SOL 401, 402 true stress, allow element rupture

[wojtekmath]

Hello,

there was the options in sol 601:
- convert dependency to true stress,
- allow emelment rupture.

Is there something similar in sol 401 402? Do i need this options?

In my job i want to calculate how much force i need to bend a rod (look at attachment). I do it with sol 402. I use bilinear material E=210000MPa and H = 2000MPa (Plastycy module).
I wonder that the material is too simple and has to big mistake.
In results in some places i have 1200 MPa stress on rod. I wonder how to determine moment when elements rupture.
Should I use enginering stress-strain curve or true stress curve?
From enginering Stess-strain curve i have true strain but not true stress. So Where i can tell to program if srain is for example 30% then element rupture?

Thanks

 

[karachun]

For Engineering/True stress and strain check Multi-Step Nonlinear User’s Guide chapter SOLs 401 and 402 - Stress-strain measures to determine what stress-strain curve you should use. In nutshell it depends on your solver options.

Element rupture is not equal to actual material fracture mechanics. I do not recommend to use in in your case, this will only give you some nice picture but not precise results.

 

[wojtekmath]

Thanks for answer, you realy help me
I checked and:

1. TRUE STRESS-STRAIN
{log (True) strain, Cauchy stress} - This is the default choice if you select large strains
(PARAM,LGSTRN,1) in your model.
This is the STRMEAS=1 option in the NCLNTG bulk entry

2. EBGINERING STRESS-STRAIN
{Biot (engineering) strain, Biot stress} - This is the default choice if you select small strains
(PARAM,LGSTRN,0) in your model.
This is the STRMEAS=2 option in the NCLNTG bulk entry.

..and I made a test.
I drew 2 shaft lenght 1m diameter 20mm (solid mesh).
Firts shaft material: Elasto-plastic bilinear (E=210000 MPa, H=2000MPa initial yeald stress 300MPa, v=0,3)
Second shaft material: plastic with Function definition Stress-strain and I drew exactly the same what I have in the first material.

Constrains:
- fix on one side of the shaft

Load:
- Displacetements on the second side of the shaft 200mm (from 1m lenght become to 1,2m lenght)

Hand calculations stress: 697,14MPa !!!

Results:
- Log Strain
first shaft 659,48MPa ??????????????? i don't undestand
Second shaft 838,02 MPa and this is correct because program convert stress strain curve to true stress. (Hand calculation: stress*(1+strain)= 697,14 * (1+0,2) = 838,56MPa) For me it is OK.

- Biot strain
first shaft 694,62 MPa <- 2,52 MPa less than hand calculation
Second shaft 698,38 MPa <- 1,24 MPa more than hand calculation

My conclusion: Log strain wokrs only with plastic material!!!
Maybe for someone my post will be useful. What do You think about my test?