Composite Stress Toolbox
Composite stress toolbox functionality.
Composite stress toolbox functionality is provided in the Composite Browser. Engineering constants, load response, first ply failure, and strength analyses are included. All analyses are accessible via the Analysis entity driven workflow. Engineering constants are additionally accessible via the rightclick context menu of relevant entities.
Engineering Constants
 Materials
 Plies
 Zones
 Laminates
 Elements
 Selection of multiple entities of the same type is also supported and generates a list in the Composite Analysis Result Viewer, from which desired results can be selected.
 Only one analysis entity can be selected and run at a given time. All analyses’ results can be accessed via the Analysis combo box in the Composite Analysis Result Viewer.
 Material data
 Engineering constants
 2D/3D material matrices
 Strength allowables
 Thermal expansion coefficients
Calculations are output in the material system. Note that 3D properties can only be calculated for materials which provide the necessary data (for example, OptiStruct MAT9OR).
 Ply data
 Engineering constants
 2D/3D material matrices
 Thermal expansion coefficients
Calculations are output in the laminate’s material reference orientation. Accordingly, the ply angle entered in the ply Orientation field is used to transform the properties from ply fiber direction to the laminate material reference orientation. For more information, refer to Fiber Orientation.
 Laminate data
 Stiffness and compliance matrices
 Homogenized engineering constants
 Normalized homogenized matrices
 Thermal expansion coefficients
 Laminate data
 Stiffness and compliance matrices
 Homogenized engineering constants
 Normalized homogenized matrices
 Thermal expansion coefficients
Additionally, stacking sequence, thickness and number of layers are summarized for each zone.
 Laminate data
 Stiffness and compliance matrices
 Homogenized engineering constants
 Normalized homogenized matrices
 Thermal expansion coefficients
Additionally, stacking sequence, thickness, and number of layers are summarized for each zone. All properties are calculated assuming midplane laminates, hence offsets in properties are disregarded.
Engineering constants calculations are also available through the analysis entity driven workflow as outline in the following for other analysis types.
Load Response/Failure
The response of a laminate due to an applied load is calculated based on its behavior derived from Classical Laminate Theory. For transverse shear, First Order Shear Deformation Theory is used. Load response/failure analysis is run through an analysis entity with Type: Load response/failure. Mandatory analysis inputs are Entity (single or multiselection of laminates or elements) and Plate load. The Plate load can be of type load, result subcases, or result simulations, where the latter 2 are only available with elements.
The Plate load type determines the solution sequence. For composite plate loads, no transformations are needed, as they are midplane loads and in a material coordinate system. For result subcases and result simulations, loads are read from the results files and transformed from an elemental system to a material system before being applied to the laminates on the elements. All results are calculated with respect to offsets provided on the element. This includes laminate properties used for the load response as well as the midplane results shown in the corresponding section.
The first ply failure (FPF) settings are optional and are used for first ply failure analysis.
 Laminate data
 Load data (in elemental and material coordinate system)
 Midplane loads (converted forces and moments, strains and curvatures, homogenized stresses)
 Material system stresses for each ply
 Apparent
 Mechanical
 Thermal residual
 Material system strains for each ply
 Apparent
 Mechanical
 Thermal
 Thermal free
 Thermal residual
 Principal stresses and strains for each ply
 Stress and strain invariants for each ply
 Optionally: First ply failure margins for each ply, as well as laminate critical ply, failure mode and failure function
Generally, Load Response/Failure results are available in tabular form or as plot. You can select the result type via the Result type combo box in the Composite Analysis Result viewer.
Strength
Strength analysis calculates the failure loads for selected laminates for applying load components individually. Unit loads used for a load response/failure analysis and critical values are determined iteratively. Strength analysis is run through an analysis entity with Type: Strength. Mandatory analysis inputs are Entity (single or multiselection of laminates) and FPF settings.
 Forces
 Moments
 Stresses (inplane, flexural, outofplane)
 Strains (inplane, flexural)
 Curvatures
 Failure mode and critical ply ID for each critical load
Composite Plate Loads
Composite stress toolbox utilizes 3 types of load vectors to calculate laminate load response. Each load vector consists of different load components. All composites plate loads are applied as midplane loads in the material system. The components are listed in the table below.
Type  Components 

Forces and moments  N_x, N_y, N_xy, M_x, M_y, M_xy, Q_x, Q_y, Delta T z_min, Delta T z_max 
Strains and curvatures  Epsilon_x, Epsilon_y, Gammy_xy, Kappa_x, Kappa_y, Kappa_xy,
Delta T z_min, Delta T z_max Note: Strains
and curvatures are treated as initial strains and curvatures
when combined with thermal loads.

Homogenized stresses  Sigma_x, Sima_y, Tau_xy, Sigma^f_x, Sigma^f_y, Tau^f_xy, Tau_zx, Tau_yz, Delta T z_min, Delta T z_max 
Temperature differences with respect to laminate reference temperature can be defined for laminate top (z_max) and bottom (z_min) independently. The temperature distribution is assumed to be linear in between, also for laminates consisting of different materials.
First Ply Failure Methods
The First Ply Failure Method is a collection of mainly composite failure criteria, that can be utilized within the certification framework and composite stress toolbox. The latter are applicable to Strength and Load response/failure analysis. They can be created from certification ribbon tools or directly from the rightclick menu of the Composite Browser.
Workflow
To set up and run an analysis:
 Create and edit all participating entities (materials, plies, laminates, composite plate loads, first ply failure methods).
 Rightclick on Composite Browser white space or the Analyses folder to create an analysis entity.
 Select the analysis type.
 Select participating entities according to analysis type.
 Run using the analysis’ rightclick menu option Run….
Solver Specific Details
Entities created in the Composite Browser are assigned the most common solver card for a typical plybased model. Properties and Shapes are filtered based on solver card to only display appropriate cards for a plybased model. Additionally, in the OptiStruct profile, the appropriate card is set for laminate and ply entities upon creation.
Entity  Supported Cards 

Laminate  STACK 
Material  MAT1, MAT8, MAT9OR 
Ply  PLY 
Zone  None 
Result file type  *.op2, *.h3d, *.h5, *.hdf5 
Entity  Supported Cards 

Laminate  Via property *SHELL_SECTION_COMPOSITE 
Material  *MATERIAL, with type ISOTROPIC, ENGINEERING CONSTANTS or LAMINA 
Ply  None 
Zone  None 
Entity  Supported Cards 

Laminate  Via property PCOMPP realized to PCOMP or PCOMPG 
Material  MAT1, MAT8, MATORT 
Ply  None 
Zone  None 
Result file type  *.xdb 
 OptiStruct: PCOMP(G), PCOMPP
 Nastran: PCOMP(G)
 Abaqus: SHELLSECTION_COMPOSITE