This content has been marked as final. Show 9 replies
What we're looking at is a jack stand. I've cut it in half for a symmetry analysis, though I've tried a full model, and every other variant I can think of (putting the loaded bar at an angle, bonding surfaces, etc). The following is my evaluation of where the problem is.
1) Incorrect material properties
*Checked and double checked.
2) Inaccurate Solidworks model
*Matches production model.
3) Inaccurate COSMOS modeling
*I've tried everything I can think of!
4) Wrong failure stress consideration
*I've primarily looked at Von Mises, since we're dealing with ductile materials.
5) Model is accurate.
*Material used in production would need to be significantly stronger than the drawings call for.
I've attached the model in a zip file here. If anyone would be willing to look at the model and provide some feedback, a fresh perspective would be greatly appreciated, especially regarding the accuracy of the model. (I'm assuming a jack stand is simple enough to understand.) In the meanwhile, I'll see if I can't do some testing of my own to see if there is some type of material yielding taking place, and maybe dust off my mechanics of materials book to see if I'm missing something! Thanks!
Few questions: Did you compare two results, each with unique mesh conditions? Convergence may not be high enough.
Did you compare a full model to the half model with symmetric bc's? Buckling, a non symmetric response, may be happening. If you are holding it to symmetry and this occurs something else has to give.
Have you compared your results to a result of a model done completely in one part using different bodies for each component? Constraint equations may be set up differently in part mode. This may generate a high stress in assembly mode.
Thanks for the feedback. I did try a few different meshes, and it seems to converge. I am trying another mesh that is beyond the detail that the slider allows to see if anything changes, but it doesn't seem like it will from the trend I've seen so far.
I did run the full model, which produced similar results. I'm using the 1/2 model to make it run faster.
I haven't tried simply using a multi-body part rather than an assembly. I was under the impression that it should work the same because COSMOS works from the mesh it creates rather than the parasolid model. Anyway, I'll give it a try since staring at a screen doesn't do any good anyway!
When you are applying your load, are you applying half the load? What type of contact condition do you have between ratchet bar and base? What kind between pawl and ratchet bar? I dl your attachment but the assembly was referencing different part models that werent' attached so it came up with mate errors. Also, Cworks configuration file wasn't included.
David, thanks for trying. I reassembled and made sure to include the CW file also. I had someone verify that it would open with load/restraints on a different system, so it should work this time. (Much larger file this time)
I am applying 1/2 load (total capacity is 4000 lb, so Force is 2000 lb). I'm using surface contacts all around. Speaking of which, I'm using 2004, so I can't define node-to-surface vs surface-to-surface, but from what I understand the setting is node-to-surface by default. I had tried bonded between the pawl and ratchet bar, which yielded similar results.
Hi Peter, I downloaded your model but, as I expected, didn't see anything obviously incorrect. Here's my best guess based on your description. You said your Engr Head stated qualitatively that there was "no yielding." To me, this suggests that a cursory visual check didn't show any features which took a gross permanent set. It may also mean, based on my experience with casual observations, that the stand worked after testing so the assumption is that it didn't yield. I think you really need to quantify the "didn't yield" comment before tearing your hair out.
As shown by the images I've attached, only a small portion of the jackstand crossed over the yield threshold so it is likely that the visible permanent set would be very small. Also, the resultant displacement in that area, with the linear model, is about 0.010" (~0.25mm) so any permanent set would likely be on that order of magnitude, again difficult to determine without measurements and nearly impossible to notice if you weren't expressly looking for it.
Also, you mentioned that your Engr Mgr was referring to a similar part, not the exact part so, with this small area of potential plasticity, it is unlikely the comparison is fair. Do you have geometry for that previous version that you can analyze and compare to this one? It might help you in your assessment of these results.
On a modeling note, I would recommend a tighter mesh on the jack stand. Your mesh was somewhat coarse for a thin walled part where the primary ara of concern is in bending. However, a finer mesh would result in higher stresses. I would probably only restrain a single vertex in the 3rd direction (not the symmetry or loaded direction) for stability. Restraining that whole face might have slightly over-stiffenened the bottom of the base. (Probably didn't matter but I always suggest checking.) Bottom line though, I think you've set your model up pretty well. Always check your mesh convergence. This will get easier in 2007... upgrading for this reason alone makes sense.
Let me know if this take on the problem makes sense.
Thanks for the response. After a few other model tests in COSMOS, I was at the point where the most likely solution was that we had a fairly accurate model. Your guess from my description that we need to quantify "didn't yield" makes the most sense to me at this point as well.
Regarding the geometry matching the test part, it seems like it would be worthwhile to adjust the model to match the tested stand by taking dimensions directly off of the test specimen when we do future testing. I imagine this could save headaches.
As for tighter meshing, I did run the same model (different files) a few more times with finer meshes. Actually, I was able to max out my memory by entering a smaller element size than the slider allowed for the collar. I suppose the slider is there for a reason! With the vertex restraint, I will have to get into that habit! I usually will put those restraints where friction should stabilize the model, but since you mention it, I can see how a full face could introduce errors.
And it will be a matter of days (i think) before I'll have access to 2007 (though we'll still have to model in 2006 for compatibility), so I'm looking forward to checking out the new toys in COSMOS.
Thanks again for your help! Hopefully we'll be able to do more quantifying for our testing in the future, before stressing out!
One other question: this being a linear analysis may result in some error. Is it reasonable to assume that a non-linear analysis would provide the same trend in this case, even if the magnitude is off? I have been trying to d/l the Companion presentation to learn a bit more, but there seems to be some trouble with the page after filling in the forms.
Hi Peter, let me know how a comparison to a real part turns out. As far as trend study with linear, in this case I think you'll be in good shape. When large displacement nonlinearities cause the stress distribution to be different than the linear small disp solution, trend studies using that linear sol'n may not be valid. In this case, especially with the small amount of post-yield response, I think you'll be in good shape staying linear.
Have a great weekend!
We tested 2 similar jack stands, though we weren't able to get strain gauges to record exact values. Instead, we did dimensional checks at various points through the testing. The first stand, which matched the SWX/COSMOS model very closely, responded with some permanent deformation at the back of the collar, like COSMOS showed. The second stand was slightly different and didn't show the deformation, but the sheet metal was slightly thicker. I haven't had a chance to run the model with the thicker wall yet to see how much deformation is to be expected on that one, but the first design is our primary one.
Thanks again for the help!