Strain History of Model 2

[MegaStructures]

Is there a way to track the strain history of all nodes on a line and report when any node/elements plastic strain exceeds the limit strain? I would like to track strain around a weld line and use 5% strain as a limiting value.

“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

 

[FEA way]

Do you use Abaqus/Standard or Explicit for this analysis ? The latter offers special keywords for such purpose. In Standard you would likely have to use subroutines.

 

[MegaStructures]

I am using Abaqus standard at the moment. I want to find the exact moment the model reaches 5% strain, I was hoping I could request PE as a history output, but I suppose it is a field variable. My strategy right now is to request more iterations and manually advance the frames until I see the strain exceed 5%, but I was hoping there was a better way.

“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

 

[FEA way]

PE is actually a history output variable while PEEQ can be requested for both field and history output. The only problem here is how to monitor this output during the analysis and terminate the simulation automatically when a particular value is reached. That's what can be achieved with subroutines. I think that it will be easier to do it manually. If you request the history output of plastic strain for each increment, you will be able to precisely find a moment when 5% level is reached.

 

[MegaStructures]

@FEA way: I didn't realize I had to select sets to get PE as a history output.

A few more questions:

i) I noticed the time intervals are still limited to how many increments I have in the model, so am I really getting any more information by requesting a history output of PE vs. a field output? The field output shows me PE at each increment as well. How will I see precisely when 5% is reached.

Edit: Can history outputs be requested at a time interval much more frequent than the analysis interval? Therefore not significantly increasing the solution time, but providing a fairly uninterrupted recording of the plastic strain? How is the progression of the history value tracked between iterations, is it simply a linear interpolation from iteration to iteration?

ii) I have been researching the difference between PEEQ and PE and I still don't understand the difference. I'm using Eurocodes Part 1-14 Design Assisted by Finite Element Analysis and it requires the 5% strain limit; however, it of course doesn't mention whether equivalent plastic strain, or simply plastic strain should be used. Do you understand the difference between these two and able to ELI5?

“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

 

[FEA way]

You can use a different frequency setting for output instead of "Every n increments". There are also "Evenly spaced time intervals" and "Every x units of time" and "From time points" settings available. For these, you can choose the "Output at exact times" option.

Equivalent plastic strain is calculated from the components of plastic strain tensor (PE) in a similar manner as von Mises stress is obtained from the components of the stress tensor. You can find the formula in the literature.