Cancel
Showing results for 
Search instead for 
Did you mean: 

Fatal Error

Creator
Creator

Hi,

 

I cant simulate this:test

i've tried it 5 times, but it dont work.

Every time i get a fatal Error.

Unbenannt.png

Has someone a Idea how to solve it?

 

Greez Anti

18 REPLIES

Re: Fatal Error

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Greez,

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.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: Fatal Error

Creator
Creator

thanks for help

 

i use 11.2.1

i packed every file on the zip (modfem-log-f06...)

http://www.file-upload.net/download-10852522/sim.zip.html

i tryed the standard analysis

 

Mfg Anti27

 

Re: Fatal Error

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Anti27,

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.   

 

 

 

nodes-dosnt-match.png

 

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?.

 

rigid-body-mode1-animated.gif

 

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...

 

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: Fatal Error

Creator
Creator

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?

(view in My Videos)

 

Mfg Anti27

Re: Fatal Error

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Anti27,

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.

 

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: Fatal Error

Creator
Creator

Moin,

 

I've tryed it 40 times, i dont understand how this work...Smiley Frustrated

Can you try it for me, so i can see how it schould work? Smiley Very Happy

 

Mfg Anti

Re: Fatal Error

Valued Contributor
Valued Contributor

Re: Fatal Error

Creator
Creator

Thank you Cfyrr Smiley HappyMan Happy

 

I have the instructions step by step followed, but I get further 2 Fatal Errors.

I can not make the assozivität.

I could not colorize the model Smiley Surprised
I'm a little bit confused

 

 

http://workupload.com/file/8LySdddQ

 

I've readed the F06 log and it says Nastran have crashed:

http://workupload.com/archive/OP9W9Ijy

 

 

Can I have your file to see if it's on the PC or on the model ?

 

Mfg Anti

Re: Fatal Error

Valued Contributor
Valued Contributor

 

Correct contact properties

 

Nl.PNG