Create Presentation
Download Presentation

Download Presentation
## modeling of composites in ls-dyna

- - - - - - - - - - - - - - - - - - - - - - - - - - - E N D - - - - - - - - - - - - - - - - - - - - - - - - - - -

**1. **Modeling of Composites in LS-DYNA Some Characteristics of Composites
Orthotropic Material Coordinate System
User-defined Integration Rule for Shells
Output for Composites
Some Characteristics of Several Composite Material Models in LS-DYNA
Closing Recommendations

**2. **Two General Classes of Composites Advanced composites have stiff, high strength fibers bound in a matrix material.
Each layer/lamina/ply is orthotropic by nature as the fibers run in a single direction.
Usually, an advanced composite section will have multiple layers and each lamina within the stack will have the fibers running in a different direction than in the adjacent lamina.
A sandwich composite section has laminae which may be individually isotropic but the material properties and thickness may vary from lamina to lamina.
A foam core composite is a particular type of sandwich composite where a thick, soft layer of foam is sandwiched between two thin, stiff plies.

**3. **Orthotropic Materials in LS-DYNA Orthotropic material constants are defined in the material coordinate system.
The material coordinate system must be initially established for each orthotropic element and, in the case of shells, for each through-thickness integration point as well. This orientation comes from three sources.
In the material definition (*mat)
See description of “AOPT” in User’s Manual under *mat_2 (orthotropic_elastic)
In the section definition (*section_shell)
A “beta” angle is given for each integration point
Optionally, in the element definition (*element_shell_beta, *element_solid_ortho)

**4. **Orthotropic Materials in LS-DYNA
As the solution progresses and the elements rotate and deform, the material coordinate system is automatically updated, following the rotation of the element coordinate system.
The orientation of the material coordinate system and thus response of orthotropic shells can be very sensitive to in-plane shearing deformation and hourglass deformation, depending on how the element coordinate system is established.
To minimize this sensitivity, “Invarient Node Numbering”, invoked by setting INN = 2 (shells) or 3 (solids) in *control_accuracy is highly recommended.

**6. **With Invarient Node Numbering(based on element bisectors)

**7. **User-Defined (Through-Thickness) Integration Gaussian or Lobatto integration rules have pre-established integration point locations and weights (NIP <= 10).
Lobatto includes integration points on the outside surfaces
Trapezoidal integration has equally spaced integration points.
For composites, the user may need to define his/her own integration point locations and weights (corresponding to ply thicknesses) and may need to reference a different set of material constants for each integration point.

**8. **User-Defined Integration (970)

**9. **User-Defined Integration (971)

**10. **Output for Composites
For composite material models, 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.
Useful option for postprocessing of fiber and matrix stresses.
Set MAXINT in *database_extent_binary to the total number of through-thickness integration points in your composite shell. By default, stresses only at the top, bottom, and middle integration points are written.

**11. **Output for Composites
Some composite material models have “extra history variables” that help to track modes of failure in each integration point. (See material documentation in the User’s Manual for details.)
NEIPS (shells) or NEIPH (solids) in *database_extent_binary should be set to the number of extra history variables needed.
For example, if you want to track the damage parameter (6th extra history variable) in mat_054, set NEIPS to 6.

**12. **Composite Material Models
*mat_2 (elastic_orthotropic)
9 elastic constants (solids); 6 elastic constants (shells).
Total Lagrangian formulation (okay for large elastic deformations).
No failure criteria.
Each of the following orthotropic materials offer a particular brand of fiber/matrix damage and failure criteria. Up to 5 strength values are given (XT, XC, YT, YC, SC).
*mat_22 (composite_damage)
*mat_54,55 (enhanced_composite_damage)
*mat_58 (laminated_composite_fabric)
*mat_158 like 58 but includes strain rate effects
*mat_59 (composite_failure(_shell, _solid)_model)
Mats 22 and 59 can be used with shells and solids

**13. **Composite Material Models
The paper "Crashworthiness Analysis with Enhanced Composite Material Models in LS-DYNA - Merits and Limits", Schweizerhof et al, 5th International LS-DYNA User's Conference (1998) provides some insight into several composite material models in LS-DYNA, including mat_54, mat_58, and mat_59. This paper (in PDF format) and other files/examples related to composites are available in ftp://ftp.lstc.com/outgoing2/jday/composites

**14. **Comparison of Several Composite Material Models
Uniaxial Tension in Fiber Direction

**15. **Comparison of Several Composite Material Models
Uniaxial Tension in Fiber Direction

**16. **Laminated Shell Theory Use of Laminated Shell Theory (LST) is important if a composite shell has layers of dissimilar materials.
LST corrects for the incorrect assumption of uniform constant shear strain through the thickness of the shell.
Without LST, a sandwich composite will generally be much too stiff.
LAMSHT=1 in *control_shell invokes LST for material models 22, 54, 55, 76
*Mat_layered_linear_plasticity (114) is a plasticity model much like mat_024 but which includes LST.

**17. **Composite Material Models
*mat_116 (composite_layup)
Orthotropic elastic resultant formulation (no stresses calculated)
Very efficient for large number of layers
Requires *integration_shell
Material constants can vary from layer to layer
Does NOT use laminated shell theory (not good for foam core/sandwich composites)

**18. **Composite Material Models
*mat_117 (composite_matrix)
*mat_118 (composite_direct)
Resultant formulation (no stresses calculated)
21 coefficients of symmetric stiffness matrix are input directly
Stiffness coefficients in 117 given in material coord system
Stiffness coefficients in 118 given in element coord system (less storage req'd)
Shell thickness is inherent in stiffness matrix. Thus uniform thickness of part is mandatory.

**19. **Composite Material Models
*mat_161 (composite_msc)
Proprietary model from Materials Sciences (requires license add-on)
Available for solids only
Offers fiber shear and fiber crush failure criteria
Can predict delamination
*mat_162 like *mat_161 but adopts damage mechanics approach for softening after damage initiation

**20. **A Few Words about Delamination Shells are generally plane stress elements (szz = 0) and thus are not well-suited to rigorous study of composite delamination.
Version 971 has ‘thickness stretch’ shell elements (ELFORMS 25, 26, 27) which DO include szz. Too soon to say if these elements are suitable for delamination studies
Delamination behavior may be approximated using multiple layers of shells tied with *CONTACT_AUTOMATIC_..._TIEBREAK in which failure of contact represents delamination.
OPTION = 8 (Dycos model) shows promise
Thin cohesive elements (solid ELFORM 19, 20) representing the bond material between composite layers is yet another alternative.
Small or zero thickness of cohesive element does not affect time step
Cohesive material is modeled with *mat_138, 184, 185, or 186
Of the approaches mentioned, there is no clear favorite at this time

**21. **Closing Recommendations Most composites do not stretch significantly before breaking. To promote numerical stability, shell thinning option should NOT be invoked. Leave ISTUPD in *control_shell set to zero.
‘Noise’ in response can be mitigated by stiffness damping in some cases. See *damping_part_stiffness.
Shell bulk viscosity (*hourglass, ITYPE=-1) may aid stability in compressive modes of response.