Re:  Hope your suggestion about Umat for composite shell!

Dear Chenhu,

to use shell elements for welding analyses with added material in the
chamfer is a possibility. I think you may not write a UMAt but only a User's
subroutine UFIELD in the sense:

1) Let your material properties be dependent from one FIELD VARIABLE. this
FV is for example equalt to 0 when the material is not present in the
chamfer and is equal to 1 when the material is present in the chamfer. So
*ELASTIC,DEPENDENCIES=1 and *PLASTIC, DEPENDENCIES=1 are the material
constitutive properties you may define. Scale material properties so these
are real for FV=1 and fictitious for FV=0 and set also the same for
FV=0.999. This is due to the fact that you will set FIELD VARIABLES at nodes
but ABAQUS always read FIELD VARIABLES at integration point. So when the
electrode in the chamfer is moving on there will be inactive elements (or
better inactive material properties) associate to one element for which some
nodes (2) have FV=1 and some nodes (2) have FV=0. At material point FV=0.5
and here the meaterial need to be scaled. So a fully real property is
defined only when for all the nodes FV=1. Material scale factor can be 0.001
for thermal properties and 0.00001 for mechanical properties.

2) Define these material ONLY for the elements of the chamfer and not for
the elements around.

3) Set *INITIAL CONDITIONS,TYPE=FIELD,VARIABLE =1 for the nodes of the
chamfer to define what elements are present or not following previous
suggestions.

4) Set FIELD variables as you want during an analysis also by usage of
User's subrotuine UFIELD but also easilu with AMPLITUDES.

Finally it is your choice to go first with a thermal analysis, take the
temperatures at the integration points and read them subsequently into a
mechanical analysis (*TEMPERATURE,FILE). It is also possible to couple the
thermal analysis and the mechanical one in ABAQUS but the need of this
procedure depends on the deformation of the structure.

I was doing so and it seemed to me that it works.

Let me know in future your results to be more confident with this method.

Best Regards and good work.

G.L. Zanotelli


----- Original Message ----- 
From: "³Â»¢" <chh1210@xxxxxxxx>
To: <ABAQUS@xxxxxxxxxxxxxxx>
Sent: Sunday, October 31, 2004 6:31 PM
Subject:
[ABAQUS]&nbsp;Hope&nbsp;your&nbsp;suggestion&nbsp;about&nbsp;Umat&nbsp;for&n
bsp;composite&nbsp;shell!


>
>
> Hello ABAQUS fans:
>     I am a chinese students using ABAQUS to simulate welding process ,some
> questions are encountered in analysis and i am confused about it ,in yahoo
> abaqus group,i have learned more about abaqus from u,so i am so sorry to
> interrupt to hope u give me some suggestion about my analysis.
>     The questions are followed:
> 1.in general 3-D welding simulation,solid element are used to model the
> welding pass ,which is suited in small model and not effective for a large
> model because so many elements and nodes are costful. so i want to realize
> that using laminated composite shell element to replace the solid element
and
> every shell layer will mean one weld pass. But a question comes ,for
welding
> using solid element ,we can model the add of weld material which are
removed
> at first time and be added sequently in proper time using *model change to
add
> or remove,but *model change only bases on the element and not available
for
> composite shell layer (which based on the section points or integrate
point),
> i know about the theory about *model change ,which means that the stiffen
> (matrix) of the removed element are decreased to a very small value ,which
> cant contribute to a total stiffen of the body ,and renew to its origin
value
> when added ,so i want to write UMAT to realize the removal  or add
procedure
> for the shell layer ,we can get the integrate points stiffen matrix from
> abaqus (right?),and when time reached, i give the points concerned a very
> small value or renew, all above ,can i realize?
>
> 2.If i can get a theory temperature value on each integrated point with
time(i
> have the fomula and i can write a program to calculate ,the fomula is
about
> the temperature changing with the time and coordinates of the points) ,can
> these value be mapping into the abaqus model as a initial temperature
> condition which are needed in welding residual stress analysis?
>
> i hope i have explained my questions, right?and i hope your suggestions
> eagerly!
>
> 3x for your reading!
>
>                                                                     your
> student:chenhu
>
>
>
>
>
>
>
> --http://www.eyou.com
> --Îȶ¨¿É¿¿µÄµç×ÓÐÅÏä  ÓïÒôÓʼþ  Òƶ¯ÊéÇ©  ÈÕÀú·þÎñ  ÍøÂç´æ´¢...ÒÚÓÊδ¾¡
>
> --http://vip.eyou.com
> --¿ì¿ìµÇ¼ÒÚÓÊVIPÐÅÏä  ×¢²áÄúÖÐÒâµÄÓû§Ãû
>
>
>
>
>
>
>
>
> Community email addresses:
>   Post message: ABAQUS@xxxxxxxxxxxxxxx
>   Subscribe:    ABAQUS-subscribe@xxxxxxxxxxxxxxx
>   Unsubscribe:  ABAQUS-unsubscribe@xxxxxxxxxxxxxxx
>   List owner:   ABAQUS-owner@xxxxxxxxxxxxxxx
>
> Shortcut URL to this page:
>   http://groups.yahoo.com/group/abaqus
> Yahoo! Groups Links
>
>
>
>
>
>
>
>



------------------------ Yahoo! Groups Sponsor --------------------~--> 
$9.95 domain names from Yahoo!. Register anything.
http://us.click.yahoo.com/J8kdrA/y20IAA/yQLSAA/PMYolB/TM
--------------------------------------------------------------------~->