debonding-cohesive zone modeling - abaqus- traction separation element 1

[lexarsmith]

Could any one please guide me how can I simulate the debonding behaviour (traction sepration elements) of the two cylinder type models in ABAQUS. It will be a life saving help from you.
Thank you!!!!
Regards

 

[xerf]

If I am not wrong....
I think you have to code the user subroutine UEL to implement a CZM element.


Also, it might be helpful to take a look at
ABAQUS Analysis User's Manual ->7.9.3 Crack propagation analysis
for the ABAQUS built-in way to simulate surface debonding.

 

[lexarsmith]

Thanks...But I think there is a built in elements called "Cohesive elements" in abaqus 6.5 version. But, when I tried to use it I could not able to run the simulation.

Also, which version of the Abaqus manual, you are suggesting?? ABAQUS Analysis User's Manual ->7.9.3 Crack propagation analysis

Thank you!!!

 

[xerf]

Actually, you are right, they added the cohesive elements in v6.5.

I was referring to the v6.4 manuals.

 

[xerf]

Did you use the information
in :
ABAQUS/CAE user's manual (v.6.5)
21.1 Modeling adhesive joints and bonded interfaces

???

I built a 3 part model in 2D , actually 2 parts and
a the 3rd very thin used for the interface. I meshed the interface with 1 row of cohesive elements.

It worked without any problem.

 

[lexarsmith]

HI, I read ABAQUS/CAE user's manual (v.6.5) 21.1 Modeling adhesive joints and bonded interfaces. It works for the plain surface geometries (like sandwich type structures) but I want to use it for the concentric cylindrical type parts. In fact, I want to model the debonding behaviour of dental posts. If you have any idea, in this regard, please suggest me.
I have spent more than one month in this...but still could not.....
If you like, I can send you my input file.

Regards

 

[xerf]

If you could supply some details maybe you could get more help from this forum.

For example you said

But, when I tried to use it I could not able to run the simulation.

If it does not work , do you get some error messages ?

Is you model 3D or axissymetric ? What type(s) of element
do you use in your model ?
...and so on.

 

[lexarsmith]

The model is 3D. It is a dental post consisting of crown, core, post, cement and dentin. I want to see the debonding behaviour at the interfaces of post-cement-dentin. The materials are linear elastic, I am using Implicit (abaqus standard) method.

Due to the complicated geomtetries, I am using linear tetrahedral fine meshes. for the cohesive zone, i am assigning "cohesive elements" with traction separation method.

The error it says "...node number might not be correct for ... element..."

 

[brep]

What element topology are you using for the cohesive zone? How are you creating this mesh?

 

[lexarsmith]

Since my geometry is very complicated, I used free meshing with tetrahedral meshes.


I am using ORPHAN mesh (created from the already existing parts). COH3D8 is the element type I am uing on the cohesive zone.

 

[xerf]

Why are you using an orphan mesh, if you have modeled the parts geometrically ?

 

[lexarsmith]

IN the abaqus manual, it is said that you can introduce the cohesive elements either in orpahn mesh (for already exisiting parts) and for model the part. So, i have used the already exisiting part to create the orphan mesh.

Please help me in this regard!!!!

 

[xerf]

I accomplished two experimental analyses so far using cohesive elements one in 2D and one in 3D.

For modeling I used CAE , but I did not create orphan meshes, I just used the geometric parts. In this way is much easier to define the surfaces based on geometric entities.

In both case I used 2 parts separated by a small interface part.Thus, I modeled the interface as a thin separate geometric part.

In the 3D case I modeled 2 concentric cylinders ( 5 and 10 mm thick, respectively) separated by the interface part about 0.01 mm thick. I assigned a cohesive section to the interface part (response=Traction Separation, initial thickness=Use nodal coordinates).

For the main parts I assigned a different isotropic elastic material and ELASTIC, TYPE=TRACTION for the interface constitutive response:

** MATERIALS
**
*Material, name=Material-inner
*Elastic
210000., 0.3

*Material, name=Material-interface
*Elastic, type=traction
1000,200,200,0

*Material, name=Material-outer
*Elastic
300000., 0.3

I had to adjust the definition of interface material with the Keyword editor.

For the interface part I used "Sweep" technique for the meshing algorithm.

I constrained the interface part to the cylinders by creating surfaces and using the TIE constraint (i.e., 2 constraints).

Otherwise, nothing special.

 

[lexarsmith]

Thank you very much for the suggestion. I will try according to this and let you know.

By the way, you did it in Standard (Implicit) or in Explicit?

Thank you!!

 

[xerf]

I did it in Standard.

 

[lexarsmith]

for my case, it says "too many attempts made for this increment"......i just used three parts....one cylider is 1.5 mm diamter and 0.01 mm interface layer and 1 mm outer tapered cylinder.

*Material, name=Post
*Elastic
116000., 0.33

*Material, name=cohesive
*Elastic, type=traction
1000000,1000000,1000000
**i varied this 100000 ...from 1000 to this value....

*Material, name=Cement
*Elastic
22000., 0.35

also used the TIE constraints....

all the parts are meshed using SWEEP algorithm.

post element - c3d8r
cement element - c3d8r
cohesive element - coh3d8

seeding size - 2 unit

Please save me.....(-:

 

[brep]

Sounds to me like you need to look at the sweep direction (which implies the SC8R element orientation) in your thin geometric zone. If you are in V6.5 (as I suspect you are) then it is unlikely that you have the orientations incorrect.

A better technique (for v6.5... In V6.6 there is a very very easy way to do this with no need for orphan meshes!) is to use the manual mesh edit tools to extrude element faces normal to the underlying mesh, thus creating "layers" of wedge or brick elements. Assign the correct element type (SC6R / SC8R) and then assign the shell section to these. By the way, you'll make your life a lot easier if you create named sets for your cohesive layers...

BTW you should use the Tools-Query-"Mesh Stack Orientation" to ensure you have the elements oriented consistently!

Good luck. If you need more help I'd be happy to post a script to demonstrate some of what I'm talking about.

 

[brep]

If anyone is interested, I quickly generated the following python script. It is not all that refined, but a commented replay file. You can download it here:

tooth.py - 0.02MB

Hope you like it!

 

[lexarsmith]

Hi Brep

I was doing the same "orphan mesh" techniqu to generate the layers of cohesive elements. instead of shell elements SC8R elements i am using the cohesive elements coh3d8...it seems my mesh orientation is ok. but still i dont know what should i do.......not able to run the problem...

 

[xerf]

"too many attempts made for this increment"

Do you get this for the very first increment ?

First, you could try to adjust the time incrementation parameters, i.e. in the Step option:
- set the initial increment size to a small value, say 0.01
- set the minimum increment size to let say 1.e-9

Second, make sure the loadings (whatever their type is) are ramped and not applied instantaneously.

What do you mean by
"seeding size - 2 unit" ?
The global seed size ?
If is that, given that the cylinders are 1 and 1.5 mm thick,
then do you have just a layer of elements for each cylinder ? Actually I think so since you used SWEEP for each part.