I was CADding something for an elevator, and I was considering having two strips of metal that are fixed at the bottom and then connected at the top where a bolt would pass-through and a rope would loop around the bolt.
(This is a very rough CAD stage and I would definitely change stuff – if you want to suggest CAD changes, that’s OK but know I wouldn’t actually run with this ‘verbatim’. )
I ran a quick Autodesk Inventor FEA where I fixed the bottom three holes, and then put an upward force on the top one, just to see how much this part could reasonably take. I was a little confused by the results, so I put it in Ansys Workbench (Student):
Here’s my question: (1) wouldn’t the bottom attachment holes experience some stress?; (2) Wouldn’t the top of the three attachment holes (2nd from top, 3rd from bottom) experience stress on the bottom?
I then re-ran it with the bottom two hole supports suppressed:
And got pretty much the same picture. To my eyes, this appears that I could remove the bottom holes entirely and nothing would change. But, I know this can’t be true. Even weirder to me is that it looks like the material under the hole experiences practically 0 stress. Wouldn’t the bottom of the hole be the thing that actually attaches it? (Given that we are pulling up…)
I have some guesses, and all boil down to inaccurate simulation: (1) I applied my constraints and loads incorrectly; (2) The tolerancing of the holes is too perfect – in reality they would move a bit and stress would change; (3) I simply haven’t put enough force (I put 150 but 150/2 would be more realistic) and that means the 6061 hasn’t gotten past elastic (??).
EDIT: As I re-read this I’m now pretty confident its because the supports might fix all the material, bottom and top.
Could someone explain my dilemma? Thanks and sorry for the badly-worded question.
It’s been a long time since I’ve used ANSYS, but I think you should have a support option called “bearing” or something like that, that will apply compressive forces to the insides of cylindrical features, but not tensile forces.
Note that this makes the solving a lot more complex, because things are suddenly nonlinear.
(1) By fixing the mounting points you have made them impossibly rigid, so it makes sense that all of the load is resolving at the first mounting point. Fixed is not an applicable boundary condition in many situations, including this one. (I model a lot of different things for my day job and I rarely use fixed).
(2) Unlikely, if modeled appropriately, the friction of the joint from the fastener will resolve the stress.
This are reasonable points, and I applaud your honest self-reflection.
In reality, if the bolts are all appropriately tight, the first bolt will be doing a vast majority of the work (the clamping force of the fastener will be 1,000-2,000lbf, generating enough friction to avoid slippage of the first fastener). Thus I would suggest you solve the following model setup first and consider what it is telling you:
I would NOT start off trying to model the contact mechanics of the bolted or riveted connections because…
Consider interrogating your results differently. A trick I use is to manually lower the peak stress corresponding to ‘red’ on the color scale until there’s a noticeable area of red. This gives a more accurate representation of the stress the device will see IRL. Super tiny high stress areas will likely just yield a little and go away without anyone ever noticing.
Got it, thanks. I’ve tried moving away from fixed because I realized it just doesn’t seem realistic, but evidently I don’t know enough to realize Cylindrical was fixed.
You said you didn’t understand what I had written before and I’m a little confused by this response so maybe there’s still poor description on my part. I was noting that there was a lack of stress (or color) on the bottom part of the attaching hole. (Compare my initial images to the one in this post.) Your and Carlos’s explanations helped explain that, so I’m not sure what you mean in this quote.
Are you saying that the bolt or rivet will be tight enough that when the little vertical metal part rubs against the cross-beam of my initial images, the normal force from the clamping fastener will generate enough friction that the parts won’t move? So that the bolt is really providing a clamping force, and that it’s not resisting a bending force? Basically this:
If so, I never really thought or internalized that. That … changes how I think of fasteners. So much I don’t know, haha.
So basically having extra connectors yield sharply diminishing returns? That makes sense.
Is this just saying model the whole thing like it’s two forces pulling against each other, not one force pulling and one holding it place? That makes sense, and is also pretty clever.
I think I understand what you’re saying but for clarification: manually adjust the coloring curve so only really large stresses are red and everything else is blue or whatever? (I got thrown off with ‘lower the peak stress’ – I think it would be ‘raise the minimum stress value corresponding to red’ ??)
I remember asking a similar FEA question and getting a great response from you quite vividly. Your responses are always so helpful and your FEA suggestions are always so cool and help me continue past just answering my question. Thanks so much.
In the “real world” (buildings, bridges, vehicles…), threaded fasteners should really only ever take axial tensile force, holding the two surfaces together. Shear is then opposed purely by the resulting friction, as you say. This is why fastener preload and the things that affect it (torque specs, lubricated threads, etc.) are such a big deal. Generally, if you really need a separate element to take shear force, you’re supposed to use a combination of bolts (holding the things together) and hardened steel pins (to absorb the shear).
As with so many professional engineering rules, though, this is often ignored in FRC. We put shear force into bolts all the time, and it’s usually fine.
