Surface contact

[ty313765]

Hello all,

I am attempting to simulate the stresses experienced in the treads of a bolt and nut. To do this I am running a static analysis in NX 8. I applied the surface to surface contacts in the simulation environment using the automatic pairing option, and fully constrained one end of the bolt. A force was applied to each of the six corners of the hex nut and I then ran the simulation. I used the iterative solver, as I have seen it recommended for tet meshes on this site.

After the simulation runs and I attempt to load the results I get a message that the results file is in the wrong format.

I then check the .f06 file for any fatal erros, I usually get:

NX USER FATAL MESSAGE 9137

or

*** SYSTEM FATAL MESSAGE 3000 (SITDELC)
ITERATIVE SOLUTION FAILED DUE TO FAILURE OF PRECONDITIONER TO FACTOR.
THIS ERROR CAN RESULT IF THE STRUCTURE IS NOT RESTRAINED SUFFICIENTLY TO PREVENT
RIGID BODY MOTION OR IF INTERNAL MECHANISMS EXIST.
1 * * * END OF JOB * * *



Also, I have allocated 2048MB to this simulation.

I have seen advice from another user to alter the input file adding the PARAM,BAILOUT,-1. Does anyone know how to do this, as well as how this would help?

Any help in resolving these issues would be greatly appreciated.

Thank you.

 

[BlasMolero]

Hello!,
If you try to simulate the "rotating motion" between nut & bolt, forget at all, this is Finite Element Method, not Multibody Dynamic Analysis. Also, please note you run Linear Static Analysis (SOL101) where small displacements are assumed. By the way, the behaviour of the fillets in a bolt is higly nonlinear, all nonlinearities exist: material, contact, large displacements, etc..

But let's suppose that "for fun" you want to study the "linear" contact between the treads of a bolt and nut. Also let's suppose that the applied load in the nut is in the axial direction of the bolt. The first thing you need is to constraint your model properly in order to arrive to a solution. The best method to stabilice your model is using symmetry boundary conditions. You can split both bolt & nut by the two longitudinal planes and study 1/4 of model (prescribing the proper symmetry constrants!!), this way the NUT will not "rotate" free at the very first instant of your analysis, this is the reason why you get error, the nut experience RIGID BODY MOTION, and a mechanism exist, then a SINGULAR MATRIX ERROR will appear.

Another option is to define FRICTION in the contact surface-to-surface propertye, then you can study the full model, but this will add complexity to contact convergence.

"PARAM,BAILOUT,-1" makes to get a solution, but this is only for debugging errors, NEVER USE IT FOR PRODUCTION MODELS!!, only to see the animation of deformed shape, you can get displacement resuls of meters, useless at all.

To learn more about the use of BAILOUT with NX NASTRAN visit my blog:

http://iberisa.wordpress.com/2011/0...run-terminated-due-to-excessive-pivot-ratios/

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[ty313765]

Thank you for your response Blas!

I am not trying to simulate the rotating motion between the nut and bolt, only trying to see what stresses build up in the corresponding threads. Since I was having so much trouble getting the simulation to completely run using the entire threaded areas, I decided to use only the face of one thread. The simulation ran successfully, and now I plan on trying it using the entire threaded area.

I'll let you know how it goes!