Bauschinger Effect modelling in ABAQUS/CAE

[atedionyahoo]

How Bauschinger Effect can be modeled in ABAQUS/CAE?
Thanks in advance

 

[Drej]

It isn't. It's modelled using an appropriate constitutive model in Abaqus itself, the choice of which is dependent on the application, in particular the rheological behaviour of the material and the loading. I suggest first, however, that you compile a more reasoned, detailed and considered question for people to attempt to help you.

Thanks in advance.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[atedionyahoo]

Drej, Thanks for your attention.
I want to model an exemplary Beam under axial cyclic loads (for example in step 1 the beam is under tension and step 2 under compression), and in ABAQUS/CAE in the MATERIAL section I use nonlinear tabular plasticity (stress – strain). However, I do not know how to model Bauschinger effect for the next cycles?
(I have attached my exemplary model “JJ1.inp”, and therein I understand the stress-strain I define is relevant to the 1st cycle and there should be somewhere to define stress-strain for the next cycles!)

 

[Drej]

See, for example: thread799-277878

See also the Abaqus manual keyword section under *PLASTIC, HARDENING= and also the links to "Metals Subjected to Cyclic Loading".


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[atedionyahoo]

ABAQUS/Standard: to carry out the hardening & cyclic loading analysis for beam element (B31), I use the following command:

*PLASTIC, HARDENING=COMBINED, DATA TYPE=HALF CYCLE

However after the program running the following error message appears:

***ERROR: THE *COMBINED HARDENING OPTION IS NOT AVAILABLE FOR BEAM-TYPE ELEMENTS WITH SHEAR STRESS

Does it mean that I should change the element type?, I browsed quickly in the help, but there was not anything relevant to limitation of element for placticity (i.e. considering the above ERROR message) . Could somebody please shed light. (NB, for clarity I have attached the inp file)

 

[mrgoldthorpe]

"19.2.2 Models for metals subjected to cyclic loading
....
These models can be used with elements in Abaqus/Standard that include mechanical behavior (elements that have displacement degrees of freedom), except some beam elements in space. Beam elements in space that include shear stress caused by torsion (i.e., not thin-walled, open sections) and do not include hoop stress (i.e., not PIPE elements) cannot be used. In Abaqus/Explicit the kinematic hardening models can be used with any elements that include mechanical behavior, with the exception of one-dimensional elements (beams and trusses) when the models are used with the Hill yield surface."

 

[atedionyahoo]

Thanks,
However I tried PIPE element (pipe31), but the solution did not converge (NB, the data check runs correctly, but its continue does not converge).
I have attached the inp file, it is a simple beam fixed at one end and the other end under cyclic displacement, I would appreciate if somebody could look at it and advise what is the matter.

 

[Drej]

The manual (see above) clearly states that these elements cannot be used. Would advise you to start with a benchmark of your problem using, say, solids or shells and move on from there.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[loki3000]

what is the bauschinger effect? hardening of the steel (tensile) due to compressive prestress if i understand correctly?
like in cold rolling?

 

[atedionyahoo]

Thanks Drej and mrgoldthorpe

From your response, it is implied Bauschinger Effect (cyclic load) can not be modeled in ABAQUS by PIPE or BEAM elements.

However, I want to model pipeline on seabed for global buckling / fatigue analysis (between pipeline cyclic operation and shut down) and as a normal practice the used element type is either PIPE or BEAM. NB, usage of SHELL / SOLIDS elements are not straightforward for my model (i.e. pipeline).

Could somebody please shed light for my case?

 

[mrgoldthorpe]

You could try the simplified "KINEMATIC" version, using an approximate plastic slope, e.g.:

*PLASTIC, HARDENING=KINEMATIC
90.039E6, 0
550.55E6, 2.07E-1

Otherwise it's a UMAT or different elements or perhaps putting in multiple elements connecting the same nodes, the elements having differing elastic-plastic response (don't ask how though).