Well, we are not magicians!. You don't post the full error found on F06 file, neither the analysis type performed, the FEMAP version used, etc.. The direct way is to post your FEMAP model here and we will take a look to it. If not possible, then at least post your *.f06 & *.log files.
Well, first at all: you have a problem with units, you have imported your CAD geometry in milimeters (mm, ie, using internally a geometry scale factor =1000) but the material properties are read from material library MATERIAL.ESP that are in inches, then results are useless, check your FEMAP setup using FILE > PREFERENCES > LIBRARY/STARTUP (or better take a look to my site at IBERISA.com to learn how to define preferences in FEMAP http://www.iberisa.com/soporte/femap/femap_tips_tricks_preferencias.htm)
Next, your model is simply unconnected: you have two bodies, meshed each other with TET10 elements, but nodes are not merged between both parts, then you have a problem of rigid body motion. If you read your F06 file you will see the following error:
^^^ USER FATAL MESSAGE 9137 (SEKRRS) ^^^ RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL. ^^^ USER ACTION: CONSTRAIN MECHANISMS WITH SPCI OR SUPORTI ENTRIES OR SPECIFY PARAM,BAILOUT,-1 TO ^^^ CONTINUE THE RUN WITH MECHANISMS.
In fact, if I run a Normal Modes/Eigenvalue analysis (SOL103) is see the following rigid body motion denoting the modeling error previously commented, OK?.
Take a look to this post in my BLOG to learn more about how to detect rigid body motions in your FEMAP model: https://iberisa.wordpress.com/2011/02/20/mensaje-de-error-de-nx-nastran-run-terminated-due-to-excess...
Thanks for solving,
I looked at the website, but i dont understand spanish :-)
how can i set PARAM,BAILOUT,-1
this two bodies have to Glide => The Platte above must glide in to the other to spread them. Is this Possible with femap?
Yes, we can!!. You should stabilize your model in the lateral direction (plane X-Z) using double symmetry, and in vertical direction (Axis Y) you can use surface-to-.surface contact between the surfaces of bot parts (By the way, again I strongly suggest to mesh with HEXAHEDRAL elements when the geometry allows, and better -when dealing with contacts- use HEX20 elements!!)
Yes, but please note according your video you have large displacements, then your problem should be solved as nonlinear using Advanced NonLinear Module (SOL601) because Basic NonLinear Module (SOL106) do not support surface-to-surface contact.
You can try linear static contact using the NX NASTRAN solver (SOL101), but if you have displacements equal or larger than the plate thickness then your problem is nonlinear for the geometry, then to account for large displacement effect you should run the problem as nonlinear, OK?. If not, you will have simply colors ...
Compare both linear & nonlinear solutions, then you will be able to arrive to reliable & accurate results.
Thank you Cfyrr
I have the instructions step by step followed, but I get further 2 Fatal Errors.
I can not make the assozivität.
I've readed the F06 log and it says Nastran have crashed: