Elastomer modeling (Mullins effect)

[ebillaud]

Hi!

I am doing some research on nanocomposite modeling (polyurea+carbon nanotubes) in Abaqus. I evaluated the hyperelastic factors from experimental data (uniaxial load).
Now I would like to model the mullins effect, I tried to use the Abaqus tool but the curve doesn't match (the second cycle loading has the same shape as the first cycle unloading).

[img]mullins[/img]

Here is my model :

Material :
strain energy potential = Ogden order 3 (mu1=-10.57, mu2=1.71, mu3=21.42,alpha1=3.78, alpha2=4.39, alpha3=-6.87, Di=0)
Mullins effect (r=2, m=1, beta=1)

1 element (3D hybrid C3D8RH)

4 steps :
1 - load1 (displacement control = 150%)
2 - uload1 (stress = 0.0001)
3 - load2 (displacement control= 150%)
4 - uload2 (stress = 0.0001)

Curve : Nominal strain/stress S22

Could explain me why my stress/strain curve does not match the theory?

Thank you!

Emilien

[skacel]

Hi Emilien,

according to my opinion there is no mismatch in your calculation. I think that your FE results seems to be correct (at least in qualitative meaning) because for Ogden-Roxburgh model of Muliins effect the unloading curve is identical to subsequent loading curve.
BTW - how did you determine the mullins-model parameters (r,m,beta)?

Pavel Skacel

[ebillaud]

Hi Pavel,

Thank you for your reply!
Actually I didn't determine the Mullins parameters (I tried with different values, but the curve didn't change). But I think it is possible by evaluate the material from test data (load/unload data).
I attached a theoretical curve for the Mullins effect (I would like to model the cycle hardening in Abaqus).
So I would like the same kind of curves for every cycles. Any ideas???

Emilien Billaudeau

[skacel]

Hi Emilien,

1/ I am not very familiar with Abaqus - I use Ansys. I am sure that something must be wrong in your task, because the (unloading) curve should change when you change the (Mullins) parameters. This works OK in ANSYS and I am sure that this must work also in ABAQUS.
2/ The curves from AXEL products you attached in previous post are not theoretical, but experimental! For Ogden-Roxburgh model the unloading curve will be identical to subsequent loading curve.
3/ I do not understand what you mean by "cycle hardening". I think that the phenomenon described by Mullins-effect models is usually called "stress softening" and it reflect the reduction of stiffness dependent on maximum magnitude of previously reached strain (or energy density, etc.). It is usually not able to describe the little difference between cycle N and cycle N+1 with the same amplitude.

[ebillaud]

1/ The unloading curves changes with the mullins effect factors (but the second load always follows the previous unload). I would like to have the same kind of cycle (just an hysteresis lag to modeling the stress softening)
3/ I agree, the phenomenon is called "stress softening". Actually I would like modeling this effect (the reduction of stiffness with the cycles). Do you have any ideas?
Thanks

Emilien

[skacel]

Emilien,

1/ The second load will always follow the previous unload for Ogden-Roxburgh type of Mullins-effect models. The hysteresis cannot be described by this model. The hysteresis can be (partially) caused by the rate-effects (viscous contribution). You may need some visco-hyperelastic model with Mullins effect for this complex description.
3/ Some "continuous damage" model may help you for the stress softening associated with loading-unloading cycles with constant amplitude. However, this is not "Mullins effect", I think.

[ebillaud]

Maybe I should try with the Bergstrom-Boyce model with Mullins effect. Do you know how can I modeling it on Abaqus?

[skacel]

Yes - if rate-effects are substantial, BB model with Mullins effect may help you. Unfortunately I am not very familiar with Abaqus. I work with Ansys.

[Jorgen]

I agree. The BB-model with Mullins effect can be very effective (since I developed that material model it must be good )

I have developed a user-material implementation for the BBM model for both Abaqus and ANSYS, and it works great.

-Jorgen

[Ivasiev]

How would you implement it in Abaqus, is it integrate into the Hysteresis parameter? If so what are the constants determined from? A material I am working with has little documentation in terms of mechanical testing so I need to choose carefully which procedures I need to carry out.