Prony series and parameters ??

[eddydonc0]

Hello everybody,

My English is poor but I try to be understood.
My question is about *viscoelastic in Abaqus ?
I have a polyurethane to study (E=4Mpa and 55Shore A hardness). I just have the compression test in experimental. How to obtain information on its viscous behavior?
In Abaqus, the prony series is used. How to obtain a relation between E the elastic modulus and G the shear modulus in a creep test data to obtain the prony parameter?
What's excactly the shear test data in abaqus to determine the prony parameter?

Thank's for all the answer.
Eddy

[Jorgen]

Hi Eddy,

What kind of compression test data do you have? The easiest way to determine the Prony seriers is to perform stress relaxation experiments.

For polyurethane you can often assume that the material is incompressible and hence convert the Youngs modulus to a shear modulus by dividing by 3, i.e. mu ≈ E / 3

Best of luck,
Jorgen

[eddydonc0]

Hi Jorgen,

Thank's to the answer !
I use a test piece of diameter 29mm and heigth 13mm for the compression test. The information is the stress-strain curve ! The strain speed is constant !
I think that i can do a relaxation test !

Eddy

Ps : your website is excellent !

[marrpi]

Hello,

I am trying to do a stress-strain analysis of a polymer part and I would like to use the viscoelastic material model (in ABAQUS).

I think you can define viscoelastic material model by using one of these procedures:
- giving shear and/or volumetric creep and relaxation data.
- by direct specification of Prony series parameters.
- material subroutine.

Please correct me if I am wrong.

My question is: if you have experimental data from a tensile creep tests, how can you transform it in the coefficients required by ABAQUS?.

Is the following process correct?:

1.From the tensile creep test I get the instantaneous tensile modulus E(t)
2.Using the relation G=E/(2(1+poisson ratio)) I get the instantaneous shear modulus G(t).
3.The instantaneous shear compliance is obtained by J(t)=1/G(t)
4.The normalized shear compliance is obtained by j(t)=J(t)/J(0)

Thank you very much

[Jorgen]

Your 3 ways to define a viscoelastic material for ABAQUS seem right. But I don't quite follow your procedure to find the shear relaxation function from creep data. What do you mean when you say "Instantaneous tensile modulus E(t)"? To me the word instantaneous to specifies time=0.

Your step 1 and 2 are fine. But #3 is only true in the limit when the time goes to zero.

In general, you can obtain the stress relaxation modulus from creep data by solving a Laplace convolution integral, or through a numerical solution scheme. You should also know that ABAQUS can find the appropriate Prony series from experimental creep data for you.

Best of luck,
Jorgen

[marrpi]

Thank you very much for your answer.

I would like to comment some points about it. I made a mistake by using the term "instantaneous" :oops: , what I ment was E(t)=tensile modulus at any time (1 hour, 100 hours): E(t)=(test tensile stress)/(strain stress at time t)


And I was not trying to find the shear relaxation function. I am trying to define viscoelastic behaviour by specifying creep test data. The problem is that ABAQUS ask for shear creep data and I have tensile creep data, and I don't know how I can find what ABAQUS call normalized shear compliance (j(t)) and long term shear compliance from my test data.

I hope I have better explained my question now.

[Jorgen]

For many elastomers you can assume that the deformation response is incompressible, hence for these materials the shear compliance is 1/3 of the tensile creep data.

- Jorgen

[sana]

Hi I have a load displacement curve on a bony shell which I want to model using ABAQUS viscoelastic model.

Can the prony series coefficients be determined using the load displacement curve? If so how is it done?
If not what additional test data would I need?

[Jorgen]

The Prony series parameters can be determined from load-displacement data at different strain rates, but it is often easier to determine the Prony series from a stress relaxation test.

You can determine the actual parameters either using a built-in feature in ABAQUS, etc., or write your own conversion tool using Matlab.

- Jorgen

[littleabaqus]

Hi Jorgen!

I have a similar question about the topic in this post..
I am currently trying to model stress-relaxation behavior in Abaqus,
based on data received in the lab from a stress-relaxation experiment.
For the experiment, we measured the dimensions of a material, and
compressed it through a displacement that was a percentages of its
original thickness.

The results from the lab experiment have been analyzed, producing stress
vs strain curves off several different percentages, and also I was able to
determine the instantaneous and equilibrium moduli. My question is
regarding inputing this data into the viscoelastic material section. I have
already set everything up, and the problem I am having is with the
shear test data input. For my complience modulus I am using the value
of equilibrium/instantaneous modulus. And for the y values, I am dividing
the stress by the equilibrium modulus, and plotting it against the
appropraite time. I keep getting errors when right clicking the material
and trying to evaluate. It says the material failed, or test failed. My
y-values are negative, and the compliance modulus looks acceptable..
I'm think I have a problem with the y-value I'm using... Is the stress
divided by the equilibrium modulus for those points correct, or am
I missing something here?

Thanks, I really appreciate it!!

Best,
littleabaqus

[Jorgen]

Hmm, I think that you want to divide the stress with the instantaneous stress at the beginning of the stress relaxation (not the equilibrium modulus). That way your normalized stress starts from 1 and goes down towards 0.

- Jorgen

[balalam]

Hi,
I want to know why relaxation test is easier than creep test to determine the prony series ?

[Jorgen]

The reason is that the Prony series is a fit of a stress relaxation data.

[hyperboolic21]

Hi,
I am actually new guy with Prony model. I wanted to get my own experimental results and use curve fitting in ANSYS in order to get my Prony coefficients. let me know plz if the procedure is right!
1) Do a relaxation test (in my case in a specific temp)
2) Get two material parameters. (in ANSYS it should be K bulk modulus and G shear modulus. however, as you said before we can assume incompressible case and K=infinity, v=0.5; right?) so I should only get G or E from the relaxation test in each interval.
3) implement my G for different time intervals in ANSYS without caring about K (how can I define bulk modulus as infinity?)
4) get the best coefficients by curve fitting. and then I have my material model.
thanks,

[dxr456]

The Prony series parameters can be determined from load-displacement data at different strain rates, but it is often easier to determine the Prony series from a stress relaxation test.

You can determine the actual parameters either using a built-in feature in ABAQUS, etc., or write your own conversion tool using Matlab.

- Jorgen

Sorry to dig up an old post, but could you suggest how the Prony series parameters would be determined from load-displacement data at different strain rates?
I have previously performed stress relaxation testing to define viscoelasticity but it has given inaccurate results, so I am looking for alternatives and I have already performed load-displacement testing at a range of strain rates on my material.

[Jorgen]

Since a linear viscoelastic material model (when calibrated) will give different stress-strain curves depending on the applied strain rate, you can therefore also calibrate a linear viscoelasticity model to different strain rate data.

To do this you need to create your own calibration procedure (or use a piece of software that I will announce soon ...)

-Jorgen

[hyperboolic21]

hi,
can we model hysteresis effect by prony series? I mean does it include damping effect as well?
Mahdi

[Jorgen]

Yes, it can be used to model hysteresis and damping.

-Jorgen

[hyperboolic21]

Does any body know if the prony series is deduced from General Maxwell rheological model or…? If yes, could you please introduce me a reference how to get the stress over strain formula depending on spring stiffness and damping coefficients for specific number of branches? And if I wanted to get the damping and stiffness in each of the branches, how to do that with a test? (suppose that I have my prony coefficients as well)
Mahdi

[manfred]

Does any body know if the prony series is deduced from General Maxwell rheological model or…? If yes, could you please introduce me a reference how to get the stress over strain formula depending on spring stiffness and damping coefficients for specific number of branches? And if I wanted to get the damping and stiffness in each of the branches, how to do that with a test? (suppose that I have my prony coefficients as well)
Mahdi

yes, prony series is deduced from GM ! See attached PDF!

[hyperboolic21]

Thanks Manfred,
Actually I do not see any attachment here; but if you mean the PDF written by Jorgen how to get Prony series by relaxation test, I know that and it works. But now I do need the spring stiffness and damping coefficient of each branch not the Prony coefficients. I calculated the constitutive equation for General Maxwell on my own. I do not know how I can from that come to Prony formula for shear Modulus. If it is something new I would be pleased if you could attached it again or send it by email [com73499@stud.uni-stuttgart.de] to me. Thanks!
Mahdi

[manfred]

Thanks Manfred,
Actually I do not see any attachment here; but if you mean the PDF written by Jorgen how to get Prony series by relaxation test, I know that and it works. But now I do need the spring stiffness and damping coefficient of each branch not the Prony coefficients. I calculated the constitutive equation for General Maxwell on my own. I do not know how I can from that come to Prony formula for shear Modulus. If it is something new I would be pleased if you could attached it again or send it by email [com73499@stud.uni-stuttgart.de] to me. Thanks!
Mahdi

. . . sorry for not having send out the PDF. But what my pdf is showing is a system of rate equations build up by the PRONY parameters to enable to calculate the stress state when the strain is given (even as function of time).

[JosefZak]

Hello,
I have completing question to this subject.

Can anyone help me with the definition of a normalized spectra within CAE?

I'm using the "Prony series" as a material characterization.
"Prony series" (Content from the realaxation times, shear relaxation modulus ratio "Gi" and the tensile relaxation modulus ratio "Ki".

I have the computed viscoelastic spectra already from IRIS software, but Abaqus requires NORMALIZED spectra.

I'm not sure how to normalized the spectra.
I have three ideas:
1)Divide every ratio value from the original spectrum by highest value of spectrum ratio
2)Divide every ratio value from original spectrum by area under them. (In spectra plot)
3)Divide every ratio value form original spectrum by tensile modulus in zero or infinite time (E(0) or E(infinite))


The alternatives #2 and #3 works, but I'm not sure which is proper...

I didn't find answer in Manual...

Can anyone help me? I have done lot of effort to found the solve by my self, but without results...

If yes,
Thank you so much...

[Seun]

Hi all,

I have a similar problem to the previous post's. From reading them I thing I have a strategy for how to use my tensile (not shear) stress relaxation test data in ABAQUS to determine the prony series parameters but would just like to check the steps:

1) Obtain E_inf (long term tensile modulus) and convert to G_inf (long term shear modulus) using G_inf = E_inf/3 (as my material is incompressible i.e v = 0.5)
2) Convert G_inf to g_inf (normalised long term shear mod.) using g_inf = G_inf/G(0), where G(0) = E(0)/3 and E(0) is found by dividing the initial stress (at time =0) by the strain??)
3) Convert my tensile stress data at each time, t, to normalised shear relaxation modulus gr at time, t, (which is what ABAQUS requires) using the following: tensile_relaxation_modulus(t) = tensile_stress(t)/strain,
then,
shear_relaxation_modulus(t) = tensile_relaxation_modulus(t)/3,
and finally,
gr = shear_relaxation_modulus/G(0) ??

Thanks,
Seun