×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Contact US

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Connection Design in Finite Element Analysis

Connection Design in Finite Element Analysis

Connection Design in Finite Element Analysis

(OP)
Hello:

I regularly create assembly models in FEA of steel connections. My process is usually to assign linear contact between the faces of the connecting components, place rigid "spiders" at the bolt holes, and connect the middle nodes of the spiders with a spring element. I then run the model and find forces in the spring, export the spring forces, and check the bolts by hand.

As I continue to do more and more research on connection design in FEA I see that linear-elastic solutions are considered useless for connection design by some of the bigger names in FEA based connection design software such as IDEA StatiCa. The claim of course is that steel connections rely on a redistribution of forces in the connection as stress concentrations yield and relax - and the code based equations represent these redistributions. However, I would argue that linear elastic solutions are actually conservative, because they show the "initial" condition of the connection and if no area is over yield stress than stress redistribution won't occur. A non-linear solution, to me, would only yield a higher capacity of the connection.

So, does anybody have any opinions on the statement "linear elastic solutions are useless in connection design" and do you design bolted connections without material/geometric non-linearity.

“Any idiot can build a bridge that stands, but it takes an engineer to build a bridge that barely stands.”

RE: Connection Design in Finite Element Analysis

Why do you bother to model the fastener holes?

RE: Connection Design in Finite Element Analysis

Hi Megastructures

I generally use non-linear static or non-linear transient analysis when doing complex connection designs, this is only done for very non standard connections on structures. I do believe that in certain cases a linear static is conservative. I deal with a lot of dynamics and hence fatigue is a big issue for me and this non-linear gives far more realistic results.

Even with FEA analysis I still combine hand calculations from code for various aspects where FEA may not be accurate or difficult to assess.

RE: Connection Design in Finite Element Analysis

Uselesss is too strong, but you will likely end up with an overly conservative design. Not too big an issue if you're doing a one-off but if builing a lot of connections it will have a big economic impact.

RE: Connection Design in Finite Element Analysis

I am not sure what your application is, but this would be a common approach in the aircraft industry (if for some reason a FEM was required):

- Fatigue analysis: Use a liner spring/beam/CBUSH/other element to represent the fastener connection (better not to model the hole but its OK too if you calibrate out the overall stiffness of the connection). Using the fastener loads, perform fatigue analysis outside of the FEM (detail analysis). Sometimes you can use empirical or semi-empirical equations to determine the spring constant for the connection (which is a function of many factors as discussed below).

- Ultimate analysis: Use a nonliner spring/beam/other element to represent the fastener connection (better not to model the hole but its OK too if you calibrate out the overall stiffness of the connection). The nonlinear load-deflection curve must be developed via test based on a representative connection. Alternatively, if you know the connection is bearing critical, you might be able to come up with a reasonable load-deflection based on the assumption that there is a relatively large amount of deformation once the yield bearing stress has occurred. You might also be able to use a linear analysis if a conservative result is acceptable (depends on some factors).

The challenge with using a FEM as you suggest is that you are attempting to create the actual nonlinear load-deflection curve from the FEM, based on the actual physics of the problem. I am not sure you realize how challenging that is. The deformation is a function of at least the following: member bearing, fastener bearing, fastener bending, fastener shear, fastener rotation (tipping), installation factors such as clamping force, fastener fit, fastener type. So unless your FEM can capture those factors (and the nonlinearities associated with them), its not going to be realistic. If you consider something like the plasticity associated with bearing deformation, that alone will be a challenge to represent via FEM. That is why we rely on test data to determine the spring constant for joint connections (and then sometimes create equations to represent that based on specific inputs of the joint). In fact, a bearing allowable (yield and ultimate) are almost "properties" in themselves and would be quite difficult to reproduce with a FEM and the actual material properties.

For the linear solution at least, this figure will give you some idea of what I mean about the factors that affect the joint stiffness/flexibility (from Practical Analysis of Aircraft Composites)


Brian
www.espcomposites.com

RE: Connection Design in Finite Element Analysis

I don't see them as useless, that is definitely an overstatement. It is clear there is some use to be had.

Quote (MegaStructures)

I generally use non-linear static or non-linear transient analysis when doing complex connection designs, this is only done for very non standard connections on structures. I do believe that in certain cases a linear static is conservative. I deal with a lot of dynamics and hence fatigue is a big issue for me and this non-linear gives far more realistic results.
I've done the same for complex connections. Only once or twice for structural steel connections. One time was for a heavily eccentric bearing seat that passed the moment through the web of another beam while shear transferring into the web. So a bit odd, nothing I've seen in text book, but nothing crazy. It made intuitive sense but FEA gave me peace of mind. Naturally I check my results with hand calcs.

I've also used FEA for storage vessel design, which I've somehow become the company expert in.

I use Inventor NASTRAN-INCAD. It options that let you place bolts and specify pretension.

RE: Connection Design in Finite Element Analysis

(OP)
On Modeling Bolt Holes

I see several comments suggesting to not model the bolt holes and I'm not clear why that is. I model everything in my CAD program before bringing the assemblies into my pre/post, so I get the holes for free, and I'm not seeing how the holes are giving an inaccurate stiffness. Seems to me the holes are there in reality, and we are trying to match reality, so why not add them. Also, using the bolts holes and assigning RBE3's to a "washer imprint" around the bolt holes seems to give a much "better" stress distribution.

ESPcomposites

Quote (ESPcomposites)

You might also be able to use a linear analysis if a conservative result is acceptable (depends on some factors).

In my work conservative is always acceptable. As long as it's safe, I'm happy. My installations have no need to fly :).

Quote (ESPcomposites)

The nonlinear load-deflection curve must be developed via test based on a representative connection...…..The challenge with using a FEM as you suggest is that you are attempting to create the actual nonlinear load-deflection curve from the FEM, based on the actual physics of the problem. I am not sure you realize how challenging that is. The deformation is a function of at least the following: member bearing, fastener bearing, fastener bending, fastener shear, fastener rotation (tipping), installation factors such as clamping force, fastener fit, fastener type.

This suggests that an assembly model can never be used to check connections, regardless of analysis type, without relying on a physical test. Surely this can't be right. Most of your points are to do with bearing, which I assume is due to the possibility of not all parts of the connection being in contact at installation, but I was under the impression that this was mostly solved by the non-linear nature of steel connections and that the materials will yield where necessary until appropriate bearing occurred.

Fastener bending and fastener shear should be accurately represented by the properties of the spring element used to model them, what is missing? I can see there being increased bending in the bolt if the mating faces in the connection aren't in contact, thus increasing the bending due to offset shear. I'm struggling to see how fastener bending is not accounted for otherwise

“The most successful people in life are the ones who ask questions. They’re always learning. They’re always growing. They’re always pushing.” Robert Kiyosaki

RE: Connection Design in Finite Element Analysis

big names in FEA advocating FEA solutions (as opposed to simple hand calcs) ? ... say it isn't so !

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

RE: Connection Design in Finite Element Analysis

(OP)
rb1957

I am definitely cognizant of the fact that they have a product to sell and thus want to make the "easier" method seem unusable. Of course, if I had the chance to hand calc something I would, but my interest here is in more complicated assemblies that need at-least a verification through FEA.

BIG FEA is keeping us down

“The most successful people in life are the ones who ask questions. They’re always learning. They’re always growing. They’re always pushing.” Robert Kiyosaki

RE: Connection Design in Finite Element Analysis

"BIG FEA is keeping us down" ... only if we let them. FEA is a tool, just one of many in the toolbox. For some it is the tool of choice, for others (older?) hand calcs may be the tool of choice.

A significant problem we have today with FEA is being asked to validate the model, which is doubling (at least) the amount of work for an FEA solution.

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

RE: Connection Design in Finite Element Analysis

Well, for the linear range, there are semi-empirical solutions for the effective "fastener flexibility" (the compliance of the joint connection), which are based off of test. Assuming the connection is bearing critical and large deformation is expected, you could develop an approximate nonlinear load-deflection curve based on the bearing yield stress and bearing ult stress. If the joint is shear critical, you won't have as much nonlinearity and a linear solution may be representative of the actual response.

We have to break the problem into two conditions though. For a fatigue analysis (loads relatively small compared to the ultimate load capability), there may be local yielding, but the fastener loads are still such that that a linear analysis is acceptable. We commonly use semi-empirical fastener flexibility solutions for that scenario. For an ultimate analysis, there can be a significant amount of deformation which allows for a redistribution of the loads on the fasteners (which you may or may not want to take advantage of).

With respect to the ultimate load condition, there may or may not be a significant amount of deformation. This will depend on the failure mode (shear critical vs bearing critical...or possibly a bolt bending failure). To actually replicate a bearing failure (and associated large deformation from bearing failure), would be a challenge. First, you should recognize that compression allowables are not designed for something like a "bulk compression" so you may not have anything to even input to the FEM with standard allowables. This is why the the stated compression allowable can be much different than a bearing allowable even though a bearing stress is basically a compression stress (how do you propose the simulate that via FEA?). If there is significant fastener bending at ultimate, you might need a 3D FEA to truly simulate that effect. I am not aware that there is a FEM analysis that can generate the actual nonlinear load-deflection of the connection using basic material properties (even if it is a 3D, contact, material nonlinear model). I am not even aware of a FEM that can generate a joint allowable (or even a bearing allowable) from basic materials properties (tension, compression, shear allowables). Give it a shot..try to predict a bearing load capability from FEA via the compression allowable.

In the end, if you want something accurate, you will have to rely on test data for the joint connection. This may come from an equation (such as the ones posted above), but that would be backed by test data. If you are aware of a FEM (even the best 3D one with all the bells and whistles) that can accurately predict the load-deflection response of a general joint connection (and the associated joint allowable), please let me know. You can probably do it for some failure/deformation modes, but I am not sure it can be done for a general connection.

RE: Connection Design in Finite Element Analysis

(OP)
ESPcomposites - There's lot's of interesting information here and I must admit I feel a little over my head. I'm going to take some time to research a bit more about each point here and respond in detail when I have a better understanding.

“The most successful people in life are the ones who ask questions. They’re always learning. They’re always growing. They’re always pushing.” Robert Kiyosaki

RE: Connection Design in Finite Element Analysis

Sounds good. Make sure to be familiar with the various deformation/failure modes and try to understand what would be required to model that in FEA.

Note that you could probably determine the linear connection stiffness via FEA (provided it is a 3D model with contact). But with a lot of effort, that just gets you back to something like the one of the equations. So its not really a good engineering approach (though is does have some interesting possibilities for research or the methods group). However, things become complicated in the nonlinear material range because of the bearing failure mode (which is primarily the mechanism that allows for significant load redistribution). Its not from the tensile stress concentration of the hole though, so don't focus on that (even though the nonlinear effect of that can be captured with FEM with relative ease). If bolt bending was predominantly affecting the nonlinear load-deflection, you might be able to capture that with a 3D contact/material nonlinear model though. In the end, you only need to test a single joint connection (and not the specific joint) to get all of that information (load-deflection curve), which is a not a difficult or expensive test (and will give reliable information). To try to replicate that via FEA would be time consuming and unless you proved that it matched test data, its not reliable. We generally would not consider that to be an "engineering approach".

Brian
www.espcomposites.com

RE: Connection Design in Finite Element Analysis

If the argument is that it is going to be difficult to capture the stresses and strength capacity of BOLTS in a connection then I would agree that is beyond the capacities of most modelling. But I'm not sure that is the argument being made, at least that isn't the argument that I am making.

The few times I've used FEA to confirm my hand calcs it has been check the tension force distribution across a set of bolts. Bolt spacing and connecting element stiffness are reviewed accordingly.

RE: Connection Design in Finite Element Analysis

Human909: You may be correct about the argument being made. So perhaps the question is what is the usefulness of a linear vs nonlinear model, even if just a spring is used to represent the connection (as opposed to using a FEA itself to determine the load-deflection response of the connection). I would think the answer to that would be relatively straightforward. For a fatigue analysis (loads are relatively small compared to the ult load), redistribution would not occur for the fastener loads. Therefore, the analysis is always linear. For the ult load condition, redistribution may or may not not occur (depends on the failure modes). If redistribution does not occur, then a linear analysis is fine (this would be the case if the connection was shear critical). However, if the connection is bearing critical (or has some other mechanism to cause a significantly deformation before fracture - maybe bolt bending as well) then a redistribution of loads will occur (nonlinear result can be quite different from the linear solution). If one can demonstrate the linear solution is acceptable, then it might be conservative depending on the specific joint (overpredicts some fasteners loads and underpredicts others).

Previously, I was further responding to this statement and should have been more specific about that.
"This suggests that an assembly model can never be used to check connections, regardless of analysis type, without relying on a physical test." We still would want test data to define the load-deflection curve of the connection (as opposed to using the FEA for that).

Also, "steel connections rely on a redistribution of forces in the connection as stress concentrations yield and relax". I don't think this is quite true, but the idea is there. While there are stress concentrations (which cause fatigue damage), if it is just relaxation, the load magnitude is such that there won't be large deformations and hence no significant redistribution of fastener loads. The load magnitude needs to be relatively large, causing significant deformation (not just small stress concentrations), for there to be a significant redistribution of fastener loads.

RE: Connection Design in Finite Element Analysis

(OP)
ESPcomposites - Impressive website, clearly you are much more experienced in FEA than me. I looked up the load-deflection response and fastener flexibility you have talked about. It seems you're talking about the response of a single bolted joint, whereas I am talking about the entire connection (picture a double angle connection). All of the research I found on fastener flexibility for use in FEA was based in Aerospace. My assumption is that the stiffness of the individual bolted joint (hole, bolt, washer, nut) is much more important to aircraft structures, because the structure itself is made with thin metals and is not overly stiff. With structural connections we have 1/2" or better steel plate that is much stiffer than the bolt.

Also, it seems that you are hitting on the limitations of checking the individual fasteners and bolt holes in FEA. My first post mentioned that I do not check the fasteners, or fastener holes in FEA, I export forces from the post-processer and design the bolts/holes by hand using industry equations that are based on physical tests.

“The most successful people in life are the ones who ask questions. They’re always learning. They’re always growing. They’re always pushing.” Robert Kiyosaki

RE: Connection Design in Finite Element Analysis

Perhaps this may help? Your first start with determining the load-deflection curve (linear or nonlinear) of the individual connection. This could from a semi-empirical equation or directly form test data. You then use the FEA to represent the actual structure (may have many fasteners), where a spring/beam/CBUSH (your choice) element represents each individual connection. I think that may be what you are doing, but I want to be clear.

Regarding the size of the fasteners w.r.t. the plate, have a look at this recent thread. If you don't have a connection interface (represented by the fastener flexibility), you won't be able to get the correct loads on the fasteners. I think you are also doing that, but it is a good example why it is still important to represent the connection properly, regardless of the size of your plate/fastener.
https://www.eng-tips.com/viewthread.cfm?qid=478490

Thanks for clarifying about what you were doing with regard to how you use the fastener loads and that makes sense. I don't think we are too far off, I just wanted to clarify some things in general (since FEA of bolted joints can mean various things).

Also, just as an extra note, the linear slope of the load-deflection curve is a function of various parameters (member thickness, fastener to member eleastic modulus ratio, diameter, etc.), but the nonlinear portion of the load-deflection curve is a function of the failure mode. For example, if the joint is shear critical (fastener fails in shear), there won't be much elongation before fracture (its not very nonlinear at all) as opposed to being bearing critical (which has a relatively large amount of elongation before fracture). In other words, you can't always expect fastener load redistribution and a nonlinear analysis would not change the result (though it is often good practice to design a joint to be bearing critical to allow for load redistribution).

Brian
www.espcomposites.com

RE: Connection Design in Finite Element Analysis

(OP)
ESPcomposites. The thing that I'm not understanding is the load-deflection curve you keep referencing. If I put in the correct stiffness properties into my CBUSH element and use RBE3's to connect the CBUSH to the washer surfaces I expect to have a reasonably accurate stiffness. Either I am way off, the grad classes and seminars I have taken are way off, or we are talking two different things.

See page 23 here for an example of a bolted joint done in the way I am referencing

The link you posted didn't mention a load-deflection curve, but simply talked about relative flexibility between plate and bolts, and suggested to use spring elements with stiffness equal to the stiffness of the bolt. Everything in that thread was easy to understand and matched my expectation.

“The most successful people in life are the ones who ask questions. They’re always learning. They’re always growing. They’re always pushing.” Robert Kiyosaki

RE: Connection Design in Finite Element Analysis

The load-deflection curve is just another way to determine the "connection stiffness" or "fastener flexibility". Its nothing more than F=kx.

The reason I chose to say load-deflection is that it implies consideration for the nonlinear range (since load and deflection are the direct outputs from test data). And when you do a nonlinear analysis for fasteners, you may be provided the load-deflection curve and then create the appropriate FEA input from that (you may have to break it down in a set of piecewise linear stiffnesses). In engineering slang, I am used to "fastener flexibility" as implying just the linear slope (a single value). Note that even the term "fastener flexibility", which is commonly used, is slang since we actually mean the flexibility of the connection (which is a function of factors beyond just the fastener).

RE: Connection Design in Finite Element Analysis

Here is a basic overview. There are some details I left out, but this is the basic concept.

1. Start with testing a single joint connection (a single fastener and its plate members). It could be singe shear, double shear, etc. Apply a load to the plate and recover the total deflection. Next, we subtract the deflection associated with the plate members (where the plate stiffness is AE/L). What remains is the load-deflection curve of the joint connection (which accounts for various factors such as fastener shear deformation, fastener bending deformation, member bearing deformation, etc.). As stated above, we would not try to determine this load-deflection curve from a FEM because it not be an engineering solution (the FEM would be quite complex).

2. From the load-deflection curve, we can determine the linear “fastener flexibility” or “connection stiffness”, which is just the slope of the curve in the linear range. If we have enough data from a variety of joints, we can create a semi-empirical equation. From the end-user perspective, this may amount to a ready-to-go equation for the linear range or we may just go back to the load-deflection (if it exists) if we want to perform a nonlinear analysis.

3. Model the connection in the FEM with a spring, beam, CBUSH, or other element where you can simulate the stiffness response from item 2 (and effectively item 1). It doesn’t matter how you get there, as long as in the end you can reproduce the basic load-deflection response of the connection. For example, if you use a beam element, you would have to “back out” what the A, E, L properties would be to achieve the desired result. A spring or CBUSH is more direct.

3b. I don’t want to get too carried away with this, but some recommend you calibrate the solution. For example, if you place a spring element directly to a quad mesh, the point load at the interface will cause the shells to locally deform. This is a function of the mesh density. One way to address this is to create a representative connection and calibrate the inputs to achieve F=kx of the connection. In other words, you would want to get back to the response from item 1. You can model the hole if you wish, but ultimately, you want to get back to the response from item 1 since that is the basis for everything. In my experience, I haven’t fastener flexibility to be such a sensitive parameter that it normally requires this calibration, but it is something to consider.

4. Linear Solution. If you are performing a fatigue analysis, a linear analysis is sufficient. This is because the loads are such that significant deformation at the connection will not occur and therefore there will not be redistribution among the fasteners. If the connection is shear critical (shear failure of the fastener), there will not be significant deformation at the connection so there is no need to run a nonlinear analysis. Now let’s assume there is a significant nonlinear behavior of the joint connection. If you can demonstrate the connection is acceptable with a conservative linear solution (because some fastener loads are predicted to be higher than if redistribution was allowed), then you may not need to run a nonlinear solution. Just to be clear, at this point, the FEM represents a more generic joint (with multiple fasteners) and not just an isolated fastener connection.

5. Nonlinear Solution. In the event that the load-deflection curve of the connection has a significant nonlinear portion (due to either being bearing critical or bolt bending critical or other), you can perform a nonlinear solution (if this is actually required – See Item 4). Again, the inputs to your FEM connection element just needs to represent the response from item 1. It doesn’t matter how you get there. The advantage of this solution is that you can account for fastener load redistribution (if it exists). The disadvantage is that you need more inputs to define the load-deflection response and have to run a nonlinear solution.

6. Post processing. After you recover the fastener loads, you check them against various failure modes (shear fastener failure, bearing failure, etc.) or directly if you have the joint allowable.


Brian
www.espcomposites.com

RE: Connection Design in Finite Element Analysis

Quote (MegaStructures)

My assumption is that the stiffness of the individual bolted joint (hole, bolt, washer, nut) is much more important to aircraft structures, because the structure itself is made with thin metals and is not overly stiff. With structural connections we have 1/2" or better steel plate that is much stiffer than the bolt.

I take issue with this assumption. In tension we normally have significant preload on the bolt the bolts behave extremely stiffly through most of their strength range. A 1/2" plate is not particular stiff in an end plate type connection.

With bolts in shear we again have the bolts bearing on the holes. Here the flexibility comes from rotation of hole slop AND also localised point yield of the bolt hole in contact with the significantly harder bolt.

So in both cases flexibility of the joint is as much if not more so from the mild steel items.

(Of course much of this discussion is pretty vauge because the first question is what sort of connection are you modelling?)

RE: Connection Design in Finite Element Analysis

(OP)
Human909 - for the sake of conversation let’s say it is the simple lap joint shown in the link I posted above

“The most successful people in life are the ones who ask questions. They’re always learning. They’re always growing. They’re always pushing.” Robert Kiyosaki

RE: Connection Design in Finite Element Analysis

Yeah so like a shear/fin plate. The flexibility is from the bolt hole and also hole deformation.



In fact some advice warns against using 'thick' fin plates because they deform less and thus the connection will behave less like a pinned connection.

RE: Connection Design in Finite Element Analysis

(OP)
human909, ok I'm seeing the point, would you recommend:

1) A non-linear solution with a physical bolt
2) A linear solution with an adjusted CBUSH spring stiffness to account for bolt hole yielding (think this is what ESP was proposing)

When would you say these considerations are negligible and allow for modeling of the connection as suggested before?

“The most successful people in life are the ones who ask questions. They’re always learning. They’re always growing. They’re always pushing.” Robert Kiyosaki

RE: Connection Design in Finite Element Analysis

Megastructrues,

No, that is not what I am saying. I think I confused you, so I will try to keep it simple. Simply input the load-deflection of the connection to the FEA (whether it is linear or nonlinear, depending on your goals)...that is all. The load-deflection curve may look something like the following figure (we might omit the clearance part or adjust for it). It doesn't matter how you get there (F=kx), as long as you can reproduce the load-deflection curve via the FEA. For example, if you just want to run a linear model, then input the linear slope (k in F=kx). This could be done with a spring, beam, or CBUSH element and the connection stiffness could be determined via an equation (original basis is from test data). This is the most common way to model joints in practice.


from "Practical Analysis of Aircraft Composites"

The linear region (linear stiffness) will *not* be a function of the failure mode. However, the nonlinear response will be a function of the failure mode. If the joint is bearing critical, there will be more elongation than if the critical mode is a fastener shear failure. For example, human909 showed a picture of what appears to be bearing elongation, which is part of the nonlinear region. Either way, you need to know what the load-deflection curve is for the individual connection, and input that to the FEM, if you want to run a nonlinear analysis.


from "Practical Analysis of Aircraft Composites". Note this figure is for general composites and the bearing-bypass mode does not exist for metals (w.r.t. ult failure).

Brian
www.espcomposites.com

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members! Already a Member? Login



News


Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close