User login

Navigation

You are here

Crack propagation with automatic remeshing in ABAQUS?

Hello,

 

 

My aim is
to carry out calculation of 2D crack propagation with ABAQUS 6.6.

Section 11.4.3
“CRACK PROPAGATION ANALYSIS” is providing an overview of what the software can
do, and I must say I am disappointed, for two main reasons:

 

   
First,
the user has to define a path for crack propagation. But there is little chance
for this path to be known a priori...
I would have expected the use of a criterion which would determine the new
propagation direction at each increment, in other words the software should be
able to find incrementally the way for the crack...

 
 
Then
in the case of the path is not known in advance, an automatic remeshing is
necessary. But here again, I can not find an obvious way to automatically
remesh around the crack tip at each increment

 

My questions
are :    Is it possible to carry out a step by step crack propagation without
defining a crack path a priori AND to do automatic remeshing with ABAQUS 6.6?

                              If not, what other strategy does one have
to apply?

 

Thanks 

I haven't  used *CRACK PROPAGATION ANALYSIS before but there is at least one solution for your first problem in abaqus. You can use principle stress/strain criterion to fail elements during your calculation. You don't need to define the failure path in advance in that way.

I don't know the definite answer for your second question. I guess that two subroutines, one for remesh and one for user element should be combined to solve your problem in abaqus. 

 

 

iam,not getting .fil file after running analysis in abaqus cae, so iam not able to do post process in hypermesh,can u help me on this regard

De Xie's picture

As we all know that at the crack tip, the stress is singular.  As a result, the stress value will depend on FEA mesh size.  The finer the mesh, the higher the stress.  You will never get converged results using stress criteria.

For this reason, we should avoid using stress/strain criteria, though ABAQUS has this option. (I suspect ABAQUS on this).

Therefore, I developed ABAQUS UEL based on VCCT (DCZM) to study the crack propagation since they are mesh independent for crack problems.  If you are interested, you may read my papers for details.

1. Xie D and Waas AM, Discrete cohesive zone model for mixed-mode fracture using finite element analysis, Engineering Fracture Mechanics, 73(2006): 1783-1796.

2. Xie D and Biggers, Jr. SB, Progressive crack growth analysis using interface element based on the virtual crack closure technique, Finite Elements in Analysis and Design, 42(2006): 977-984.

3. Farahmand B, Saff C, Xie De, and Abdi F, Estimation of fatigue and fracture allowables for metallic materials under cyclic loading, 48h AIAA/ASME/ASCE/AHS/ASC Structures, Structural Dynamics & Materials Conference, AIAA-2007-2381. Honolulu, Hawaii. April 23-26, 2007.

To my understanding, simulation of the arbitrary crack propagation is still remained unsolved as one of the most challenging topics in solid mechanics.  Although, someone (or some FEA packages) have claimed their approaches are blah blah.., however, when you really touch it, you will know it is not as you expected.

So, my point view is that, at current stage, we still rely on our knowledge and experience to solve such problems.  For example, we should be able to identify our major concerns in a problem.  If we study a delamination in sandwich composites or debonding of a stiffener from the skin, we know the crack path (our concern) a prior. Therefore, we can put our interface elements along the potential crack path (our concern).  This is the practical way.  This requires engineering judgments and experiences. If we expect the FEA packages to give the right answers by simply pushing a button, we will definitely be disappointed (or despaired), even though some packages may have claimed they can do so. 

Profesor De Xie, i really have an issue, i'm afraid is because i don`t know much about abaqus, i want to model a crack growth in a polimeric material, cause the objective is to estimate the life time of a pipe, the thing is that im not sure if i`m modeling it right or how can i interpretated the history outputs of the contur integrals, what is the graphic saying

Dan Cojocaru's picture

The built-in capabilities of ABAQUS v6.6 for simulating crack propagation rely on a node releasing approach. Therefore, one cannot simulate directly arbitrary crack propagation via geometric representation of the crack surfaces (edges).

However, in context of LEFM frame, using ABAQUS Scripting Interface and with some programming effort,
one can code some remeshing algorithms and repeatedly investigate the results database and update the FE model to simulate arbitrary crack propagation.

Teng Li's picture

Dan,

Can you provide some related publications, if any, on the remeshing for crack propagation in ABAQUS? Thanks. 

hi

1)how can i apply crack propagation with abaqus and xfem method

2)how can i apply for example twelve crack increments of a = 3 mm .

Dan Cojocaru's picture

Prof. Teng Li,

Unfortunately, I am not aware of any publication describing how to implement arbitrary crack propagation in ABAQUS via remeshing techniques.

I know there has been much work done on using remeshing to simulate arbitrary crack propagation. For example, the work of people from Cornell Fracture Group is very relevant to this topic (FRANC2D/ FRANC3D). However, I could not find much on implementation using commercial FE software. Usually, researchers prefer to build their own FE software.

My previous statement was based solely on my personal experience with ABAQUS.

madhuks's picture

I have simulated crack propagation without specifying crack path a priori in ABAQUS. I did this by dispersing cohesive elements in a region. This was easiest way to do in a short time, may be still is. I got rid of artificial compliance effect by specifying still initial response in a bilinear traction separation law.  The predicted crack path was matching with experimental path very well.

Coming to your problem, if you want to simulate crack propagation with remeshing, then you may want to write a python script and predict crack kinking direction and re-mesh after every step (for a static probelm, if the problem is dynamic then in abaqus explicit). I have not done this but this might work, Please let me know whether I am right.

- Madhu 

Sprunger's picture

 Guillaume,

Abaqus has an add on product called "VCCT for Abaqus".  The VCCT add on was developed for Boeing and is available to Universities.  

VCCT for ABAQUS is an add-on capability to ABAQUS/Standard that allows brittle interfacial crack propagation due to delamination/debonding to be calculated using the Virtual Crack Closure Technique (VCCT). VCCT is a well-known public domain postprocessing and remeshing technique that provides progressive crack growth between bonded surfaces based on the fracture toughness of the bond and the strain energy release rate at the crack tip. VCCT for ABAQUS is based on patented technology licensed by ABAQUS that allows VCCT to be calculated at runtime rather than as a postprocessing exercise.

http://www.abaqus.com/vcct/

Hi,

 The latest version of Marc (2007r1) from MSC Software has automatic crack propagation options based upon VCCT for 2D. You can use automatic remeshing and get growth along a calculated crack growth direction. You input the initial crack tip, the fracture toughness and a crack growth increment and the rest is automatic.

For the case that you do know the crack path you can connect the parts with glued contact or MPCs and let the program figure out when to grow the crack. Also here you only specify the initial crack tip or crack front and Marc figures out automatically what to release. 

-Per

http://www.mscsoftware.com/products/marc_whatsnew.cfm

 

What you want (2D crack propagation with automatic remeshing so that
node release can be done in arbitrary directions) is possible,if you
write your own pre- and postprocessing code. I have done this and am
using this currently in my research. However, it is a rather involved
program. If you are interested in more details, contact me. I try to add an example image here, but I'm not sure if this works.

Dear Martin,

 

Sorry for this late reply.

Yes, I am very interested for details. Especially how to modify data in the database of ABAQUS at each increment, and not simply when the whole 

calculation is done. Please contact me directly at:

guillaume.parry@gmail.com

 

i would like to know how we can use remeshing code work , if don,t have any problem in sharing with me , as it will help me for my project. i am looking for crack propagation in dovetail attched of annular disc.

waiting for your assistance

prashantsharma8@gmail.com

thanks & regards

prashant

Gouse's picture

Hi,

I am trying to simulate crack propagation in ANSYS, I was using maximum normal stress criterion for propagation now after reading the above discussion I understood that its not appropriate. Can able to use any other way for simulating crack propagation in ANSYS.

I have tried with Cohesive zone modeling as well but I found its not working since my case is not interface delamination. I am simulating compression test on a brittle material.

Now I thought of adding another Fracture toughness along with max normal stress as fracture criterion. Can it be possible implement my new fracture criterion in ANSYS if yes how can I do that.

Regards

Gouse

IIT Madras 

Octavio A. González Estrada's picture

There's also the option to use XFEM for modelling the crack without remeshing. There are some approaches that have been discussed in this post: link

Surendran M's picture

how to simulate crack propagation in abaqus

Subscribe to Comments for "Crack propagation with automatic remeshing in ABAQUS?"

Recent comments

More comments

Syndicate

Subscribe to Syndicate