I am bit new to femap.
I am tryiing to do flutter analysis in femap. But i am having problem with geomtry and mesh association. When i try to associate my geomtry and imported mesh(ansys or hypermesh) using MEDIFY>ASSOCIATIVITY>AUTOMATIC mostly it gives error and says (some #of elements and nodes) does not associate with geomtry.
Can someone plz help me and tell me that how can i assiciate my unassociated elements and nodes with geomtry?
How can i solve ths issue?
Solved! Go to Solution.
Is a question of tolerances, but without the model in hand is impossible to know exactly the reason, post the input files here and we will take a look to it, OK?.
Thnx for your time.
i attched 2 mesh (.nas) files from ANSYS one is with 82k elements and one is with 10k elements and .stp from catia. When i import mesh i define properties and materials in NX NASTRAN by my-self and then proceed.
The reason why you get errors when importing mesh in FEMAP is because not any property was defined in the source preprocessor, the third field PID = 0 (Property identification number of a PSOLID, PLSOLID, PCOMPS, or PMIC entry) should be > 0, but has a value = 0, then the error.
GRID, 48447,, 4.533365324E+003, -7.901700000E+003, 2.365613503E+002 $ $ MESH ELEMENTS $ $ Elements <SECTION=ELEMENTS> CHEXA,1,0,176,113,519,517,177,143,+C1 +C1,580,518,1061,1062,2074,1247,1245,1060,+C2 +C2,2078,2073,1150,1151,2075,1249
Apart of this, the solid geometry coming from CATIA has interferences and penetrations, you need to be aware of this, meshing with solid elements directly this geometry will cause later problems like "lack of continuity in displacements", in summary, not possible to define a consistent mesh. Please note meshing with solid elements parts with thin walls (ie, very low thickness compared with other two dimmensions) require to have at least three elements in the thickness to capture properly the stress gradient in the part, then you will realize the resulting model size will be millions & millions of nodes, not hardware exist to compute this model, OK?.
And the imported mesh is poorly extremely shaped, HEX elements terrible skewed, if I run in FEMAP the command TOOLS > CHECK > ELEMENT QUALITY I see a lot of elements failed to pass the minimum quality required by FEMAP, for instance you have a TET ASPECT RATIO (ie, TET COLLAPSE) bigger than 159!!, then the NX NASTRAN solver will give you error for sure when solving!!. Having FEMAP, not reason to import any mesh, in FEMAP you have powerful tools to repare geometry, idealize geometry and mesh with quality elements.
Element Quality Quality Check Number Failed Worst Value Aspect Ratio 2541 23.25683 Taper 0 3.181146 Alternate Taper 76 0.55632 Internal Angles 69632 113.296 Skew 33476 0.384287 Warping 35 22.64136 Nastran Warping 0 0. Tet Collapse 1219 159.0267 Jacobian 2232 0.9819 71305 Elements Failed out of 82448 Checked.
In summary, here the error message when trying to associate mesh & gometry is the less important, you have to solve previously the important decision of the MESHING APPROACH to follow to mesh this problem properly, I will give you ideas:
Great, thanx alot @Blas_Molero,
thnx for your kind help.
I just started using femap for flutter anaysis 2 months ago so i am new and for sure my meshing is very terrible in femap. That is why am importing mesh from other softwares like hypermehs or ANSYS. I searched alot but havent found any effective video.
Can you kindly send me any link from which i can learn basics of meshing in femap effectivly? this will help alot.
Waiting for your kind reply,
Flutter dynamic analysis is for expert FEA users where the basic concepts of meshing is supposed to have acquired already, don't pretend to perform a dynamic analysis of an airplane meshed with millions of tetrahedral solid elements, simply impossible, this is not linear static analysis (SOL101), then you need to learn the basic: how to mesh, what finite elements to use and why, how to prepare and idealize geometry, etc.., I suggest to ask training to your FEMAP provider, this is the first point to request help.
You can also visit my FEMAP & NX NASTRAN SUPPORT web site (http://www.iberisa.com/soporte.htm) and BLOG (https://iberisa.wordpress.com/) where you have plenty of videos & posts to learn the basic. Also enter in FEMAP and go to HELP > EXAMPLES, there you have a lot of examples to practice and get trained in FEMAP, OK?.