Stress Contour

[GalileoG]

This is a very basic theory question that I am hoping someone would clarify for me.

The image below will lead you to an image from my Staad model displaying the plate contour stresses.

http://i37.photobucket.com/albums/e80/combatkirbyh/PlateStress.jpg

The green and yellow regions represent a stress between 200 and 250 MPa.

Now, I am a recent graduate so this is all very confusing for me. I posed the following question to my supervisor:

How do we know how much is too much stress on the plates?

And he responded by saying, "When it goes above the yield stress"

That's it? When it goes above the yield stress? I don't understand it! What about support spacing? etc..

Now, I've never really worked with plates before or FEM for real projects and my theory is a bit hazy. Can someone please clarify this for me?

And here is a totally unrelated question: Does the size of the mesh significantly alter the stresses on the model? (Meshing in Staad is a pain, so I am really hoping the answer to that question is a no)

 

[csd72]

Clansman,

needs a bit of clarification, what is this that you are modelling?

 

[GalileoG]

csd72,

It's a hopper for a crushing plant. Here's a picture of it below where you can clearly see the steel plates and the vertical and horizontal stiffeners:

http://i37.photobucket.com/albums/e80/combatkirbyh/P1.jpg

 

[40818]

Right, maybe its your bad luck today because i'm in a bad mood by another post, so dont get upset, but listen and digest my comments.

looking at your contour plot:
Your element definition is cr*p, you have too many triangular elements which are unecessary. And also a finer mesh would do you better.
Your peak stress is shown to be a single node, which is either a constraint or load application point, your post does not make clear. But it is probably spurious.

Now onto your education, you say that your a recent graduate, but i must ask the question that did you take some sort of solid mechanics/stress analysis/any other similar course when you did your time??

If you want to become an engineer, then i suggest you do some serious reading about the basics about the subject. Your question by the fact of you posting it gives grave reservations about your abilities and i would sack you on the spot even it you were an intern of mine.

I wont even answer the last part of your question regarding the mesh sizing and quality issue because if you cant stress by hand how the hell do you expect the pc to do it for you?

If you want to explore how meshing sizes affect the stress levels in FE create a simple quad cantilever beam with a point load, and alter the mesh density around the constrained end, watch as the stress goes to infinity and beyond. Then think about why this happens, then come back to this post with your answer, only then will i believe you have the curiosity/determination to become a decent engineer.
Please, take up the simple challenge and start to develop, you made it to eng-tips in the first place, so you must have some common sense!!

You have finished your education in the field, now you must start to learn.

 

[SWComposites]

Pull out your Strength of Materials text and review the strength theories for metals. If you never had a Strength of Materials class you had better take one soon. Your analysis (hand calc, FE model) will predict stresses based on the geometry of the structure, loads, material properties, etc. Then you check the stresses against a failure criteria to determine whether the structure will fail. A typical metal failure criteria is that failure occurs when the von_mises stress equals the material yield strength.

Yes the mesh size affects the stress results. Go get out your FE text and review it. Also see the many posts on the Finite Element Analysis engineering fora on this site. If you don't understand the effects of the mesh on the model results you have no business running a FE analysis. If you never had an FE class you should take one of those soon also.

 

[jike]

Yes, the size of the mesh will definitely affect the stress especially where the stress contours are close together.

The particular code that you are designing to will specify the level of allowable stress or the load factors and phi factors for LRFD. I generally ignore small hotspots as yielding will generally redistribute those stresses. Don't forget to look at buckling and overall stability if these are important considerations.

 

[csd72]

40818,

I think he understands the subject matter better than you give him credit for. Someone who didnt understand it would accept that the yield stress is the limit and thats that.

The question may be phrased poorly but I think the OP is requesting guidance on how to take the buckling of the plate into account when checking the stress.

Clansman,

Keep at it and dont be discouraged, this is a hard one for straight out of college.

csd

 

[40818]

csd72, i disagree with you there i'm afraid, i dont believe the OP has the basic knowledge you give credit for. Fair play for sticking up for him though.
I belive however that the OP has no usuable knowledge of buckling though, just looking at the FE mesh gives me that indication. If the FE was serious about buckling then it would be very non-linear, the plot shown doesnt even show the stiffening members and you need at least 3 quads to properly represent a free flange at its most basic.
If the OP is requesting buckling information then he would have said.
One thing i do not want to do is to discourage young engineers, but they must step up to the mark, as their education system is letting them down. They end up spending longer and longer just getting to know the basics.
One good point of the OP is that he/she is brave enough to put their head above the parapet and ask, which will stand him/her in very good stead in the future i hope. Because we have all made mistakes and had to start wher thay are now.

 

[GalileoG]

Let me clarify,

1. My question was about the criteria that we use to define failure of the plates. Why do we consider yield only and not something like deflection for example... will deflection never govern if plate is below yield point? (Deflection is what I meant when I said support spacing in the original post)

2. The geometry of the structure is extremely complex. I have panels at many different beta angles and horizontal, vertical and diagonal stiffeners all over and in order for me to avoid beam plate connectivity issues in Staad, I had to model the elements the way they are shown in the screenie. But if you think that is not necessary, perhaps you can give me a few words of advice for an alternative path?

3. Where you see the hot-spot in the screenie, there is a support leg on the other side of that panel (not visible in the screenie,) which is why I think that hot-spot is present there and not because of erroneous results.

4. I acknowledged that finer meshing will improve results, my question was whether or not making my meshing finer would SIGNIFICANTLY alter the stresses that I already have. I'm pretty sure it will and I will do just that, but I just thought I might as well ask.

Again, this is my very first FEM task and I am learning.

Thanks.

 

[40818]

Clansman,
You should always check the deflection of your structure to ensure it is within allowable limits. You can have quite large deflections in reality and still be linear, it depends upon the radius of curvature of the item. If your new to FE, then i would keep with a linear model, rather than try to understand non-linear large displacement FE. Just be carefull if you wish to show stability with a linear FE (i.e have very good margins) because Linear FE Buckling is pretty much nonsence. Yield point is a handy failure point for the basis of an analysis, but not the only one. Ultimate strength, max deflections are also used, some structures have high fatigue requirements and need to have very low working stresses. Depending upon the application, its governing criteria and the engineer in charge, the failure criteria will be defined.
Without knowing what your actual structure looks like it is hard to say what the mesh should look like, though try your best to not have triangular plates as they are overly stiff.
The peak stress is developed very locally around a single node and a better element definition around the area would smooth it out. I would still tend to ignore the peak as being nonsense here though.
If you have a very fine mesh your model is closer to reality. However, just by throwing fine meshes at it wont make it a good model. You can end up just sending your stresses up and up by simply increasing the mesh density. You need to understand what is truth and what is lies with FE. Its been said many times about nonsense in = nonsense out and this is so true with FE, always think about what you want to achieve with the model and what you expect the answers to be. To this extent do hand calcs so you know your in the right ball park.
No matter how long somebody is in the business they will never know anywhere near all their is to know. Thats one of the beauties about places like this forum, where you can ask advice from the field experts. What should be carried out before posting of a question is trying to determine the answers themselves. You can do this by reading books, searching the web etc. This helps the person develop their own understanding rather than just being blindly told what to do. Many young engineers fall initially into the trap of believing they know all they need to know because they are still on the high of graduation. And because of this its hard to get them to "learn". I dont think you fall into this catagory however. Dont take my comments as any personal dig, firstly your college should teach you about things like this, and also point you in the right direction to decent books. Your boss should also give better guidance and explanation to help you understand. Your part would be to take these pointers from your college and boss and then research them. Places like this help that research, but do not complete it. Keep plugging away.

 

[DaveVikingPE]

Did you use the mesh generator? (Probably yes...)

Here's how I would approach the problem (and how I approach a project that I know will require a lot of FEM - using STAAD, 'cos that's what I've got - iterations based on a lot of loading cases): I draw the framing first and make sure I understand my coordinates and such. With STAAD, you can either draw it directly in STAAD using the StructureWizard or not, or you can draw it in a CAD program and import the model, etc. Then I set up the framing, in STAAD, giving all the framing members their properties, materials, etc., etc. THEN, run a self-weight analysis. From this, I get all my reactions - this is the kind of stuff I can check by hand. I can also do simple beam calculations by hand and check these hand calcs vs. what STAAD spits out. Once I've got the framing working, then I would start adding the plates - I prefer to model structures the way I envision them being constructed - and I would check the different stress contour plots STAAD will output.

Personally, I feel that the maximum FEM calc I want to check by hand is a 6X6 matrix, anything more than that will take me too long - and why bother? If you've got things set up properly, your hand calcs vs. STAAD results should match.

There are also, if I recall correctly, some example "bin" and hopper calculations in one edition or another of the Structural Engineering Handbook and other books (maybe Blodgett's welding books?) - seek them out and check them vs. STAAD. Are you getting the same results? If so, then build from that.

OK, plates. When do you define failure? How much deflection can be tolerated? If it's permanent, then you might end up wrecking any machinery associated with the hopper - just speculation on my part. Even it's it's elastic, there's got to be a limit - find out what that limit it. Can you tolerate the material rupturing? Or plate-plate welds breaking? Probably not. I'm from the allowable stress generation and thus it's my opinion that it's conservative to keep things below yield.

What about how you're applying loads? Do the stress contours make sense to you? From the picture you've linked to, I can't really tell how you're applying loads other than a lot ends up on a corner or "hot spot" as you call it. (OT: does the support leg fail in buckling?). Go through all of the output (probably 10,000 pages or more...) and spot-check the stress calculations.

Working all night (and weekends) on problems like this - for no extra pay, since we're "exempt" personnel - is the way expertise is gained. It's also the way we're expected to work at and solve problems. Enjoy it!

 

[GregLocock]

You might like to use the search functions for the effect of mesh density.

By eye I would use /at least/ 3 times the linear resolution you have currently got, say 10 times as many elements.

You have identified a couple of hot spots. Do they make sense? You might well need to increase the resolution in those areas, and model the joints in much greater detail.

FEA is a tool. There are different ways of using it. I have built useful and accurate models with fewer than 80 elements. But, as mentioned above you do need to understand the tool On the other hand you are asking good questions rather than just accepting the result, so that is a good start.

In my opinion lack of correlation data is likely to be your biggest problem.


As to what stress is acceptable, in my industry we don't have code values to design to. For different parts, and loads, we might design to UTS, yield (quite common) or fatigue strength (most common). However much of our structure is limited by stiffness considerations, and the tricky stuff is all beyond yield (crash).





Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[UcfSE]

40818 gave you some good advice. You should listen. I would advise doing your homework before posting questions like this. Even if you understood what to design to, looking at that mesh suggests it wouldn't help you much anyway. A pain or not, garbage in = garbage out.

Designing to yield is not the only way and not necessarily the most common. Look up "failure criteria", to being with.

 

[aggman]

Something I might ask, coming from someone who works with these sort of structures daily. What exactly are you trying to solve for this structure? Is it existing and having problems or are you designing a new one that is similar? I think that you are probably going overboard trying to do an FEA on this and I am not real sure why anyone would pursue this unless they were in trouble or trying to get someone in trouble. Looking at the basic geometry from your photo I could solve this thing using hand calcs in a few days. Break the problem down. You have the basic panel size. Hopefully you know or someone in your office knows how to calculate the normal loads on the plates. You can check the plate and mostly size it for normal bending. Then you can size your stiffners and then the top and bottom flanges. Yes you do have several plate angles and different walls to deal with but very easy to solve for each. Follow your load paths on the hopper and resolve the loads to the ground. If you approach the problem this way first of all you will have a much better understanding and feel for what you end up with and second someone should be able to actually follow your analysis. You will spend a bunch of time on the FEA and in the end have something that looks pretty (I hope anyway) but you will probably have no idea if the results are correct. Many, many hoppers are designed today without the use of computers at all. Some of that is because the guys doing the calculations are old school, but mostly it's because the amount of work involved to get accurate results far exceeds the effort to design a satisfactory structure by hand. Also these structures are typically abused beyond reason so the extra material and strength that is discounted using hand calcs is well used over the life of the structure. FEA looks like an easy solution to something like this when in reality it's not. Go to the Lincoln Arc Welding Foundation website and purchase Troitsky's Tubular Structures. Also check your local university library for a copy of Gaylords design of steel bins for the storage of bulk solids. Also check ACI 313-97. These are very useful books that will help you work through the normal assumptions of load paths, etc. Also I challenge you to really try and work through the problem and truely understand the analysis. This is a great field to work in and not a lot of engineers understand hopper design. You might just find yourself a nitch! You already have made the right steps by just having enough intuition to say...you know I am not sure about what I am doing here and I think I need some help. Good luck.

 

[rb1957]

my 2c ...

the mesh does look crap ... too many triangles (even if they are better than they used to be i think they should be avoided). the model looks as through it has several facettes and the intersection of these looks like it creating trouble for your mesh generator. don't just accept the auto-mesh, but as you say you don't have much expereince ... where's your supervisor in this ? what guidance is he giving you ? (not much ??)

2nd, think about your model ... is there something in it that would cause a localised stress peak ? (constraint, point load, ...) these (point loads and point hard constraints) are an artifice of the FEM and not truly representative of the real world; this is why we'll sometimes discount these stress peaks.

i was really surprised by your comments "When it goes above the yield stress? I don't understand it! What about support spacing? etc.." ... this doesn't sound like someone who understnadds what the FE is doing. Of course the FE is taking your supports and constraints into account. It would have been a really sensible comment if you had mentioned buckling (maybe you have already, i remember some comments about this, but (mea culpa) i haven't read the entire thread) ... ie the allowable stress ccan be less than yield in thin sheets; but maybe your supervisor knows this and knows the design better than we do, so he might have been telling you how to solve your particular problem, rather than how to solve any problem.

 

[csd72]

clansman,

I do not do FE, but I will try and answer your questions from a general structural engineering standpoint.

1. Why is deflection so important for these plates? It is an industrial machine and people expect it to move and shake a little during operation. Figure out what size plate you need to satisfy strength and then tell your supervisor what deflection you have, they will either okay it or ask you to reduce it.

2. In the past I have found that complex structures become even more complex if you try and model them in their entirety. Break the structure down into constituent components and do hand calculations to get a feel for sizes, then put these sizes into the FE if you feel you have to (personally I feel that FEM is over the top for any building, but thats just me). Look at roarks stress and strain for formulii for a plate and check the worst case which will be a bottom corner plate.

3. and 4. - cant help you there, but if you have done your hand calcs then you will know what to expect.

csd