did you try raising the convergence tolerance as requested?
what is your long term goal with this? I think there is a very similar example in the afnor guide or the verification problems
to note, what you're trying to do is the most challenging analysis you can do with nonlinear and will require some "effort" with the solver parameters. generally I have had to get guidance from the developers.
Jared, thank you for your comments. I have certainly tried to increase the convergence tolerance as requested (I experimented between 0.2 and 0.0001), the same result appeared (a sudden error just after start of simulation).
However, I have successfully managed to run the simulation with a little spline swing in the middle of the stick (an eccentricity of 3 mm). On the left is a sweep trajectory, on the right - simulation parameters, on the bottom - simulation results.
I guess that straight beam cannot be calculated in non linear buckling case because of the assumptions of the software. I think the solver tries to compress the stick in ideal manner, so the eccentricity does not even appear, which would make the stick to buckle. Where as in real life situations, the material integrity, the shape of the stick and the direction of the force would never be ideal, this way creating buckling.
Trying different cases of this simulation, I came to a few more questions:
1. This simulation runs perfectly with Newton Raphson iterative technique, but doesn't work at all with Modified NR. Reading about that in the help:
is giving me an opinion, that different iterations should give different solution time, and possibly a slightly different accuracy. But why NR works, and MNR fails completely? Where could I find more information on using these iteration choices in other cases?
2. Simulating this stick (with a swing on the middle) with NR iteration and all three different integration options (Newmark, Wilson Theta and Central Difference) gives the same results and takes the same time to solve. The help on this topic is almost empty. Where could I find more information of these integration techniques?
3. Having the same model of the same stick, I run the nonlinear simulation with "Force" control, and "Arc length" control. Applying 10 kg on the top of the stick, the results are next: with a force control, I get almost no deflection, and maximum 2 MPa stress (yes, two megapascals). While using the Arc-length, the simulation makes the stick to buckle completely (as in the image above), reaching hundreds of MPa of stress. The load, fixtures, mesh are the same. I made a static analysis to check - it gives 2 MPa of maximum stress, identically as Nonlinear with force control. So I guess I am setting up the Arc-length study incorrectly. As the loads and the fixtures are the same, and the Simulation parameters are visible in the screenshots below, maybe I could be advised of the source of the mistake in Arc length study?
I would be happy to purchase a book on amazon or somewhere, which would cover these topics. But I am afraid to get the literature duplicating basics of Simulation, and not covering deeper topics like these. If something could be recommended with a good feedback, I would be grateful for the advice.
I think you have a misunderstanding of the theory.
Non-linear simulation won't give you a bucking shape from a straight rod with any settings you may have there.
You have the answer right there in the error message : "The solution may be at a buckling or a limit point..."
Non-linear simulation will always stop at critical load, because the solution after the critical load is not real anymore, it is a complex solution and needs eigenvalues and eigenvectors solving (F=(A-lambda*I)*u) which is totally different than what non-linear simulation is using (F=K*x).
For finding the buckling shape and the critical load you need to do a a buckling study, which will give you approximately the same value of the critical force (the last value of force when the non-linear simulation stoped).
After you have found the buckling shape (which is the first eigenvector) you may continue to load the new shape as you have done already with the excentric rod, but in this case non-linear simulation can continue solving because now with the new shape the dominant load is bending instead a pure compression load.
The snap-through happens only in a bridge/ arc loading or a road already buckled with a transversal load, so it will not apply here in your situation:
Andrei, thank you for the explanation. Now I understand how this type of a problem should be solved, appreciate your detailed answer.
In addition, I would still be happy to receive recommendations on information source for explanation/usage of options in advanced simulation parameters: iterative technique, integration methods, correct usage of arc length method, and other advanced options
You're welcome Ben. I think all you need to know is already in help:
you have at the bottom of this help page a link towards Knowledge Base with more details.
also this article:
As I said, arc length control does not help you at all because does not apply to your problem.
And nothing would change with any integration method you choose, the solution would converge to the same value.
I would use incremental load control and I would ramp up the applied load from 0 to 1 sec, 0 to 100 N.
in your solution time you have there time increments of 0.1 with 5 adjustments, I will explain what this means.
it means that the solver will step up the time by 0.1 which is 10 N increment at each iteration.
if the solver stops at time 0.14 (14%) that means your critical load is about 14 N.
so the solver will solve the first iteration at 0.1 then it will proceed to solve the second at 0.2 (load at 20 N) but at that load the problem is already in the unstable domain and the solution is complex and the solver would not converge. in this case the solver will halve the time step once, so that the next iteration to calculate would be 0.1+0.05 but the load would be 15 N and the solution again is complex and would not converge and the solver would halve again the interval second time.
Next iteration would be adjusted to 0.1 + 0.025 = 0.125 at which time you have 12.5 N and the solution is in the real domain because is lower than the critical load.
Next iteration would be 0.125 + 0.025 = 0.150 and again the force would be 15 N beyond the critical load and the interval would be halved once so the next iteration time would be 0.125 + 0.0125 = 0.1375 which means the load would be 13.75 N.
At the next iteration the load would increment again above the critical load and again the time increment would need to be halved until the solution is below the critical load, and so on, you can have 5 halvings of the time interval and if after 5 halvings the solution does not converge, this means that the last time the solution was found was for the last load just before the critical load.
To find the critical load more accurately you can run again the simulation with a ramp between 0 to 1 sec, 0 to 15 N, so this time the solver will stop at about 93 % and you may find the critical load with a precision of 1.5 N/2^5 = 0.05 N.
If you run a buckling study you may find the same critical load value as the first eigenvalue.
you can use the incremental displacement method too, but in this case instead of defining an initial load, you have to define an initial ramp of displacement in a point let's say between 0 to 1 sec, 0 to 1 mm. The solver will increment the displacements just as described above and will stop just before the critical load is reached. To find the value of the critical load you have to pick the reaction force value in the point you applied the displacement from the solution found at the last iteration.
Andrei, thank you again for the very detailed answer, it has certainly appended my knowledge. The link to the arc-length thread in the forum was also useful.
One more basic question about arc-length method: lets say I am not sure if my simulation will reach a point where force/displacement slope is zero, that it where force or displacement calculation would fail. For this reason I would use arc-length control method. But if a calculation appears to fit around yield's stresses, then all three control methods should give similar results. This is almost the same question as the third from my previous post: 5 kg load is applied to the end face of the stick in perpendicular direction, the other end of the stick is fixed. Force and arc-length control gives very different results:
Arc length control gives error at around 63% (about buckling), but this is how it looks at that point (true scale plots ):
As you may see, the maximum stress is 4571 MPa, maximum displacement is 122 mm
But using force control :
Max stress is 142 MPa, max displacement is 67 mm
This being a very different results, how should they be understood?
I think the results should be and are the same either you use Force control or Arc length control method, although the control parameters are different. First of all the start time and end time are not used by the arc length control, so you cannot compare the maximum values because they are different. In the force control the maximum value would be 50 N when the end time is 1s while in the arc control method I see in the menu that you can set the maximum displacement for translation DOF 100 mm which means the method would stop when the max displacement value is reached. So the maximum values would be different, but to compare the methods you should compare the solutions (Stress and Load Force values) for the same displacements. Take the values from 10 mm displacements and compare them, are they the same?
I never used arc length method until now, so I am curious about this comparison. And I don't know what maximum load-pattern multiplier is, probably means that the initial load of 5 kg would be multiplied by this maximum number to reach the maximum displacement, if one of them is reached first, the simulation stops. So arc length control method continues to find solutions way beyond the force control is capable to do.
the fidelity of the screenshots makes it hard to see where you are reading the information
are you looking at the max displacement at the tip and the max stress at the fixture? likely a location for a stress concentration?
and to summarize the issue, without any buckling, your expectation is that all 3 control methods will have the exact same answer when the exact same load magnitude is applied but you aren't seeing that?
most of this is in the sim premium training, the cosmos manuals (in the solidworks kb) and the solidworks kb
as mentioned, most of your questions are covered in the simulation premium training, the cosmos documentation and the solidworks kb.
and regarding a lot of your indepth questions about what options to choose...etc. arc length is the way to go for nonlinear buckling and the rest of the options are basically used to work through convergence issues. when one doesn't work, go with the other...etc. there are no hard set guidelines.
and the solution you found about adding assymmetry is one of the recommendations in the solidworks kb