Tek-Tips is the largest IT community on the Internet today!

Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!

Register Log in
  • Congratulations MintJulep on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!

Viewing delamination/ matrix cracking in Abaqus? 1

Status
Not open for further replies.
Mohcine

Mohcine

Mechanical
Joined
Dec 26, 2012
Messages
37
Location
US
After obtaining some results from impact simulation, how to observe the resultant delamination damage/crack damage, having inputted the resultant failure criterions like Hashin failure, Puck failure, and Interlayer damage (delamination).

Or will this be visible automatically by Abaqus.


My Supervisor suggest I study the stresses at each note and see the if that particular node failures or note by using the failure criterion.

This is will be time consuming...any help would be appreciated.


Thanks
 
Sort by date Sort by votes
Hi Mohcine,

Share some more details on how you are modeling this impact simulation:

- How are you modeling the composite plies? Solid or Shell? Layered elements (multiple plies in one element using a composite layup) or 1 element per ply?

- How are you using the Puck failure criterion? I know Hashin is available in Abaqus but Puck???

- How are you trying to capture "Interlayer damage"? VCCT, Cohesive Elements, Ply Stresses?

I should be able to help out here once I know more.

Regards



Firehole Composites
 
Upvote 0 Downvote
Section 31.5.6 in the Abaqus Analysis User's Manual will help. You will want to output MAXSCRT and QUADSCRT and see when those values reach a value of >=1.0 (failure initiation).

Firehole Composites
 
Upvote 0 Downvote
For Pluck failure criterion I used QUADSCRT similar to that I used for cohesive layer, but no results are obtained indicating any matrix crack....am i inputting in the wrong place? there are not much option available apart from MAXSCRT and QUADSCRT.

Thanks compositesFEAguru :)
 
Upvote 0 Downvote
Do I have to define a VUMAT? Is it possible to get the code from for puck and just input it in?

PS (ignore the attachment for the previous comment, I typed it unknowingly)

Thanks
 
Upvote 0 Downvote
Yes I am.....It is the only method mentioned in the paper i linked to earlier... How did they input the matrix cracking criterion? Any model you would recommended using in Abaqus ?

Thanks alot :)
 
Upvote 0 Downvote
If you want to use the Puck failure criterion you have two options:

1. Write (or obtain) a VUMAT. The output variables you view would be defined within the VUMAT and would have a SDV1, SDV2, etc. label.
2. Use a 3rd party software product for composite material analysis with Abaqus that contains the Puck failure criterion (an example would be Helius:MCT).

The Hashin failure criterion is integrated into Abaqus and has a matrix failure mode. You should read section 23.3.2 in the Abaqus Analysis User's Manual for details on how to define the Hashin failure criterion in your model and the output you should look at.

Firehole Composites
 
Upvote 0 Downvote
I have looked at the section you recommended reading...I modeled a 2D shell composite and defined the parameter for hashin and requested the relevant outputs (eg, HSNFTCT, HSNMTCRT,....) when I request a field output, the following errors causes the job to be aborted:

Output request hsnftcrt is not available for this option

When I remove the selection of HSNFTCT, HSNMTCRT, etc, the job runs fine until completed.
I tried using history output to and results just fine, however, they were in form of graphs which are of no particular good.

Any suggestion of how to overcome this?
As always, I can not express my gratitude enough for all your help thus far :).
 
Upvote 0 Downvote
Copy and paste the following keywords from your input file that did not run:

*Damage Initiation

Everything under **Output Requests
(I'm assuming you created this input file using CAE)

Firehole Composites
 
Upvote 0 Downvote
*damageinitiation, criterion=HASHIN, alpha=1
*damageevolution, type=ENERGY
*density
*elastic, type=LAMINA
*mass, elset="ASSEMBLY_IMPACTOR-1__PICKEDSET6_POINT MASS_"
*surfaceinteraction, name="HARD CONTACT"
*shellsection, elset=ASSEMBLY_PART-3-1_COMPOSITELAYUP-1-1, layup=COMPOSITELAYUP-1, composite
*rigidbody, refnode=ASSEMBLY_IMPACTOR-1_IMPACTOR-REFPT_, elset=ASSEMBLY_IMPACTOR-1_IMPACTOR
*rigidbody, refnode=ASSEMBLY_IMPACTOR-1_IMPACTOR-REFPT_, elset=ASSEMBLY_IMPACTOR-1_IMPACTOR
*shellsection, elset=ASSEMBLY_PART-3-1_COMPOSITELAYUP-1-1, layup=COMPOSITELAYUP-1, composite
*mass, elset="ASSEMBLY_IMPACTOR-1__PICKEDSET6_POINT MASS_"
*rigidbody, refnode=ASSEMBLY_IMPACTOR-1_IMPACTOR-REFPT_, elset=ASSEMBLY_IMPACTOR-1_IMPACTOR
*initialconditions, type=VELOCITY
*initialconditions, type=VELOCITY
*elementoutput, directions=YES
*elementoutput, directions=YES
*rigidbody, refnode=ASSEMBLY_IMPACTOR-1_IMPACTOR-REFPT_, elset=ASSEMBLY_IMPACTOR-1_IMPACTOR
*output, field
*output, field, numberinterval=30
*output, history, frequency=200
*Step, name=Step-1
*Step, name=Step-1
3 sec
*dynamic, explicit
*output, field
*elementoutput, directions=YES

***ERROR: OUTPUT REQUEST HSNFTCRT IS NOT AVAILABLE FOR THIS OPTION
***NOTE: DUE TO AN INPUT ERROR THE ANALYSIS PRE-PROCESSOR HAS BEEN UNABLE TO
INTERPRET SOME DATA. SUBSEQUENT ERRORS MAY BE CAUSED BY THIS OMISSION
*output, field, numberinterval=30
*elementoutput, directions=YES

***ERROR: OUTPUT REQUEST HSNMTCRT IS NOT AVAILABLE FOR THIS OPTION
*output, history, frequency=200
*contactoutput, cpset=CONTACT
*endstep
*surface, type=ELEMENT, name=ASSEMBLY_IMPACTOR
*surface, type=ELEMENT, name=ASSEMBLY__PICKEDSURF88
*surface, type=ELEMENT, name=ASSEMBLY__PICKEDSURF268
*surfaceinteraction, name="HARD CONTACT"
*surfacebehavior, pressure-overclosure=HARD
*boundary
*boundary, type=VELOCITY
*Step, name=Step-1
*dynamic, explicit
*contactpair, interaction="HARD CONTACT", mechanicalconstraint=KINEMATIC, cpset=CONTACT
*output, field
*output, field, numberinterval=30
*output, history, frequency=200
*endstep



P R O B L E M S I Z E


NUMBER OF ELEMENTS IS 3030
NUMBER OF NODES IS 3084
NUMBER OF NODES DEFINED BY THE USER 3084
TOTAL NUMBER OF VARIABLES IN THE MODEL 17469
(DEGREES OF FREEDOM PLUS MAX NO. OF ANY LAGRANGE MULTIPLIER
VARIABLES. INCLUDE *PRINT,SOLVE=YES TO GET THE ACTUAL NUMBER.)





THE PROGRAM HAS DISCOVERED 2 FATAL ERRORS

** EXECUTION IS TERMINATED **



END OF USER INPUT PROCESSING
 
Upvote 0 Downvote
You are a guru indeed :)....it worked, like magic. You sir, are my saviour. I'm finally making some serious progress in my dissertation.

Many thanks!
 
Upvote 0 Downvote
I spoke too soon.... The results I get from cohesive element are not good..the element gets extremely distored ( see the pic I have added, plz ), and the delamination is rather odd ( I add a pic of it
I modeled the cohesive element as COH3D8... the elastic properties (E/Knn, G1/Kss, G2/Ktt) i used 25 because the time increment was no taking very long. I tried 50 and 100 and the time increment just too hours to finish.

I used the surface tie constrain between the layers (eg the cohesive element and the composite plies) , I did not use the nodes tie constrain, although my mesh is the same for the cohesive element and the composite.

The other thing I defined but not sure about is , the "general contact" I applied (I included a pic of the setting)
Is it possible to model the cohesive layer as a 2D planar?
Any suggestions?

As always thank you for all your help.

ps using cohesive surface gave this results :Which are much more sensible
 
Upvote 0 Downvote
I managed to solve it :)...the problem was resulting from the partition on the cohesive element not being selected when I defined the surface tie constraint.

I have a question relating to viewing the results....
It is possible to view the delamination through all the layer at the same time?

I can view damage on each individual layers , no problem.

or if I copy and paste the pics for different layers on top of each other and use some "transparency" photo editor to try and view the over all damage from all the layers...is this a good way to do it?
 
Upvote 0 Downvote
You should be able to view just the damaged elements by creating a Display Group (Tools - Display Group). Select Elements under Item and Result value under Method. You can then adjust the type of ranges you want to see (for example all elements with DMICRT >= 1).

Firehole Composites
 
Upvote 0 Downvote
Not quite what I desired to get , but it is useful nonetheless :)
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

I
  • Question Question
Wear in abaqus
Replies
8
Views
15K
Rama27
R
D
  • Question Question
(ABAQUS) Earlier Failure and Unrealistic Cracking of Reinforced High Strength Concrete Beam Under Bending Simulation
Replies
4
Views
15K
Daniel_LEE
D
A
  • Solved
Applying Local Coordinate System for BC in Abaqus
Replies
1
Views
3K
FEA way
FEA way
jball1
  • Question Question
Accumulation of error in Abaqus Explicit?
Replies
4
Views
760
FEA way
FEA way
mj345
  • Question Question
Selecting the arcs in ABAQUS/CAE
Replies
2
Views
401
mj345
mj345

Part and Inventory Search

Sponsor

Back
Top