## You are here

# Cohesive elements parameters

Sun, 2010-08-08 04:32 - parisa

Hi,

I am working a long time on using cohesive elements in ABAQUS but up to now my efforts have be unsucessful.

I want to use of cohesive elements with the following paramters:

Damage initiation: Normal stres= 1.9 MPa, shear stress= 6.2 MPa

Damage evolution: Mode I fracture energy= 0.5307, Mode II farcture energy= 0.6623

Could any body kindly let me know that what would be my model E/Knn, E/Kss parameters?

Thank you,

Parisa

»

- parisa's blog
- Log in or register to post comments
- 16169 reads

## Comments

## Re: Cohesive elements

Hi Parisa,

these both parameters are the slope of the elastic part of the material curve. Be careful that the elastic energy is much lower than the total energy, because if you put a very low E you will get problems. I will recomend you to use the following controls for the cohesive section:

*Section Controls, name=mikel_controls, VISCOSITY=0.001

As the convergence is hard to be achieved, this will help to improve it. Please, prove that the orientations of your cohesive elements are the correct. The second direction has to be perpendicular to the fracture plane in the 2D elements and in the case of 3D cohesive elements is the 3rd direction the one that is perpendicular.

Regards,

Mikel

## Cohesive element

Hi,

Thank you for your reply. Is it possible to enter that code in ABAQUS CAE because I do not know any thing about command

I always use of ABAQUS CAE.

Meanwhile, how to calculate the E values based on the values in my previous post?

Thank you,

Parisa

## Cohesive Element

Hi,

look on the help about the command *Cohesive Section and there you can see how to link the controls to the section. It is not difficult. I always type it directly in the input file. Otherwise you can get something undesired when you export the parameters. You can calculate the elastic energy for each mode as (Sigm_max)^2/E. I will recommend to choose a value of E so that the elastic energy is on the order of minimum 5 - 10 times the total energy, if you do not have any available data.

Regards,

Mikel

## Hi Parisa, The E value

Hi Parisa,

The E value does not have any relationship with the values in your first post. Actually, its value is calculated based on the Es(E value of solid element around it) and r(ratio of its elemental thickness to the characteristic length of solid element around it). E/r should be higher enough than Es to represent the un-crack material. According to our experience, if r>=100, E could be equal to Es. For more details, please see our published paper on cohesive element:

Z.J. Yang, X.T. Su, J.F. Chen, G.H. Liu, Monte Carlo simulation of complex cohesive fracture in random heterogeneous quasi-brittle materials, International Journal of Solids and Structures, 2009,46(17): 3222-3234

## E values

Hi, Thank you for that.

I have an orthotropic material with E1=12000MPa, E2=600MPa and I have used cohesive element 0.01*1mm in 2D modelling. What do you think would be the best En, Es?

I am now facing many numerical problem when selection E1=4000, E2= 5222.

Thank you,

Parisa

## Parisa , It depends the

Parisa ,

It depends the crack direction to choose E1 or E2.

r is the retio of cohesive element thickness to characteristic length of solid element around it. Therefore, the latter value should be provided.

mikel15186's suggestion could help on your numerical problem.

## E values

Xiangtin;

I appreciate your reply. The thickness of my element is 64mm so the dimension of cohesive layer would be 0.01*1*64mm.

I now use of En=4000, Es=5222; I don't know are these values ok or not?

Thank you,

Parisa

## E values

Hi Parisa,

in case you are not sure which should be the correct Ex values, set them to a very high value, for example 100000. In the cases I have studied, the most important parameter is the fracture energy, and the rest of the parameters are less important. The maximum stress is important, but only because it use to be proportional to the fracture energie. In my experience, the only thing you have to think about when setting the Ex is to make them high enough to make the material model coherent. The error introduced by higher Ex values is going to be much lower than other introduced by other hypothesis.

Regards,

Mikel