There have been a few topics where Finite Element Analysis (FEA) has been presented and discussed. Some questions are popping up about various aspects of FEA and how to get reasonable answers. Rather than clutter up random threads with such discussion I thought a new thread would be useful.
This thread should be a place for:
Presenting FEA results
Reviewing FEA results
Any questions related to FEA setup and execution
Requesting FEA of a part/system for funsies and/or to help inform a design decision
Ranting and raving about FEA topics in general
Why on earth should you listen to me? I do models/modeling/FEA for my day job. I have learned from a wide variety of modeling experts and modeled many different things, from simple single-part structural analysis through multi-component multi-physics analyses.
I believe strongly in the ability of FEA to help engineers make informed decisions and save time and money in their projects. I also believe strongly that FEA misuse can waste plenty of time and money and inform potentially dangerous decisions. Getting things right is critical! So here we are to chat about it.
What about 2x1x1/8th tubing only pocketed on the tall side (1inch wide side unpocketed) vs unpocketed 2x1x1/8th vs 2x1x1/16th while being loaded in the āwrongā direction as if a robot ran into the frame with bumpers as commonly used on drivetrains and drivetrain impacts.
If I understand correctly, 2x1 tubing in dt impact loads gets most of its strength from the 1in wide unpocketed face on top and the large face doesnāt provide much impact resistance.
@Oblarg@nuclearnerd here is a quick study on mesh sensitivity. This model shows bending of an aluminum tab with a sharp inside corner, a big stress riser. By changing the mesh of the part we get remarkably different answers about the stress level in the part.
What we see is that we need the finest, or at least second-finest, mesh I arbitrarily picked to get a viable results. Increasing mesh resolution systematically until we get a repeated answer is important! We do not want our mesh choice to influence the result.
Now, the way I did this mesh study is a bitā¦ ham-fisted. I made the WHOLE GOSH DANG MODEL meshed very finely. Now that I know where the problematic area is I can apply a local mesh refinement to capture the interesting behavior and let the rest of the model use a much coarser mesh, saving precious electrons and computational time.
Applying a local mesh control results in the meshing and solution solving MUCH more quickly (solver time ~#elements^2 for most physics).
A similar mesh sensitivity sweep, but only with local refinement, solves super fast and provides basically the same result. Solution time was likeā¦ 15min for the full-silly-mesh model, and <1min for the locally refined version.
You can see the corner inside the pocket is a little stress riser.
This is incorrect, assuming the bending load is coming into the 2in side of the 2x1 tube as most chassis are made. I ran a similar model with pocketed tubes.
What we can infer from these results (and some solid mechanics equations that I wonāt get into at the moment) that the tubeās stiffness is driven by the webs that are furthest from the neutral axis (center of the beam, for our purposes) relative to the bending moment.
I hope this makes senseā¦ if not I can explain more at a later time. Thereās a lot going on here!
Makes sense as 1/8th tubing doesnāt add thickness in a useful direction like 2x1 does compared to 1x1.
Is there a pocketing scheme that would efficiently save weight for dts because they only tend to be loaded in one direction or is the move just to use thinner tubing?
Thinner tube ftw. If you want to ball outta control 2x2x1/16 is lighter than 1x2x1/8 and tremendously stiff in both bending directions.
The simple explanation is that any pocketing adds stress risers (and takes time and energy to manufacture). So thinner wall has won out every time Iāve modeled it.
Do you have a fea between 1x1, 2x1, and 2x2? Obviously thicker would be better when loaded in the long direction but how would they hold up for loading in the short direction?
Stress ~ 1/(heightĀ³ x width) and ~ 1/(wall thickness)
Stiffness ~ heightĀ³ x width and ~ wall thickness
So, 2x2 is about 2x2Ā³=16x stiffer and stronger than 1x1 of the same wall thickness. 2x2 will be 2x as stiff and strong as 1x2 bending the long way, and 2Ā³=8x stiffer and stronger vs 1x2 bending the short way.
I knew about those but based on experience it can be a bit more complicated because the faces on the tubing can start getting wrong direction loads in which those shortcuts donāt hold up anymore and the tube fails much earlier
I meant to take some time to chat with you at Granite State and Greater Boston about this, but I unfortunately didnāt find the time to do so.
Even before you started this thread, I really admired how you often went the extra mile and took the time to do the math & stress analysis on some of 95ās parts. Whether it be quick back-of-the-napkin math or FEA, your explanations on how, and why, you do those analyses & how you arrive at certain conclusions has been tremendously helpful and enjoyable for me to read through and digest.
As a Mechanical Engineering major taking my first stress analysis (and materials science) course this term, itās been truly incredible going to class and learning all of these extremely applicable topics that I can, and frequently do, utilize in my everyday life. Itās even more reinforcing when I open ChiefDelphi to see you explaining the exact topic that I learned in class that very same day! And to hear it from an engineer like yourself in the context of FRC truly does help develop my understanding of those topics even further.
Itās been really cool being able to understand more and more of your explanations and math as I progress through my class. Of course, thereās definitely times where you lose me, so expect a lot of clarifying questions as this (and 95ās) thread progresses
Just figured Iād let you know that your time spent on in-depth explanations is greatly appreciated and extremely helpful for me, both in FRC and in my studies/future career.
Have you compared these results to analytical models? Timoshenko+stress concentration tables should give a very good result with a case like this. I ask because the difference in results between mesh sizes might be the result of mathematical singularity in the corner, and itās possible that one of the coarser meshes gave a more accurate result (despite showing lower stresses)
Have you done any analysis on the various tubing with some of the drilled holes having a face to face clamping force added onto them to represent a through bolt or something. Kinda curious how that might affect the strength of the tube.
Iām sure James will reply and I look forward to reading it, but I had a question:
I donāt fully understand what youāre saying here (current frc student getting introduced to FEA) but what Iām getting is that youāre mentioning how perfect corners in CAD will produce larger amounts of stress than the real world which has tiny filleted corners due to material imperfections.
Is that right?
If so, how do you/can you determine when youāre overmeshing an area? Is there a way to do this or is this real-world testing and experience? (You mentioned Timoshenko and stress tables ā what if these canāt be applied to a certain part or can they cover pretty much any FRC case?)
Not exactly what Iām saying. With a perfect corner, you may sometimes get artificially large stresses in FEA even compared to a ārealā perfect corner (if such a thing ever existed). Theoretically, with perfect corners, itās possible that the smaller your mesh, the larger the stressed youāll find, up to infinity (i.e. miniscule elements, enormous stresses). This isnāt because of real world physics but because of the mathematical model the computer uses to solve the analysis.
Side note (not what you asked but you made me think about it), when you have stress concentration in corners like in the example above, you may sometimes see stresses far beyond the yield point, and that might be okay. If itās a static load (which it almost definitely is in FRC), the part will deform very slightly in the stress concentration area and āadjustā to the high stresses. The end result will be a yielded, plastically deformed part, but so slightly deformed that you couldnāt tell the difference and without hurting the partās functionality.
You can usually identify these situations in two ways:
If the stresses in the stress concentration are are high but the stresses one or two elements away are below the yield point (especially with a fine mesh)
After spotting stresses above the yield point, by performing a non-linear analysis, you can see exactly how much (or how little) the part will deform, and decide whether or not that amount of deformation is acceptable to you.
I have not. We would also want to model whatever is attached to the tube in this case as it would likely change the stiffness, and thus stress distribution, of the tube.
Excellent point! No, I have not done this for these FRC models. Since I created nominally the same concentration in all the parts with the same mesh the relative answers ought to be valid. If we were looking for an answer that was absolutely correct we would do more hand-calc checks like you suggest.
Bang-on explanation!
Expanding a little:
Even before yielding there will be āstress spreadingā behavior due to the elastic nature of all materials. Stresses spiking to infinity is an edge case that I have not often encountered, but it is important to know that it can happen and to keep an eye out for it.
Doing a hand calculation of a comparable, but simplified, case to estimate your expected results is an important part of good analysis practice.
Admittedly I do not usually do this for FRC freebie models (you get what you pay for ). Iāve been doing this long enough, and these beam problems are simple enough, that I take shortcuts. E.g. if the peak stress is where I expect it to be and one case is not wildly different than the others then I am reasonably confident that the result is sane.
IRL I will go beyond hand-calcs and design experiments with my colleagues to evaluate a given modelās validity. This provides the opportunity to calibrate a model to reality, e.g. tweaking assumptions and simplifications to more closely match emperical results.
(This type of tangent is what I meant when I said 'ranting and raving about FEA )
In CAD its easy to have perfectly sharp corners, and actually hard to avoid doing it! In the real world, sharp inside corners are hard to make. Actual extrusions always have a radius inside the corner and a radius on the outside corners too. Welds smooth the transition between parts (assuming you donāt do a bad job on the weldā¦).
Another thing in your favor is the fact that ductile materials will undergo local yielding that acts to spread out the stresses. The trick is understanding when that will occur and when it will fail catastrophically With brittle materials (like cast iron and ceramics) you donāt get this extra room. Thus, brittle materials require much more careful design work!
While this makes sense in terms of stiffness, I have always viewed strength as the bigger issue with a lot of pocketing. It seems like the real world failures of pocketed extrusions tend to be buckling failures of the ligaments. My mental picture of this has been that if you take an rectangular extrusion, and load it in bending then one face goes into tension, one face goes into compression and the other two faces go into shear. A typical ātriangular trussā pocketing scheme does not do well with compression loads compared to a thinner, unpocketed face as the individual ligaments of the ātrussā carry these concentrated compression loads and experience buckling instability at a lower global load than the thinner, unpocketed wall. The thinner, unpocketed wall gets quite a bit of buckling resistance from the presence of the corners of the extrusion (especially with the āreal worldā fillets in those corners). The shear web faces also have less stability as the shear loads are converted into tension and compression in the truss ligaments and the ligaments that are under compression again suffer from buckling instability.
)
With brittle materials (like cast iron and ceramics) you donāt get this extra room. Thus, brittle materials require much more careful design work!