Plastic Strain Data Input 2

[Grindhouse]

Hello All,

I am trying to input the plastic strain data into Abaqus for my aluminium material.

Now I know the Yield Stress is in MPa but what is the Plastic Strain value?

Is it the percentage of elongation?

Thanks for any help

 

[corus]

Strain has no units. It's elongation per length.

 

[PamCrash]

Since plastification starts above Yield stress the plastic strain at yield stress is zero

 

[Grindhouse]

Hi Gents,
Thanks for your responses.

The strain values I have are 0.001 in/in elongation.

For example, this is the data I have:

Stress (MPa) / Strain (10^-3 in/in)
0 / 0
12.0 / 0.219
26.0 / 0.417

and so on...
From graph, the yield point is around 380 MPa.
(First three points)

Stress (MPa) / Strain (10^-3 in/in)
380.0 / 5.40
390.0 / 5.61
396.0 / 5.80


My question is what format do I input this as into Abaqus which asks for both Yield Stress (understand this field) and the 'Plastic Strain'?

Is the above (5.40) style correct or do I extrapolate this i.e. 0.00540

 

[PamCrash]

plastic strain = total strain - elastic strain

elastic strain = stress / youngsmodulus

 

[mosgef]

you should have something like
*ELASTIC, TYPE = ISOTROPIC
(380e+06/5.4e-03), poissons ratio,
*PLASTIC
380.0e+06, 0.0
390.0e+06, (5.61-5.40)e-03
396.0e+06, (5.80-5.40)e-03
etc....

Both stress and strain need to be input in consistent units, so if your value of measured strain is 5.4e-03 at a measured stress of 380MPa, that's how Abaqus wants it.

 

[khalid20]

For which aluminum alloy??

 

[bkal]

You might need to consider if you need to use engineering or true values and what values do you have in the table, from memory I think that ABAQUS expects true values.