Dear all,
I am simulating a material softening region for steel.
For plastic information, the input data is set up following the curve in the figure. This data is extended larger for the input data in comparison with the experimental data. I hope it helps to avoid automatical interpolation in ABAQUS.
However, the result seems out of control. The von Mises of one critical point ( a selected node in necking happens) shown in the second figure has a dramatic drop.
The third picture shows a necking result. Of course, this includes large deformation. My current wonder why von Mises has dramatical drop even input stress-plastic strain are smooth.
Could you give me some comments and advice, please?
Thank you very much,
Bac
i belive your problem is due to element size. you Von Mises drop dramatically due to Large element size where your model fail to capture necking!. try to refine your element specially in necking regions.
Dear Bac,
Your input curve shows material softening. Are you sure that the stress is true stress (i think you are using engineering stress as input which is wrong). You must convert engineering stress to true stress upto the maximum engineering stress. The true stress (determined from uniaxial tensile test) is only valid upto maximum force. The curve must be extrapolated after this point.
In case you have captured material softening by some method then your results will always remain mesh dependent, because of this softening, unless you use regularization method or nonlocal mothods.
Dear Tamer and Muhammad,
Thank you very much,
With Tamer's suggestion, I have meshed the geometry smaller, but the result seems not change much.
With Muhammad's suggestion. I used true stress-strain already. The relationship is logarithm strain computed from an uniaxial test. The experimental data is taken by using a 25mm extensometer for relative displacement and machine force. That is used to compute true-strain curve.
I am also wondering that it may be not appropriate for the necking regime. As your idea, we can not provide softening information in the plastic window in ABAQUS? Do you mean we have to use the damage window (for example, "damage for ductile metal") and stick with one criterion?
Cheers,
Bac
The true stress strain curve which you make from uniaxial test is valid only until the uniform strain. Once the test crosses the maximum force (ultimate tensile stress point) the strain will not remain uniform and thus you cannot use the same formula to convert the forces/engineering stress into true stress.
Beyond the maximum force point, you must extrapolate the true stress strain behavior (or experimentally determine the stress strain behavior at large strains with a shear test). If you extrapolate the curve then do not make the stiffness (slope) negative otherwise it will induce material softening (or damage). You will still get necking due to geometric softening which is the case for most of mild (IF) steels. The point of initiation of neck depends upon the hardening exponent. Material softening or damage is not required to model necking.
You must use damage (or material softening) only if you think it is important and can influence the necking point. Remember, with damage (or material softening) the results are mesh dependent unless you use some special techniques to remove it.
Is your problem load- or displacement controlled? For problems with softening, displacement control is usually better because it can deal with instabilities
Dear all,
Thanks for helping me.
I appreciate Muhammad's advice. It is very useful.
Cheers,
Bac
hi
please be sure to use finite strain type of element in order to consider true stress-true strain curve. i advise you frist to create new model using only one element (finite strain type of element such as cps4r simulating uniaxial tensile test and compare it with experimental results. in this model use displacement control. this model will elimintate the dought about stress-strain curve then you concenterate on the meshing arround the necking.
i am modeling steel angle bolted connection , when plot stress strain curve for an element in the top angle(red one) , the curve far away from input data (blue one)
can anyone explain please
- Badges
- Science topic