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 right-click context menu of relevant entities.

Engineering Constants

Engineering constants and relevant material/laminate matrices can be calculated for:
  • Materials
  • Plies
  • Zones
  • Laminates


Figure 1.
Dependent on the selected entity type, different analyses are executed upon selection of Engineering Constants.
  • Selection of multiple entities of the same type is also supported and generates multiple tabs in the Engineering Constants result view which contain the corresponding results.
  • Results can be marked with left-click (or Ctrl + left-click for multiple results) and then saved to clipboard with Ctrl + C for transfer to spreadsheet.
Materials
Material results include:
  • Material data
  • Engineering constants
  • 2D/3D material matrices

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).

Plies
Ply results include:
  • Ply data
  • Engineering constants
  • 2D/3D material matrices

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.

Note that 3D properties can only be calculated for plies which have an assigned material which provides the necessary data (for example, OptiStruct MAT9OR).


Figure 2.
Laminates
Laminate results include:
  • Laminate data
  • Stiffness and compliance matrices
  • Homogenized engineering constants
  • Normalized homogenized matrices
If all plies of a laminate have an assigned shape, the analysis is provided for all zones of the selected laminate. If one or more plies in a Laminate do not have a Ply Shape assigned, no Laminate Zones are generated. Accordingly, laminate calculations are provided for the full stacking sequence as defined in the laminate.


Figure 3.
Zones
Zone results include:
  • Laminate data
  • Stiffness and compliance matrices
  • Homogenized engineering constants
  • Normalized homogenized matrices

Additionally, stacking sequence, thickness and number of layers are summarized for each zone.

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 multi-selection of laminates) and Plate load. The first ply failure (FPF) settings are optional and will be use for first ply failure analysis.

Load response results include:
  • Laminate data
  • Load data
  • Midplane loads (converted forces and moments, strains and curvatures, homogenized stresses)
  • Material system stresses and strains for each ply
  • 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

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 multi-selection of laminates) and FPF settings.

Strength results include:
  • Forces
  • Moments
  • Stresses (in-plane, flexural, out-of-plane)
  • Strains (in-plane, 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. The components are listed in the table below.

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 right-click menu of the Composite Browser.
Type Components
Forces and moments N_x, N_y, N_xy, M_x, M_y, M_xy, Q_x, Q_y
Strains and curvatures Epsilon_x, Epsilon_y, Gammy_xy, Kappa_x, Kappa_y, Kappa_xy
Homogenized stresses Sigma_x, Sima_y, Tau_xy, Sigma^f_x, Sigma^f_y, Tau^f_xy, Tau_zx, Tau_yz

Workflow

To set up and run an analysis:

  1. Create and edit all participating entities (materials, plies, laminates, composite plate loads, first ply failure methods).
  2. Right-click on Composite Browser white space or the Analyses folder to create an analysis entity.
  3. Select the analysis type.
  4. Select participating entities according to analysis type.
  5. Run using the analysis’ right-click menu option Run….
In the result view, combinations of entities and results can be picked. When any of the participating entities are changed, the analysis must be run again.


Figure 4.

Solver Specific Details

Entities created in the Composite Browser are assigned the most common solver card for a typical ply-based model. Properties and Shapes are filtered based on solver card to only display appropriate cards for a ply-based model. Additionally, in the OptiStruct profile, the appropriate card is set for laminate and ply entities upon creation.

OptiStruct
Entity Supported Cards
Laminate STACK
Material MAT1, MAT8, MAT9OR
Ply PLY
Zone None
Abaqus
Entity Supported Cards
Laminate Via property *SHELL_SECTION_COMPOSITE
Material *MATERIAL, with type ISOTROPIC, ENGINEERING CONSTANTS or LAMINA
Ply None
Zone None

The first ply failure methods “Wrinkling-honeycomb” and “Wrinkling-foam” are not yet supported for Abaqus.

Nastran
Entity Supported Cards
Laminate Via property *SHELL_SECTION_COMPOSITE
Material MAT1, MAT8, MATORT
Ply None
Zone None