Isotropic Hardening

[hklatte]

Hi, from Abaqus manual it says that the material will go prefectly plastic after the von Mises stress state reaches the end of the strain-stress curve. However, it's not un-usual (at least for me) to have von Mises stress higher than the max stress in the input.

For example, in the inp file I have below, although the strain-stress curve ends at 178120ksi, the von Mises stress in my model gets 230+ ksi. If the material does go prefectly plastic, am I supposed to get the max of 178120ksi in the model?

----------
...
*Material, name=steel
*Elastic
30e6, 0.3
*Plastic
94290., 0. ** yield strength
178120., 0.19291 ** ultimate strength
...
----------

Thank you for any idea/input in advance!

 

[xerf]

How do you know
"the von Mises stress in my model gets 230+ ksi" ??

If this statement based on information from banded contour plots?

 

[hklatte]

Thank you for replying, xerf.

The stress is at the nodal location. I understand that the actual FEA calculated von Mises stress is at the integration points, from where the nodal output gets extrapolated. However, looking at the size of elements, an extrapolation from 178 to 230 ksi just seems impossible.

Do you have any insight regarding this? Thank you.

 

[Yoman228]

There is 2 ways I can suggest.
1)Calculate the gradient of the material curve based on the last 2 data, and assumed it will continue as the same gradient to a strain that your model will not reach.

Or

2)Use Ramberg-Osgood behavior if you know the UTS


Notes that ABAQUS use true stress and strain, so you need to convert it from engineering stress and strain that from test data specially after yield.

 

[Yoman228]

opp.. sorry mis-read the question.

 

[xerf]

It is not impossible if you have a stress gradient and/or coarse mesh. Also, if you have contact, constraints etc.

The nodal values are obtained from IP values. There will be several values obtained at one node, depending on how many elements share that node. These values can be different, and for plotting purpose they are averaged. This averaging process can be controlled using Menu-> Results Options.

You can see the discontinuities in the fields extrapolated from IP to nodes by selecting:
Results Options -> Quantity to Plot-> Discontinuities

In conclusion, you should use quilt contour plot which uses the stresses at integration points.