Engineering Stress Strain to True Stress Strain

[MegaStructures]

Hello,

I'm trying to convert engineering stress-strain to true stress-strain using an Abaqus model and an iterative approach. I understand that up to the yield point engineering and true stress-strain is identical, up to the necking point they are similar and can be related by:

σ[sub]T[/sub]=σ*(1+ε)

(1)​

ε[sub]T[/sub]=ln*(1+ε)

(2)​

After the necking region this approximation cannot be used, because the stress state in the necking region is too complex and includes multi-axial stress states and high deformations. I have found several research papers that describe an iterative method to determine the true stress-strain properties from an engineering property graph [1][2][3][4]. However, these papers, appear to be missing small pieces of critical information needed to complete the process. I think I understand the method each paper describes, but I wanted to come here to get confirmation from someone else that has gone through this process before.

Below is how I understand this process:

[ol 1]
[li]Perform tensile test of coupon, obtain engineering stress-strain data[/li]
[li]Convert engineering test data to true data using equations 1 and 2.[/li]
[li]Correct true data after necking using power rule equation recommended by Callister to obtain preliminary true stress-strain graph[/li]

σ[sub]T[/sub]=K*(ε[sup]n[/sup]T)

(3)​

[li]Create tensile specimen in Abaqus[/li]
[li]Enter preliminary true stress-strain data into Abaqus (do not enter failure criterion)[/li]
[li]Perform tensile test in Abaqus, measure strain between two points in reduced section and total force[/li]
[li]Plot strain in reduced section and force, compare to engineering stress-strain graph[/li]
[li]Reduce or increase plastic material properties past the necking point by some uniform percentage based on results of test[/li]
[li]Repeat process until force-displacement results in Abaqus match experiment[/li]
[/ol]

Does this appear to match what others interpret to be the process? Should ductile failure criteria be entered? Should the material data be adjusted past the necking point by some uniform percentage as I propose? If so, what would be a reasonable way to determine that percentage?

Bonus Question: Does anybody understand the process to track a change in "gauge" length in Abaqus? Is there a way to set up a sensor between two arbitrary points?

References:

[1] K. S. Zhano and Z. H. Li, “Numerical analysis of the stress-strain curve and fracture initiation for ductile material,” Engineering Fracture Mechanics, vol. 49, no. 2, pp. 235–241, 1994.

[2] Y. Ling, “Uniaxial true stress-strain after necking,” AMP Journal of Technology, vol. 5, pp. 37–48, 1996.

[3] Hyeong Do Kweon, Eun Ju Heo, Do Hwan Lee, and Jin Weon Kim. A methodology for determining the true stress-strain curve of sa-508 low alloy steel from a tensile test with finite element analysis. Journal of Mechanical Science and Technology, 32(7):3137–3143, 2018

[4]Peter Matic. Numerically predicting ductile material behavior from tensile specimen response. Theoretical and applied fracture mechanics, 4(1):13–28, 1985.

“The most successful people in life are the ones who ask questions. They’re always learning. They’re always growing. They’re always pushing.” Robert Kiyosaki

 

[rb1957]

Engineering stress assumes no change in section, true stress is (as you've noted) based on the true (necked) area.

I don't know Abaqus but you need to implement "large scale defection" and material plasticity and model with 3D elements (20 node bricks ?)

another day in paradise, or is paradise one day closer ?

 

[FEA way]

In Abaqus you can use the built-in material calibration tool for that. Check the "Converting Engineering Stress-Strain to True Stress-Strain in Abaqus" post on Simuleon’s blog.

To automate such an iterative procedure you could use Isight (if you have access to it) or Python scripting with Abaqus.

 

[MegaStructures]

FEA way:

I believe (I could be wrong) that Abaquses tool uses the analytical approximations valid for pre-necking only.

I have access to, and know how to use, the python scripting interface. I really just don’t know how to adjust the stress-strain graph each iteration. I could use the power rule (equation 3) and adjust n based on the difference between ultimate strain in the experiment and numerical model, but that equation does have 2 constants K and n. That being said K appears to be an “intercept” and may be able to be set by matching the power equation to the necking stress, since there can’t be a discontinuity in the graph.

“The most successful people in life are the ones who ask questions. They’re always learning. They’re always growing. They’re always pushing.” Robert Kiyosaki

 

[MegaStructures]

I believe I have figured it out. The exponent in eq. 3 can be calculated by performing linear regression on the true stress-strain data in the plastic region (post-yielding, pre-necking) and then that value can be carried through to the post-necking region.

In the post-necking region a weighted value can be added to the power equation to adjust the scale of the slope.

A detailed explanation and more thorough equations are provided at the following link:

https://www.hindawi.com/journals/isrn/2011/656401/

“The most successful people in life are the ones who ask questions. They’re always learning. They’re always growing. They’re always pushing.” Robert Kiyosaki