Modeling viscoelasticity in ANSYS

[mccasllo]

Hi,

I am trying to create a model of a polymer in ANSYS and I am having some trouble finding out how to get the Prony series or shift function for it. I have storage and loss modulus data for a single frequency as a function of temperature. I am wondering if this is enough data to find the Prony series and shift function for this material.

I found a .pdf file on this site explaining how to find a Prony series from dynamic testing data, but I'm afraid I haven't been able to extract a Prony series from my data. I attempted to solve the equations given in that .pdf file with the equation solver in Matlab, but I believe I have too many variables to get a real solution.

Any help with this problem would be appreciated.

Thanks a lot.

[Jorgen]

I assume that you are referring to the following document (http://polymerfem.com/forums/showthread.php?t=37).
The procedure described in that document can be used to convert from storage modulus and loss modulus to a Prony series.

In your case, however, you also need to know the storage and loss modulus as a function of frequency, for at least one temperature.

- Jorgen

[mccasllo]

Yes that is the document. Just to make sure I have this straight, I will need to use data points at N frequencies to solve for my coefficients. Is that correct?

I have some more questions. I have read that the WLF shift function can only be used at temperatures near the Tg of a material. The process I am modeling goes about 80 degrees below and 75 degrees above the Tg of the polymer I am modeling. If I get storage/ loss modulus data as a function of frequency at a single temperature, what temperature should I get it at? What should I use to shift the Prony series outside the ranges where the WLF shift function applies?

[NeiNastran]

What version of ANSYS are you using?

[mccasllo]

I am running ANSYS 11.0

[mccasllo]

I am again trying to model a viscoelastic material in ANSYS and I have some questions. Where do you specify G_infinity? I thought that it was just the elastic modulus but I get different results for my model after a long time with different TBDATA coefficients and the same elastic modulus. For example, with one set of coefficients I will get the fully relaxed stress to be around 1 MPa but with another set I will get the stress to be 3 MPa. What is going on?

I've since found out that the prony series specifies a reduction in the modulus over time, but I still am not sure how the long term modulus is defined in ANSYS.

[NeiNastran]

Hmmmm.....

Well have you check this yet:

http://www.ansys.com/customerportal/

[mccasllo]

I've found out the answer to my question so I will post it here for reference.

In ANSYS, the relative modulus terms specify what percentage of the modulus has the time constant associated with it. So for a material with the input paramenters:

tb,prony,1,1,1,shear
tbdata,1,1,5

100% of the shear modulus will decay with a time constant of 5, meaning that approximately 63% of the shear modulus will be gone in 5 seconds.

Any percentage of the modulus not accounted for in the input parameters will be taken to be the modulus at t = infinity, so for the input parameters:

tb,prony,1,1,1,shear
tbdata,1,.5,5

50% of the modulus will decay in 5 seconds leaving 50% as the shear modulus at t = infinity.

Hope this helps anyone struggling with a similar problem.

[NeiNastran]

Your posts are always appreciated!

[chiduk]

Hi every one..,
this is chidu
hey can any one tell the in prony equation where should be the shifting terms used..,weather in numerator or in denominator for ANSYS defined equation..,
Thank u all

[Jorgen]

Can you explain what you mean by "shifting terms"?

- Jorgen

[chiduk]

Hi jorgen..,

I have calculated shear modulus decay for reference temperature.., with no shift factor.., and now i want to calculate shear modulus decay for lower and higher temperature other than reference.., and i have to use a shift factor in exponential .. term of prony equation.., so that reference temperature curve will be moved accordingly..
i stuck up weather i have to use this shift factor in numerator or denominator..,
please help me..,
Thanking you

[Jorgen]

Most FE programs have built-in support for the WLF equation. All you need to do is to specify the required material parameters and activate the time-timperature superposition principle. Why do you need to worry about the nominator vs. denominator? Also, the nominator/denominator of what?

- Jorgen

[chiduk]

Hi Jorgen

Thanks for the reply.., ya i know all FE packages have built in support.. and i just want to explore the how the Prony series for shear modulus decay is been implemented.., and i know WLF constant and thus shift factors and relaxation times and prony constants (say upto 8 terms) and at reference temperature (say at 50 deg C) i calculated shear modulus decay by Prony equation which is exatly matching with experimental results.. and now.., i have to calculate shear modulus decay at lower (say 25 deg C) and Higher (say 75 deg C) such that results got by Prony series and Experiments should get matched .., what happens in FE packages means that all the calculation is done for reference temperature and for temperatures other than reference,, calculations are shifted by using these shift factors..,
So i just want to explore the things that how that shifting is going to be happened..,


Thanks a lot jorgen..
Chidu

[Jorgen]

Oh, I see. Sounds like a fine exercise.

The WLF equation gives the shift factor which is used to scale time. You can simply use the a factor to multiply the time (or characteristic times).

-Jorgen

[nandish.rv]

i am having problem in using ansys software.

my problem is uni-axial compression of solid rubber cylinder between two rigid plate. i have taken axisymmetric model and doine analysis. i have taken two rigid plates top and bottom, bottom plate is fully contrained and top plate is made to move and deform the rubber placed between two plates.

i am getting good loading curve matching with experimental results but not getting unloading curve. it is tracing the same path of loading curve.

here i have given the input file, if any changes has to made in unloading please suggest as early as possible

/PREP7
!*
ET,1,PLANE182
!*
KEYOPT,1,1,0
KEYOPT,1,3,1
KEYOPT,1,6,0
KEYOPT,1,10,0
!*
!*
MPTEMP,,,,,,,,
MPTEMP,1,0
MPDATA,EX,1,,179
MPDATA,PRXY,1,,0.49967
MPDATA,DENS,1,,0.00000094

!NEO-HOOKEN MODEL
TB,HYPE,1,1,2,NEO
TBTEMP,0
TBDATA,,59.6798,0.0000442458,,,,

RECTNG,0,40,0,80,
RECTNG,0,60,0,-5,
RECTNG,0,60,80,85,
FLST,2,1,5,ORDE,1
FITEM,2,1
AESIZE,P51X,4,
MSHAPE,0,2D
MSHKEY,1
!*
CM,_Y,AREA
ASEL, , , , 1
CM,_Y1,AREA
CHKMSH,'AREA'
CMSEL,S,_Y
!*
AMESH,_Y1
!*
CMDELE,_Y
CMDELE,_Y1
CMDELE,_Y2
!*
/UI,MESH,OFF
!*
!*
/COM, CONTACT PAIR CREATION - START
CM,_NODECM,NODE
CM,_ELEMCM,ELEM
CM,_KPCM,KP
CM,_LINECM,LINE
CM,_AREACM,AREA
CM,_VOLUCM,VOLU
/GSAV,cwz,gsav,,temp
MP,MU,1,.8
MAT,1
R,3
REAL,3
ET,2,169
ET,3,175
KEYOPT,3,9,0
KEYOPT,3,10,2
R,3,
RMORE,
RMORE,,0
RMORE,0
! Generate the target surface
LSEL,S,,,7
CM,_TARGET,LINE
TYPE,2
LATT,-1,3,2,-1
TYPE,2
LMESH,ALL
! Generate the contact surface
LSEL,S,,,1
LSEL,A,,,2
CM,_CONTACT,LINE
TYPE,3
NSLL,S,1
ESLN,S,0
ESURF
*SET,_REALID,3
ALLSEL
ESEL,ALL
ESEL,S,TYPE,,2
ESEL,A,TYPE,,3
ESEL,R,REAL,,3
LSEL,S,REAL,,3
/PSYMB,ESYS,1
/PNUM,TYPE,1
/NUM,1
EPLOT
ESEL,ALL
ESEL,S,TYPE,,2
ESEL,A,TYPE,,3
ESEL,R,REAL,,3
LSEL,S,REAL,,3
CMSEL,A,_NODECM
CMDEL,_NODECM
CMSEL,A,_ELEMCM
CMDEL,_ELEMCM
CMSEL,S,_KPCM
CMDEL,_KPCM
CMSEL,S,_LINECM
CMDEL,_LINECM
CMSEL,S,_AREACM
CMDEL,_AREACM
CMSEL,S,_VOLUCM
CMDEL,_VOLUCM
/GRES,cwz,gsav
CMDEL,_TARGET
CMDEL,_CONTACT
/COM, CONTACT PAIR CREATION - END
!*
!*
/COM, CONTACT PAIR CREATION - START
CM,_NODECM,NODE
CM,_ELEMCM,ELEM
CM,_KPCM,KP
CM,_LINECM,LINE
CM,_AREACM,AREA
CM,_VOLUCM,VOLU
/GSAV,cwz,gsav,,temp
MP,MU,1,0.8
MAT,1
R,4
REAL,4
ET,4,169
ET,5,175
KEYOPT,5,9,0
KEYOPT,5,10,2
R,4,
RMORE,
RMORE,,0
RMORE,0
! Generate the target surface
LSEL,S,,,9
CM,_TARGET,LINE
TYPE,4
LATT,-1,4,4,-1
TYPE,4
LMESH,ALL
! Generate the contact surface
LSEL,S,,,2
LSEL,A,,,3
CM,_CONTACT,LINE
TYPE,5
NSLL,S,1
ESLN,S,0
ESURF
*SET,_REALID,4
ALLSEL
ESEL,ALL
ESEL,S,TYPE,,4
ESEL,A,TYPE,,5
ESEL,R,REAL,,4
LSEL,S,REAL,,4
/PSYMB,ESYS,1
/PNUM,TYPE,1
/NUM,1
EPLOT
ESEL,ALL
ESEL,S,TYPE,,4
ESEL,A,TYPE,,5
ESEL,R,REAL,,4
LSEL,S,REAL,,4
CMSEL,A,_NODECM
CMDEL,_NODECM
CMSEL,A,_ELEMCM
CMDEL,_ELEMCM
CMSEL,S,_KPCM
CMDEL,_KPCM
CMSEL,S,_LINECM
CMDEL,_LINECM
CMSEL,S,_AREACM
CMDEL,_AREACM
CMSEL,S,_VOLUCM
CMDEL,_VOLUCM
/GRES,cwz,gsav
CMDEL,_TARGET
CMDEL,_CONTACT
/COM, CONTACT PAIR CREATION - END
/MREP,EPLOT
GPLOT
FINISH
/SOL
!*
ANTYPE,0
NLGEOM,1
PSTRES,1
NSUBST,800,3000,40
OUTRES,ERASE
OUTRES,ALL,-800
TIME,120
FLST,2,1,4,ORDE,1
FITEM,2,7
!*
/GO
DL,P51X, ,ALL,
FLST,2,1,4,ORDE,1
FITEM,2,9
!*
/GO
DL,P51X, ,UY,-40
/STATUS,SOLU
SOLVE
OUTRES,ERASE
OUTRES,ALL,-800

TIME,240
GPLOT
FLST,2,1,4,ORDE,1
FITEM,2,9
!*
/GO
DL,P51X, ,UY,0
/STATUS,SOLU
SOLVE

with regards,
nandish rv

[Jorgen]

Can you provide a stress-strain figure showing the experimental data and the model predictions?

- Jorgen

[nandish.rv]

thank for reply

here i attached an stress- displacement curve. and i know only bulk modulus of 2250MPa.

can you provide some method to find the other properties like shear modulus, youngs modlus and poissons ratio

[Jorgen]

Can you plot stress-strain instead ?

[nandish.rv]

Dear sir,

i have only stress - displacment and load-displacement graph, both are similar in shape.

[nandish.rv]

Dear sir,

i have only stress - displacment and load-displacement graph that is given by my guide, both are similar in shape.