ANSYS material model for PMMA around its Tg

[sunilbelli]

Hello,
I am trying to model PMMA just above its glass transition temperature, around 110deg C. I plan to apply a pressure of 5-6 MPa on it at that temperature (for different holding times) and find out the strain.
Which material model should I choose?
PMMA is an amorphous polymer material and has a non-linear viscoelastic material properties. I dont have a whole lot of experience in polymer engineering but based on the reading I have done, I guess the Non-linear Prony model with Williams-Landau-Ferry shift function would be appropriate.
I just want to confirm if this is correct. Are there any other models available in Ansys 8.0 which I may have overlooked.
Any help would be appreciated.

Thanks.

[Jorgen]

The pressure that you are planning on applying is that hydrostatic or uniaxial? The material model that you mentioned sounds reasonable, provided that the strains are not too large. If the strains are larger than about 5 to 10% then you might want to use a more advanced and accurate model. Also, if you are only interested in one single temperature then you don't need to use a shift function.
Best of Luck,
Jorgen

[Armin]

Hi all,

I only want to mention that in ANSYS a "FINITE linear viscoelastic" model is implemented (from Holzapfel). Therefore you can combine viscoelasticity (TB,PRONY) and hyperelasticity (TB,HYPER). The range of strains is only limited through the hyperelastic modell you use.

[sunilbelli]

Armin,
I have tried combining viscoelasticity (TB,PRONY) and hyperelasticity (TB,HYPER). This is what I am doing to model the PMMA (just above Tg) in ANSYS.
I am getting creep curves (displacement vs. time) from a lab mate at a constant load at different temperatures just above Tg of PMMA(115, 120, 130 deg C). From these curves, I calculate strain, relaxation modulus, shear modulus and bulk modulus. shear modulus,G = E/2(1+v) and bulk modulus,K = E/3(1-2v) where E and v are the relaxation modulus and poisson's ratio at that temperature. I understand that the poisson's ratio changes with time at temperatures above Tg. Since I havent found any literature which gives me the values of change in poisson's ratio for PMMA at my working temperatures, a constant value of 0.375 is assumed.

I use these values of K and G in my ANSYS viscoelastic material model (material model-->viscoelastic-->curve fitting) to calculate PRONY CONSTANTS.

I also have stress-strain curves for PMMA at my working temperatures which I input in my hyperelasticity material model (material model-->hyperelastic-->curve fitting) to get parameter for the Mooney-Rivlin model.

Is my approach correct? Do you know anything about this? Am i putting in more information than necesary?

Would appreciate a reply.

Thanks,
Sunil.

[sunilbelli]

Jorgen
I am opening this old problem again..I never quite followed it up last time around. Are there any new thoughts/insights you would like to share about this problem.

Thanks,
Sunil.

[Jorgen]

Sunil,
You approach still sounds OK. The main thing you need to be careful about is that that strains are sufficiently small that the material still behaves in a linear viscoelastic manner.

Jorgen

[sunilbelli]

jorgen,
Thanks for a quick reply...
I have small strains most of the time...Which model is used if the strains are large? Later on I may have to work on some problem that have large strains..

Thanks again,
Sunil.

[Jorgen]

Predicting the large strain behavior is more challenging and will likely require a more advanced material model. I would use the DNF model (http://www.polymerfem.com/modules.php?name=User_Subroutines).

- Jorgen

[Armin]

Sunil, Jorgen

sorry I didn't see the reply last year...

I want to add some comments:

- Be careful using creep test data in the time domain to calculate the relaxation behavior in this way. As far as know thats only possible in the Laplace or frequency domain. In the time domain you have to evaluate a convolution integral, I think. As Jorgen mentioned, relaxation test data would be more straight forward.
- the "Holzapfel" model uses hyperelastic models for the elastic part. So the strains can be finte. Jorgen is right, saying that for finite strains the viscosity is not linear anymore. But in this model this is assumed in the sense that the viscosity is modeled with a generalized Maxwell model. This means viscosity is a constant and does not depend on any other parameter like strains, stress, strain velocities etc. Jorgen, do you agree?
- Using tb,prony and tb,hyper in ANSYS is correct to model such a behavior. There is no need to put in any other initial constants. This is done defining the constants for the hyperelastic law which represents the "fast load limit".
- Of course Jorgen is right that there are better ways describing viscoelasticity at finite strains...

Armin