How to simulate plates connected by bolts?
How to simulate plates connected by bolts?
(OP)
Hi,everyone:
I want to simulate two plates connected by bolts,but how to do it? I mean what type of element should be used.Some papers says use 3D solid element for the plates and prestress beam for the bolts, and make contact pair between them, but the papers don't show the detail process. Is there some papers show the detail?
I want to simulate two plates connected by bolts,but how to do it? I mean what type of element should be used.Some papers says use 3D solid element for the plates and prestress beam for the bolts, and make contact pair between them, but the papers don't show the detail process. Is there some papers show the detail?





RE: How to simulate plates connected by bolts?
sure: Ansys help is very detailed on that point. If you're interested in very realistic analysis of a bolted joint, use 3D model and Prestress elements (not beams). Warning: the interpretation of the results may be a bit tricky... take care, and know what you're doing...
RE: How to simulate plates connected by bolts?
-"Defining pretension in a joint fastener" under the Loading section
and the
-Contact Technology Guide
in the Ansys documentation. Both are well written and contain very extensive information. If I recall there's a pretty good pretension example. Neither on of these two subjects is considered easy and should be backed up with hand calculations to validate/verify your results. Good luck!
-Brian
RE: How to simulate plates connected by bolts?
thanks Stringmaker for your very good answer.
As said, the topic is difficult and should be assessed with a plurality of instruments: VDI 2230 is a very good source, but it may not be accepted as valid outside European Comunity. Be careful also with the "analytical" calculations: bolt pretension is mechanically so complicated that VERY high uncertainties exist even with the most sophisticated theories: you will sooner or later struggle against semi-empirical coefficients or corrections (for example: how would you EXACTLY account for embedding effect?). If your connection is safety-critical and the calculated stresses are high though acceptable, I'd suggest to set up a test system with load cells, extensimeters and so on... in order to correlate / correct the simulation(s).
But, Liweisc, don't lose your faith: in many cases, a properly set 3D simulation with ANSYS gives pretension/elongation results far within 5% dispersion w.r.t. live test. Be careful especially (but not limitedly) to: normal contact stiffness, mesh type and refinment, absence of unwanted edge effects or other unrealistic discontinuities, material properties, contact allowable penetration (don't leave the "controlled by program" option activated), contact stiffness update (each iteration!).
Good luck!
Regards
RE: How to simulate plates connected by bolts?