It seems to me that you are meshing the crane using 2-D SHELL elements, correct?.
If this is the case, then the reason of the problem is the lack of NonManifold Sheet body creation: you need to use command GEOMETRY > SURFACE > NonManifold-Add to stitch all surfaces together, this command allows you to essentially Boolean Add sheet solids to one another.
The following image shows you the difference between NonManifold-Add surfaces (also named General Body Add) and Sheet Surfaces and Solid bodies, please be aware of the different icons used in the Model Info tree:
The use of Non-Manifold Geometry can be very useful (I will say CRITICAL) in creation of mid-surface models with “T-Junctions”, models where shell elements (2-D) and solid elements (3-D) need to be connected and portions of the shell mesh are embedded into the solid mesh, and “solids” with internal “surfaces” used in certain types of analysis.
Set by default the use of Incremental Checking option in Processing Method, it will check the body is valid after each sheet surface is added to the “general body”. If adding a surface causes the “general body” to become invalid, the command will revert one step to before the particular sheet surface was added, then skip it and try to add the next one.
The Standard option in Processing Method is very similar, but does not do any incremental checking and will error if any surface cannot be added in properly to create a viable “general body”.
The Express option in Processing Method attempts to use a single operation in Parasolid to create a “General Body” from the selected surfaces, therefore performance can potentially be improved.
It is highly recommended to try using the default Tolerance of 1.0E-6 before trying a larger tolerance.
This way you can mesh with success any complex sheet surface geometry, enjoy!.
Thanks so much for the last answer. In the new model that I am doing, although I check all nodes and performed Non Manifold, they merged all sufaces. However I always showed error as below picture. Could you help to let me know the reason why?
To investigate the reason of the error is required to have the FEMAP model in hand, please post the model, surely you have a rigid body motion, one plate is not correctly node merged and goes to fly.
You can run a Normal Modes/Eigenvalue analysis using SIMCENTER NASTRAN (SOL103) and locate the reason of the error, this is explained in my blog in the following address, simply animate your first mode shape that will show you the rigid body motion vibrating at a frequency of 0 Hz:
My model is quite heavy(400,000kB) so it can't be up loaded. I tried to use Normal Modes/Eigenvalue but in NX Nastran, not used SIMCENTER NASTRAN(SOL103) and I'd like to know how I can download SIMCENTER NASTRAN.
The FEMAP model size is not a problem, use www.wetransfer.com (free till 2 GB) and post the link here, OK?.
SIMCENTER NASTRAN and NX NASTRAN is the same, is the new brand name of the nastran solver we will run in FEMAP 2019_1.