ProductsAbaqus/StandardAbaqus/CAEAbaqus/Viewer Application descriptionComposite hulls are used routinely in the yacht industry. Composite materials allow manufacturers to create high-performance marine vessels that incorporate the complex hull shapes that engineers have derived from computational fluid dynamics analyses and from experimental testing. Composites also provide the strength, rigidity, and low mass that high-performance yachts require. However, incorporating many layers of material with varying orientations in a complex three-dimensional finite element model can be time consuming. The addition of local reinforcements complicates the process. These issues are described by Bosauder et al. (2006). The composite layup capability in Abaqus/CAE simplifies the process of composites modeling by mirroring the procedure that manufacturers follow on the shop floor—stacking sheets of composite material in a region of a mold and aligning the material in a specified direction. The Abaqus/CAE composite layup editor allows you to easily add a ply, choose the region to which it is applied, specify its material properties, and define its orientation. You can also read the definition of the plies in a layup from data in a text file, which is convenient when the data are stored in a spreadsheet or are generated by a third-party tool. GeometryFigure 1 shows the hull, mast, rigging, and keel of the yacht model. The geometry of the model is imported as a single part from an ACIS (.sat) file, as shown in Figure 2. The part models one half of the hull, and symmetric boundary conditions are applied. The hull represents a high-performance 20-meter yacht with reinforced bulkheads that stiffen the structure. The infrastructure above the deck does not play a role in modeling the performance of the hull and is not included in the model. Sets are created that correspond to the regions of the composite layup to which plies are applied. MaterialsThe model is partitioned into 27 regions. Each region contains plies of glass-epoxy cloth surrounding a Nomex core. Most regions contain nine plies—four glass-epoxy plies on either side of the Nomex core. However, additional plies are added to reinforce regions of high strain. Some bulkheads are reinforced with stringers made of glass-epoxy cloth with an effective Young's modulus of 128000 N/mm2. Table 1 shows the material properties of the glass-epoxy cloth, and Table 2 shows the material properties of the Nomex core. Figure 3 shows several rows of the composite layup table and illustrates how plies and material orientations are assigned to a region of the model. Figure 4 shows a ply stack plot of the same region. Boundary conditions and loadingThe center of the model is constrained to be symmetric about the y-axis, as shown in Figure 2. The following loads are applied:
Abaqus modeling approaches and simulation techniquesA single loading case is considered that uses a static analysis to study the effect of the loading on the composite layup. Mesh designThe model is meshed by Abaqus/CAE using the free meshing technique and quadrilateral-dominated elements. Loads
ConstraintsA kinematic coupling transfers the weight of the keel to the base of the hull, and three distributing couplings transfer the load from the rigging to the hull. Analysis stepsA single static load step is defined for the analysis; nonlinear effects are not included. Output requestsBy default, Abaqus/CAE writes field output data from only the top and bottom section points of a composite layup, and no data are generated from the other plies. In this model, output is requested for all section points in all plies. This allows you to create an envelope plot of the entire model that indicates which plies in each region are carrying the highest strain. FilesYou can use the Abaqus/CAE Python scripts to create the model and to run the analysis. You can also use the Abaqus/Standard input file to run the analysis.
References
Tables
FiguresFigure 1. The yacht model.
Figure 2. The symmetric model.
Figure 3. Assigning plies in the layup table to a region of the model.
Figure 4. A ply stack plot from the cockpit.
Figure 5. Envelope plot of strain in the critical plies in the center of the hull.
Figure 6. Strain (E12) across the thickness of an element.
|