Learning Forum

[Kyle]

Hi all, I am a new user of LS-DYNA software. I have a question about the output of LS-DYNA. Basically, I have used the software to do tensile tests numerically and I have an issue with output. My question is how to output the engineering stress/strain, and/or true stress/strain? And if the outputs are effective stress (von Mises stress) and effective plastic strain, how can I convert to true stress and strain and/or engineering stress and strain? Looking forward to hearing from you guys!

Many Thanks,

Kyle

[Kyle]

If you guys can give me a guide on how to set up output in Dyna software that will very much appreciate it !!!!!

[Andreas Koutras]

, the stresses and strains calculated in LS-DYNA and shown in LSPP are generally true stresses and true strains. The stress tensor components are written by default in d3plot. After you load d3plot in LSPP, you can fringe a stress component or the effective stress through the "Fringe Component" menu and you can plot element stress time histories through "History". Alternatively, you can include *DATABASE_ELOUT in your input to output the stresses of the elements specified through *DATABASE_HISTORY_OPTION. To write the (true) strain tensor components in d3plot and elout, you need to set STRFLG=1 in *DATABASE_EXTENT_BINARY.
To calculate the engineering stress, you just need to divide the applied force over the initial (undeformed) cross-sectional area. The engineering strain will be (L-Lo)/Lo, where L is the current gage length and Lo is the initial (undeformed) gage length. To convert between true and engineering stress and strain, you can use the well-known analytical relationships. You can search for them online.
LS-DYNA offers the option to extract the area of a part across a specified cross section by using *DATABASE_CROSS_SECTION. This returns the forces acting on the cross section, the current area of the cross section, and other quantities in the output file secforc (which can be loaded in LSPP). Dividing the cross-sectional axial force over the current area is a way to calculate the average true axial stress across the cross section. See the manual on how to anchor DATABASE_CROSS_SECTION to a local coordinate system.
I hope this helps.

[Kyle]

!!!
Great thanks for your responses!!! It really helps out for my current issue!
As your comments:
I have obtain the force and area simulation data to obtain the true stress;
I have obtain the element effective strain from elout
Then, to plot the true stress and strain data.
I think it is very correct way to obtain the data from simulations!
Again, Thank you so much for your help!!!
Kyle