a combination of Combined Curves, Combined Surfaces and /or Feature Suppression.
I was using 0.02 element size as a Tet mesh. which was causing error.
I appreciatre for the detailed informtion, but I am just wondering that If I will use mesh size less than 0.000356 it will be too core.