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

[rodicav]

Dear sunilbelli, Dear all

you have successful to modeling pmma with ansys?

what pmma material data you used for curve fitting for tb,prony and tb,hyper? can you suggest me where can I find material properties for this near Tg?
I have to simulate with ansys a similar model as you and I need to find material [properties for pmma near Tg 100, 110, 130, 150 degree.

Thank you,
Rodica

[rodicav]

How can I define DNF model in ansys?

where can I find more information about this.. this model appear in ansys multyphysics?

Thank you
R

[rodicav]

Hy,

I need material properties for PMMA at 100, 110 C - 130 C to can simulate with Ansys a structural with contact analysis.

Can you help me with this?
Thank you,

Ro.

[Jorgen]

The DNF model is a material model that I developed. It is commercially available as part of the PolyUMod (http://polymerfem.com/content.php?10-PolyUMod)library of user-material models.

I can run the necessary experiments for you. Send me a private message (http://polymerfem.com/sendmessage.php)if you want a quotation.

Thanks,
Jorgen

[jay_bkk]

Dear Jorgen,

I read your threads about PMMA behavior. I can run simulation in Ansys WB using Mooney Revlin constants but I need to get stress relaxation and viscoelastic flow with time. I even tried Prony series constants which is given in literature with shift function and run transient simulation but i never get viscoelastic flow with time. What is wrong with my simulation what I am missing.. PLease hlep me to figure this out. I am attaching all nonlinear properties of PMMA with Ansys boundary conditions. 430431432

[Jorgen]

The linear viscoelastic model that you listed should have given you a time-dependent material model (with creep/stress relaxation).
I do a lot of non-linear viscoelastic simulations using ANSYS WB and have not had that problem. I am not sure what went wrong in your case :(

-Jorgen

[jay_bkk]

The linear viscoelastic model that you listed should have given you a time-dependent material model (with creep/stress relaxation).
I do a lot of non-linear viscoelastic simulations using ANSYS WB and have not had that problem. I am not sure what went wrong in your case :(

-Jorgen

Here is the detailed version of my problem: Material PMMA (transparent acrylic)

1) Mooney model : C10= -.0303e6 C10 = 0.4503e6 d = 0 at 150 DC (reff: JOURNAL OF MATERIALS SCIENCE 40 (2 005)399–410) also used long range of constants using given equation in paper.
2) Prony model = TB,PRONY,matid,,9,SHEAR
tbdata,,0.09,1,0.02,10,.054,100,.07,1000,0.1,10000 ,0.2,100000,0.223,1000000,0.3,10000000,0.6,1000000 00
(reff: Lai, J., Baker, A. (1996), ”3--D Schapery Representation for Nonlinear Viscoelasticity and Finite Element Implementation,” Computational Mechanics, 18, pp. 182--191)
3) used static as well as transient analysis
4) Solution doesn't converge due to element distortion after certain deformation
5) Solution converges by using only Mooney Revlin model (but after I include Prony model element shows distortion)
6) Pressure I used 1 bar to 6 bars (Uni axial)
7) Used both frictionless and frictional contact pure penalty and augmented Lagrange
8) Both solids are kept deformable and also tried rigid mold in static analysis defining displacement BC
9) Simulated with and without temparature and shift functions
10) Updated stiffness each iterations
11) element solid 185 and solid 186 UP formulation and shape checking aggressive mechanical, dropped Mid side nodes and using midside nodes also.

Final result after trying all these options: only element distortion no convergence

I cannot use re mesh option as it have limitation about using models and elements

I expect help from you that how did you perform this kind of analysis and if you find any problem with my BCs and material please tell me.

Thank you

Jay

[Jobie.Gerken]

Jay, I haven't really studied the details of your problem, but I have a few quick comments. For the TBDATA command, you can only enter up to 6 values per line, so the command you give is invalid - issue a TBLIST command to see that the material constants are correctly entered. However, the constants are not likely to produce a good result as the relative moduli terms in the prony pairs should not add up to more than 1.0.

I suggest constructing a simple uniaxial simulation consisting of a few elements so that you can quickly validate that you are getting the desired results from your material model.

/batch
!---------------------------------------------------------
! Preprocessing
!---------------------------------------------------------
/PREP7

! Geometry and mesh
Lx=1
Ly=1
Lz=1
BLOCK,0,Lx,0,Ly,0,Lz
ET,1,SOLID185
KEYOPT,1,6,1
ESIZE,Lx/2.
MAT,1
VMESH,1

! Material
c10 = -.0303e6
c01 = 0.4503e6
c11 = 0
tb,hyper,1,,3,mooney
tbdata,1,c10,c01,c11

TB,PRONY,1,,3,SHEAR
tbdata,1,0.09, 1,
tbdata,3,0.02, 10,
tbdata,5,.054, 100,

!---------------------------------------------------------
! Solution
!---------------------------------------------------------
/SOL
ANTYPE,STATIC
NLGEOM,ON
NSUBST,20,20,20
OUTRES,ALL,ALL
cnvtol,f,1,1e-5

! Fix surfaces
NSEL,S,LOC,Y,0.
D,All,Uy,0.
NSEL,R,LOC,X,0.
D,All,Ux,0.
NSEL,R,LOC,Z,0.
D,All,ALL,0.

ALLSEL,ALL
NSEL,S,LOC,Y,Ly
D,All,Uy,Ly/5
TIME,1.0
ALLSEL,ALL
SOLVE

save
!---------------------------------------------------------
! postprocessing
!---------------------------------------------------------
/POST26,

nn=node(0,0,0)
en=enearn(nn)
ESOL,3,en,,EPEL,Y,TStrn_y
ESOL,4,en,,S,Y,TStrs_y

prvar,3,4

FINISH

[jay_bkk]

Thank you very much Jobie. Finally I could solve my problem with your suggestions.

Best Regards

Jay