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
  • Elements
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 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.
Materials
Material results include:
  • 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).

Plies
Ply results include:
  • 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.

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
  • Thermal expansion coefficients
  • Out-of-plane shear properties
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
  • Thermal expansion coefficients
  • Out-of-plane shear properties

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

Elements
Element results include:
  • Laminate data
  • Stiffness and compliance matrices
  • Homogenized engineering constants
  • Normalized homogenized matrices
  • Thermal expansion coefficients
  • Out-of-plane shear properties

Additionally, stacking sequence, thickness, and number of layers are summarized for each zone. All properties are calculated assuming mid-plane laminates, hence offsets in properties are disregarded.

Note: For laminates, zones, and elements, the ply type potentially affects the shown stacking sequence, for example when “Unidirectional Weave” or "Wound" is used. For details, see Plies and Laminates and Ply-Based Models. For elements, full DRAPE table information (n slices) is supported.
Generally, Engineering Constants results are available in tabular form or as a plot. You can select the result type via the Result type combo box in the Composite Analysis Result viewer.
Figure 4.


Line plots illustrate the selected properties over a range of angles. Multiple entities and results can be selected, and lines are named accordingly. For materials, the range represents an actual orientation of a material. For plies, the range refers to an orientation change with respect to the orientation defined on the ply. And for laminates, the range refers to the laminate rotation from its reference. Hovering over a line will activate the tool tip, showing the numerical value of the selected point (results are available in 1° steps).
Figure 5.


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 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 property assigned to 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.

Generally, Load Response/Failure results are available in tabular form, as a through-thickness plot or as contour. You can switch between table and through-thickness plot via the Result type combo box in the Composite Analysis Result viewer. Post-processing for contouring is available when selecting elements as entity.
Figure 6.


Table minimum and maximum values are indicated by blue and red cell background to quickly spot the extreme values of each result.

Numerical load response results include:
  • 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
Figure 7.


Through-thickness plots illustrate the results (one at a time) at the recovery planes of the various plies of the laminate. Tool tips are available at reach result to retrieve the exact numbers. Lines for each ply are colored with the corresponding ply color, when only a single selection is active for an entry, load and result. The selection of multiple laminates or elements, loads or load cases, and results allows for easy comparison.
Figure 8.


Contouring results include:
  • Element mid-plane strains, first-ply-failure margins and critical ply ID
  • Ply recovery planes’ (middle, top/bottom, top/middle/bottom) stresses and strains in corresponding ply material system, and first-ply-failure margins
Elements can be selected from the contour plot for detailed post-processing with full tabular results and through-thickness plots.
Figure 9.


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. 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
Forces and moments are defined as illustrated below. Moment definitions are opposite of the ones in OptiStruct and Nastran.
Figure 10.


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 right-click menu of the Composite Browser.

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 in the white space of the Composite Browser or the Analyses folder to create an analysis entity.
  3. Select the analysis type.
  4. Select participating entities according to analysis type.
    Figure 11.


  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.

  6. Export results from the Composite Analysis Result Viewer to .csv file for numerical results and line data of plots, as well as .png image file for the plots themselves.
    Image files will be saved in the same size as displayed in the viewer at export time.
    Figure 12.


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, MAT2, MAT8, MAT9OR, MATMDS
Ply PLY
Zone None
Result file type *.op2, *.h3d, *.h5, *.hdf5
Abaqus
Entity Supported Cards
Laminate Via property *SHELL_SECTION_COMPOSITE
Material *MATERIAL, with type ISOTROPIC, ENGINEERING CONSTANTS, LAMINA, or USER MATERIAL
Ply None
Zone None
Nastran
Entity Supported Cards
Laminate Via property PCOMPP realized to PCOMP or PCOMPG
Material MAT1, MAT2, MAT8, MATORT
Ply None
Zone None
Result file type *.xdb
Elements are supported for ply-based as well as zone-based properties for the following solver profiles and properties:
  • OptiStruct: PCOMP(G), PCOMPP, PSHELL (MAT1, MAT2, MAT8)
  • Nastran: PCOMP(G), PSHELL (MAT1, MAT2, MAT8)
  • Abaqus: SHELLSECTION_COMPOSITE

Element offsets are considered for load response calculations by using the ZOFFS values for PCOMP(G) and PCOMPP properties in OptiStruct and Nastran. For PSHELL with MAT1 or MAT8 material (MID1) assignment, the value of ZOFFS is also used and the analysis is run using MID1 material to compute in-plane, bending and transverse shear properties. Other MID (2,3,4) assignments are disregarded. For PSHELL with MAT2 assigned, MID4 can be used to introduce coupling effects. MID4 data is incorporated into the classical laminate theory calculations, while indicating Z0=-0.5 (mid-plane) in the laminate data, as the actual offset is unknown. PSHELL is treated as a single layer for all analysis types.