User login

You are here

cohesive zone modeling of interface fracture

Rui Huang's picture

It appears to me many have been struggling with various issues in cohesive zone modeling of interfacial fracture, despite the fact that it has been well established theoretically and has been demonstrated many times in various forms. A common question (which we share) is with the use of the cohesive elements implemented in ABAQUS. Apparently, the standard implementation of the cohesive traction-separation laws in ABAQUS differs subtly from many other implementations in literature. Of course, ABAQUS has the flexibility for customized implementation through user subroutines, but many may not go that way. For some industrially oriernted applications, we have tried to use the standard cohesive elements in ABAQUS with limited success. Attached is a conference paper in which we share our understanding from this experience. There remain many unanswered questions (mostly numerical), and we welcome discussions and sharing of both sucessful and unsuccessful experience.

This paper may be cited as: H. Mei,  S. Gowrishankar, K.M. Liechti, and R. Huang, Proc. 12th IEEE Intersociety Conference on Thermal and Thermomechanical Phenomena in Electronic Systems, 2010. DOI: 10.1109/ITHERM.2010.5501290.

AttachmentSize
ITherm2010.pdf355.73 KB

Comments

Laurent Champaney's picture

 I've just posted some comparisons on the same topic :

http://imechanica.org/node/7418

L. Champaney
LMT Cachan/ENS Cachan
France

Dear Dr. Huang,

Thank you for starting this discussion. I have had several questions on using cohesive elements with Abaqus. The documentation is a little vague in parts and a thread like will help several students and researchers alike. 

I have some questions on the applicability of cohesive elements in modeling bonded polymer specimens. I am modeling my experimental specimens (made of polycarbonate); it has two halves bonded at an interface using an adhesive (Weldon). Now, the interface also includes a crack (a/W=0.5). This specimen is subjected to Iosipescu shear. For this case I have some questions. 

1) Can I model the adhesive interface using cohesive elements?

2) I use a cohesive interaction between my two parts in Abaqus 6.9.1. Since this is a zero thickness cohesive element, I use a large elastic modulus value (about 10x) for my cohesive elements. Does this look reasonable?

3) Can I model both Mode-I and Mode-II interactions (two different cohesive laws) using cohesive elements in Abaqus and if so, how can I do it with Abaqus?

Let me know if I should provide more details of my model.

Thanks
Arun

Rui Huang's picture

Dear Arun,

I believe there are many who can answer your questions. I will start with my understanding (mostly theoretical and limited). Hopefully others can chip in to offer more wisdom.

 

1) Can I model the adhesive interface using cohesive elements?

Theoretically, yes.

 

2) I use a cohesive interaction between my two parts in Abaqus 6.9.1.
Since this is a zero thickness cohesive element, I use a large elastic
modulus value (about 10x) for my cohesive elements. Does this look
reasonable?

To define the constitutive behavior of the cohesive element, you need at least 5 parameters as described in the attached paper. Among them, the initial elastic stiffness (K) is a mysterious one. Little attention has been paid to its effect, perhaps partly because it lacks a fundamentally physical intepretation (unlike the strength and toughness). Past literature has suggested using a large value for the stiffness (as large as you want), most likely for numerical purposes. In addition, the K-values for the opening mode and shearing modes are often taken to be identical, which seems to be unphysical but simplifies the analysis of mixed-mode cracks.

 

3) Can I model both Mode-I and Mode-II interactions (two different
cohesive laws) using cohesive elements in Abaqus and if so, how can I
do it with Abaqus?

In ABAQUS, you can define the strength and toughness for mode-I (opening) and mode-II (shearing) independently, thus four more parameters. The interaction between mode-I and mode-II is govened by the criteria you choose for damage iniation and for damage evolution until final failure. There are several options for these criteria in ABAQUS. In the attached paper, we derived the mixed-mode strength and toughness based on one of the options.

 

Regards,

RH

Laurent Champaney's picture

Dear all

For bonded joints, one usually uses :

kn = (E/d), for normal stiffness

ks = (G/d), for secant stiffness

[E Young's Modulus, G = E/(2 (1 + nu) shear modulus, d thickness, of the adhesive]

This corresponds to uniform deformation in the thickness of the adhesive layers.

If you want to take into account nearly incompressible material, you can use:

kn = (E.(1+nu))/(d.(1-nu)(1-2nu)), for normal stifness

 please see :

- http://mms.sagepub.com/cgi/content/abstract/4/2/201

- http://dx.doi.org/10.1016/S0020-7683(99)00072-4

for detaiis.

 

L. Champaney
LMT Cachan/ENS Cachan
France

Dr. Huang and Dr. Champaney

Thank you for your earlier comments and valuable suggestions. Using thickness for an adhesive is a somewhat of an issue in finite element modeling. Can you comment on the following questions?

Is it reasonable to assume a thickness for an interfacial adhesive in cohesive calculations? Usually, it becomes diffcult to ascertain the actual thickess of the adhesive experimentally. It could be of the order of micrometers.

How much will an error in adhesive thickness affect the output properties? If I use a thickness of several hundred micrometers instead of a couple of micrometers, will this significantly affect the model?(say, fracture properties)

Rui Huang's picture

This is a tricky question. ABAQUS allows one to use zero-thickness cohesive elements but asks for an artificial thickness to calculate the stiffness (K = Eh). On the other hand, I have seen others using finite-thickness cohesive elements, where the thickness and stiffness can be better defined physically. Theoretically I like to consider an interface as a zero-thickness layer with the constitutive behavior defined by the traction-separation relations. If a finite-thickness adhesive is present, the adhesive can be modelled as a solid layer of finite thickness along with its own mechanical properties (elastic or not). Practically, if the thickness of adhesive is small compared to the other dimensions of the model (e.g., beam thickness in a sandwich specimen), I think the zero-thickness interface model could be a good approximation.

RH

Dear Dr.Huang:

     Now i have a queston. If we use ABAQUS-UEL to implement the cohesive constitutive modeling instead of using cohesive module in ABAQUS, then how do we perform the post-processing since ABAQUS cannot acquire the calculation results using UEL. Thank you!

 

 

Rui Huang's picture

Dear Pengfei,

Unfortunately I have no experience using ABAQUS-UEL. Others may come to help. Typically I would think you can use UMAT instead of UEL to define the traction-separation relationship for the cohesive elements, for which the standard post-processing should work.

RH

Dear all

Is it possibe to extract traction-separation plot in abaqus6.8 without user subroutines.If yes please tell me how to extract this plot.

Thanks in advance

 

 

Regards,

Pradeep T

Rui Huang's picture

Pradeep,

The standard implementation of cohesive elements in ABAQUS allows one to define several types of traction-separation relationships. If you want to extract the traction-separation curve to check your result, you will have to output both the traction and the displacement of specific elements (or nodes). I never did this myself, but my student showed me similar plots.

RH

Dr.Huang

 

Is it possible to cut along cohesive element using a cutting tool. Is it possible to do withoout Umat?

Aliff Farhan's picture

Dear Dr. Huang & Dr. Champaney

I have some question to ask. Is it posible to write Abaqus subroutine for modeling cohesive zone model for strain rate & Number of Cycle depedencecies? As we know already, Abaqus is already implement temperature dependent for CZM in term of stiffness, critical fracture energy and etc.

 

Thanks

Aliff Farhan

Hi,

   i am using ansys to model cohesive zone at fiber matrix interface of a composite. I generated the mesh and solved it but i am facing convergence issues. Can u please guide me in this regard. Thanks.

I shall be extremely grateful

(nadeem_53@yahoo.com)

Liming Jiang's picture

when I'm simulating an interface with cotact 173 in ANSYS ,I got a problem. I used the CZM property when defining the properties of the contact elements, but I found it's not possible to use an absolute stiffness--ansys provides fkn to define the initial stiffness, and we can set fkn with a negative value ,which can be treated as an absolute stiffness in the calculation. But the problem is that the initial stiffness (an absolute one) would not change even if the debonding happened.

so, how to define the absolute stiffness(not a factor) when considering the debonding of the interface

mystar_bkc10's picture

Nguyen van Hoan Viettel R&D 380 Lac Long Quan, Ho Tay, Ha Noi, Viet Nam. HandPhone: +84 976 190428 Yahoo: mystar_bkc

 

Dear Liming Jiang !

I saw that you did CZM in Ansys Multiphysic, i am trying to model it but i havent done even though i tried to follow Help !

pls, guide me in detail how to make CZM in Ansys multiphysic as the problem i posted before :

http://imechanica.org/node/11669#comment-17970

Thank so much

Dr.Huang,

Is there any existing cohesive zone model with temperture dependence property? I have to include a cohesive zone between my two parts, which are not of geometry composed of simple lines but of collection of line segments and curvature. Also I must use dynamic thermal mechanical explicit mode in abaqus. Thanks.

Hi,
I'm newborn in ABAQUS. I want to make a static analysis of RC frame with the
bondslip effect after apply cyclic loading to the frame.

At the moment,I tied the reinforcement bars with the concrete. And manage to
plot hysteress curve of the frame. what I'm aspect was degradation of stiffness
and perhaps I can see pinching behaviour in the hsteresis curve which is not
happen to the current plot.
Detail of my model;
1.2D beam model (beam element for beams and column, truss element for
reinforcement bars)
2.Concrete damage plasticity-concrete model
3. Have inlude damage material properties to concrete and steel.

Hope to get help from you all.

Regards,Ayda

Dear friends,

 Could you please let me know how I can assign section to the adhesive of type traction separation law with zero thickness?  as, it wants me to select a section, while we have no surface for the cohesive zone, but only have line between two surfaces.

 

thanks,

ehsan

Respected All,
 I have written a code for a beam element to solve problem of stress analysis of beam by using inbuilt B21 element.After that I have made necessary changes in the input file to run the code but it is aborted.Following UEL property is assigned in my input file E=1e6,I=108,P=10,Ymax=3. the error is coming when i click on plot contours on deformed shape in visualization mode"There is no valid step data available on the database.if the analysis is running the database must be closed and reopened once the requests have been initialized.The request operation has been cancelled."

 

Subscribe to Comments for "cohesive zone modeling of interface fracture"

Recent comments

More comments

Syndicate

Subscribe to Syndicate