Higer stress from results than in elasto-plastic curve

Dear all, I am using elasto-plastic material curve with these properties:

Maximum stress is roughly 111 MPa. When I solve the model (nonlinear analysis, nnlin geom ON), I get maximum stress values (both Von Mises and principal maximum) higer then the highest value in the stress-strain curve (this affect a wide part of the model, it isn’t just a few elements). This sound strange to me, expecially because the material has a perfect plastic behaviour from a certain strain. Here the two images of the model:
Principal stress

Von Mises

Thanks in advance for any help!

In the majority of cases, this is caused by the extrapolation of stresses from the integration points to nodes. You would have to check the stresses directly at the integration points (it can be done in the .dat file or with a script: Stresses at the integration points in ParaView - #2 by mkraska).


when magnify is high, it can be used as sign to do mesh convergence study. refinement is required in these areas. still discrepancy will exist due to extrapolation.

1 Like

@synt thank you for your advice: as you suggested I adopted a finer mesh in the area of interest, going from an average el. size of 0.5mm down to 0.1mm: results didn’t change, I still have values around 140MPa instead of the maximum value in the curve, 111 MPa.
Moreover, I tried with another material (same model, same loads, just different material) less ductile than the first I used, again adoptin gelasto-plastic behaviour such as this:

Young’s modulus is roughly 3 times higher than the initial material.

@FEAnalyst I see your point and I would agree if for one reason: maximum stress in stress-strain curve is lower than the value I should find in any of the integration points. Interpolating integration points to the nodes, should give me at least not accurate stress, but I don’t expect this huge difference (110 vs 140MPa in wide areas of the model is roughly 25% of difference!!!)

Hi Lorebergo,

¿What stress are you comparing with?. Not clear to me as your curve says “DATA”.

is maximum plastic strain located at the same nodes? if not, probably cause of over-constraint in model and simplification, thus unrealistic results.

Check this thread as well, it’s an interesting discussion about a similar problem: Load variation in non-linear material problem

Maybe your plastic card is not right ?¿? Make sure you wrote it correctly and there are not warnings on the monitor like:

*WARNING reading *STEP: parameter not recognized:
*WARNING reading *STEP. Card image:

It should say

Sometimes, if the error is not critical the analysis can end up but with unexpected result.

1 Like

It’s because temperature is plotted in the same graph so there are different quantities on the Y axis. But temperature can be ignored here so it’s just yield stress - plastic strain plot of the input data for *PLASTIC.

it seems not possible to do typo, since these feature is available in menus.of PrePoMax

also, being restricted to modify accidentally by the user in Edit CalculiX Keyword.

any reason to do manually typing or modify/overwrites even possible?

when typo as guessed, there will be no results shown and a warning message appears.

If you use the Field Output (on one of the most loaded elements), you will get the stress results in the integration points. Check this stress to see its real value.

1 Like

Don’t you mean history output ?

Yes, I am sorry, the History output.