Delamination and Tiebreak Contact

Although the jury is still out, I think people are finding tiebreak contact to be less problematic than cohesive elements.

Section 3.5.1, "Composite Delamination", of the Modeling Guidelines Document (MGD), available under "Resources" at http://awg.lstc.com, offers some pertinent tips.


See also the example "Ballistic Impact on Composite Plate" at
http://awg.lstc.com/tiki/tiki-index.php?page=QA+test+example+7.

First of all, for modeling delamination, you'd need to model each ply with a layer of elements.
                                                                                                            
*contact_automatic_one_way_surface_to_surface_tiebreak with OPTION 6,7, or 9 (solids) One approach would be to model a layer of shell or solid elements for each composite layer and bond the layers with a tiebreak contact, e.g., or OPTION 8,10, or 11 (shells).

input variables in *mat_138 as follows:
Refer to *mat_138 for a detailed description of the behavior of tiebreak OPTIONs 9 and 11.
The input variables in *contact_automatic_..._tiebreak OPTION 9/11 correspond to the input variables in *mat_138 as follows:

*CONTACT 
*MAT_138          
Comments
NFLS
T
peak traction in stress units
SFLS
S
peak traction in stress units
PARAM
XMU
Pos = Power law; Neg = B-K law
ERATEN
GIC
Area under traction vs. displ curve; units of stress * length
ERATES
GIIC
Area under traction vs. displ curve; units of stress * length
CT2CN
ET/EN           
Thus CT = CT2CN*CN just as ET = ET/EN * EN
CN
EN
Units of stress/displ.  CN, if given, overrides default contact stiffness
n/a                 
UND,UTD         
Ultimate displacements not required; (calc from stiffness, peak traction, and energy release rate)

This correspondence and units are demonstrated by
http://ftp.lstc.com/anonymous/outgoing/jday/small_mod_i.cohes138_vs_dycos_tiebreak.k

For an example application of OPTION=9, see "Simulation of Ballistic Impact on Composite Panels", available by searching on "DYCOSS" at www.dynalook.com.

For OPTIONs 6 thru 11 of *CONTACT_AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE_TIEBREAK, you can fringe the failed tiebreak surface via the component labeled "contact gap" in the intfor atabase (*database_binary_intfor). 

The "contact gap" on the slave side of the tiebreak actually represents a damage value ranging from 0 (tied, no damage) to 1 (released, full damage).

Here is a test case: 
set the slave side contact print flag on Card 1 of the *contact_..._tiebreak, and include "s=fname" on the execution line.
http://ftp.lstc.com/anonymous/outgoing/jday/modeI_sols_and_shls.case1only.k

To output the intfor database, include "s=fname" on the execution line,  include the command *database_binary_intfor in the input deck, and set the slave side contact print flag on Card 1 of the *contact_..._tiebreak.

A couple of caveats:
Bug 8454 documents an issue of MPP exhibiting apparent "healing" of tiebreak damage in intfor.  In truth, the damage is just reset to zero when the surfaces exceed a certain separation. By toggling "Frin" to "XFrx" when fringing "contact gap" from the intfor data, the peak value through all time is fringed.  This would be adequate for visualizing the final debonded area.
To go a step further, I can delete or inactivate a range of states using theState button in LSPP.   Then, the fringe plot with "XFrx" invoked will only consider the active states and so the debonded area for the final active state First, total delaminated area and energies are written for each interface is displayed.
Ticket#2015031510000018 mentions an SMP bug that is triggered only when there are also non-tiebreak contacts present in the model and those non-tiebreak contacts are frictionless.   The bug is fixed in version dev/r96688 and R8.0/r96689.

An ASCII file for DYCOSS automatic tiebreak contact OPTIONs 9 and 11 is written by adding the command *DATABASE_ATDOUT (automatic tiebreak damage). LS-PrePost can read and plot the time history data in atdout. This was added for options 7 and 10 on 1/13/2011.
First, total delaminated area and energies are written for each interface followed by slave node data (damage, mode_mixity and stresses). *DATABASE_ATDOUT added to the User's Manual on August 6, 2012 (Tobias). Output of atdout is not implemented for MPP.

_____________ Begin description of atdout ___________________

The atdout file reports time histories of total delaminated area and energies for each tiebreak contact followed by slave node data (damage, mode_mixity and stresses).

_i or I refers to mode I (normal) separation of the interface
_ii or II refers to mode II (tangential) separation of the interface
if_id = interface ID
area_delam = delaminated area
damage = value between 0 (no damage) and 1 (delaminated)
The next 3 values are energies associated with delamination. These energies are zero prior to delamination.
Gtot_delam = total energy dissipated by delamination = GI_delam + GII_delam
Delamination is occurs when "damage" reaches 1.0. Damage begins to accumulate when the damage initiation displacement (function of failure stresses input by the user) is reached. As damage accumulates, the bond softens and stresses are relieved.
GI_delam = energy dissipated by mode I delamination
GII_delam = enegy dissipated by mode II delamination
mode_mix = mode mixity = deltaII / deltaI where deltaII is separation in the tangential suggested that a segment set be used to define the slave side (as opposed to a part ID) so that direction and deltaI is separation in the normal direction
sigma_i = stress in normal direction
sigma_ii = stress in tangential direction
Refer to *mat_138 for details.

_____________ End description of atdout ______________

See readme.intfor for information on visualizing locaton of delamination for certain automatic contact OPTIONs.

I recommend setting IGNORE=1 when using an automatic tiebreak.   Also, make sure segment/shell normals are oriented so as to point toward the opposing surface (for proper assessment of failure). Also, since stress is evaluated based on tributary area of each slave node, it is suggested that a segment set be used to define the slave side (as opposed to a part ID) so that only the segments in that segment set are considered in the evaluation of the tributary area.
                                                                                                          
As an alternative to tiebreak contact, 8-noded cohesive elements (modeled with a cohesive material model, e.g., mat_138) can be used to model the interlaminar bond between composite plys. See also notes in the text file "cohesive" (available on request).

Similar examples illustraing Mode I type bond failure are:
http://ftp.lstc.com/anonymous/outgoing/jday/mat_186_dcb.k  (uses cohesive elements)
http://ftp.lstc.com/anonymous/outgoing/jday/modeI_sols_and_shls.case1only.k  (uses automatic tiebreak OPTIONs 9 and 11
Or, for direct comparision of cohesive elements to DYCOSS tiebreak contact, see the secforc data created by http://ftp.lstc.com/anonymous/outgoing/jday/compare_cohesive_to_tiebreak_from_tobias.k                                                                                                            

Moreover, delamination is dependent on sig-zz and thus our common shell elements aren't well suited to prediction of delamination (sig-zz is zero in plane stress shell formulations). In v. 971, the exceptions are shell formulations with thickness stretch (25,26,27). These new 'thickness-stretch' shell formulations are still somewhat experimental and their application in successfully predicting delamination is, as far as I know, unproven. 

For more, see http://ftp.lstc.com/anonymous/outgoing/jday/shell_25_26.pdf from Thomas Borrvall.

General notes on shells with thickness stretch:
In v. 971, shell formulations with 'thickness stretch' are 25 (Belytschtko-Tsay, underintegrated), 
http://ftp.lstc.com/anonymous/outgoing/jday/squeeze_thickness_stretch_shells.k
26 (fully integrated), and 27 (triangular).
These formulations calculate a 3D stress state and use extra 'scalar' nodes to store 2 additional DOF for the linear variation of strain through the thickness (see Remark 7 under *section_shell and *element_shell_DOF, and *node_scalar in the 971 Users Manual).
Actually, the code will automatically create the extra scalar nodes if Card 2 of *element_shell_DOF is left blank.
IDOF in *section_shell must be set to 2 if triangular thickness stretch elements are present.  If ESORT is set to 1 in *control_shell, triangles assigned formulation 25 or 26 by the user will automatically be assigned formulation 27 by LS-DYNA (bug reported to Borrvall, 10/16/06).
For an example wherein shell formulations 25 and 26 are crushed in the thickness direction, see
http://ftp.lstc.com/anonymous/outgoing/jday/squeeze_thickness_stretch_shells.k

Material models especially suited to composite delamination when used with solid elements 
are mats 22, 59, 132, and 161/162.
Mat 161/162 requires a supplemental license fee paid to the third party developer. 

- J. Day