Depending on the model, strain is LE (logarithmic strain for non-linear analysis) or NE (nominal strain). Displacement is U. Elastic strains are EE. Stresses are alsways elastic since there is no such thing as a "plastic stress".

All variables are described in the manual chapter 4.

BTW, your mesh looks not too good - note that a rule of thumb is that adjacent elements should not differ by more than a factor of 2-3 in area.

Dear Richard, 

These are no elastic and plastic stresses only strains.

U- displacement 

EE- elastic strain

PE-platic strain

LE or E- total strain

To find out the maximum values click on Contour plot options - Limits - Show location.

 Thanks & Regards,

Ranjith.

You can use the probe tool (Tool->Query) to check the nodal displacement or elemental stress/strain, and output the ones you clicked on. Another option is the report menu, firstly by selecting the nodes or elements, and then output the variables in a *.rpt file. With these data you can find the maximum or minimum values in excel.

Thank you very much guys.

Honestly your answers have taken me a long way.Please I have one little problem still:

I don't know if anyone have experienced same situation before.I have been trying to see the values of the Plastic Strain from the Output variable strain components of PEEQ and PEMAG but I can only see Zeros all through down the list.I guess this means the plastic strain was not calculated. Same also with Yield Stress.Please could this be for some kind of Technical issue with Abaqus software or did I miss  or omit any step in designing?

And which is the Output Variable component for elastic stress?

Also how do can I separate the Plastic region from Elastic region after running analysis? 

Please if  you have any clue,your answers are really appreciated.Thanks again.

Did you define plasticity correctly in your material model (the input file should contain the *Plastic card)?

By "separating Plastic from elastic region" do you want to see which parts have deformed plastically at all (use PEEQ for that) or which are currently plastifying (for that there is the variable ACYIELD)?

Yes Marthin,Thanks again.

On the material model,I did the following

Yield Stress            

2000 

2100

2400

2600

2940

Plastic Strain

0

0.1

0.2

0.3

0.4

For the plastic deformation,I check PEEQ for that and all I can see is 0.000e+00 all through down the list.So that's why I am worried maybe I have omitted(which I'm not sure) a step in my designing.so the system did not compute for that.

For separating Plastic from elastic region,I want to see the elements under plastic and elastic region separately.

So is the Mises stress in any point larger than 2000? (What units are those, BTW - 2000MPa would be quite a bit?) What's your value of Young's modulus?

My  Young Modulus is 570 and Poison ratio 0.23.

The Mises Stress is max of 7.866e+02

I am working with Meters and Pa

So if your max mises stress is 786, you are below the yield stress, therefore PEEQ is zero.

"I am working with Meters and Pa"

Are you? I hope that your Youngs modulus is in GPa and your yield stress in MPa, so you enterred 570e9 for Youngs modulus (what material is that, BTW, that's quite a large value) and 2000e6?

Please make sure that all units are in agreement - otherwise your numbers will tell you nothing. (If you want, you could upload the inp-file.)

Oh Martin,

Thank you so much I have just increased the load to get a higher stress value.And it worked and I can see the PEEQ values.Like you said the stress on the material was just below the yield stress.So the plastic strain values could not be calculated.

Thanks alot !.....Meanwhile for the elastic   and plastic  region ,Please do you know how I can identify and separate them in the viewport? 

@Aa

PEEQ is the total (integrated) plastic strain, PE11 is the plastic strain 11-component and so on.

Elastic strains are EE.

I have  drilling process between bit and rock and I want to make hole in rock which model damage can I use please I use concrete damage plasiticty but no fracture happen can any body help me please

How to find peeq at a particular node, I have analysed chip flip package and need to find strain in solder balls at node corners.

It helped me too

How can I see the values for elastic recoil and dog-boning? for example in case of stent simulation.