I am attempting to simulate a leaf-spring which undergoes two stages of deflection.
The spring is deflected by a plane with an enforced displacement and contact constraints applied between the plane and the appropriate surfaces of the spring. After a certian range of deflection, the rear surface of the spring is intended to contact a second plane which limits the deflection of one of the members of the leaf spring, while allowing the other to continue deflection.
I have applied two sets of contact constraints in the simulation. The first is between the moving plane and the "front" surfaces of the leaf-spring. The second set of contact constraints is between the stationary plane and the "rear" surfaces of the leaf-spring. When I run the simulation, the software recognizes the first set of contact constraints and the spring deflects in response to the moving plane as expected. However, the software does not seem to recognize the second set of contact constraints and rather than the leaf-spring becoming constrained by the stationary plane, the spring continues deflecting through the surface (I've included an animation of the deflection shape at the end of this post for clarity).
Is the software only able to recognize one instance of surface contact per simulation, or is there perhaps something else that I'm overlooking? Perhaps a linear static simulation isn't even the appropriate module for use in this type of analysis. If there is a better package/process for simulating this type of leaf-spring I'd greatly appreciate any direction regarding how I might go about simulating this properly.
Thanks in advance!
You may be able to get some type of results from a linear static analysis if the source region for each contact pair is the plane and the search distance is large enough in the second pair that the contact elements are created at the beginning of the solution.
However, due to the large deformations, this analyis should really be done using a geometric nonlinear (large displacement) solution such as SOL 401 or SOL 601.
I appreciate the response. Your comment regarding the contact search region makes sense, as I believe I had left the search distance at the default value of 0 - 1mm for the rear surface contact constraint while the gap between those objects is more like 1.5mm. I will try increasing the search range to see if the solver picks up the contact in that region.
Also, I completely agree that this problem is more well suited to the 601 solver, however I don't think my company currently has a license for that functionality. In the event that I can get the simulation to run in 101 and my results are outlandish, I'll talk to the higher-ups to see about getting a license for 601 since I believe we'll be wanting to perform more, similar, simulations in the future.
Thanks agian, and I'll follow up regarding whether or not increasing the search distance worked.
I assume that you use SOL101.
1. Keep in mind that in SOL101 the results and therefore animation, too, only represent the final state of deformation and stresses. You can't have both touching points one after another in SOL101 and therefore, interpretation of that is really misleading as SOL101 is not made for that analysis problem.
2. Keep in mind that in SOL101 the directions of intersection and contact forces are not modified during solution, therefore, the bending of spring and the sliding of and large movements of touching point are poorly introduced.
I believe, your problem is too complex for simple contact.
Best wishes, Michael
SOL601 is also for dynamic analyses. The difference of 601 and 701 is that SOL601-129 is an implicit dynamic solver and SOL701 is explicit or direct solver.
Additionally, SOL601-109 is an implicit static solver (which can use quasi dynamic methods to get better convergence and more robust solutions).
Both are usable for highly complex and non-linear behavior. Both are not basic NASTRAN but a development of Klaus-Jürgen Bathe and his fellows and in the basics from ADINA: https://en.wikipedia.org/wiki/ADINA
Therefore, the modeling assumptions are a little bit different and other elements are available, too. And,THE BIG BOOK TO KNOW is
Finite Element Procedures, 2nd ed., Cambridge, MA, Klaus-Jürgen Bathe, 2014
See in version 10 : advanced_nonlinear_tmg
I believe your problem is not involved in high velocities and if you don't want to get mass inertia forces you don't have to use SOL601-129 or SOL701 but SOL601-106. There are a lot of switches and different opportunities to get lost in. But that doesn't mean that it makes work easier, oh no.
Best wishes, Michael
PS: SOL106 itself is also non-linear but can't work with contact.