Load Extraction Procedure in Bolted/Riveted Joints

[Burner2k]

Hello,
We need to come up with a procedure for extraction of bearing-bypass load for joint analysis (currently metallic joints and thus focus is on fatigue related) from FE model. Typical FE representation of joints include a Spring/DOF 1D element for fastener and 2D shell representation of sheets. We want to start simple with riveted joints.

In our initial attempts, we were focusing on a 3 row riveted joints with single fasteners in each row. Further, we had included holes and rigid elements and we got good correlation with hand calc. Unfortunately, the above is turning out to be a little complicate and not so accurate when we expand the joints to multiple rows of fasteners with multiple fasteners in each row (currently we are at 3 x 3).

So seeking help on getting some reference materials which might provide us with an idea on how to proceed. My search on Google so far has yielded some material but none of them provide satisfactory guidelines.

I had created a similar thread in General FE forum, but this being an aircraft specific issue, thought it may get higher eyeballs in this section. Apologies for duplicate threads. I can delete the other thread if mods/Admin deems necessary.

 

[Sparweb]

Double-posting is frowned upon. You divide the answers up, and half of the respondents don't know what the other half are saying.
If you red-flag your other post, this one can live on.

It sounds like you are re-inventing the wheel, there. Have you read Switft's papers? Do you have Niu's aircraft design textbooks?

STF

 

[SWComposites]

1) what do you mean by "included holes and rigid elements"?

2) what method are you currently using? provide details.

3) what do you mean by "not so accurate" for 3 x 3 type joints? If you are comparing to a hand calc, how do you know the hand calc is "accurate"?

4) getting bearing forces from the FEM should be simple, so presumably your issue is with "bypass" forces?

5) once you get the bearing and bypass forces, how are you calculating joint margins?

SW

 

[Burner2k]

Sorry for double posting and it seems like the admins have already deleted the other thread. Thanks for doing the same.

Also, it seems like perhaps I did not convey my issues lucidly in my post. But let me try to answer couple of SWComposites questions.

Please disregard hand calc method comment for 3 x 3 joint. That was made in haste. But we do have numbers for a 1 x 3 joint...which we calculated based on displacement compatibility equations. Further, I have to make it clear that currently we are targeting metallic joints only. The objective is to determine Fatigue critical locations in the structure rather than calculating joint margins.

Currently, we use two methods to model joints.

1. We represent the fastener holes in the DFEM/Local FEM structure. The rivet or fastener is still represented by 1D CBUSH element but it is attached to the hole nodes using RBE2/RBE3 rigid elements.

2. No holes are modelled in the GFEM or even DFEM. The rivet or fastener is represented by 1D CBUSH element.

In method 2, at the point/node of the fastener attachment, due to a large point load (bearing force/reaction) acting, the peak stresses in the plates would be at this particular location (which would be unrealistic anyways). My issue is how far from the attachment point & perhaps how many elements should be considered to obtain bypass stresses or loads. These stresses or loads would be sans SCF and we will manually account for SCF later.

I learnt that one of the OEMs typically follow a procedure where they consider a rectangle or square of length 'w' centered around the fastener attachment point. The length w is calculated based on fastener pitch and/or edge distance.

I just want to explore or learn further either about the above method or similar methods which could provide us with some pointers.

 

[aerostress82]

Method 2 will give you the best accuracy on this, but you need to be careful:
1) Model each fastener one by one as CBUSH elements (with 6 dof, out of plane rotational stiffness being a dummy/small value just to avoid singularity in your model)
2) Have your coincident nodes CBUSH element located at the "interface" plane of the 2 parts. (If you can't manage coincident CBUSH nodes due to your geometry complexity, add an RBE2 between the shell and CBUSH nodes with 6 degrees of freedom)
3) Make sure to have almost the "perfect" quad elements around the fasteners, and try to make them similar sizes - that will help you with below explanations,
4) Have at least 3 shell elements between any fastener,
5) Make sure to work with only your CBUSH forces for bearing & tension loads,
6) This is a linear model I assume. So, average the surrounding 4 QUAD shear & axial forces & moments for each fastener,
7) Derive your axial & bending stresses from these averaged QUAD loads,
8) Use your CBUSH shear load for your bearing stress,
9) Apply your fatigue concentration factors (from Peterson's Stress Concentration Factors) to those derived stresses,
10) Have fun with your fatigue rainflow cycles and everything else from here on.

I know it gets a little tough at first when you are doing it for the first time, I had this problem 6 years ago - that's why I wanted you to have it all clear and as accurate as it gets.

I would also advise you to automate this process if it is not automated yet. I was planning on using Patran PCL functions for this a couple years ago. Just never had the chance. Hope you have it.

I would advise method 1 once we get those "so promised quantum computers". Then you could integrate your pre-tension/friction at the nut and head and pretty much everything else. Spider RBE2s are not good for linear models. Try to avoid them as much as you can for joints. Only use them when you are representing a bracket with CONM2 card with accurate stiffnesses and you are connecting this bracket to joint locations. Otherwise, RBE2s really cost you the model. Try dummy CBAR etc. connections if applicable to your future cases.

With each bad RBE2 application, you will lose your model "element by element"
Good luck!

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer

 

[Burner2k]

Hi Aerostress82,
Thanks for replying.

>> 6) This is a linear model I assume. So, average the surrounding 4 QUAD shear & axial forces & moments for each fastener.

This 4 elements rule is independent of the fastener dia & element length?

Man, I don't know how to write PCL functions. Perhaps its high time I start learning...

 

[rb1957]

the big analysis issue is fastener stiffness. Huth tends to be the equation of choice, but there are others, Boeing, Douglas, etc.

do you need a full blown FEA for this ? You can get there using a much simpler compliance model.

the 4 elements referred to are the four that share the common CBUSH node. Make sure you have several elements along the rivet pitch, 4 sounds like a minimum (ie 1/4 pitch elements).

watch how you constrain the model ... don't over constrain.

many a/c have thicker skins at the rivet lines ... watch how you model this.

secondary bending is going to be a problem ... in practice (well, in my practice) minimised by having the (external) patch terminate on the adjacent stringers, so that the stringers help the skin carry the secondary bending (as torsion).

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

 

[SWComposites]

Ok, averaging the elements connected to the cbush works, sort of, if you know what are doing. The averaged loads are greater then the true net bypass load (net bypass is the load that is not reacted by the fastener) but are smaller than the true gross bypass load (gross bypass is the total load coming into the joint). Now when you use these loads to write margins you have to sort all this out. If you use only the averaged plate element loads to get a Kt at the hole it will be unconservative. If you combine the bypass Kt applied to the averaged loads with the bearing Kt applied to the bearing load (from the cbush) it will be conservative.

If you want to understand all this you need to run a series of two fastener axially loaded joint test models with different mesh densities for both applied far field tension and compression loads. Compare hand calcs to the FEM results.

And sorting out what to do with FEM moments in the elements in a modelled joint is an even bigger mess. Most of the moments in FEM models of joints are artifices of the model and not real.

There is really no substitute for hand free body analysis of joint loads. And if you cant do that you should not be running a FEM.

SW, ROGOFs

 

[aerostress82]

Thanks SWComposites for the additional explanations. Just a couple more comments and one correction with regards to what you mentioned about 4 elements at the fastener pitch:
1) Using 4 elements instead of 3 elements at every fastener pitch is a lot better approach actually. This will help you have better QUAD elements surrounding your CBUSH elements. The size of these elements should be consistent almost everywhere around your CBUSH elements. Then, you will have the "best" stress and load extraction from these elements. Given that your fastener pitch is likely to be at least 4D (D: fastener hole diameter), you will be able to manage this without any problem.
2) If you use the Ktg values from Peterson's graphs, that will account for "actual" net section area between the fastener holes. So, you will be as accurate as possible.
3) Regarding the CBUSH moment and forces, I have seen what both rb1957 and SW composites mentioned so many times. And I did my own study for the best solution to this. I'll let you know about it because aerospace -especially commercial aerospace- is very serious given that we may be heading to commercial hypersonic vehicles soon. I'll bullet them below:
a) Make sure to have your 2 contacting plates modeled as shell elements at the interface and offset them via property cards in Patran (or FEMAP or any other code).
b) Make sure you have the perfectly coincident CBUSH nodes.
c) If you can't achieve the modeling in "a" due to the machined part's geometry complexity, still have your CBUSH elements located at where your 2 connected parts would interface each other in CAD model.
d) Now you can use the moments if you have a "single" row of fasteners. But since you sounded like you have 3 rows of fasteners, I would advise you to use dummy 6dof and decide what your 45 dofs would be with a workbench+hand calculation on how to accurately "grab" these rotational stiffnesses for these fasteners. (a 3D detailed bolt FEA model for each type of fastener you are using and retrieving the rotational deformations of fasteners under applied moments to this workbench model, and then dividing your moment load by the deformation would give you a really good stiffness value for those 45 dof stiffnesses.
e) If you don't have the budget and time for item "d", go ahead and use a dummy 1000-10000 for 45 dofs if there are 3 rows of fasteners, or calculate a simple stiffness value with respect to K=GJ/L formulation. Whatever you want to use is up to you but confirm this with your principle stress engineer to make sure he agrees to this depending on your structure. If you only have 1 row of fasteners, go ahead and use a dummy value like 10^10. This will grab every single moment, so these moment loads will be too conservative and for fastener axial (tension compression) analysis, you will need to include your prying load on these fasteners.
f) So, your fatigue calculations for fastener axial behavior will actually get a little bit more complicated if you are dealing with the softening of the fastener in time due to fatigue life effects (don't overthink this yet. all above is really good. this will be something where your 15-20-30 years experienced engineers will need to be added to the discussion).
4) And finally your fatigue calculation will be in 3 parts:
a) Bearing (double-single shear distinction should also be integrated - whichever condition you have)
b) Axial (from the shell forces on your 4 QUAD elements around your CBUSH)
c) Bending (from the shell moments on your 4 QUAD elements around your CBUSH again)

If you have a good judgement on Item 3 above, you will overcome most of the complications of a FEA model.
Also if you would prefer to go back to 1980's, you might wanna calculate everything of shell elements. And then progress from there on by calculating all effective panel/stiffness & etc. coefficients to evaluate your fastener loads. It is not hard, just a 6 months project if you don't have a certified method from your OEM/company for it. Anything is really possible. It is all a matter of time/budget/accuracy. You may just go study anything mentioned above from everyone in detail and learn it for yourself and your teams in the long run. Not everyone is enthusiasts about stress engineering as I've seen it at times, so being the guy to secure every open end is not a bad thing in the long run

Also I'm only 7.5 years experienced, so any parts open to discussion, please feel free to comment/correct.
Good luck & Enjoy your weekend. Work is on Monday

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer