Hi,
This article does a fair job of describing the relationship between the event simulation runtime and the input. See "This Event Simulation model will exceed the allocated Tech Preview run time limit of 12 hours" in F.... Here are some of my thoughts (and clarifications) on how to reduce the runtime.
- The time step size is fixed by the equations used to solve the analysis. You cannot make the time step size larger to reduce the runtime. (At least you cannot change the time step size directly.) To get to a certain event duration requires X steps, where X = the duration/time steps size. X number of steps require a specific time to solve, and that is how the software predicts if the total time will be greater than 12 hours. Therefore, you can only reduce the duration of the event to reduce the runtime. For example, if simulating a drop-test, move the model close to the floor. There is no need to simulate the 6 foot (2 meter) drop. For example, if applying a force or enforced motion, apply the load over 0.01 seconds instead of 1 second. (This changes the kinetic energy, but the kinetic energy may be small compared to the total energy depending on the analysis. In other words, the speed of applying the load may not have a drastic effect in some models.)
- The number of steps that you specify under the Setup is the number of results that are saved. The analysis will still calculate X steps, but only save the number that you specify. I suspect there is a small difference between saving 10 steps versus 100 steps when it comes to the total runtime.
- Do not use the quasi-static (no inertia) if trying to reduce the runtime. The quasi-static does the same analysis as the dynamic, but it changes the total duration to minimize the kinetic energy. Therefore, the quasi-static analysis may run the analysis 2, 3, or 4 times, with longer durations for each cycle.
- Increase the smallest mesh size. The time step size of the analysis as fixed by the solver is related to the smallest element in the mesh. If you can eliminate fillets and rounded corners, or adjust the mesh on those features so that they are the same size as the rest of the model, then the analysis time step size will be larger.
Although those factors will reduce the runtime, they do not improve the accuracy. It does not change the limitation that 1 solid element through the thickness of a thin wall is not enough to capture the stress gradient from the inside to the outside (especially in the buckling example where the bending is about multiple axes).
The better solution is to use Inventor Nastran (version 2021) where you can use shell elements to perform the analysis.
John Holtz, P.E. Global Product Support
Autodesk, Inc. If not provided, indicate the version of Inventor Nastran you are using.If the issue is related to a model, attach the model! See What files to provide when the model is needed.
