Bolt Preload Ansys vs Reality

[Vitkacy1989]

Hi Folks,

Today's question is about preload of the bolt simulated with solid elements - cylindrical shape of the shaft only, thread details omitted.
Ansys uses Bolt Pretension feature to create PRETS179. My understanding what is going on during the pretension is following:

- In REALITY: Bolt is tensioned and elongated while plates are compressed (see figure below)
- In ANSYS: Bolt is not elongated, quite opposite, the bolt is shortened - question why is this happening and when this is OK?

 

[karachun]

This is ok. At first step bolt axial stiffness changed to near zero value, bolt preload forces applied. Then bolt axial stiffness set back to initial value, all operating loads applied.

 

[Vitkacy1989]

@karachun thanks for the answer, could you please explain further why shortage of the bolt during the preload is OK in Ansys?

 

[karachun]

Actually, I tell you about bolt preload algorithm when bolt modeled with 1D Beam element. The case with 3D solid mesh is clearer.
Ansys (and many other FEA solvers) calculate preload at two steps. At first step solver chop bolt at the middle. Now there are two sets of coincident nodes, one for top bolt part and another for bottom part. Solver apply preload to these nodes and pull two parts of bolt to each other/ Parts connected by bolt are tied together. Two parts of bolt now have some overlap At second step solver constraint position of these nodes on interface so parts remain tied, remove preload forces and apply all operational loads.
There is no elongation on FEA bolt and this is normal.
Check this link Link at the bottom of page you can see animated deformed view, there is small overlap between bolt parts.
Capiche?

 

[Vitkacy1989]

Thanks this rises following questions:

1. You are saying there is no elongation, so if there is a shortage how Ansys generates tensile stress in bolt due to preload?

2. I need to simulate real preload with the bolt elongation, how to do it in Ansys?

Regards!

 

[karachun]

1. Read again my previous post/documentation/make test example in Ansys I explain as clear as I can. I have counter question to you. If I have bolt and nut modeled like one solid body (how it is actually modeled in FEA) how can two parts be tied together and distance between bolt head and nut will have elongation at the same time?
2. Why elongation is important in your case? First thing, that comes to mind is to model bolt and nut with thread, apply torque to nut. This will be very difficult task; you will have millions of elements, many sliding contact surfaces and bad convergence in result.
The main difference of FEA bolt against real bolt is that nut in real bolt can move along bolt axis by threat but FEA nut cannot.

 

[Vitkacy1989]

1. That is true! Exactly as you have explained.

2. I need to simulate the following thing. There is a bolt which is torqued with the know moment. Bolt end is in standard contact with other plate. FEA should give results what pressure this bolt is exercising onto the given plate. (kind of vise, clamp etc). So now you understand the case.

 

[karachun]

At first estimation, you can calculate bolt preload from torque and then apply it on part of bolt between head and nut.