a) why can't you make a FE model yourself to compare to this analysis?
b) is this a homework problem?
c) the rivet length is no where near 1.0 inch; why would that be used in a model??
d) and why would the fastener be modelled with dia = 0.406, when the actual diameter is 0.19 inch??
e) have you tried using the fastener distribution s/w here: https://www.espcomposites.com/software/advanced.ht...

Hi SWComposites.

a) why can't you make a FE model yourself to compare to this analysis? I do not have access to FEM.
b) is this a homework problem? No for work.
c) the rivet length is no where near 1.0 inch; why would that be used in a model?? As explained above this is a methodology suggested by Boeing to calculate bearing and bypass loads with FEM. You assume fastener length is equal to 1 inch and calculate what diameter fastener gives a value of fastener flexbility calculated previously per Swift.
d) and why would the fastener be modelled with dia = 0.406, when the actual diameter is 0.19 inch?? Explained in c above.
e) have you tried using the fastener distribution s/w here: https://www.espcomposites.com/software/advanced.ht... I have not but have my own excel tool to do that. I want to see how FEM compares.

Bragi

You've said this is a problem for your work. So you're asking people to freely perform an analytical verification for you? That's not really the purpose of this forum.

Also, in the future, please refrain from cross posting in multiple forums.

This is a topic that has been studied at length in the industry. If you have no access to FEM and aren't willing to get it, then I suggest you look for existing publications and reference papers which have compared 1D stiffness-displacement based Load Transfer to FEM.

Since these models assume a truly 1D scenario, the results are never going to be an exact match. The LT is also going to be influenced by your choice of fastener flexibility equation.

In my experience I've found Swift's equation to predict the highest peak LT compared to other equations (it is the stiffest fastener model).

Keep em' Flying
//Fight Corrosion!

LiftDivergence thank you for your warm and positive response. I work in a small company that does not have the resources that others have. I have in my past time been very interested in this subject and have read a lot of papers, thesis and standards on the subject. I found this Boeing course I took a long time ago and started working through it and was intrigued to see how their FEM suggestion would compare.

I m sorry if I stepped on your precious toes and i hope they did not fracture.

On a cursory check I found in my stash the following documents which include a comparison of FEM results for individual fastener loads to hand calculations:
https://apps.dtic.mil/sti/pdfs/ADA613855.pdf
https://soar.wichita.edu/bitstream/handle/10057/11...

I'm sure you could find more with some searching.

However, in the end, the method written by Swift which you reference above is a form of the matrix-force method of analysis. This was very common when analysis semi-monocoque flight structures started t0 become much more sophisticated. Argyris has written extensively about it's application to airframe structural analysis.

Matrix method is essentially a precursor to FEA. FEA in no way obviates hand analysis, if the model is small enough (which in this case, it definitely is). You may recall from study that FEA basically works by assembling a global stiffness matrix and relating it to a displacement matrix. You may find a solution using a number of matrix algebraic steps. For example, in college, I was taught Galerkin's method. The reason complex FEM software packages exist is that generally the size of the model we want to deal with is too cumbersome to solve by hand.

What I'm saying is that you don't need to have extensive resources to do simple FEA. You could probably make a script to perform 2D FEA to check your answer pretty neatly. Fortran would work, or possibly even VBA.

Keep em' Flying
//Fight Corrosion!

Thank you LiftDivergence.
I have read the second thesis. Problem with theses is they very often leave out pertinent details as they are often sponsored by corporate. Like these sponsored by Saab Aircraft.
https://www.diva-portal.org/smash/get/diva2:550529...
http://liu.diva-portal.org/smash/get/diva2:17841/F...

The example i posted above is the only one where I have found step by step instructions on how to model the joint and that is why I was curious how it compares.

All the answers I get is people offering up different type of hand calculations or estimations from graphs. Makes you really wonder how good and reliable the FEM models industry is using.

Bragi

If you're familiar with hand coding Nastran decks, try building a model in Mystran.
Also take a look at the Huth formulation for fastener flexibility.

Ng2020. What type of elements would you use for the fasteners?

Here we are years end with experts that are eager to comment and indicate they have all the answers but nobody offering concrete advice for a simple problem that is used widely in all structural analysis. Where are we as a world if we cannot share how exactly we do things in our work. Sorry for my frustration but I have so much had it with engineering kinga that think they know it all but are afraid to share their knowledge.

For a simple model I'd try:

Straps = rod elements, collinear.
Fasteners = Cbushes at the coincident nodes using huth formulation for shear stiffness.

The really contentious part of these types of problems is the assumed formulation for the fastener stiffness. As for the calculation method, whether you use fem or a hand calc matrix solution the results should be very similar. Some further consideration is required if it's an unusual joint, eg thick stack up, multiple straps, composites, varying fasteners.

Happy new year, good luck...

Hi Bragi,
I hear your frustration but this may come from a mismatch in expectations.
Since you have already excerpted a bunch of figures from good textbooks like Niu and say you have Schijve's, I am at a loss as to what you are missing. I'm glad to see you here posing interesting questions, but at some point I don't hold your hand any more and you're able to take it on your own. If you also have the Boeing course notes then shouldn't every step of the method be right there before you?

At various times your posts have appeared to ask questions at the student level, rather than as a practicing engineer. Perhaps that's a mistaken impression but on the slight chance that you are in fact a student, please make sure you are taking full advantage of the educators and training materials available to you at your institution, all of which should be able to help you.

https://www.eng-tips.com/userinfo.cfm?member=Ng202... why do you use rod elements that can only carry axial loads and torsion and not bar elements that have bending?
The Huth fastener flexibility gives values with units of m/N. Do you just use the inverse of this for the PBUSH K stiffness value?
What length do you use for the CBUSH element?

Regarding element type:
For fatigue analysis of a fairly conventional lap joint (using the proprietary methods that I'm used to) the effect of moments due to loadpath eccentricity are addressed separately, not in the loads model. By that method you can use a 1d model such as the one I've described to calculate joint load distribution (bearing and bypass loads).
In short, yes, you need to account for loadpath eccentricity somewhere in the analysis.

Yes, stiffness is the inverse of flexibility.

Cbush length is Zero: nodes are coincident, it's a 1d model. Though see my note about accounting for eccentricity somewhere in the analysis.

Ng2020. If you have more complex joints such as doubler and tripler do you still use a 1D model for that as well?

I'm a few years out of practice, but you could well make quite a complex 1d model, as long as you're confident you are accounting for eccentricity elsewhere in the analysis. For example you might use SN data that's based on a joint of similar or equivalent configuration.
I'd try to get a good handle on the simple example you mentioned before pushing the capabilities of the method.

You can try out eDistribution as well (https://www.espcomposites.com/software/download.ht...). There is an input for a manual fastener flexibility.

Brian
www.espcomposites.com

I got it to work using the beam methodology above with a fastener length of 1 inch. I had to use Y-symmetry on all nodes to guide the whole structure along the X axis. Great to know that this works as it is a very simple approach. Does not include secondary bending but gives me bypass and bearing loads.

TLDR ...

this is a "simple" compliance model, equating the deflections along different paths, like the displacement in the skin over the first pitch + the displacement of the 2nd rivet = the displacement of the doubler over the first pitch + the displacement of the first rivet. The first rivet has load P1, the second P2; the load in the doubler is P1, the load in the skin is P-P1. Then similar for second fastener pitch ... now load is doubler is P1+P2, load in 3rd rivet is P3, load in skin is P-P1-P2. Repeat to CL. A bunch of simulaaneous equations, solve for P1, P2, etc. Niu has all this in his book.

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

read last post ... shouldn't need to assume a fastener length (beyond Tsk + Tdblr)

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

You missed the point rb1957. The excercise was all about using a fastener length of 1 inch.

well, yeah, I missed that point. I thought you were trying to solve a real problem. As shown in your first pic, the three vertical arrows (which look like axial load on the fasteners) should be horizontal, as these are shear loads in the fasteners.

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

rb1957 still a real problem to determine bearing and bypass loads

not with 1" long fasteners. fastener length should be (AFAIK, AFAIC, IMHO, IMAO) (tsk+tdblr)/2. By using 1" long fasteners you're using an artificially high shear stiffness, to capture the behaviour of much shorter fasteners. The real problem is easily solved with a compliance model, which is equally easily transferred into the FEM world (oh, but then that's the point of the post ... you're starting with fastener shear compliance, based on the Boeing stiffness calc [1]). You're modelling a 3/16" rivet that is joining two sheets, 0.05" and 0.04" thk, as a beam 0.406" diameter and 1" long ... and this makes sense ? what kills the problem solution is the increased offset between the load and the reaction (what should be 0.045" is now 1") ... this is not good modelling. I'm not sure what you're learning (or supposed to learn) from this.


[1] an interesting take away is how different are the formulations for fastener stiffness (compare Boeing, Douglas, Huth)

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

Rb1957 explain to me in detail how you would setup a finite element model to model this? I actually like this approach because it makes it very visual especially if you have several straps. The offset between applied load and the reaction is the same as I have adjusted the diameter of the fastener as well to be artificially big and hence you get correct results as expected.

Bragi, nobody uses this method.
You could try (nastran) celas elements if you want to visualise the individual straps.
See also eng tips thread825-358723: CBUSH elements with non-coincident nodes

I'm also confused by the direction this thread is going...

Quote (rb1957)

which is equally easily transferred into the FEM world (oh, but then that's the point of the post ... you're starting with fastener shear compliance, based on the Boeing stiffness calc [1]). You're modelling a 3/16" rivet that is joining two sheets, 0.05" and 0.04" thk, as a beam 0.406" diameter and 1" long ... and this makes sense ? what kills the problem solution is the increased offset between the load and the reaction (what should be 0.045" is now 1") ... this is not good modelling.

Quote (BragiBaldursson)

Rb1957 explain to me in detail how you would setup a finite element model to model this?

From the start it seemed like the question was not regarding the 1D load transfer analysis itself. OP stated they had that worked out but either didn't trust the results or just wanted to verify them using FEA. Problem is OP doesn't have access to FEA software and was asking someone in the forums to do it for them instead.

I said:
1. This has been studied extensively and there are probably a plethora of papers doing that exact type of verification
2. You don't need software necessarily to do simple FEA.
3. Myself and others pointed out the questionable usefulness of this effort since 2D plates width actual width will not perfectly approximate the 1D compliance model results, and also secondary bending due to eccentricity needs to be accounted for.

OP basically cast some insults and now the discussion has shifted to:
-people giving advice on how to perform 1D compliance model calculations (not the question at hand)
-discussion of specific FE modelling practices, even though OP has stated they don't have access to any software.

Overall there is a lack of clear communication in what we're looking for. So OP, are you still looking for someone to create a FEM for you, or are you simply looking for any software which will automate your hand calcs? Because that is not the same as validating. If you are using the tool ESPcomposites linked to, that is not a verification, it will be using the same method you've already done by hand.

Keep em' Flying
//Fight Corrosion!

This is getting to be quite the exciting post. If you read my original post I was working a problem from a Boeing 777 structures course by hand and I wanted to know how it compared with FEM as the course suggests and the modeling it suggests. That was the question and that is all. I have since then found a suitable FEM software to work it as suggested and got the result I was hoping to get. My hopes from the community was to get details out of it how you model in FEM. Ng2020 offered up using Mystran and bush elements in a 1D problem, which is another alternative. I wanted to know how state of the art modelers model a problem like this with the little details and explain it to the community.

Oh, I forgot, 1D Elements can handle this problem as well ( https://www.structuralfea.com/1D_Elements/1D_Eleme... ). It uses MYSTRAN and I attached an example.



Brian
www.espcomposites.com

Problem solved see https://www.eng-tips.com/viewthread.cfm?qid=490812

Either method can be used actual 1 inch beams of large diameter or springs.

Just to let you know (FYI), I’ve got a calculation template using the compliance model. I know the method as strain matching. Using the information provided (with the swift equation), I obtain the following fastener loads, 300.6 lbf, 189.5 lbf and 259.9 lbf.

there's one (a compliance model) in Niu. It's simple to set up in excel.

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

and please don't post your email ... at least not without disguising it I think you should edit that post.

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