Connection Design in Finite Element Analysis

[MegaStructures]

Hello:

I regularly create assembly models in FEA of steel connections. My process is usually to assign linear contact between the faces of the connecting components, place rigid "spiders" at the bolt holes, and connect the middle nodes of the spiders with a spring element. I then run the model and find forces in the spring, export the spring forces, and check the bolts by hand.

As I continue to do more and more research on connection design in FEA I see that linear-elastic solutions are considered useless for connection design by some of the bigger names in FEA based connection design software such as IDEA StatiCa. The claim of course is that steel connections rely on a redistribution of forces in the connection as stress concentrations yield and relax - and the code based equations represent these redistributions. However, I would argue that linear elastic solutions are actually conservative, because they show the "initial" condition of the connection and if no area is over yield stress than stress redistribution won't occur. A non-linear solution, to me, would only yield a higher capacity of the connection.

So, does anybody have any opinions on the statement "linear elastic solutions are useless in connection design" and do you design bolted connections without material/geometric non-linearity.

“Any idiot can build a bridge that stands, but it takes an engineer to build a bridge that barely stands.”

 

[human909]

My assumption is that the stiffness of the individual bolted joint (hole, bolt, washer, nut) is much more important to aircraft structures, because the structure itself is made with thin metals and is not overly stiff. With structural connections we have 1/2" or better steel plate that is much stiffer than the bolt.

I take issue with this assumption. In tension we normally have significant preload on the bolt the bolts behave extremely stiffly through most of their strength range. A 1/2" plate is not particular stiff in an end plate type connection.

With bolts in shear we again have the bolts bearing on the holes. Here the flexibility comes from rotation of hole slop AND also localised point yield of the bolt hole in contact with the significantly harder bolt.

So in both cases flexibility of the joint is as much if not more so from the mild steel items.

(Of course much of this discussion is pretty vauge because the first question is what sort of connection are you modelling?)

 

[MegaStructures]

Human909 - for the sake of conversation let’s say it is the simple lap joint shown in the link I posted above

“The most successful people in life are the ones who ask questions. They’re always learning. They’re always growing. They’re always pushing.” Robert Kiyosaki

 

[human909]

Yeah so like a shear/fin plate. The flexibility is from the bolt hole and also hole deformation.

In fact some advice warns against using 'thick' fin plates because they deform less and thus the connection will behave less like a pinned connection.

 

[MegaStructures]

human909, ok I'm seeing the point, would you recommend:

1) A non-linear solution with a physical bolt
2) A linear solution with an adjusted CBUSH spring stiffness to account for bolt hole yielding (think this is what ESP was proposing)

When would you say these considerations are negligible and allow for modeling of the connection as suggested before?

“The most successful people in life are the ones who ask questions. They’re always learning. They’re always growing. They’re always pushing.” Robert Kiyosaki

 

[ESPcomposites]

Megastructrues,

No, that is not what I am saying. I think I confused you, so I will try to keep it simple. Simply input the load-deflection of the connection to the FEA (whether it is linear or nonlinear, depending on your goals)...that is all. The load-deflection curve may look something like the following figure (we might omit the clearance part or adjust for it). It doesn't matter how you get there (F=kx), as long as you can reproduce the load-deflection curve via the FEA. For example, if you just want to run a linear model, then input the linear slope (k in F=kx). This could be done with a spring, beam, or CBUSH element and the connection stiffness could be determined via an equation (original basis is from test data). This is the most common way to model joints in practice.

from "Practical Analysis of Aircraft Composites"

The linear region (linear stiffness) will *not* be a function of the failure mode. However, the nonlinear response will be a function of the failure mode. If the joint is bearing critical, there will be more elongation than if the critical mode is a fastener shear failure. For example, human909 showed a picture of what appears to be bearing elongation, which is part of the nonlinear region. Either way, you need to know what the load-deflection curve is for the individual connection, and input that to the FEM, if you want to run a nonlinear analysis.

from "Practical Analysis of Aircraft Composites". Note this figure is for general composites and the bearing-bypass mode does not exist for metals (w.r.t. ult failure).

Brian

http://www.espcomposites.com