The test problem of cantilever beams of contact which ran successfully in SOL 101, showed deflection of magnitude way in to nonlinear range...so decided to familiarize myself with SOL 601 process of running a contact analysis. I went through Femap examples as well as several other threads to make sure I've entered inputs as correctly as possible. Trouble is, SOL 601 just quits running way early in to the analysis. I don't think it even enters in to substepping of loads phase.
I am posting pics of my various settings. May be I've missed something.
I also tried running with Largest Step Multiplier set to 1, but did not run.
*** ISHELL PROGRAM 'NXNA' STARTED *** *** ADVANCED NONLINEAR ANALYSIS *** *** START SOL 601 *** *** TEMPORARY FILES tmpadvnlin.* WILL BE CREATED DURING ANALYSIS RUN *** *** PROCESS NASTRAN DATA *** *** MAXIMUM MEMORY FOR PROCESSING NASTRAN DATA = 2748 MB *** *** ADNAST (03/26/15 15:37) *** *** Reading Nastran data ... *** New internal database created. ***ERROR: Discontinuity is not allowed in TABLED2 1. *** Allocating 2748 MB of memory ... *** FATAL ERROR: PROCESSING OF NASTRAN DATA FOR SOL 601 FAILED. *** ADVANCED NONLINEAR EXIT CODE 0 *** *** ISHELL PROGRAM 'NXNA' COMPLETED *** ^^^ USER FATAL MESSAGE ^^^ ERROR IN ADVANCED NONLINEAR MODULE 0 ^^^SOL601 FAILED
The above message is cryptic and gives little info as what went wrong.
I was able to run other SOL 601 contact analysis, including the Femap supplied example and one more SOL 601 contact analysis, which is posted on this forum.
The error, "***ERROR: Discontinuity is not allowed in TABLED2 1" indicates a problem with a function.
Are these beams modeled with shells or beams? When you use shells, I recommend the following settings for the connection property.
Thanks folks for replying.
I tried redefining the function as well as incorporating changes that ChipFrikle has suggested. The analysis ran!!!
Appreciate the help.
This is more of a general nonlinear FE question rather than specific to FEMAP.
For SOL 106, 601 etc., to take advantage of nonlinear conditions accurately, it is necessary to define beyond yield properties of the material (Al 2024)? (either via Stress-Strain curve or by bilinear rule etc)
Cause in the above problem, I am getting barely noticible differences (< 1%) between the linear & nonlinear analyses (particularly in deflection output numbers). Although my experience will nonlinear is very limited, in other simple cases I've worked with, I have noticed significant differences.
For ex: I was trying a long cantilever beam subjected to tip load and I get significant differences between the tip deflections b/w Sol 101 & 106/601. But in that problem, I did not remember defining nonlinear property for the material (Al 2024).
ChipFrikle, I have modeled the plates using shell elements. Also, can you please provide insights on why you recommend particular Contact Property settings for shells?
In order to evaluate material nonlinearity, you need to define the stress/strain curve beyond the yield limit, otherwise, the Advanced Nonlinear Solver will assume E as the slope of the stress/vs strain curve.
The option for Double-sided Contact will test for penetration between time steps. If the time step is too large, contact may not be detected if this option is not turned on.
Offset Type option setting for Half Shell Thickness will check for contact at the top/bottom of the shell element instead of the normal mid-plane. This is assuming that you've meshed at the mid-surface of the shell.
There is more information in the Advanced Nonlinear Theory and Modeling Guide found under the Help > NX Nastran command in Femap.