Stop criteria on Abaqus 1

[3JC]

Dear collages:

I'm performing an analysis of a bolted connection, and I want to know if it is possible to define a criteria of maximum deformation (and then, the analysis stop). For example, about the maximum deformation of the bolt. I send to you in attach a screenshot about results that I have (and the analysis is yet running... Thank you very much.

 

[IceBreakerSours]

Yes; using subroutines.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[burningDiesel]

or if you are using explicit:

Halting the analysis when the extreme value criterion is met
You can choose to halt the analysis when the extreme value criterion is met. The analysis will stop at the end of the increment following the one in which any of the specified element or nodal variables exceeded the prescribed bounds.
Input File Usage:
Use the following options:

*EXTREME VALUE, HALT=YES
*EXTREME ELEMENT VALUE and/or *EXTREME NODE VALUE

 

[3JC]

Dear friends:

Thank you very much for your responses. Could you please tell to me additional information about the both two procedures: to develop a subroutine and to perform an explicit analysis (if I have made all the model as implicit)?

Thank you very much.

 

[3JC]

Dear collages:

I have some questions about the use of subroutines. Is it possible to define a subroutine into Abaqus CAE? If not, how it could be defined, in the *.inp file? As mentioned, my interest is to stop the analysis when a level of deformation is reached on elements. Is it possible to define these elements through the instance where they procede? In my model I have 3 different materials (the bolt, the plate and the profile), with a lot of elements, and I want to define a maximum level according to the material of each instance.

Thank you very much. Regards,

Juan José

 

[IceBreakerSours]

Juan:

The specific subroutine of interest to you is XIT which can be called by almost all subroutines. If you google, you will find plenty of information related to subroutines.

With regard to explicit analysis, try out a few examples in the documentation.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[akabarten]

Hi,

The thitd option is to use *FILTER keyword. Unfortunatly it works only with Abaqus/Explicit.
For details see Abaqus documentation: Abaqus Analysis User's Manual, 4.1.3 Output to the output database, Filtering output and operating on output in Abaqus/Explicit, Stopping an analysis when an output variable reaches a prescribed limit.

Subroutines are write with FORTRAN and if you do not have experience it can be difficult at the beginning.
You need to choose any subroutine which have access for outputs, see Abaqus User Subroutines Reference Manual:
- 2.1.6 Obtaining material point information in an Abaqus/Standard analysis
- 2.1.7 Obtaining material point information in an Abaqus/Explicit analysis
- 2.1.9 Obtaining node point information
Next as "IceBreakerSours" alrady mentioned you can use XIT routine (see
2.1.15 Terminating an analysis) or STDB_ABQERR (see 2.1.14 Printing messages to the message or status file) to stop the analysis.

You can also use UAMP subroutine + sensor output and use lFlagsDefine(iStopAnalysis) argument.

Regards,
Bartosz

 

[3JC]

Dear collages,

Thank you very much. Dear sdebock: could you please give me more information about how to use a halting? How do you specify this in the input archive, you write it? And how do you send the model (I'm a CAE user).

Thank you very much. Regards,

jJ