Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-20-2015 03:03 AM - edited 08-20-2015 03:40 AM

Hi,

I cant simulate this:

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

Every time i get a fatal Error.

Has someone a Idea how to solve it?

Greez Anti

Solved! Go to Solution.

18 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-20-2015 03:51 AM

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/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-20-2015 04:42 AM

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

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-20-2015 08:08 AM

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.

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...

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/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-20-2015 08:22 AM - edited 08-20-2015 08:40 AM

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?

Mfg Anti27

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-20-2015 12:42 PM

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/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-21-2015 04:08 AM

Moin,

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

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

Mfg Anti

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-21-2015 11:38 PM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-24-2015 04:10 AM - edited 08-24-2015 04:19 AM

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 could not colorize the model

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

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

08-24-2015 02:37 PM

Correct contact properties

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc