foam hardening data input format in Abaqus and LS-Dyna

[umud]

Hi,
I would like to ask if the foam hardening input data format for crushable foam models in Abaqus and LS-Dyna is the same as the one used for metal plasticity. In metal plasticity, I use the following format for hardening data:

effective plastic strain= total true strain - true stress/E
true stress = (engineering stress) * exp(true strain)

However, in Abaqus Getting Started manual section 12.9, there is an example (circuit board drop test) where foam hardening data (plastic strain and yield stress in compression (Pa)) is given. Plastic strain data is given from 0.0 to 10.0. I think this is volumetric strain as seen in Figure 12-7, I don't know if I have to input volumetric strain or effective strain.

Thanks in advance,
Umud.

[Jorgen]

The foam hardening input data follows a similar structure - see the manuals for the details.

I think it is common to assume that the Poisson's ratio is close to 0 for crushable foams, hence the plastic strain is the same in uniaxial compression and in volumetric compression.

[umud]

Ok but, I stil don't understand how plastic strain of a uniaxial compression test data can larger than 1. In Getting started manual Table 12-3, yield stress in uniaxial compression versus plastic strain is tabulated for values up to plastic strain=10.

[Jorgen]

There is no limit on how large the (true logarithmic) plastic strain can get. This is true even in uniaxial compression.

- Jorgen

[umud]

Dear all,
thanks to Jorgen and after some trials, here is how I succeeded to input the hardening data in the right way.

1) true stress is not equal to (engineering stress) * (1+engineering strain) or as in metal plasticity, because the volume changes in deformed state. Assuming the cross section of the crushable foam does not change in compression, true stress can be taken as equal to engineering stress.

2) Assuming again that the cross section does not change during deformation, plastic strain is equal to volumetric strain. Abaqus requires input of absolute value of the plastic strain. Be careful that the nominal strain is negative in compression in

plastic strain=ln(1+nominal strain)-true stress/elastic modulus.