modelling fasteners using zero-length bushes

[jedstress]

Hi everyone,

I am currently working on a repair job which is as follows: the part being repaired resembles an L shaped bracket which attaches to the parent structure via fasteners. fatigue issues have arisen due to undesirable design features, and therefore straps on both sides of this joint are to be used to repair the problem area.

my questions is:
what is the best way to represnt the fastener(s) securing the stack which consists of four 2D shell elements (parent flange, bracket flange, aforementioned sandwiched by the two straps).
i believe that modelling the offsets (by creating shells at their true mid planes) is proabably vital if you are concerned about the bending sttifnees of the structure. However, in my case, the structure bending sttifness at htis local rea is not important.therefore, I am trying to keep it simple by minimsing changes to the provided FEM (where parent flange and bracket flange share commomn nodes at fastener interface). i will model the straps without offstes thus creating coincident nodes at the relevant poisitions. now, what is a reasonable way of attaching these straps to the existing joint?
the client has asked to try the common node approach and an alternative approach which represents the bolt/joint stiffness. I was planning to use the Huth stiffness method to assess the in-plane stiffness but i am unsure how to do that when your stack of four elements are all co-incidnetal.for huth sttifness, should I halve the thickness of elements being shared by two bushes? i hope that makes sense. so to summarise, how do i calculcate the in plane translational stiffness(es) for all three bushes of a four element stack, using Huth method? also, how to use axial stiffness AE/L to ensure total axial sttifness of bushes equals axial stiffness of bolt?

thanks

 

[rb1957]

you Could model the 2D shells at their CLs and use RBEs and CBUSHs to model the rivet.

you Could use beams with a bending stiffness to match the fastener flex from your formula of choice (huth is popular these days)

you could use co-incident 2D plates and CBUSHs.

you could use solid elements and RBEs and CBUSHs, but that seems like overkill.

 

[jedstress]

Thanks rb1957 for the valuable feedback. If bar elements are used to join element nodes at the CL of the plates, wouldn't its length and the cross sectional area, along with E, pre define the bending stiffness?therefore could I use bar elements as mentioned,and use bushes to represent in-plane bearing sttifness?huth formula seems to gives joint in plane stiffness based upon fastener stiffness,bearing sttifness i.e. Can you specifically calculate bearing stiffness?and in your opinion,what's the best way to represent a joint consisting of stack of four plates.3 bars,3 bushes?and how to use huth formula for positions where for instance one node is shared by top and bottom bush?Would halve the thickness be used when calculating huth stiffness for top and bottom bush?I hope it's not confusing.thanks again and sorry for the length questions.

 

[rb1957]

you control the bendng stiffness of bar elements with I. Length is defined by geometry, E and I can to chosen to suit your problem ... they don't have to match the geometry of the fastener. i'd do a test case to check that the beam is deflecting the way i expect it too ... calc a stiffness, determine an equivalent beam, apply a load, is the deflection of the end nodes = P/k ?

for CBUSHs, input the fastener stiffness calc'd (eg huth).

for multiple layers, I'd use a huth stiffness based on two adjacent layers, so the one fastner could have different stiffness along it length ... clear as mud ?

 

[jedstress]

sorry Rb1957, I meant to say that second moment of area I gives bending stiffness.by the way,does huth stiffness account for bolt bending stiffness?I thought it did. If not, and if I was using cbushes to represent the entire joint, what formula would you use to reasonably calculate bolt bending stiffness?if I assumed the bolt was a beam clamped at both ends and was reacting a shear load,I could re-arrange max deflection formula to give k=p/x. Could this method be used to give the bolt bending stiffness?I was worried that this method assumes full fixity which in reality is not the case.

can bush elements be of zero-length?and if so I assume that their length has nothing to do with their stiffness?

I am just trying to think of the various possibilities and better understand how such elements work.

Thanks for all your valuable input.

 

[rb1957]

ok, we're getting confused here.

1st, huth calculates the shear stiffness of the fastener; ie displacement = P/k.

if you model the fastener as a beam, it not the bending stiffness i'm interested in, but rather the displacement of the ends. you can control this displacement to get the result you want (P/k) with I or E.

I thought CBUSHs were zero length. so you would use a rigid RBE to create co-incident nodes, and the CBUSH would have the huth stiffness.

i suggest running some test models to see how things work. either approach (beams or zero length springs and RBEs or zero length springs alone) is valid, though zero length springs alone is trickier to model is a large assembly.

what are you modelling ? if it's a splice joint, a compliance model would be just as good.

 

[jedstress]

Hi rb1957.thanks for the clarification.when you say "use rigid rbes to create co-incident nodes",are you referring to instances where the relevant nodes (which are at the element(s) CL) are a distance apart?so create co- incident nodes which are connected by cbushes and in turn connected to the CL node(s) using rbes?
when using cbushes,assuming yz plane is shear plane, K1=axial stiffness,K2=K3=huth,K4=rotational=0 in my case, and K5=K6=? (previously I have been advised to assume k5,k6=1e6 i.e. Very stiff).what is your opinion?
and yes I agree that cbushes are typically of zero-length but,being 1D elements, they can have length? Right?if so,I was interested in the effect this would have (just for my knowledge).
Thanks again.

 

[rb1957]

yeah, if your nodes are offset (being on the mid-plane of different sheets) then i'd use an RBE to create the co-incident nodes for the CBUSH.

K2 = K3 = huth, K1 = K4 = K5 = K6 = whatever, 1, 1000, ...
shouldn't make much difference anyways

never tried CBUSH with length ... try it and see !

 

[jedstress]

Rb1957 thanks alot for the explanation.you have been great help.I will play around with the various approaches and see how they affect the output.

 

[jedstress]

hi rb1957. i created a simple FE model representing a simple lap joint with the two surfaces of equal thickness (represnted by shells) modelled 3mm apart to simulate eccentricity. i have idealised the fasteners as bar elements. however, i cant understand why one end of the bar element(s) are seeing huge bending moments whilst the other is seeing negligible amounts. i was expecting the moments to be more or less equal on both ends, but the results seem to suggest one end is pinned. i have checked the bdf sevral times to ensure both ends are fully built in. have you ever come across such an issue before? am i overlooking something here?

please refer to the attached file for details on the results, including bdf and f06.