turn on suggestions

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

- Siemens PLM Community
- Simcenter
- CAE Simulation - NX Nastran Forum
- Re: USER FATAL MESSAGE 4676 (NMEPS)

Options

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

Not applicable

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

07-09-2009 06:00 AM

Hi,

i am actually performing a non linear analysis on an assembly with contact using

gap elements using NX Nastran V6.1

my solution converges at a 0.3 load factor and then issue a fatal error message

*** USER FATAL MESSAGE 4676 (NMEPS)

ERROR EXCEEDS 90.00

PERCENT OF YIELD STRESS IN ELEMENT ID= 52191

^^^ USER INFORMATION MESSAGE 9005 (NLSTATIC)

how can i oblige NX Nastran to ignore the error on the yield function so that it

completes the analysis?

NB : i did a static linear analysis and the stresses were unreasonably high so i

wanted to perform a non linear analysis to get a better ensight on the level of

stress on the same area.

So how can i oblige NX Nastran to ignore the error on the yield function so that

it completes the analysis?

Many thanks,

Engrequest

5 REPLIES

Highlighted
#
##### Re: USER FATAL MESSAGE 4676 (NMEPS)

"lamyaa tahlil" wrote:

>

>Hi,

>i am actually performing a non linear analysis on an assembly with contact

>using

>gap elements using NX Nastran V6.1

>my solution converges at a 0.3 load factor and then issue a fatal error message

>

>*** USER FATAL MESSAGE 4676 (NMEPS)

> ERROR EXCEEDS 90.00

> PERCENT OF YIELD STRESS IN ELEMENT ID= 52191

> ^^^ USER INFORMATION MESSAGE 9005 (NLSTATIC)

>

>how can i oblige NX Nastran to ignore the error on the yield function so that

>it

>completes the analysis?

>

>NB : i did a static linear analysis and the stresses were unreasonably high

>so i

>wanted to perform a non linear analysis to get a better ensight on the level

>of

>stress on the same area.

>

>

>So how can i oblige NX Nastran to ignore the error on the yield function so

>that

>it completes the analysis?

>

>

>Many thanks,

>Engrequest

>

See FSTRESS on NLPARM.

NLPARM Remark 12 from the QRG:

12. The number of subincrements in the material routines (elastoplastic and

creep) is determined so that the subincrement size is approximately

FSTRESS * SIGMAequiv (equivalent stress).

FSTRESS is also used to establish a tolerance for error correction in

the elastoplastic material; i.e.,

error in yield function < FSTRESS * SIGMAequiv

If the limit is exceeded at the converging state, the program will

exit with a fatal message. Otherwise, the stress state is adjusted

to the current yield surface

Not applicable

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

07-09-2009 09:31 AM

"lamyaa tahlil"

>

>Hi,

>i am actually performing a non linear analysis on an assembly with contact

>using

>gap elements using NX Nastran V6.1

>my solution converges at a 0.3 load factor and then issue a fatal error message

>

>*** USER FATAL MESSAGE 4676 (NMEPS)

> ERROR EXCEEDS 90.00

> PERCENT OF YIELD STRESS IN ELEMENT ID= 52191

> ^^^ USER INFORMATION MESSAGE 9005 (NLSTATIC)

>

>how can i oblige NX Nastran to ignore the error on the yield function so that

>it

>completes the analysis?

>

>NB : i did a static linear analysis and the stresses were unreasonably high

>so i

>wanted to perform a non linear analysis to get a better ensight on the level

>of

>stress on the same area.

>

>

>So how can i oblige NX Nastran to ignore the error on the yield function so

>that

>it completes the analysis?

>

>

>Many thanks,

>Engrequest

>

See FSTRESS on NLPARM.

NLPARM Remark 12 from the QRG:

12. The number of subincrements in the material routines (elastoplastic and

creep) is determined so that the subincrement size is approximately

FSTRESS * SIGMAequiv (equivalent stress).

FSTRESS is also used to establish a tolerance for error correction in

the elastoplastic material; i.e.,

error in yield function < FSTRESS * SIGMAequiv

If the limit is exceeded at the converging state, the program will

exit with a fatal message. Otherwise, the stress state is adjusted

to the current yield surface

Not applicable

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

07-09-2009 09:48 AM

on the NLPARM entry.

You almost certainly have a totally unrelated convergence problem in your

model - possibly because as a non-linear problem your physics may be

unrealistic. If you have a look at the values listed under EPI and EWI in

your .f06 file, you will probably find they are diverging a long way off the

values of 1e-3 and 1e-7 respectively required (by default) to achieve a

converged solution.

Your load may be way too high, or your load increments may be too large. If

it's a buckling collapse type problem you should use an arc length method

(NLPCI) or if you are expecting to simulate plastic strains above ~10%

and/or material failure you should use the Advanced Non-linear option.

You should perhaps also try to make your gap elements less stiff. If you

are trying to make the gap elements penetrate no more than, say, 0.001 mm,

they are probably too stiff, and the solution will have difficulty

converging. Unless you are doing a Hertzian contact problem, the gaps can

be more flexible, which makes convergence easier. Oh, and constrain the

rotational degrees of freedom at each end of the gap if they are connected

to solid elements.

Best Regards,

Vernon McKenzie

EnDuraSim P/L

"lamyaa tahlil"

news:4a55bfad$1@bbsnotes.ugs.com...

>

> Hi,

> i am actually performing a non linear analysis on an assembly with contact

> using

> gap elements using NX Nastran V6.1

> my solution converges at a 0.3 load factor and then issue a fatal error

> message

>

> *** USER FATAL MESSAGE 4676 (NMEPS)

> ERROR EXCEEDS 90.00

> PERCENT OF YIELD STRESS IN ELEMENT ID= 52191

> ^^^ USER INFORMATION MESSAGE 9005 (NLSTATIC)

>

> how can i oblige NX Nastran to ignore the error on the yield function so

> that it

> completes the analysis?

>

> NB : i did a static linear analysis and the stresses were unreasonably

> high so i

> wanted to perform a non linear analysis to get a better ensight on the

> level of

> stress on the same area.

>

>

> So how can i oblige NX Nastran to ignore the error on the yield function

> so that

> it completes the analysis?

>

>

> Many thanks,

> Engrequest

>

Not applicable

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

07-09-2009 09:58 AM

"Jim Bernard"

>Thanks Jim,

i did change the value of the FStress in NLPARM card into higher value (0.99) just

to get the analysis going but it does stop for high stress in element nodes.

i was hoping if there is any way to force nastran to finish the analysis even if

the error is exceeded.

Thanks

>"lamyaa tahlil"

>>

>>Hi,

>>i am actually performing a non linear analysis on an assembly with contact

>>using

>>gap elements using NX Nastran V6.1

>>my solution converges at a 0.3 load factor and then issue a fatal error message

>>

>>*** USER FATAL MESSAGE 4676 (NMEPS)

>> ERROR EXCEEDS 90.00

>> PERCENT OF YIELD STRESS IN ELEMENT ID= 52191

>> ^^^ USER INFORMATION MESSAGE 9005 (NLSTATIC)

>>

>>how can i oblige NX Nastran to ignore the error on the yield function so

>that

>>it

>>completes the analysis?

>>

>>NB : i did a static linear analysis and the stresses were unreasonably high

>>so i

>>wanted to perform a non linear analysis to get a better ensight on the level

>>of

>>stress on the same area.

>>

>>

>>So how can i oblige NX Nastran to ignore the error on the yield function

>so

>>that

>>it completes the analysis?

>>

>>

>>Many thanks,

>>Engrequest

>>

>

>See FSTRESS on NLPARM.

>

>NLPARM Remark 12 from the QRG:

>

>12. The number of subincrements in the material routines (elastoplastic and

> creep) is determined so that the subincrement size is approximately

>

> FSTRESS * SIGMAequiv (equivalent stress).

>

> FSTRESS is also used to establish a tolerance for error correction in

> the elastoplastic material; i.e.,

>

> error in yield function < FSTRESS * SIGMAequiv

>

> If the limit is exceeded at the converging state, the program will

> exit with a fatal message. Otherwise, the stress state is adjusted

> to the current yield surface

>

Not applicable

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

07-09-2009 10:16 AM

"lamyaa tahlil"

>

>Hi,

>i am actually performing a non linear analysis on an assembly with contact

>using

>gap elements using NX Nastran V6.1

>my solution converges at a 0.3 load factor and then issue a fatal error message

>

>*** USER FATAL MESSAGE 4676 (NMEPS)

> ERROR EXCEEDS 90.00

> PERCENT OF YIELD STRESS IN ELEMENT ID= 52191

> ^^^ USER INFORMATION MESSAGE 9005 (NLSTATIC)

>

>how can i oblige NX Nastran to ignore the error on the yield function so that

>it

>completes the analysis?

>

>NB : i did a static linear analysis and the stresses were unreasonably high

>so i

>wanted to perform a non linear analysis to get a better ensight on the level

>of

>stress on the same area.

>

>

>So how can i oblige NX Nastran to ignore the error on the yield function so

>that

>it completes the analysis?

>

>

>Many thanks,

>Engrequest

>

One way to solved such a problem is to reduce the loading to a value where the stress

is not so excessive, and the analysis completes. If the stresses are a result of

very poor elements, local remeshing could be the easiest answer.

Not applicable

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

07-09-2009 11:12 AM

Thanks Vernon,

I did reduce the stiffness of the gap elements to help the solution to converge

and it does converge :

0 N O N - L I N E A R I T E R A T I O N M O D U

L E O U T P U T

STIFFNESS UPDATE TIME 98.69 SECONDS

SUBCASE 1

ITERATION TIME 3.57 SECONDS

LOAD FACTOR 0.4800000

- - - CONVERGENCE FACTORS - - - -

- - LINE SEARCH DATA - - -

0ITERATION EUI EPI EWI LAMBDA DLMAG FACTOR

E-FIRST E-FINAL NQNV NLS ENIC NDV MDV

5 1.0271E-01 1.6715E-02 1.7246E-04 1.0000E-01 2.9818E-01 1.0000E+00

2.6250E-01 2.6250E-01 0 0 0 1

6 1.9313E-04 9.4615E-03 2.4436E-05 3.3302E-01 1.3172E-01 1.0000E+00

1.2363E-01 1.2363E-01 1 0 0 1

*** USER INFORMATION MESSAGE 6186 (NCONVG)

*** SOLUTION HAS CONVERGED ***

SUBID 1 LOOPID 183 LOAD STEP 0.480 LOAD FACTOR 0.48000000

*** USER FATAL MESSAGE 4676 (NMEPS)

ERROR EXCEEDS 99.00

PERCENT OF YIELD STRESS IN ELEMENT ID= 50919

*** USER FATAL MESSAGE 4676 (NMEPS)

ERROR EXCEEDS 99.00

PERCENT OF YIELD STRESS IN ELEMENT ID= 52191

^^^ USER INFORMATION MESSAGE 9005 (NLSTATIC)

^^^ THE SOLUTION FOR LOOPID= 183 IS SAVED FOR RESTART

^^^

^^^ USER INFORMATION MESSAGE 9210 (NLSTATIC)

^^^ NONLINEAR STATIC ANALYSIS COMPLETED.

when i view the results, the elements have a nodes with high stress, is it because

of distorted elements?

i need to redo the analysis with constraining the rotational degree of freedom at

each end of the gap elements and see whether it helps.

Many thanks!

"Vernon McKenzie"

>You have obviously already increased FSTRESS from its default value of 0.2

>

>on the NLPARM entry.

>

>You almost certainly have a totally unrelated convergence problem in your

>

>model - possibly because as a non-linear problem your physics may be

>unrealistic. If you have a look at the values listed under EPI and EWI in

>

>your .f06 file, you will probably find they are diverging a long way off the

>

>values of 1e-3 and 1e-7 respectively required (by default) to achieve a

>converged solution.

>

>Your load may be way too high, or your load increments may be too large.

>If

>it's a buckling collapse type problem you should use an arc length method

>

>(NLPCI) or if you are expecting to simulate plastic strains above ~10%

>and/or material failure you should use the Advanced Non-linear option.

>

>You should perhaps also try to make your gap elements less stiff. If you

>

>are trying to make the gap elements penetrate no more than, say, 0.001 mm,

>

>they are probably too stiff, and the solution will have difficulty

>converging. Unless you are doing a Hertzian contact problem, the gaps can

>

>be more flexible, which makes convergence easier. Oh, and constrain the

>rotational degrees of freedom at each end of the gap if they are connected

>

>to solid elements.

>

>Best Regards,

>Vernon McKenzie

>EnDuraSim P/L

>

>

>"lamyaa tahlil"

>news:4a55bfad$1@bbsnotes.ugs.com...

>>

>> Hi,

>> i am actually performing a non linear analysis on an assembly with contact

>

>> using

>> gap elements using NX Nastran V6.1

>> my solution converges at a 0.3 load factor and then issue a fatal error

>

>> message

>>

>> *** USER FATAL MESSAGE 4676 (NMEPS)

>> ERROR EXCEEDS 90.00

>> PERCENT OF YIELD STRESS IN ELEMENT ID= 52191

>> ^^^ USER INFORMATION MESSAGE 9005 (NLSTATIC)

>>

>> how can i oblige NX Nastran to ignore the error on the yield function so

>

>> that it

>> completes the analysis?

>>

>> NB : i did a static linear analysis and the stresses were unreasonably

>> high so i

>> wanted to perform a non linear analysis to get a better ensight on the

>> level of

>> stress on the same area.

>>

>>

>> So how can i oblige NX Nastran to ignore the error on the yield function

>

>> so that

>> it completes the analysis?

>>

>>

>> Many thanks,

>> Engrequest

>>

>

>

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc