Abaqus for dummies: Composite Laminate Definitions

Getting started with Abaqus Introduction

Hello everyone, I’m Tijmen and thank you for following my journey to Start with Abaqus, Download and install the Abaqus learning edition and Get started with Abaqus.
Let’s continue the blog series dedicated to exploring the vast capabilities of Abaqus. Over the coming months, we will embark on a journey through various example problems, unraveling the multitude of options and possibilities that Abaqus has to offer.
For engineers, researchers, and enthusiasts alike, Abaqus stands as a beacon of innovation, empowering users to simulate and analyze complex mechanical behaviors with unparalleled accuracy. However, navigating through its extensive features and functionalities can sometimes feel daunting.
In this series, we aim to demystify Abaqus by breaking down example problems into digestible segments, allowing you to grasp its essence and harness its full potential. Whether you’re a novice seeking to enhance your skills or a seasoned professional looking to delve deeper, this series will cater to your needs.
Each blog post will delve into a specific example problem, we will look at some animations and discuss the analysis. Through this series, our goal is not only to showcase the capabilities of Abaqus but also to inspire creativity and foster a deeper understanding of finite element analysis concepts. We encourage active participation, questions, and feedback from our readers, as together, we embark on this educational journey.

Analyzing composite yacht hulls

In the realm of yacht construction, composite hulls are commonly employed. These hulls utilize composite materials to facilitate the creation of high-performance marine vessels. These materials enable manufacturers to incorporate intricate hull designs derived from computational fluid dynamics analyses and experimental testing. Composites offer the necessary attributes of strength, rigidity, and low mass essential for high-performance yachts. However, the process of integrating multiple layers of materials with varying orientations into a complex three-dimensional finite element model can be time-consuming. Furthermore, the inclusion of local reinforcements adds further complexity to the process.

The composite layup feature within Abaqus/CAE streamlines the composite modeling process by emulating the procedures employed by manufacturers on the production floor. This involves stacking sheets of composite material within a mold and aligning them in a specified direction. With the Abaqus/CAE composite layup editor, users can effortlessly add a ply, designate the region of application, specify material properties, and define orientation. Additionally, users have the option to import ply definitions from a text file, facilitating the process when data is stored in a spreadsheet or generated by a third-party tool.

Abaqus Yacht hull geometry

The illustration below depicts the various components of the yacht model, including the hull, mast, rigging, and keel.

The geometry of this model is imported as a unified entity from an ACIS (.sat) file, showcased below.

The imported part represents one half of the hull, with symmetric boundary conditions applied. This hull is characteristic of a high-performance 20-meter yacht, featuring reinforced bulkheads to enhance structural rigidity. It’s worth noting that the elements above the deck are not factored into the hull’s performance modeling and are therefore omitted from the model.

To facilitate the application of plies in the composite layup, sets are established to correspond with specific regions of the yacht’s structure.

Abaqus Yacht hull materials

The model is divided into 27 distinct regions (see figure below), each comprising plies composed of glass-epoxy cloth encasing a Nomex core.
In most regions, there are nine plies present—four layers of glass-epoxy cloth on either side of the Nomex core. However, additional plies are introduced in regions experiencing heightened strain to bolster structural integrity. Certain bulkheads are reinforced with stringers crafted from glass-epoxy cloth, possessing an effective Young’s modulus of 128000 N/mm^2. The composite layup dialog box makes it possible to easily define the layup for each region, also shown below.

The figure below depicts a ply stack plot illustrating the arrangement of plies within the same region.

Abaqus Yacht hull Boundary conditions and loads

The model is symmetrically constrained about the y-axis. Various loads are imposed as follows

Hydrostatic pressure is applied to the hull, with the pressure incrementing linearly along the z-axis.

  • Concentrated forces, simulating tension from the sail rigging, are exerted on the front, rear, and sides of the deck. These forces act along the x-axis of a datum coordinate system, with each system originating from the load location and oriented towards the mast’s top.
  • Load from the mast is directed downward (z-direction) at the base of the hull.
  • The keel is represented by a lumped mass connected to the hull via a kinematic coupling.
  • An inertia relief load is applied at the hull’s center to ensure model equilibrium post-loading.

Approaches to Abaqus Modeling and Simulation Techniques

For this analysis, a single loading scenario is examined using static analysis to assess its impact on the composite layup.

Mesh Design

The model’s meshing is conducted in Abaqus/CAE, employing the free meshing method and prioritizing quadrilateral elements.


Various loads are applied to simulate real-world conditions, including tension loads from sail rigging distributed unevenly across the hull’s front, rear, and side. Additionally, a significant load is applied at the mast’s base.

Modeling of Components

To represent the keel’s weight, a lumped mass of 10 metric tons is included in the model. This is managed through a kinematic coupling to ensure accurate weight distribution to the hull’s base. Moreover, distributing couplings facilitate the transfer of rigging loads to the hull.

Analysis Steps

A single static load step is defined for the analysis, focusing solely on linear behavior without considering nonlinear effects.

Output Requests

In default settings, Abaqus/CAE records field output data only from specific section points within the composite layup, neglecting data from other plies. However, in this particular model, data from all section points in all plies are requested. This comprehensive data collection enables the creation of an envelope plot, offering insights into which plies within each region endure the highest strain.

Results and Discussion

The results are visualized below, illustrating an envelope plot of in-plane shear strain (E12) in the middle of the hull.

Composite layup yacht hull Abaqus reference

This blog post is based on the “Using a composite layup to model a yacht hull” from the Abaqus Example Problem manual. More details can be found here.

Do you have questions about this blog post or do you want to be informed when the next post is released? Contact me at tijmen@4realsim.com.