I have to calculate some knuckle-boom crane and first time meet some problem with this.
knuckle boom = two hydraulic cylinders that I model witha beam with pin flag in DOF5 which gives me hinges at the ends of cylinders.
Anyway I got message about excessive pivot ratios, so I put the Bailout = -1, and it seems that all is ok with a model.
Total displacement (for 20 m-long crane) is about 30 mm (not loaded, only gravity), as it was expected, so my question is how, except the epsilon value, can I evalate numerical corectness of the solution?
Epsilon with value -6.4252664E-10 I assume to be correct.
The stress (for bailout =-1) are also fine, so Is it always like that that we shouldn't relay on results obtained when bailout is switched to -1 ?
Solved! Go to Solution.
PARAM,BAILOUT,-1 should be used for debugging the FE model ONLY, but not for final results, then I strongly suggest to prepare your FE model correctly. You have a rigid body motion, and this is the reason of the error. To detect where is the problem located the trick is to run a normal modes analysis (SOL103), animating the modes with 0 Hz will show you the singularities found in your model.
To learn more please visit my BLOG in the following address:
Thank you Blas for that tip. Really helpful.
What are my feeligns about that. It was not a first time when I tried to do similar simulaiton, so I was quite suprised that the simulation didn't pass without this "bailout" entry.
When I run SOL103, the output was clear. There was no 'internal' rigid body motion. First modal mode was for about 2 Hz-2.5 Hz and related to all the structure.
The problem was related only to the one mesh, which didn't pass the solution. When I went to f06 file all the grid nodes were in one mesh. I do not know why, but this problem appears only dor Quad8 (and Tria6) elements. Never meet it for first order elements. Indeed for some areas the second order elements are not necessary like it was for those areas, but still, it is sometimes hard to find out what is happening.
Summing up, there was no problems with mechanisms in general, due to freeing some degrees of freedom for cylinders of the crane, it is more a problem with a midnodes (?).
Did you meet similar problems before ?
PS. when it comes to the results, there was almost no difference between results for analysis with and without 'bailout = -1' entry.
Thanks for help
Then the problem is related with the use of high-order CQUAD8 elements. In fact, the use of Parabolic 8-nodes Shell elements is only recommended for nonlinear analysis, I do not use at all in linear static analysis.
In fact, in the past I remember to have similar problems, the only remedy was to use PARAM,MAXRATIO,XX increasing slowly its default value 1E7.
But actually with NX NASTRAN V11.0 release I note that the current solver is much more robust, then not need to take the "dangerous temptation" of using either BAILOUT or MAXRATIO, OK?.
Dear Blas, dear Tomek,
I have those problems with parabolic shell elements, too. But I can't bring myself to use linear shell elements because of the quality of linear SOLID elements.
What's the way to combine linear shell elements with parabolic solid elements in NX Advanced simulation?
Best wishes, Michael
Production: NX10; Development: VB, TCL/TK, FORTRAN; Testing: NX11
Kudos for good posts! And if you find my post helpful, and it answers your question, please mark it as an "Accepted Solution"