Hello Ma:

Okay; modeling viscoelastic materials using Abaqus:

The easy way and I tried this method when modeling viscoelastic materials such as flexible polyurethane foam!

1- Go to materials in Abaqus and create it

2- Under General Menu; you can select density and add value, watch for units, also density is important if you are running jobs dynamically but not needed for quasi static equilibrium but I like to have there just for other reasons.

3- Under Mechanical select Elastic then Hyperplastic, then click on right side under test data and enter your stress strain data as Uniaxial (tensile OR compression) or Biaxial, or simple shear, the more data you have is better. Now, which is the best data type should you pick? I will answer you as the following; it depends on your application or testing! If your test is in tensile mode;  it is better to have uniaxial, if it is shear then use shear, if it is a combination such as torsion or bending, then use every single test you have but if I am in your shoes,  I will use one test data the beginning to make it simple. Then if you see response is not good, then I will start building more data test based on other loading such as shear, biaxial etc.

4- What we have so far is the elastic portion of the viscoelastic model, now to get the viscous part, you need to go to Mechanical, then Elasticity, and then go all the way down to viscoelastic. Under viscoelastic, you pick either time or frequency domain. IF you pick the time domain, then you need to enter for Prony or Creep or Relaxation. I usually pick Prony, and then you need to get G1, K1, Tau1 and G2, K2, Tau2 values from the following.

5- Get out of the Edit material box, and go directly to the material that you are trying to evaluate or calibrate; then right click on your mouse and click evaluate, then you will have several options to evaluate, you will not be able to evaluate if you material is not elastic or hyperplastic, otherwise it will give you an error message. Please refer to Abaqus menu on this step for more clarification. After evaluation, I like to pick up polynomial 2, then when you ready to calibrate or evaluate; Abaqus will give you G1, K1, Tau1 and G2, K2, Tau2 values. Get these values then go back to Step 4 and enter these values in the Prony series.

A question comes here why 2 or 3 polynomial, answer is; it is all depends on error required in the evaluation method. Again go to Abaqus menu on hyperplastic material evaluation method for more help.

Then you material is ready to go, you can confirm your calibration by correlating the computational method with experiments. If computational versus experiment sounded reasonable with not more 10% error, to me this is enough, if not then go back and either enter more elastic test data or pick different polynomial to fit your experiment better. The hard thing about this is that the first model is the hardest, but then when you capture behavior of the first model, every other model after that becomes so easy since you know what to do!!

I hope this will get you to start your modeling, let me know if you need further help and good luck!!

Best Regards,

Mohamed F. Alzoubi, PhD.

Dear Ma Ay,

one way to define your time-dependent viscoelastic properties in ABAQUS is to use UMAT subroutine where you can define your material behaviour with all related parameters.  

Please do not hesitate to contact me if you have any additional questions.

Regards,

Robert

thanks for replying but i still don't know hot to assign those material properties into abaqus

E0 = 6.5 kPa, E∞ = 4.3 kPa, ν = 0.5, τ = 15.4 s

i could assign the poisson's ratio into elastic property section and the relaxation time which is tau_i "as i think"

but i still don't know how to assign the instantaneous and equilibrium behavior into abaqus

i get "k_i prony" and "g_i prony" in the time dependent viscoelastic properties and i read about them in the documentation but i could not understand 

my work is based upon a previous paper.. and i should assign those material properties into my model but i don't know how

and i don't understand why i should use UMAT or something like this to assign the properties

please help me 

thanks

Hello Ma:

Okay; modeling viscoelastic materials using Abaqus:

The easy way and I tried this method when modeling viscoelastic materials such as flexible polyurethane foam!

1- Go to materials in Abaqus and create it

2- Under General Menu; you can select density and add value, watch for units, also density is important if you are running jobs dynamically but not needed for quasi static equilibrium but I like to have there just for other reasons.

3- Under Mechanical select Elastic then Hyperplastic, then click on right side under test data and enter your stress strain data as Uniaxial (tensile OR compression) or Biaxial, or simple shear, the more data you have is better. Now, which is the best data type should you pick? I will answer you as the following; it depends on your application or testing! If your test is in tensile mode;  it is better to have uniaxial, if it is shear then use shear, if it is a combination such as torsion or bending, then use every single test you have but if I am in your shoes,  I will use one test data the beginning to make it simple. Then if you see response is not good, then I will start building more data test based on other loading such as shear, biaxial etc.

4- What we have so far is the elastic portion of the viscoelastic model, now to get the viscous part, you need to go to Mechanical, then Elasticity, and then go all the way down to viscoelastic. Under viscoelastic, you pick either time or frequency domain. IF you pick the time domain, then you need to enter for Prony or Creep or Relaxation. I usually pick Prony, and then you need to get G1, K1, Tau1 and G2, K2, Tau2 values from the following.

5- Get out of the Edit material box, and go directly to the material that you are trying to evaluate or calibrate; then right click on your mouse and click evaluate, then you will have several options to evaluate, you will not be able to evaluate if you material is not elastic or hyperplastic, otherwise it will give you an error message. Please refer to Abaqus menu on this step for more clarification. After evaluation, I like to pick up polynomial 2, then when you ready to calibrate or evaluate; Abaqus will give you G1, K1, Tau1 and G2, K2, Tau2 values. Get these values then go back to Step 4 and enter these values in the Prony series.

A question comes here why 2 or 3 polynomial, answer is; it is all depends on error required in the evaluation method. Again go to Abaqus menu on hyperplastic material evaluation method for more help.

Then you material is ready to go, you can confirm your calibration by correlating the computational method with experiments. If computational versus experiment sounded reasonable with not more 10% error, to me this is enough, if not then go back and either enter more elastic test data or pick different polynomial to fit your experiment better. The hard thing about this is that the first model is the hardest, but then when you capture behavior of the first model, every other model after that becomes so easy since you know what to do!!

I hope this will get you to start your modeling, let me know if you need further help and good luck!!

Best Regards,

Mohamed F. Alzoubi, PhD.

Dr. Mohamed,

i am really grateful for your valuable answer

but i only have those material properties " time-dependent viscoelastic properties (E0 , E∞ , ν , τ ), where E0 is the instantaneous elastic modulus, E∞ is the equilibrium elastic modulus, ν is poisson’s ratio, and τ is the characteristic relaxation time"

i only have these properties from previous paper and i should  assign these properties only to my model

i don't have k_i or g_i but i have tau_i 

and to be honest, i don't know what is prony series 

so please can you tell me how to insert these properties

regards)

Hello Ma:

Since you have only four values; then go to Material and under viscoelastic; choose

Time domain - Prony Series

Then you need to fill for g_i Prony, K_i Prony and Tau_i Prony, in your case g_1, K_1 and Tau_1; Where

g_1,: Shear relaxation or shear traction relaxation modulus ratio; This value could be ration between  E0 and E∞, I am not sure!; just copy hyperlink below to confirm:

http://jmorw140231dbe:2080/v6.13/books/usi/default.htm?startat=pt03ch12s09s01.html#usi-prp-mechanical-elastic-viscoelastic-time

K_1: Bulk relaxation or normal traction relaxation modulus ratio, since you don't have this one, choose it as same as for g_1 above

Tau_1: Relaxation time, you have this one.

Also under same material; you need to select elastic, select Isotropic under Type, then select Instantaneous under Moduli time scale (for viscoelasticity) , don't check No compression and no tension, finally add Young Modulus, you should have this value and of course you have Poisson's Ratio!

BTW; Prony Series is used to simply simulate viscoelastic material, please refer to attached file for more details.

I hope this will get you started, let me know what happens after you try,

Best Regards,

Mohamed,

thanks a lot Mr. Mohamed

now i am able to insert all the values except for k_i and g_i

i dont know how to convert elastic modulus to a shear mdulus"g_i"

thanks

As an approximation and for Isotropic materials; use the formula

You should have at least elastic modulus for the material. If not ; refer to http://www.matweb.com/ to find out the modulus

and for shear modulus use equation:

G = E / (2(1+Nu)

Where G: Shear modulus

E: Elastic modulus

Nu: Poisson's ratio

for bulk modulus use

K = E / (3(1-2Nu)

Also, refer to attached file for a the reference.

Dr. Mohamed

i should get G0 and G-infinity from the first equation but how can i get g_i ?

and also i will get k0 and k-infinity from the second equation but how i will get k_i ?

thanks

Okay Ma:

To find g_i & k_i which is in your case and since you don't have the relaxation curve will be g1 & k1, it means you have 1 term of Prony series:

Prony Series is a series that used to simulate relaxation curve for viscoelastic materials such as tissues;

Therefore, for linear elastic isotropic material behavior;

G(t) = Go [ 1 - gi(1- EXp (-t/Tu) ]  ; 1 term 

at t = ∞ , G(t =∞) = G∞ = Go(1 - g1 (1 - EXP (-∞ / Tu)); EXP (-∞ / Tu) = 0, therefore,

g1 = 1 - (G∞ / Go)

Also

K(t) = Ko [ 1 - ki(1- EXP (-t/Tu) ] ; 1 term, same as above k1 = 1 - (K∞/Ko), usually the bulk modulus doesn't change with time as G∞ but you can calculate it to find the value.

Now, I hope this will be able you to solve it and get some good answer and share it with us.

Good luck and have a very nice weekend!

BR

Mohamed,

Dr. Mohamed,

from the following equation K = E / (3(1-2Nu)

i have E0 and E-infinity and i Need to get K0 and K-infinity

but the Problem is that the poisson's Ratio is 0.5 so when i Substitute for it, i get  K=E/0

how can i write this value into abaqus ?

thanks

Ma:

How did you measure the Poisson's ratio of 0.5??

I am simulating the tissue behavior on the cell level

and the human tissue is super viscoelastic

can i assume it to be 0.4999999 ?

Yes; use 0.48 or so, to make the math sounds right. Notice, from physics, when you replace Poisson's ratio with .48 or 0.5, you will end up with almost zero bulk modulus. This means, the material becomes very highly viscous with negligible elasticity characteristics. In another words, the material will behave as incompressible materials and pretty close to liquid's characteristics. Run the model with this assumption and I am pretty sure you will get good results, incase you didn't, try to use hybrid elements when you create your mesh rather than brick elements. But Don't use this till you use the first assumption above.

BR

Mohamed F.

Dr, Mohamed,

can you please try to insert those properties into abaqus and send a screenshot

i will assume E0 = 6.5 kPa, E∞ = 4.3 kPa, ν = 0.499, τ = 15.4 s), where E0 is the instantaneous elastic modulus, E∞ is the equilibrium elastic modulus, ν is poisson’s ratio, and τ is the characteristic relaxation time

i have been trying to work this out for 2 weeks but i can't

please help me with this

thanks

Hello Ma:

What error type do you get??

Mohamed,

too many attempts made for this increment

i tried to Play with the step time

but i still get the error

also i am not quite sure whether i inserted the correct material properties or not

Can you share with me the input file?

Mr. Mohamed,

this is the Input file of my model

i am trying to indent 30% of the hight of the box

Dear Mohamed,

i went through your valuable explanation on how to define G1, K1, Tau1 and G2, K2, Tau2 values  from evaluating the material by selecting a strain potential energy i.e. polynomial N=2.

in your explanation you have mentioned that Abaqus will give G1, K1, Tau1 and G2, K2, Tau2 values but, after evaluate my material I didn't find these values. it shows only D1, C10, C01 and so on. 

in contrast with the question that I asked you before, do you think is that necessary to add the viscosity in my problem? if yes for the glass or adhesive?

the glass and steel defined as purely elastic material and adhesive (sealant) defined as hyperelastic material.

thanks

__

Hi Everybody,

I am beginner in simulation for HDPE in ABAQUS.

I need tips for g(real), g(imaginary), k(real) and k(imaginary). How can abaqus generate values of these constants for me ?

your feedback is required.

Hi,

I got the same problem as Amin. I went through the guideline an end up with values for D1 C10 and so on. Does anyone know how to transform them into G1, K1, Tau1 ? Or is there another way to implement them?

_______________________

Thank you very much all of you. I am performing my experiments. I shall be asking more and more from you friends whenever I have an ask.

_______________________

Dr. Mohamed ,

The following link is not working. Is it possible for u to put it once again?

http://jmorw140231dbe:2080/v6.13/books/usi/default.htm?startat=pt03ch12s09s01.html#usi-prp-mechanical-elastic-viscoelastic-time

Thanks in advance

Interested

Thanks for this information.

Thanks for this information.

Thanks for this information. This information is very handy to model viscoelastic model in ABAQUS.

Hello . I'm a phd student in mechanical engineering department. I'm trying to model a human head model in ABAQUS. I have a huge problem with material model. I read all answers about viscoelastic modelling in ABAQUS but i couldn't find an answer. I have specific material values as G(0), G(inf), Beta and K. Those are short-term shear modulus, long-term shear modulus, decay constant and bulk modulus respectively. As you guess i need Prony coefficients. I read all the documentations, your answers, articles but i couldn't find the critical answer. i can calculate g(i) as Mr. Mohamed said but i couldn't calculate k(i). Can someone suggest me an idea please? Mohamed F Alzoubi Ma Ay

Mohamed F Alzoubi

_______________

I have relaxation test data for HDPE, I used the same method as you mentioned in first. After material evaluation of relaxation test data, abaqus says;

"No convergence for any order n for the viscoelastic shear test data."

What does it mean ?

Does it mean that data not correct ?

_______________

Good morning everyone, could someone help me with the development of Kelvin Voigt's model using ABAQUS? Thank you.

Trank you Tarkes Dora Pallicity , Do you know how I can access and start writing in UMAT? Do I need to install any program?