Cancel
Showing results for 
Search instead for 
Did you mean: 
Highlighted

USER FATAL MESSAGE 4676 (NMEPS)

N/A

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

Re: USER FATAL MESSAGE 4676 (NMEPS)

N/A

"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

Re: USER FATAL MESSAGE 4676 (NMEPS)

N/A
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" wrote in message
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
>


Re: USER FATAL MESSAGE 4676 (NMEPS)

N/A

"Jim Bernard" wrote:
>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" 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
>

Re: USER FATAL MESSAGE 4676 (NMEPS)

N/A

"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
>

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.

Re: USER FATAL MESSAGE 4676 (NMEPS)

N/A

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" wrote:
>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" wrote in message
>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
>>

>
>