Spherical joint in tension 1

[EnginerdNate]

Hi all, aero structures guy needing some help. I normally analyze things that don't move (running loads in bonded aircraft longeron/spar/bulkhead joints for example) so I'm a bit out of my wheelhouse here. We've got a test setup in which we need to pull on a ball joint. The joint geometry is dictated by flight hardware that I have no control over, and we're a sub on this project so I don't have direct access to the info on how the joint was originally designed.

The TLDR is--a ball in a two-piece socket made up of two plates bolted together, each with half of the sphere machined into it with an exit hole large enough to clear the ball's mounting shank plus some space for angular misalignment. This gets a tension load applied to it during the test. I could see the socket shearing out or bearing out, the ball deforming enough to pull out, or the socket deforming enough elastically to let the ball pass through, depending on material choice and geometry, but I don't see a straightforward way to run some hand calc checks on this. Is there any kind of industry standard calc for this type of situation or am I stuck resorting to contact modelling in my FEM program?

Thanks,
Nathan

 

[rb1957]

the bulb pulling through the mounting … is that "just" 3D tear-out (where a lug is 2d tear-out) ? Effective shear area = pi*D*t ?

another day in paradise, or is paradise one day closer ?

 

[IRstuff]

Have you looked in Roark?

TTFN (ta ta for now)
I can do absolutely anything. I'm an expert!

https://www.youtube.com/watch?v=BKorP55Aqvg

faq731-376 forum1529 Entire Forum list

http://www.eng-tips.com/forumlist.cfm

 

[GregLocock]

Does it have a plastic liner? or is it metal on metal?

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[BUGGAR]

This sounds similar to the loading on a typical car spindle ball joint and this might be an avenue of research (SAE).

 

[FEA way]

I suggest using FEA for this calculation. I don't think you can obtain realstic results with hand calcs in this case. I've found two articles that may be helpful:
- "Process Design of a Ball Joint, Considering Caulking and Pull-Out Strength" by B.S. Sin et al.
- "Investigation of Suspension Ball Joint Pull Out Force Based on FEA Method and Experimental Study" by A. Rutci et al.

If you decide to perform such simulation, remember to make use of symmetry when possible. Feel free to ask any questions regarding the analysis setup. Which software do you use ?

 

[EnginerdNate]

I've run basic shear out and bearing calcs based on the OD of the ball and the ID of the exit hole (Projected area for bearing, circumference at OD * material thickness for shear out) and the margins are extremely high.

My concern is primarily with the fact that in comparison to a lug, a larger percentage of the load has to be carried by surfaces that are at some oblique angle to the load, and the "lug" in this case doesn't wrap fully around the "pin" in the direction of the load, the analogous situation would be a lug in which some portion of the center of the lug was sliced out and the load had to be carried by the leftover "ears" partially wrapping the pin.

it's metal on metal, this thing needs to work once or twice. My thought was to simply grease up the ball prior to assembly.

The ball joint papers should prove informative, thanks for that.

I've worked up a quick FEM in Femap/NX Nastran using linear contact on the ball to socket faces and the global stresses/deformations look acceptable, but I'm not getting a good pressure distribution on the mating faces (peaky pressures with very large discrepancies between different surface nodes) so I'm not getting a warm fuzzy from it just yet. I'm working on redoing it using a hex mesh vs tets to see if that improves things. I have a reasonable amount of experience modelling contact using the Abaqus Explicit solver and Abaqus CAE for pre/post but I'm a complete novice at doing the same in Nastran.

I'll look through Roark, one of the other analysts here told me he did a quick review of his literature to see if there was a hand calc for this available and he didn't find anything. I'd been pursuing the FEM route in the meantime.

Thanks for all the input!

Best,
Nathan

 

[EnginerdNate]

Just took a look at my latest results and they look much more reasonable. Primary difference was switching the contact algorithm to eliminate any gaps/initial penetrations at the beginning of the run.

 

[FEA way]

Can you show your results here ? You should try with nonlinear contact since linear one will work like tie constraint in Abaqus - keep the surfaces glued to each other without the possibility of separation or sliding.

 

[EnginerdNate]

Are you sure on that? There are separate options for a glue constraint vs contact. There's a coefficient of friction specified etc so there has to be some level of sliding allowed.

I can't share anything here unfortunately.

 

[EnginerdNate]

The info here implies that some sliding is allowed with the contact card I'm utilizing:

http://www2.me.rochester.edu/courses/ME204/nx_help/index.html#uid:index_User:id502361

http://www2.me.rochester.edu/courses/ME204/nx_help/index.html#uid:index_QRG:id518467:id507341

 

[FEA way]

I don't know Femap and I thought that it offers linear contact in the same form as in other FEA programs - like tie in Abaqus. But apparently it features additional type of contact where stiffness changes and material nonlinearity are omitted. It is of course limited by maybe it's sufficient in your case.

 

[EnginerdNate]

I've struggled to find good reference reading on this specific tool in nastran beyond how it's setup. If I find something more detailed I'll be sure to share it here.

 

[Tmoose]

So not a stamped plate, but plates with thickness approaching half the ball diameter, or even thicker ?

"I can't share anything here unfortunately."
I'm thinking there is a COTS component complete with load ratings that does just what you need.

https://medias.schaeffler.com/medias/en!hp.ec.br/GE..-UK-2RS?#GE..-UK-2RS

Or, turn the thing sideways and hide an axle in there.

https://medias.schaeffler.com/medias/en!hp.ec.br/GAKR..-PW?#GAKR..-PW

 

[EnginerdNate]

I'd love to use a commercial rated part, but the ball itself is an integrated component of the system under test. Customer supplied engineering so I have to work around it. The setup is kind of a glorified trailer hitch.

 

[Tmoose]

"the ball itself is an integrated component of the system under test. "

So the ball is removed to install the holey plate ?
Or, the plate is split ?

 

[EnginerdNate]

Plate is split and fastens around ball. Fastener torque/clamp up prevents the two halves of the plate from separating. To make the fasteners as effective as possible I've fit as many as I can in a circular pattern (maintaining edge distances) at a fixed radius out from the center of ball. The fasteners will run completely through each plate and are installed with nuts on the backside so that all parts involved have a specced load capacity. I've run a few different variations of the FEM model with different CBUSH stiffnesses in tension to verify that my fasteners have enough tensile strength to handle the induced prying load from pulling on a sphere. The classic EA/L calc (Huth for shear, but shear load in this situation is almost nil) for tensile stiffness K1 gives me something in the order of 1k lbf max, taking that value up to 1e6 as a conservative "overly stiff" fastener increases the load to around 4800lbf, which is still acceptable (with reasonable margin) for the fasteners I've chosen. I'm calculating with an additional 2x factor of safety on the actual test load as well for conservatism. The expectation is for something in the system under test to let go well before the 200% point.

As an aside, I found a calculation for stress in two spherical bodies (One male, one female) in Roark but it made no accommodation for the area missing where the ball's shank exits the fitting so I don't think it's useful in this situation.

Thanks,
Nathan

 

[EnginerdNate]

Wanted to post an update on this. I created a FEM using Hex elements to model the ball and tets on the two plate halves. I used linear contact between the two plate halves and the ball and at the mating face between the plates. I fixed the ball in space and also fixed one point on one of the plate halves to prevent any weird rigid body motion (I realize there are more nuanced ways to do this, but when I vetted the model there was less than 1% of the applied load going through this constraint and it did the job). I modeled the contact with a small amount of friction (less than I anticipated there would be in reality) to improve model stability and accuracy while maintaining some conservatism.

The analysis passed muster with my internal reviewers and with our customer and the design performed admirably on test day. A win all around. Thanks for everyone's help.

Cheers,
Nathan

 

[rb1957]

thx for the follow up … we don't get it near enough. better that it was successful.

another day in paradise, or is paradise one day closer ?