Logarithmic Strain 1

[Capko]

Hello everyone,

I'm trying to obtain the strains from a model. I request the "E" variable into the .INP in order to do so but what I found into the ODB is the "LE" (logarithmic strain).

Does anyone knows why? Is there anyway to change between them mathematically?

 

[StefCon]

Hello,
I think LE refers to the true strain and not engineering strain. You see true stress, you input true stress and true strain. It seems good to see true strain.

21.1.2 Material data definition
"When giving material properties for finite-strain calculations, “stress” means “true” (Cauchy) stress (force per current area) and “strain” means logarithmic strain. For example, unless otherwise indicated, for uniaxial behavior epsilon = ln(L/L0)"


10.2.2 Stress and strain measures for finite deformation
"where L is the current length, L0 is the original length, and epsilon is the true strain or logarithmic strain."


E is "All strain components. For geometrically nonlinear analysis using element formulations that support finite strains, E is not available for output to the output database (.odb) file."

 

[Capko]

So, if I well understood, if I use non-linear geometry it's impossible to show the E ?

 

[StefCon]

I think so. But if you recall a stress-strain diagram with engineering and true values plotted, the difference between these curves is small at smaller strains. Perhaps this isn't really an issue in most cases?


LS-Dyna support page
"From engineering to true strain, true stress
First of all, you may check that your experimental data from a uniaxial tension test is expressed in terms of true stress vs. true strain, not engineering stress or strain.

True strain = ln(1 + engineering strain) where ln designates the natural log"


So for Rp0.2 the true strain is

et = ln(1+0.002) = 0.00199800

which is very close to 0.002.


What do you think?

 

[Capko]

Is very close, yes, but the problem is that I'm trying to compare two models and I can't if I only can obtain the LE instead E

 

[Dave442]

This is discussed in the Abaqus Users Guide:

Section 1.2.2 Conventions - Stress and Strain Measures
Section 4.2.1 Abaqus Standard Output Variable Identifiers - Strain Output

Total strain (E) is only available in geometrically linear analyses. For geometrically nonlinear analyses, you can output logarithmic (LE) and nominal strain (NE).

 

[Capko]

And why Abaqus do this? What are the advantages?

 

[StefCon]

LE is the true strain, the strain you would measure with a strain gauge. For measuring strain it should be advantageous.

Same thing with stress, it is the actual stress and not a "fake", constructed, stress.

You are comparing two models, correct? I agree that comparing two logarithmic values can be questionable but even if you could compare engineering strains it would be strange since your geometry is not linear (otherwise you would have E).

 

[Capko]

Ok, understood, but there is no way to compare the strains between a linear model and a non-linear model?

 

[StefCon]

How large are your strains? If they are low, it doesn't matter if they are logarithmic or not in my oppinion (I could be wrong).

If the strains are high or you have some nonlinear geometry behaviour then the model assuming linear behaviour could be incorrect.

What you could do to compare is to manually calculate strain by looking at displacement and original length of some chosen part of the geometry, or from section forces maybe.