I want to know which are the main differences between this NX Nastran non-linear solutions SOL601 and SOL701.
For example, I want to run two cases with plastic materials curves one for Steel and other for Cast Iron, the case has plastic behavior. If the model has glue contacts and pre-tensions bolts which SOL must I have to use?
Solved! Go to Solution.
the core difference is the integration schemes for these solutions. sol601 (106 or 129) is an implicit solver, sol701 is an explicit one. So their nature causes differences in applications, parametres etc etc.
For plastic strains anaysis you may use sol 601,106 or sol106.
There are many, many key differences between SOL601/701 solvers, I suggest to read carefully chapter 1.2.1 of the Advanced Nonlinear User Guide. As an add-on one important note is that higher order 3-D solid elements such as CTETRA 10-node tetrahederal, 20 and 27 node CHEXA brick elements are only available in implicit analysis SOL601, not supported by SOL701. They are not used in explicit analysis because no suitable mass-lumping technique is available for these elements.
In my opinion the decision is clear: SOL701 is only for explicit nonlinear high-speed dynamic analysis like crash analysis or metalforming analysis wave propagating problems, the rest of nonlinear problems can be solved perfectly with implicit SOL601 (both 101 & 129).
Since Advanced Nonlinear module handles both Solution 601 and Solution 701 with very similar inputs, the user can in many cases restart from one analysis type to the other. This capability can be used, for example, to perform implicit springback analysis following an explicit metal forming simulation, or to perform an explicit analysis following the implicit application of a gravity load.
It can also be used to overcome certain convergence difficulties in implicit analyses. A restart from the last converged implicit solution to explicit can be performed, then, once that stage is passed, another restart from explicit to implicit can be performed to proceed with the rest of the solution.
I am planning on simulating a compression bending forming of an aluminium profile. I know that Abaqus might be suited for this task, but seeing as I have little or no experience in Abaqus I would prefer to use Nx Nastran for the task.
The reason for the need of simulation here is that we are having difficulties with some defects. I would like to recreate these defects in an FEA. Then I would use this setup to change geometries, parameters or add inlays to try and prevent unwanted deformations without having to conduct expensive experiments.
Which solver would you think best suited for this task?
Start with 701 Explicit followed by 601 implicit springback? This forming process is rather slow and I would not call it a high-speed dynamic analysis. Is 701 still good?
hoping for a good answer here. I find little information on the world wide web.
Explicit solvers (i.e. 701) have a minimum stable time step, typically on the order of 1e-6 seconds or smaller. For large models, events lasting a second or longer can require a prohibitive number of time steps.
If the analysis is truly "slow" (several second duration) and dynamic effects are negligible, a static analysis (SOL 601, 106) could be sufficient.