The linear solver is much more forgiving to certain issues. You need to make sure nothing can move in unintended directions, like the bolts for instance. Friction is often handy in stabilizing things even though it can make certain analysis more challenging. Symmetry can be really handy also. Does it fail in the first step? Does it fail in a subsequent step. Hard to help when you don't say much about what went wrong.
Bill - I apologize for the vagueness in my initial question, I was really just trying to see if anyone had some guidelines for how to model a nonlinear bolted connection effectively without using the build in "bolt connectors" in solidworks as the stress directly under the head is important and because of the rigid link/spider elements that type of connector uses from what I understand and have seen in past simulations the stresses within ~1x diameter around the bolt head/nut are not accurate.
I have done some additional modeling of this simplified system and what I have found is that the nonlinear analysis is extremely sensitive to (a) how the contact sets are defined (b) mesh size and (c) transitions between contact areas (ie: sharp corners vs. small radii vs. larger radii). I would really like to model this with an actual 3D solid model of a bolt with no-penetration contact however my solution times seem to just exponentially explode - a simple nonlinear model (using nonlinear solver only - NO nonlinear material properties and NO nonlinear geometric conditions) with two plates and a fully modeled 3D bolt/nut clamping them together took somewhere between 2-3 hours to solve. My final goal is to have several more fasteners and adding 2 more nonlinear "plate" elements (a rubber gasket and plastic sheet both with non-linear material properties) in the final model and I just don't see how that is possible without the solve time becoming unreasonable. I was hoping that someone might have some experience/tips on how to make this goal attainable. Note I am not concerned with the stresses in the bolts themselves so they could be rigid or flexible/deformable.
Below is the simplified model I am trying to prove out the concept with.
Below is an example of a linear analysis I was able to achieve with decent results on the final assembly model. This is what I would like to achieve with the nonlinear solver so I can properly evaluate it with nonlinear material properties for the rubber and plastic components. I was unable to get the nonlinear solver to evaluate this model successfully even with only linear material properties.
Here are some thoughts:
part of the problem maybe be the defaults in the NL solver. the initial step size is 1%. So under optimal conditions it will need 7 steps to apply the pre load. Depending on how non linear things are or aren't a larger initial step size may lead to a much faster solve time. I would try 1 on your "figure it out model". Further, I would add the pre-load as a delta T to get the bolt tension. I would use a friction coefficient of .25, and surface to surface contact on all contact sets. I would use all linear materials. I would start with draft elements. I would try a coarse mesh - which would still decently refined around the key contact areas. I would use a quarter symmetry model with a single fastener And ensure the only restraint are the 3 symmetry planes, 2 of which go through the cl of the fastener axis. Get that to work. Then get the non draft elements to work. Then refine to get a decent stress solution you like. Then add the NL materials. Once u have that construct your real model and repeat the solve sequence or modify to suit your confindence on what worked previously.
changing the restraint system to something less ideal on the "real" problem maybe where your real challenges may arise so make sure you get that to at least solve first. And then u can complicate as required. Also, a contact solution has much reduced "noise" with a fine mesh - ie the normal pressure distribution gets much smoother as the element count goes up. A smooth distribution in my humble opinion is indicative of a good contact solution. If you want the Hertzian contact stress distribution to be reasonable you will a very fine mesh at all contact hot spots.
Thank you so much for your input - I had no idea about the draft elements, I think that will definitely aid in creating a workable solution as it will really show whether or not I am converging toward a solution as usually i can tell if the simulation will work or not however sometimes its hard to tell if it will take 3 hours or 30 hours! That should be first on the list of every "troubleshooting" page and your response was the first I had heard about that - thank you!! I will definitely play around with the step size, however in the limited fiddling I have done thus far it sometimes means the solution will not converge as the initial load application is too high.
Also do you have any recommendations for the setup/properties tab? I've heard of changing from the "simplified" to "more accurate" solver to get the model to solve? The main change I made there some time ago was to use the direct solver as from what I have read and experienced it handles no penetration contact much, much better than the iterative solver.
I've seen some recommendations to simulate preload with a temperature delta however I'll have to do some research into that - I can't imagine the hertzian contact for that is anywhere near accurate? Would just using a spider/rigid link in the built-in "bolt connector" be a better start or is there another advantage to using the temperature differential method? Speaking of which on a related note - I asked a question about custom spider/rigid link connectors (Custom Spider Connectors / Rigid Links - are they possible in Solidworks Simulation? ) - do you know if its possible to create custom connectors of this type in solidworks?
Thanks for all your help, I was really stuck there for a while but your advice is starting to help me get unstuck!
Please disregard my note about spider/rigid links - I have found the capability under connectors, it was right underneath my nose. I am having a little difficulty getting them to work properly but I'm sure thats something I can figure out (despite the fact that there doesn't seem to be a whole lot of documentation on the topic.....)