Hello,

I have a model of a large structure consisting of ~800 surface bodies and a few springs. The surfaces all mate up nicely and I have created split lines where bodies meet up. Contact is set to bonded global. It meshes with shells perfectly, matching nodes across all the joints, and has about 130k nodes in total.

When I run a linear static analysis it meshes in 49sec and solves in 45sec. All the contacts/loads/restraints are applied correctly and the stresses/defections are what I would expect both.

I would like to run a nonlinear static analysis on the structure to determine when it starts to buckle. To do this I ramp up a small load from t=0-0.1s to set the initial condition that will allow the onset of buckling. Then I apply an increasing load from t=0.1-1s. When the analysis runs it typically jumps to very small time steps (0.01s and less) initially, and takes 5-6 hours to solve each, reaching roughly t=0.03s over a period of 15+ hours. Looking at the linear static solution for the t=0.1s loads, the deflections are small and the stresses only ~10% of yield so its certainly not in a highly nonlinear area.

I have gotten previous (and slightly simpler geometry) versions of this model to solve, taking 8-12hrs to reach t=1 in ~17 time steps. This still seems like a very long time considering each static mesh+solve cycle is <2min on its own.

What could be causing this behavior?

I am running Solidworks Simulation Premium 2013 x64 SP4.0 w/32GB ram.

Thanks!

Post buckling can be tricky and the fact that is solves in linear is not something that should provide a lot of faith in being menaingful. Consider that you have a strucutre that has, as it is loaded, a small insifginifcant peice of strucutre that buckles at almost no load but does not really compromise the integrity of the structure as a whole - some little bracket some where trips at a small fraction of the over all structures capacity. This can cause your solution to hit the ditch lickety split. Displacement and arc length controls allow you to avoid the solution stoping at some inflection such as this, the reasons for which you can do some research on. Now notwithstanding what Gerry (post edit: sorry I meant Shaun and not Jerry - sorry about the sp as well) said, in SWX sim you can not apply a fixed displacement as a load in a displacement controlled solution - you need to apply a force. What happens is the the solution process sort of gets reversed. In the displacement control dialog you need to pick a node - a vertex in SWX Sim - and a single degree of freedom - displacement in the direction your are concerned about or mroe loosely the direction the load is applied in. Pick a spot whose deflection and direction would be meaninful in assessinghte buckling response of the structure. Then you need to specify how far this DOF needs to go to resolve (buckle in your case). then what happens is the solver advanced the dof and calculate the load required to get it to whatever increment it is attempting and converge the force to achieve the displacment. This avoids ttying to iterate to convergence onto a peak of hte force dispalcement trajectory where the force tangent has a slope of zero. Force control will always have some difficulty overcoming buckling if the force slope goes to zero.