Composite models
For shells of orthotropic/anisotropic materials, there are 3 coordinate systems to consider: global, element, and material. PSI in *ELEMENT_SHELL_BETA and the BETA angles in *SECTION_SEHLL affect only the material coordinate system. The element coordinate system is determined by the connectivity (N1toN2 is x; z is normal to the shell).
Regarding output, if CMPFLG in *database_extent_binary is 0.0 (default):
 d3plot database: stresses/strains are in the global coordinate system.
 elout file: stresses/strains in shells are in the element local coordinate `system (note the word "local" in the elout file).
If CMPFLG is 1:
 All stress and strain output for composite materials is in the material coordinate system.
Materials models dealing specifically with composites are:
22  composite_damage 

54,55  enhanced_composite_damage [1]  
58  laminated_composite_fabric [1,7]  
59  composite_failure(_shell, _solid)_model [1]  
114  layered_linear_plasticity 

116  composite_layup 

117  composite_matrix  
118  composite_direct 

161 

Notes:
 The paper "Crashworthiness Analysis with Enhanced Composite Material Models in LSDYNA  Merits and Limits", Karl Schweizerhof et al, 5th International LSDYNA User's Conference (1998) provides some insight into several composite material models in LSDYNA, including mat_54, mat_58, and mat_59. Per Klaus Weimar, Figure 2 in the paper has a typo (the value 0.3 should be 0.03).
 A set of examples that include mat_22 and mat_114 and which illustrate *integration_shell are assembled in sandwich.tar.gz The tar file contains the following:
 readme
 shell8.k
 shell8.lam22.k
 shell8.mat114.k
 solid8.k
 sandwich.gif
 See also notes in the text files sandwich_composites and orthotropic_materials.
 Stresses (and strains) will be written in the material coordinate system rather than the global coordinate system if CMPFLG (and STRFLG) is set to 1 in *DATABASE_EXTENT_BINARY.
 Delamination is dependent on sigzz and thus our shell elements aren't suitable for prediction of delamination (sigzz is zero for our shells). Mat_022 and mat_059, when used with solid elements, include a delamination failure criterion.
Mat_161 offers delamination prediction using solid elements. According to Al Tabiei, tied contacts with failure or tiebreaks don't properly represent the mechanics of delamination. Tiebreaks perhaps do offer a firstorder approximation of failure. Dr. Tabiei mentioned that use of tiebreaks will generally trigger a nonrealistic chain reaction of failure (an 'unzipping') which can be tempered with mass damping or stiffness damping.
Dr. Tabiei has developed his own micromechanicsbased composite material models which include delamination effects. None of these models are currently included in LSDYNA. Dr. Tabiei has developed a twoday short course on Composite Modeling which is given periodically at LSTC in Livermore. Consult www.lstc.com for a class schedule. Dr. Tabiei can be contacted at atabiei@aol.com to arrange for onsite instruction or consulting.  A number of references on modeling of composites can be downloaded from www.dynalook.com.
 For mat_58, the rate at which tensile stress decreases relative to increasing strain is dependent on ExxT, the strain at tensile strength. The greater the value of ExxT, the more gradual the stress decrease. See element 1 in m58.k .
For mat_58, the scalar quantity "effective strain" which is evaluated against the failure strain ERODS appears to be computed from 2 inplane normal strains and the shear strain. This is not equivalent to the "effective strain" available for output in LSPREPOST which is computed from the 6 global strain components. The 3 values of strain that go into computing the internally calculated effective strain for mat58 are available for output as extra history variables 10, 11, and 12 with 12 being the shear strain.
For mat_058 with rate effects, use mat_158.  Regarding what's available as extra history variables in mat_059 (shells)...
hist variable # variable name in subroutine "plastic strain" ef (tensile fiber mode) 1 ec (compressive fiber mode) 2 em (tensile matrix mode) 3 ed (compressive matrix mode) 6 efail 7 dam (damage parameter)  A model with single shell elements comparing mats 2, 22, 54, 55, 58, 59 are in composites (see allin1_ortho*.k).
jpd 12/2002
revised 3/26/03 (added note 5)
revised 6/25/03 (Tabiei contact info)
4/1/04 added note 8
5/13/04 add note about mat_158
8/24/04 added mat22 and mat58 as applic for solids (delamination)
23/01/05 restructured and prepared for www.dynasupport.com
9/24/09 links updated
11/28/11 link to jday/faq added