×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Logarithmic Strain

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?

RE: Logarithmic Strain

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."

RE: Logarithmic Strain

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

RE: Logarithmic Strain

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?

RE: Logarithmic Strain

(OP)
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

RE: Logarithmic Strain

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).

RE: Logarithmic Strain

(OP)
And why Abaqus do this? What are the advantages?

RE: Logarithmic Strain

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).

RE: Logarithmic Strain

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

RE: Logarithmic Strain

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.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources