Applying Stress-Strain curve in Abaqus
Applying Stress-Strain curve in Abaqus
(OP)
Hi,
I would really like to clear this up I have some stress stain curve data as follows:
stress (MPa) %
0 0
567 0.0008
600 0.021
640 0.053
690 0.11
680 0.1022
Can I apply this data directly into Abaqus? It seems that the first values can not be zero. I have also defined a elastic modulus and Poisson's ratio.
Thanks
I would really like to clear this up I have some stress stain curve data as follows:
stress (MPa) %
0 0
567 0.0008
600 0.021
640 0.053
690 0.11
680 0.1022
Can I apply this data directly into Abaqus? It seems that the first values can not be zero. I have also defined a elastic modulus and Poisson's ratio.
Thanks





RE: Applying Stress-Strain curve in Abaqus
stress (MPa) %
0 0
567 0.08
600 2.1
640 5.3
690 11
680 10.22
RE: Applying Stress-Strain curve in Abaqus
0 0
567 0.08
Then define plastic behavior with curve from:
600 0.021
640 0.053
690 0.11
680 0.1022
But why does your strain drop at the last value?
RE: Applying Stress-Strain curve in Abaqus
Another piece of advice, make sure that you are inputting true stress-true strain curves, and not engineering stress-engineering strain curves. ABAQUS is designed to input the former, not the latter.
RE: Applying Stress-Strain curve in Abaqus
total strain : sigma / E
plastic strain : .002
elastic strain = total - plastic
Also for the true stress/trus strain I have found some information here, is this the correct procedure for converting engineering to true data?
http://www.drd.com/techsupport/eng_true_strain.htm
Thank-you for all you input and help.
P.S. sdebock, the drop off at the end is the fracture point, it would probably be better to leave this piece of data out.
RE: Applying Stress-Strain curve in Abaqus
And yes, leave out the fracture point, and website seems to give the correct formulas.
RE: Applying Stress-Strain curve in Abaqus
------------
See FAQ569-1083: Asking questions the smart way on Eng-Tips fora for details on how to make best use of Eng-Tips.com
RE: Applying Stress-Strain curve in Abaqus
Still need to clear one last thing about TGS4's comments
Can anyone shed some more advice on this and how this should be done in good practice?
Thanks
RE: Applying Stress-Strain curve in Abaqus
RE: Applying Stress-Strain curve in Abaqus
So these equations hold true?
total strain : sigma / E (at yeild point)
plastic strain : .002
elastic strain = total - plastic
RE: Applying Stress-Strain curve in Abaqus
So, you will have:
elastic strain = Yield Stress/E
plastic stain = total strain (the strain in your raw data) - elastic strain
Clearly the elastic strain is not necessarily exactly 0.002 if using the offset method to get Yield Stress.