Stresses go beyond yield limit in perfecly-plastic model...

[ISC214]

Hi all,

I have a problem with perfect-plasticity material model in Abaqus. I this simple 2D analysis, I am modeling a beam fixed at both ends and applying temperature loading on it that will cause yielding. The material model is perfectly plastic with,

*PLASTIC

4.85 E8, 0.0

The problem is, stresses go beyond yield limit (4.85 E8) which should not be the case for the perfectly-plastic material model. Inp file attached. I would appreciate any comment/help/suggestion.

Regards,

Soner

 

[TGS4]

The state of plasticity is determined by the state of stress calculated at the Gauss point in each element. If an element has not gone plastic, then it's stress-strain state is elastic. Accordingly, when the stresses are extrapolated to the nodes, it is possible that you could have stresses that exceed yield. This is a mesh-refinement issue.

 

[mrgoldthorpe]

You have plane strain elements with both ends fixed. Therefore, the individual components of stress can exceed the yield stress according to the yield criterion. The ENCASTRE boundary condition will certainly help to elevate the individual components of stress. Note, however, that the von mises stress should be 4.85e+08 in all yielded elements

(Yielding depends on shear stresses. If you apply a pure hydrostatic load to a single element there is no yielding: the components of stress can increase indefinitely.)