Yield limit with plastic strain correlation 1

[Pawel27]

I often use perfectly plastic material model in FEM analysis.
I have noticed where stress are above yield limit, there is
often no plastic strain. Plastic strain appears in the area
where stress are much more above yield limit. Any comments and hints about this material model behaviour will be very valuable.

 

[EdR]

You really need to look at the specific material model you are using and the users guide for whatever code you are using for some hints as to how the model is implemented....

There are a number of methods that may be used when implementing material models (some methods only show the total strain and do not break it down into elastic and plastic strains....(particularly if they do not use a flow rule).....There are also many methods for detecting when yielding has occurred and some may "overshoot" and/or not detect yielding as quickly as others......

Ed.R.

 

[cbrn]

Hi,
you have two kinds of "problems" to assess:
1- the yield criterion and the associated flow rule. Before all, you of course must know which is the criterion thanks to which the program "knows" that the material has yielded. As far as I know, despite some Norms prescribe the Trescà yield criterion for some checks (e.g. the Gross Plastic Distorsion check of EN-13445), most FE programs, if not all, use the Mises yield criterion instead. If you expect the program to detect yielding with the "wrong" criterion, of course you will find a discrepancy
2- the yielding, just like all the "integrated" results (stress-related results), is calculated in the integration points of the elements (Gaussian points), NOT in the nodes. The results are generally extrapolated to the nodes using the appropriate elements formulations, but when you speak about yielding this will of course lead to irritating results, such as nodes having equivalent stress value higher than yield limit (which, with a zero-tangent-modulus "pure" plasticity, is of course nonsense!).
In order to get rid of this absurdity, you need to directly transfer the integration-points results to the nodes. Every FE program may have its own command to do that. ANSYS, for example, uses "ERESX,NO".
Please note that some programs THINK they are very clever and activate the direct transfer automatically when they detect that the element have yielded. Trouble is, that the yielding is detected element by element, not node by node, of course. So, before the algorythm detects it needs to activate the direct results transfer, it is already too late (well, I'll be a little less severe: "it MAY be already too late").

Regards

 

[Pawel27]

Some comments:

It is interesting that reduced stress (Von Mises) are at the same level in a certain area, but only small region of this area has equivalent plastic strain (Ansys). Yield criterion is fulfilled in all area, but only on a small region of it has plastic strains. I know about things mentioned above (maybe to little), but it is still mysterious for me. More detailed comments are desirable.

 

[cbrn]

Hi,
in your first post, you mentioned that plastic strain "appears in the area where stress are much more above yield limit". But, as you know, when you use an "ideal plastic" constitutive law, i.e. a constitutive law where the tangent modulus is zero, if the analysis is correct you CAN NOT have values higher than the yield value... IF... if the constitutive law is the correct one to describe the effect you want. In this case, BKIN (bilinear kinematic) without other "exotic" effects.
Of course things can get really different if you are speaking about "real-life" material models with complicated constitutive laws.
You should provide much more details about how you setup the non-linear-material problems for which you suspect troubles.
Regards

 

[Pawel27]

Yes... it is ideal plastic material. "Much more above yield limit" - I mean that stress are sufficient above yield limit to catch plastic strain. I can have stress values above yield limit for ideal plastic material - it is related to extrapolation.

In fact when I have any area with THE SAME STRESS VALUE in this area, only small region of it has plastic strain. Not all area has plastic strain.

 

[Pawel27]

I have question to EdR:

"(particularly if they do not use a flow rule)...."

Flow rule determines the direction of plastic straining.
Is it possible that in any FEM software flow rule is not used?

 

[EdR]

Pawel27:

Absolutely.....In some cases inelastic behaviour is modeled using nonlinear curves for moduli...also where a cracking reinforced concrete (or brittle material model) is used there may be no way to compute a "plastic" strain value...

A flow rule (either associated or nonassociated) determines the magnitude (and sign) of the plastic strain i.e. epsp = lamda * df/dsig (where f represents the yield surface) and if the particular model being used does not operate using this type of implementation (i.e. no yield surface or multiple (concrete/steel) yield surfaces) then no "plastic" strain can be computed.....Also note that good results can be obtained using these types of models even though no "plastic" strain is computed or available....In such cases the total strain will be available it is just not broken down into elastic and plastic parts....

As I noted earlier you must understand the specific model being used in order to asses whether "plastic" strain exists and how it is obtained......

Ed.R.

 

[EdR]

p.s. Make that "assess" not asses.....fumble fingers....

Ed.R.

 

[Pawel27]

Please explain sth more about "nonlinear curves for moduli". Why plastic strain may be not computed?

 

[EdR]

I guess I don't understand the question....Some material models may use curves to describe the elastic moduli (E,nu,G or K,G, etc) an example might be a model for Aluminum using a parabolic stress/strain curve...which is effectively a nonlinear representation of the moduli...(E=dsig/deps)

In such a case how would one compute a "plastic strain"?? The definition of "plastic strain" is as I noted in a previous post so if you do not have a yield surface it is not possible to compute a "plastic Strain"....This is not to say that for special cases, such as a uniaxial stress/strain curve, the value of plastic strain cannot be computed. The real question becomes how do you do it for more complex cases i.e. 3-D and non-uniaxial stresses....generalized load/unload and several other types of problems....

Also as I noted consider brittle material models where the question becomes ... after cracking occurs are the strains "plastic"????...

I suppose one can make your own individual definition to these kind of questions but providing a general definition that meets accepted engineering definitions for all cases becomes impossible .... and then what have you gained should you have some global definition of "plastic" strain......

Ed.R.

 

[kellnerp]

Here is some data on the real behavior of various Aluminum alloys including cyclic data. There are some FEA correlations as well.

Aluminum Data



TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."