Stress Concentration in Aluminum T-Joints

[PhilipFry]

Hi. I'm still a bit new to the stress world, but I think I know just enough to get me into trouble. We've been discussing stresses in t-joints here recently and it came up that we should not be looking at the peak stresses in the fillets for static loads. It's been suggested that we use the nominal stresses away from the fillet. My mechanics of materials book says that stress concentration factors are often neglected when using ductile materials. Is that right? What about results from non-linear material runs that are meant to account for the strain-hardening of the ductile material?

 

[dozer]

There is a very good article on this in the Jan. 6, 2005 edition of "Machine Design". Don't let the title of the article, "How linear FEA helps in fatigue analysis", fool you, it has some good info on static analsis. Here's the link:

http://www.machinedesign.com/ASP/viewSelectedArticle.asp?strArticleId=57766&strSite=MDSite&catId=0

 

[PhilipFry]

Thanks. I actually found this article earlier today. Small internet world.

Unfortunately, the article raised a few more questions. The article repeated mentions that MOST engineering applications ignore the stress concentration, owning it to localized strain hardening. The example shown in the article uses a solid notched bar...and as expected, shows some concentrated stresses at the notch. Ignoring the localized stress raisers is all well in good for a solid bar, but what about my case? I have a hollow tube with a .035 wall thickness. Is the assumption that the rest of the cross section distributes the load valid in this case? I don't exactly have a whole lot of material to rely on here.

 

[rb1957]

i wouldn't mind neglecting stress concentrations for a static analysis, 'cause the yielding that would occur would LIKELY be very localised and not affect the overal strength of the strcuture. it'd be your opinion anbout your particular instance, but it'd be particularly important that there was material available to take on the extra load, and there's the possibility that the yielding MAY form a plastic hinge and become more large scale than you can accept.

i wouldn't neglect stress concentrations if the load was fatigue (repeated).

 

[zcp]

It all goes back to what you are trying to analyze. Maybe you ignore the stress concentration for an ultimate load case, but it will be the driving force in a fatigue analysis. Also, keep in mind that there are large allowances in (as an example) weld size and profile when comparing your theoretical weld to what is actually there in production. In this case, there may be a large stress concentration that would effect the static case (due to loss of material, thinning, etc.)

Always ask yourself "what am I trying to accomplish / what question am I trying to answer with this FEA?"

ZCP

http://www.phoenix-engineer.com

 

[PhilipFry]

"Always ask yourself "what am I trying to accomplish / what question am I trying to answer with this FEA?""


That's a difficult question to answer without test data...how do I know what the failure mode is? I'd like to know if I should be concerned about static loading (high loads) on the t-joint fillet, or if I should just assume that it will only fail because of fatigue (lower loads, but cyclic). Is one asumption more valid than the other?

 

[GBor]

I think ZCP is trying to say that you should use a little engineering judgement. If your load is static, I don't think you can completely ignore the stress riser that your FEA is showing you, but there are some guidelines to make sure that what you are looking at is valid. If your FEA is showing you a maximum stress of 40ksi in your part and 30ksi of it is in a single element at your stress concentration, then you can either refine the mesh to see what happens to the results, perform a non-linear analysis (probably not warranted until you've tried the mesh refinement), or ignore those highly localized results. BUT if failure of your structure would injure people...you need to investigate further!

If you have cyclic loading, then you need to perform a fatigue analysis and make certain that you aren't going to have problems.

These are two different cases, but it doesn't rely on test data. You investigate both and see what you EXPECT your failure mode to be. Not knowing your application, it is pretty much impossible to render a reasonable opinion.

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.

http://www.borowskiengineering.com

 

[zcp]

Thanks, GBor. Exactly.

mae1778, based on your response, I am not sure which direction to nudge you. If you are saying that you need to see the failure (test data) before you can predict how it will fail......then that is worrisome. Give us a little information on your background (so we have a frame of reference). Then maybe give us some specifics on your application so we can determine how to help you and answer your questions.

ZCP

http://www.phoenix-engineer.com

 

[PhilipFry]

Yes, it is worrisome, which is why I think I need some direction/encouragement. My background is that I've recently graduated from college with masters in mech eng, with no real industrial FEM experience, no real stress experience, but I’m concerned about the corporate trend of just pushing parts out of the door to satisfy our customer. I'm skeptical at work, it gets me in trouble at times, but I have a hard time letting things like this out the door until I understand the rationale behind it. Afterall, someone's life could be at stake.

As far as the application goes...

I don't think I can get too technically detailed, but I’d like to describe to you my engineering judgment. I have a thin walled, pressurized, welded t-joint. The static load show high stresses around the diameter of the tube at the fillet of the t-joint, not limited to a single element. These stresses exceed the yield strength of the material when considering the reduction of strength in the HAZ portion of the tube. My engineering judgment says that though the stresses should probably be a bit smaller when you take into account localized strain hardening, the elevated stresses still exist at that location and should still be considered a point of possible failure. My gut tells me that using the nominal stress and running a lighter fatigue load will result in stresses acceptable on paper, but I wouldn’t want to be standing anywhere near it when they do a proof test. My boss is telling me otherwise.

The point of my original post was to determine when using a Kt in a ductile material is justified when looking at static loads.

I hope this helps explain my situation.

 

[zcp]

A couple of questions on your application:

Is the static load due to pressure only? What does it simulate? An ultimate load case or a service load or the proof test load?

Are you governed by any applicable code or standard? You should not be getting that close to yield unless this is an ultimate load case that you just have to survive once. If it is piping (ASME) for example, you should be looking at allowables which have a FS built in...

Have you done a mesh convergence study to insure you do not have stress raisers due simply to the model?

Have you modeled in the additional material associated with the weld (i.e. the fillet)?

As far as your original post question goes....if you have an FEA model that accurately predicts the geometry of the actual part (meaning the weld, etc. has been modeled), then you have modeled in the Kt. That is often how you determine a Kt, you do an FEA to compare the stress concentration effects with the nominal.

Back to reality.....instead of butting heads with the boss, get him to teach you why he isn't worried. Don't argue your side, just listen. Then go back to your model and look at the big picture and make sure your FEA is answering the right questions.

Often, fresh out of grad school engineers have "paralysis by analysis" and need to look more to the big picture and experience of engineers around them to learn how to make the classroom stuff they have just seen useful in the real world.

I know because I was once that fresh out of grad school engineer working on stress analysis projects....

Hope this helps.

ZCP

http://www.phoenix-engineer.com

 

[PhilipFry]

Q: Is the static load due to pressure only? What does it simulate? An ultimate load case or a service load or the proof test load?

A: No, but pressure is the biggest contributor. If I don't divide by the Kt, the part shows stresses higher than yield in almost every load case.

Q: Are you governed by any applicable code or standard?
A: We design to a SF of 1.

Q: Have you done a mesh convergence study to insure you do not have stress raisers due simply to the model?
A: Yes, I'm certain that the stresses are "real" and not a singularity issue with the FEM.

Q: Have you modeled in the additional material associated with the weld (i.e. the fillet)?
A: No, that is not the department standard.

"you do an FEA to compare the stress concentration effects with the nominal"

What exactly is the definition of nominal stress? I started looking into how Kt's are calculated and got a headache. How far away from my high stress area is far enough...how much is too far?

"Back to reality.....instead of butting heads with the boss, get him to teach you why he isn't worried. Don't argue your side, just listen. Then go back to your model and look at the big picture and make sure your FEA is answering the right questions."
I think that's good advice. I'll work to do that in the near future.

 

[zcp]

Where are you getting the Kt to divide by?

Are you the only one doing these analyses or are there previous ones to compare to?

Have you checked your model for consistent units / correct BCs / etc.?

Have you done a mesh convergence study to get the highest stress values?

What stress value are you pulling out of the FEA? (Von mises, max principal, directional, etc.)

What are you comparing it to....Sy, Se, Sut?

Kt is basically max / nominal. In other words, stress with a hole divided by stress without. In your case, the component by itself without the joint might be the nominal and what you have now might be the max....thus Kt.

So what you are saying is that you are analyzing for an ultimate load case that will only occur once in the life of the component. So what happens if it yields? Are you below ultimate?

And now the thought that just hit me.....are the weld strengths higher than the base material?

ZCP

http://www.phoenix-engineer.com

 

[PhilipFry]

You are starting to open the same can of worms that I have on my desk.

Q: Where are you getting the Kt to divide by?
A: That's the $64,000 dollar question around here. There is no definitive answer for that question.

Q: Have you checked your model for consistent units / correct BCs / etc.?
A: Yes, my units are good. I've run a free-free case and found no erroneous results.

Q: Have you done a mesh convergence study to get the highest stress values?
A: Yes, increasing the mesh density does not significantly change the results.

Q: What stress value are you pulling out of the FEA? (Von mises, max principal, directional, etc.)
A: Mostly Von Mises. I've also looked at Tresca.

Q: What are you comparing it to....Sy, Se, Sut?
A: Depends on the load came. Sy for a limit load, Sult and Tult for a ultimate case.

Q: Kt is basically max / nominal. In other words, stress with a hole divided by stress without. In your case, the component by itself without the joint might be the nominal and what you have now might be the max....thus Kt.
A: Exactly the basis behind my question. Am I wrong that removing the stress concentration factor from FEM assumes that the failure mode will be in fatigue and not static?

Q: So what you are saying is that you are analyzing for an ultimate load case that will only occur once in the life of the component. So what happens if it yields? Are you below ultimate?
A: These are low cyle events...that is, they will certainly occur more than once during operation. And no, if I'm considering HAZ, I am not below ultimate...unless I remove the stress concentration factor from the FEM.

Finally, the weld strengths are at or near the strength of the parent material.

Thanks for the help!

 

[zcp]

Ok, I get your issue now.

Kt is often ignored in static cases for ductile materials. The thought is that any localized yielding for that ONE TIME loading will not fail the component due to plastic strain hardening, etc. Since the event in your analysis occurs more than once, then yielding at all would not be a good thing especially since you are using FS=1 (and the contents under pressure may leak). You should do a low cycle fatigue analysis via strain-life method, or assume a crack is present due to the welding and do a fracture mechanics approach.

Before doing all this, I would ask yourself how well you know the load you are applying. Often times a larger load is applied and compared to yield with FS=1, knowing that the actual load is lower and thus FS is actually >1.

For a lot of products, more material is so inexpensive compared to the cost of the analysis we are discussing above that you are better off going that route.

Also, what material are you welding that you are knocking the strength of the HAZ so much?

Finally, if you are sure of the load cases, sure of the geometry, sure of the material properties, you have properly meshed and converged an FEM, and you show stresses higher than the material strengths, then you have an issue.

You may eventually show through non-linear analysis that the thin wall tubes strengthen due to the plastic strain at yield and can ultimately handle the load at FS=1 instead of FS=.99, but plan on spending some time and money.

May be better to get thicker material or to take some of the estimation / overestimation out of the load cases.

ZCP

http://www.phoenix-engineer.com

 

[PhilipFry]

The loads were provided to us through our loads department. I'm sure there is some conservatism in those estimates, but none of us really know how much.

The culprit in question here is non-aged, non post heat treated, al 6061-t6.

Thank you again for your suggestions. I know we had planned on doing a high cycle fatigue analysis from random vibration. I'll have to look into the low cycle stuff.