How to simulate plates connected by bolts?

[Lirock]

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?

 

[cbrn]

Hi,
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...

 

[Stringmaker]

This is not an easy subject to address via the internet but here it goes. Solid elements will be your only option in this analysis. If you're only interested in the results due to compression and axisymmetric analysis is quick and dirty. If your plates are loaded with any net force then you'll need to do a 3D analysis. Contact should be relatively easy to set up between bolt, washer, plate, etc. You will need a contact pair for each location. For tensioning the fastener the easiest way to do that is to use pretension elements (PRETS179) through its cross section. The documentation explains each well and gives good examples of both. See:

-"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

 

[cbrn]

Hi,
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

 

[Lirock]

Thank you, guys.I will read around the chapters about this in the ANSYS document