I'm no expert on nonlinear analysis but seeing as nobody else has stepped up to the plate I'll take a crack at it.
There seems to be some strange "wrinkling" effect on the threads as well - lines coming out radially from the root of the thread where material seems to have been displaced. That and the wavy stress distribution makes me think that your simulation may be running into a kind-of stick slip scenario - my other thought was that perhaps your time step is too large. See below:
1) What is your friction coefficient, both under the head and on the threads? I would try reducing it -possibly even all the way down to zero if the model will run- and seeing if you can get it to a point where it looks correct. Solidworks may not be able to handle a medium to high, or even realistic, friction coefficient under these conditions - I'm not sure, you might want to research for documentation pertaining to modeling thread/bolt stress in solidworks nonlinear simulations.
2) Try reducing the time step. It may be trying to jump too far ahead and applying the load in too large of an increment - very small increases in the angle that a fastener turns corresponds to very large increases in load.
3) Try reducing the torque/angular displacement that you have applied to the model for the same reason as #2.
4) Lastly, what does the animation look like as it is loaded? Watching that animation in the key areas of concern may provide some insight as to what is happening - if you can post it I would be interested to take a look.
Thank you for your answer. The last days i made a couple of tests (40+) and played with almost every settings:
1 Tried with different frictions from 0 to .8, the result was not excatly the same,still come with ten wave thingies, the only different is the transition, sometimes harder and sometimes softer.
2 I reduced to extremely fine stepping with 100 steps, at max diameter about 0,0000628 mm/step movement. It wasnt too small to calculate so ran without any fail. Also played with the time but speed doesn`t change anything
3 see Nr. 2
4 Uploaded, also the model, the waves are rotating togeother with the bolt (maybe hard to see but i confirm) . Yea the mesh is really row but the number of triangles does not show any correlation with this type of failure so, it was effective to give some fast try.
Only pull: Rotated after the pull:
yup, not too fine steps but has the same result when i take 8 or 100.
What i also tried after every FEA settings:
-Edit the 3D model, made a new one with another method for the thread (instead of Combine/subtract use simple revolved boss/cut) , same result.
-When i only pull the bolt, it looks as should without any problem, but when after the pull i rotate, waves are coming as seen as on the picture (displacements,the helix at the outer edge of the thread).
It possible to count them because they are soo clear : ) exactly 10 / round. why 10?
-Rigid Nut: same result. Is it physically possible when the nut is Rigid the bolt threads looks like this?
After this Rigid result im really confused and looks like to me maybe it has a computational difficulty, but have still some idea.
I didnt find any reference/study/video/something with solidworks Simulation and 3D thread with rotational movement, with 2D siplified there are many of them, maybe this is why?
also you can find here the uploaded assembly, when someone has time and joy to take some try : )
M12.zip 1.4 MB
I have looked at your CAD model. I notice there are no fillets on the thread. This could lead to stress singularities there. Perhaps this causes the stress result that you are seeing.
Can you also upload the model with the simulation studies in it?
There is definitely some strange behavior going on here. Unfortunately I tried opening your model however I was unable to - I am using an older version of solidworks (2013) so that may be the reason.
Just a few notes looking at your description and images as well as after brainstorming for a while:
1) I hope its sort of a silly question but I assume you have modeled the threads per ASME/ANSI/ISO standards for proper fit between male/female threads correct? If the clearance is too small or zero there may be an issue with how the threads behave in the model. I know there are allowable thread fits that are zero clearance or interference however they may not behave properly or as expected in a simulation. Additionally does your simulation start with initial contact or clearance between the threads as well as under the head? I might try it both ways and see if you get a different result - of course you would have to change your loading conditions accordingly as the fastener would have to go through additional rotation if it starts out with clearance.
2) You said there is a "rigid nut" - it may be worth attempting the model with the both the male and female threaded components as flexible. I don't know exactly how solidworks treats rigid bodies but it may be somehow affecting the simulation.
Also are the female threads meshed with the same type (compatible) and size elements? How is the underside of the bolt head and face of the mating component meshed and how is it behaving (stress/force distribution, etc..)? The bolt head is a significant contribution to how the fastener behaves under torque and may be having an effect on the model.
3) The actual stress distribution, in addition to the noted "waves", looks a little strange. The most apparent of which is the fact that there looks to be a high stress area on the 6th engaged thread - this is counter to what is expected as typically that 6th thread should carry less than 10% of the load (see below). Maybe you want to look at a contact pressure plot and the forces exerted on the threads and see if they match what is theoretically expected? This is the case with both the rotated and pull simulations.
Additionally it may be just the way the snapshots look, but it almost seems like the stresses are increased/biased towards one side of the fastener (perpendicular to the central axis of the bolt) instead of decreasing along its length (parallel/along the central axis of the bolt). If that is not just a trick of the eye it may be a key that the contacts are not behaving as expected.
Janko: i also made a model with full of fillets without any sharp edges ( really without any fillets were everywhere) , but it does not do anything with this deviation only the calculation
time will longer, this is why i didnt use it. I dont want to upload the simulation file because its possible i made a mistake and repeat it every time, and when some do it self and looks the thread normal that means the fail is between my monitor and the chair and not in SW : )
1 Thread clearance:
about 0,1 mm, tried from 0,05 to 0,2 but it does not change anything (i mean with the strange stress distribution)
also tried with or without initial contact (so the two surface touch each other after a little bit of radial movement)
2: tested every combination
i made a new model only for the test without the head, so its faster and eleminate additional confusing factors.
3: yes there shoould be a singularity or failure because of the sharp nut thread runout, its not always there (depend on mesh and surface settings)
I was so curious so made a little bit investigation (ye not a bit, more like dozens of simulations with different "thread-like spiral" models)
looked for dependency and i have found one thing: the number of the waves depend from the pitch (from the gradiant angle): the more of the angle there more number of waves appearing : )
I`ve made 3 full thread, and marked them from thread 1 to 3 (1 is the first which has the most load) in the picture . The pitches are from 10 to 2 mm with constant 12mm outer diameter.
But it doesnt need to bee a full thread to reach these deviations,1/4 thread and bamm its there.
i have some more idea to try but im start running out of them and as i mentioned earlier i still have not find any reference with Solidworks until now, so maybe it cannot handle this situation or i dont know what should i think.
For #2 there was absolutely no difference in rigid vs. flexible nut? Also did you put an equally fine mesh on the female threads on the nut side as well?
Your results for the increasing thread pitch are very interesting indeed, although I wonder what the introduction of fixtures is doing to the model as you eliminated the head - looks like you've restrained translation in all directions. Were your previous models using any fixtures on the bolt itself?
I would be really interested in what the solidworks team has to say about this type of simulation - I wonder if theres a way to escalate it or get one of their mods to look at this. My gut feeling is that due to the complex nature of the helix contact and then compounded with the complex loading in the bolt and threads (torquing of bolt = torsional and axial loading) as the bolt moves through its rotation may be extremely computationally heavy and causing issues for the solvers that solidworks uses. Maybe a solidworks expert with more advanced knowledge of the solvers could chime in and explain why.
As a side note, I initially thought that the lopsided stresses in the bolt may be due to these difficulty that solidworks is having in analyzing the model. Now that I think more about it, it may be due to the fact that whichever side has the first (uppermost) thread in contact may bias the stresses/loading to that side of the bolt as well as the 45 degree shear plane due to axial tension in the bolt as can be seen in the models (division between red/green in stress plot). Maybe thats not valid and someone more knowledgeable could provide some insight, I'm just attempting to rationalize what I'm seeing.
What type of mesh are you using? Based on your screenshot, it looks like the standard mesher which follows the U-V curves of the surface and may sub-split surfaces. Do the oscillations of stress seem to match the mesh sub-splitting? Here is my result with the blended curvature mesh which I believe should reduce the effect of splitting.
Have you tested refinement of the mesh and compared results with previous runs to see if the oscillations decrease in magnitude?
Hi Shaun, can you please upload the assembly with your simulation setup? I remeshed the model in blended-curvature mode but the result was the same as always an not as at you.
Actually, I was looking for a version of your model with studies on it in this post, but I couldn't find one. Did I miss it somewhere? So much faster to offer suggestions and detect errors with such a study.
I have not read all replies, nor tried this in Solidworks. One question is if SW is capable of combining contact and large deformations? This problem has to be run with large deformations, or else you will have incorrect results. I'm not 100% sure SW can do this.
Another question is what is the purpose of the analysis? Can it possibly be simplified into ignoring the helix angle of the treads, so as to model the threads as "grooves" instead? Such a joint can't be assembled, but it can be analyzed in 2D, which significantly simplifies the analysis.
I did something of this sort, when this capability (combining large displacements, contact and plasticity) came in Creo Simulate some years ago (2011), while I was working for a PTC reseller. I made a presentation on Youtube, but that is all in Swedish, so it's not much help.But here is a screen shot from that presentation. You can see how the contact load declines as you move away from where the load is applied.
Where I sit now, I unfortunately don't have access to Creo/Creo Simulate, instead I'm stuck with SW and ANSYS.
Now, having access to ANSYS, this is a type of problem where Ansys is really more suitable, where you have a combination of two nonlinear phenomenae(large deformation and contact) , and where the nonlinear solver might have difficulties reaching convergence.
Why must this problem be run with large deformations? I don't see anything here that would require it. The bolt is only moving through a small fraction of a turn and the relative twisting/stretching of the shank and threads should be tiny in comparison to the rest of the model.
As far as the purpose of the simulation Bence looks to be specifically looking at the interaction between applied rotation/torque and stresses/load in the threads so a helix angle cannot be ignored. See previously that he has successfully run a pull simulation only (no rotation/torque - and including helix angle) and is looking to repeat the results with a rotation/torque simulation. See my earlier replies as well - I noted the reduced loading he should be expecting in the threads as they move away from the first thread in contact.
Look at the earlier post by Shaun, it looks like there may be an issue with meshing and interactions of the meshes between contacting surfaces. I'm interested to see where it goes - I had a hunch that may be the case.
Large displacement analysis will update the geometry and use the new geometry for the next time-step
If you don't use LD it will use the original shape for contact.
There may be a disconnect somewhere here - the exact wording Mats used was "large deformation" and deformation means to me strain/deformation which would be the "large strain" option which did not make sense to me as the strains should be rather small.
Of course the simulation should be run in large displacement - that really goes without saying. I guess I should have asked Mats to clarify what he meant - perhaps he can chime in.
Large displacement, yes that is the correct term... Large strain is not necessary.
yes i also tried to run with and also without large displacement / large deformations, with different solvers, increased convergence tolerance, different singularity elemination, iterative technique, different and same materials, but these pattern are always there.
I had not got too much time the last days to investigate more this problem but i have found a non-SW a reference:
The purpose of the analysis is to figure out that can SW handle this problem or not : ) Its not for a project/presentation or something like but, but i think good to know the possibilities of SW, because when we need something similar urgent simulation next time we will know the answer and dont need to waste the time to figure out that its not working.
Almost forgot my last test: supposed it can be similar as "buckling", so the calculation has difficulties with the perfect geometry when the two surfaces touch each other and made a model with two offset helixes, not too much, about 0,01 mm to the rotational axis, without initial contact. It was possible to see the light differences/loads between the sides but i think unnecessary to say also with the pattern...
I was able to run up to a torque of 100 ft.lbs without convergence trouble. I didn't try anything above that. Just using Intel Sparse with a half-cosine load increment with large alpha damping worked pretty well.
I started bumping into convergence problems when I began playing around with Nonlinear materials (Etan = 1/20*E), but perhaps I just need to increment the torque more slowly once it gets close to yield or use a slowly incremental stress-strain relation.
Are we sure the wavelet deformation isn't supposed to be present? I guess if you look carefully at the colors in the result I presented, it may be present on mine as well, but less pronounced. Maybe the wavelet deformation is similar to what you would get if you imagine trying to push a piece of paper through a small hole.
I was mulling over what you said about the wavelet deformation and I think you may be onto something. I did some light research but its difficult to find anything on this exact type of analysis - really a NAFEMS benchmark problem would be ideal but I don't have access to their membership only documentation and I don't know that they have one for thread analysis like this. If you are as interested in this as I am and want to do some research me know if you are able to pull anything up - I'm going to try and dig into this further as I am now very curious whether this is the expected response due to the deformation in the threads as torque is applied.