In cohesive zone there are two types of tractions that cause the material to fail (normal & shear). Check the following documents:

Article Analysis of mechanical failure at the interface between grap...

Article Debonding Mechanisms at the Particle-Binder Interface in the...

In your geometry, the vertical joints will fail differently than the horizontal depending on your load application. I think the load is horizontal, then the vertical joints are failing due to normal tractions and horizontal due to shear tractions. Since normal traction reaches the limit earlier thus the joint fails, in horizontal joints stresses are not developing that much.

I would suggest applying different conditions for nominal tractions normal/shear. Also, you can vary the fracture toughness to delay the fracture in a specific direction.

Noman

Hi Alexander,

Instead of modeling a separate part of cohesive element, you can try cohesive surface method by defining contact constraint in interaction.

In ABAQUS, CZM approach can be used with either cohesive elements or cohesive surface methods. Both methods follow almost the same formulation with a traction-separation law. However, In cohesive elements, the cohesive constraints are defined at material points while in cohesive surfaces, these constraints are imposed at slave nodes. Compared with cohesive element method, cohesive surfaces improves the runtime of the analysis.

Hope it helps.

Regards,

Mohsen

For your simulation even if the mesh size seems small enough in the "teeth", it may be useful to have several layers of elements.

Mechanically speaking you should test with adding rounding to the sharp edges, with a proper mesh in the vicinity (on one tooth to compare), to prevent crack initiation. But is it possible in the current scale ?

Yours sincerely,

JF ANTOINE

Dear Alexander,

As others have said, I have good experience using cohesive surfaces.

You need to define an interaction "type=SURFACE TO SURFACE", then in the interaction properties you set "Cohesive Behavior", "Damage Initiation", "Damage Evolution" and "Damage Stabilization".

In the input file you should have something like this:

** INTERACTION PROPERTIES

**

*Surface Interaction, name=Cohesive

1.,

*Cohesive Behavior

4.22072e+06, 1.748e+06, 1.748e+06

*Damage Initiation, criterion=MAXS

1000.,10000.,10000.

*Damage Evolution, type=DISPLACEMENT

1.,

*Damage Stabilization

0.01

** INTERACTIONS

**

** Interaction: Cohesive1

*Contact Pair, interaction=Cohesive, small sliding, type=SURFACE TO SURFACE

sCohesive1, mCohesive1

Best Regards,

Nicolo'

Thanks for all responses :)

Ive tried varying the cohesive damage initiation and fracture energies but the results always end up with only very few elements/none deleting early in the simulation.

Nicolò Grilli thanks for the help, Ive experimented with the problem with cohesive surfaces so Ill try and use parameters similar to yours specified. I used cohesive surface interactions previously and the load/displacement results were encouraging.

My only concern was that the tensile loading applied at the ends of the joint leads to the interlocking teeth experiencing compressive forces; under these circumstances I have read that the cohesive surface wont enable stiffness degradation and eventual mechanical failure, that was my reasoning for using the element based approach.

Dear Alexander,

Not sure about your specific geometry, but you can set mixed mode failure in the interaction properties, so you can have failure with both traction and shear.

For instance:

1000.,10000.,10000.

in my input file means failure 1000 MPa in traction and 10000 MPa in the two shear directions. If you set these numbers to 1000 MPa, you will have failure in both traction and shear.

That means failure can take place also if you have compression + shear at the interface of your teeth.

Hope this helps,

Nicolo'

I'm not an Abaqus expert but my thoughts are that the problem is related to the sharp corners you are modelling. Here there is a sharp change from shear to tension. Maybe you should model a small radius to avoid this issue.

BTW an explicit colleague of mine told me explicit analysis is great as it always gives an answer. It might not be the right one, but you have an answer...

Andrew Main : using cohesive surface interaction I have modelled successfully also sharp corners, for instance, triple junctions in a polycrystal, where three cohesive surfaces describing grain boundaries meet at one point

I'll take a step back. Maybe Abaqus is indeed right, given the model that you built... What I mean by this is...

-- Are you sure failure should occur at every point of the interface? Do you have experimental data (from yourself or the literature) to expect that the interface should fail everywhere?

-- You should look at stresses at the interface without cohesive elements, i.e. a simple elastic analysis. Look at normal tensile stress and shear stress, as proxies for respectively Mode I and Mode II failure. What are the effect of the contractions due to Poisson's effect? Given the geometry, they may be important. Looking at these features should help you understand the problem.

-- Looking at your model and thinking about single-lap joint geometry, it seems that the vertical side of each teeth is subjected to a state of local tension at the interface and cohesive elements fail. On the horizontal face of the teeth, shear likely dominates and cohesive elements do not fail. Thus, to get complete detachment, you have to weaken Mode II behavior of cohesive elements. In particular, it seems that cohesive elements on horizontal faces are indeed activated, thus the problem is probably not about initiation but about propagation. You need to decrease the value of Energy Release Rate in Mode II (or, conversely, decrease the value of the crack shear displacement at failure).

-- Not all the vertical faces however fail. Why? It's an unloading mechanism. In the picture you show, you have pair of teeths still bonded along the shared vertical face, but with the other vertical faces failed. The bonded vertical interface is there because the tensile load is not sufficient to break it, and that is due to the fact that the load in those two teeth is decreased by the failure of the other two vertical faces (I hope it's clear, look at your picture to understand what I'm saying).

In summary, I suspect Abaqus may be right this time. You need to understand the physics behind the results you're getting.

Happy to discuss it further if you want.

Regards,

Luca

Ansys or Abaqus has cohessive or adhessive bonding option to be specified , when you define a contact surface. Based on details (Value of cohesive force) of allowable provided, tool shall decide (If contact force exceeds allowable), the contact pair between those zones, gets deactivated. This is a famiair practice used to simulate the delamination in layered composites as well.

As I've said I only know about Marc and Nastran. In these codes we don't use force or stress but cohesive energy. It's this that enables the gradual release behaviour. There are several models which can be used, the simplest is the bilinear where the loading increases until the adhesive opens by a critical amount. This stage is reversible. After we exceed the critical opening then the adhesive fails linearly, giving the area under the load/displacement curve as the cohesive energy (similar to fracture toughness)

Luca Di Stasio Thanks so much for your reply, I think youve helped me think about the problem a little more clearly.

I have experimental data that Im trying to replicate and use to guide future experiments based on optimising the micro-structure geometry

In many ways the simulation does resemble the testing as the joint seems to fail locally at the interlocking sites, although from in-situ microscopy of the interface it appears to occur initially once the features have become sufficiently bent and slide past each other (at the vertical faces previously in compression in the attached image), with the crack coalescing prior to rapid failure.This feature sliding is probably quite tricky to completely achieve in the modelling.

Based on your recommendations, I have lowered the shear damage initiation criteria as well as the fracture energy. The load-displacement curves are very similiar to the experiments. Although the model might not be completely replicating the real-life failure mechanisms it might be a suitable tool for guiding future experiments.