Logarithmic Strain
Logarithmic Strain
(OP)
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?
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?





RE: Logarithmic Strain
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."
RE: Logarithmic Strain
RE: Logarithmic Strain
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?
RE: Logarithmic Strain
RE: Logarithmic Strain
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).
RE: Logarithmic Strain
RE: Logarithmic Strain
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).
RE: Logarithmic Strain
RE: Logarithmic Strain
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.