RE: solids vs. tshells If you have one element for one layer, I would think that a simple 1-pt brick element would be sufficient to obtain a 3D stress filed. The strain assumptions made by thick shell 5 are intended to allow many or even all layers of a composite to be modeled with a single shell element. However, if you want to use tiebreak contact between layers, you obviously cannot use the one element approach since you will need multiple element through the thickness to allow separation. If you have one element per layer, a 1-pt brick should be sufficient to give the overall section good accuracy. I can think of 2 cases where you might want to tie together thick shells. The first case when there is a lot of delamination, and you want reasonable bending stiffness in the layers after delamination. The other case is if you have many layers in a composite, and you want to model more that one layer per element. For example, you might model 4 or 8 layers in one element and then the next group in another element. Of course you would need to know ahead of time where delamination would occur so that you could have the tiebreak contact in the right place. lb 11/2/16 Ticket#2016102810000194 _____________________________________________________________ Automatic Tiebreak OPTIONs -9,-11 added in dev to incorporation temperature dependence to OPTIONs 9,11. tb added to Manual 3/28/19 _________________________________________________________ Simulation of delamination can be approached in different ways. 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 https://awg.lstc.com/tiki-index.php?page=QA+test+example+7. The target in this example using 1-point solids (hourglass type 2) of mat 161/162 (special license req'd). I don't like the example since each individual ply of the target is a single layer of 1-point solids. Generally speaking, this way of modeling doesn't render any bending stiffness in the individual plies. It's only by virtue of there being multiple plies being tied that bending stiffness is provided. That composite action is lost if the tiebreak contact fails. First of all, for modeling delamination, you'd need to model each ply with a layer of elements. 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., *contact_automatic_one_way_surface_to_surface_tiebreak with OPTION 6,7, or 9 (solids) or OPTION 8,10, or 11 (shells). 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 shown below. AUTO tiebreak, Cohesive, Comments OPTIONs 9,11 *MAT_138 ______________ __________ ______________________________ NFLS T peak traction in stress units SFLS S peak traction in stress units PARAM (def=1.0) 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) B-K law exponent (invoked when PARAM (XMU) < 0): n/a GAMMA default GAMMA is 1.0 but can be set to 2.0 Expressed in terms of the tiebreak variables: Displ. to peak traction = NFLS/CN (or SFLS/(CT2CN*CN)) Max displ. = ERATEN*2/NFLS (or ERATES*2/SFLS) << Check: Max displ. should be greater than displ. at peak traction http://ftp.lstc.com/anonymous/outgoing/support/EXAMPLES/small_mod_i.cohes138_vs_dycos_tiebreak.k This example compares 2 solids bound by a cohesive element to 2 shells bound by a tiebreak contact. Writes intfor (include s=intfor on exec. line) and if run on SMP, an atdout file. See the comments in the input deck. An example comparing tiebeak contact between 2 strips of solids to tiebreak contact between 2 strips of shells: http://ftp.lstc.com/anonymous/outgoing/support/EXAMPLES/modeI_sols_and_shls.tiebreak.k (uses automatic tiebreak OPTIONs 9 and 11) Mode I failure is simulated. For direct comparision of cohesive elements to DYCOSS tiebreak contact, see the secforc data created by http://ftp.lstc.com/anonymous/outgoing/support/EXAMPLES/compare_cohesive_to_tiebreak_from_tobias.k which uses mat_138 cohesive elform 19 elements in one case and tiebreak OPTION 9 in the second case to bond two strips of solids together. Mode I failure is simulated. 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 determine the status of the tiebreak surface by reading the intfor database into LS-PrePost and fringing the component labeled "contact gap". 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: http://ftp.lstc.com/anonymous/outgoing/support/EXAMPLES/modeI_sols_and_shls.tiebreak.k To create the intfor database, include the command *database_binary_intfor in the input deck, set the slave side contact print flag to 1 on Card 1 of the *contact_..._tiebreak, and include "s=fname" on the execution line. A couple of caveats: 1. 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 the State 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 is displayed. 2. 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 (see bugzilla 1378) nor can it be written to binout via BINARY=2 in *database_atdout. _____________ 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 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 GI_delam = energy dissipated by mode I delamination GII_delam = enegy dissipated by mode II delamination Above 3 values of G in atdout have units of energy, while the input variable ERATEN,ERATES have units of energy/area. 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. damage = value between 0 (no damage) and 1 (delaminated) mode_mix = mode mixity = deltaII / deltaI where deltaII is separation in the tangential 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 soas 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/support/EXAMPLES/mat_186_dcb.k (uses cohesive elements) http://ftp.lstc.com/anonymous/outgoing/support/EXAMPLES/modeI_sols_and_shls.tiebreak.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/support/EXAMPLES/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/support/PRESENTATIONS/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), 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/support/EXAMPLES/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.