×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

debonding-cohesive zone modeling - abaqus- traction separation element

debonding-cohesive zone modeling - abaqus- traction separation element

debonding-cohesive zone modeling - abaqus- traction separation element

(OP)
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

RE: debonding-cohesive zone modeling - abaqus- traction separation element

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.

RE: debonding-cohesive zone modeling - abaqus- traction separation element

(OP)
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!!!

RE: debonding-cohesive zone modeling - abaqus- traction separation element

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

I was referring to the v6.4 manuals.

RE: debonding-cohesive zone modeling - abaqus- traction separation element

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.

RE: debonding-cohesive zone modeling - abaqus- traction separation element

(OP)
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

RE: debonding-cohesive zone modeling - abaqus- traction separation element

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

For example you said

Quote:

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.

RE: debonding-cohesive zone modeling - abaqus- traction separation element

(OP)
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..."

RE: debonding-cohesive zone modeling - abaqus- traction separation element

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

RE: debonding-cohesive zone modeling - abaqus- traction separation element

(OP)
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.

RE: debonding-cohesive zone modeling - abaqus- traction separation element

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

RE: debonding-cohesive zone modeling - abaqus- traction separation element

(OP)
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!!!!

RE: debonding-cohesive zone modeling - abaqus- traction separation element

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.

 


RE: debonding-cohesive zone modeling - abaqus- traction separation element

(OP)
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!!

RE: debonding-cohesive zone modeling - abaqus- traction separation element

I did it in Standard. smile

RE: debonding-cohesive zone modeling - abaqus- traction separation element

(OP)
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.....upside down

RE: debonding-cohesive zone modeling - abaqus- traction separation element

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.

RE: debonding-cohesive zone modeling - abaqus- traction separation element

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:

[URL=http://www.zshare.net/download/tooth-py.html]tooth.py - 0.02MB[/URL]

Hope you like it!

RE: debonding-cohesive zone modeling - abaqus- traction separation element

(OP)
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...

RE: debonding-cohesive zone modeling - abaqus- traction separation element

Quote (lexarsmith):


"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.




RE: debonding-cohesive zone modeling - abaqus- traction separation element

(OP)
hi xerf, with the interface material of 0.01 thickness...

the initial increment time is 0.01 and also i put increment size as 1e-20.
Also the load is
time - load
0-0
0.5-5
1-10.25

but still i get the same error "too....increment"

the global seeding size is 2.

I also changed the meshing technique from SWEEP to the FREE meshing, but still the same problem....

RE: debonding-cohesive zone modeling - abaqus- traction separation element

Maybe you should try a finer mesh, a thinner interface part, just do not give up smile, mkay.

RE: debonding-cohesive zone modeling - abaqus- traction separation element

(OP)
Hi brep

how do you assemble the orphan meshes of two concentric cylinders? Why cant I use the assembly-constrain-coaxial to put the concentric cylinder's orphan meshes?

Thanks

RE: debonding-cohesive zone modeling - abaqus- traction separation element

Create a csys on each of the orphan mesh parts. Use an edge-to-edge assembly constraint (using the appropriate axis from the csys as te "edge")

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources