## Welcome to the World of Modelling and Simulation

### What is Modelling?

This blog is all about system dynamics modelling and simulation applied in the engineering field, especially mechanical, electrical, and ...

### Double Cantilever Beam Model to Predict Mode I Fracture for Pinned and Unpinned Laminates

This post shows the finite element (FE) model development with Abaqus CAE [1] for a double cantilever beam (DCB) to predict the mode I fracture of the z-pinned and unpinned laminates [2, 3]. This study first develops a DCB test model in Abaqus CAE with the geometric information from (ASTM D5528) [3]. The report is organized into three fundamental sections according to the project requirement.

1. Development of the DCB test model
2. Development of the Finite element model
3. Results and discussions of the DCB model test
3.1. Unpinned laminate simulation
3.2. Z-pinned laminate simulation
3.3. Comparison between standard test and model
3.4. Parametric study

1. Development of the DCB test model
For the geometrical shape and size of the DCB test setup, we choose the length of the beam as 100 mm where there are two parts: 70 mm length for the adhesive material and rest 30 mm length. The adhesive layer has a depth of 1 mm, and the beam part has also a depth of 1 mm. The following schematic drawing shows the geometry for the DCB model.

The following image depicts the implementation of the schematic geometry in the Abaqus CAE.

We have chosen materials for the cohesive and beam parts separately. The following table documents the major properties that have been implemented in the DCB test. The traction type is selected for the elastic material properties and its values are shown in the following table. For the damage criterion, the ‘Quads Damage’ option is chosen. In the ‘Damage Evolution’ module, we choose the type as ‘Energy’, then softening as ‘Linear’, then degradation as ‘Maximum’, then mixed mode behaviour as ‘BK’, then mixed mode ratio as ‘Energy’, and finally power set to 2.284. For the ‘Quads Damage’ option, we select the XFEM as ‘Normal’, where the tolerance is set to 0.05 and position is centroid.

2. Development of the Finite element model
After the geometry is created, next we move on to develop the FE model for this study. At first, we begin with meshing the geometry. The beam is meshed as ‘Quad’ and ‘Structured’ from the Abaqus meshing option, where a CPE4R beam element is selected for plain strain problem. For the cohesive part of the adhesive materials, for the mesh control, we select ‘Quad’, then we further select the ‘Sweep’, and consider the portion of highlighted orientation. We chose the cohesive element with COH2D4, where we set the viscosity to 0.00005. The following image shows the meshing for the whole structure in Abaqus.

Next, we develop to create constraint in the DCB model so that the laminate is attached in between the cantilevers. We use tie constraint between the top surfaces of the cantilever beams to the bottom surfaces of the cohesive layers. In this way, we tie the cohesive material layer to both of the cantilever beams. The following image shows the tie constrain simulation in Abaqus.

3. Results and discussions of the DCB model test
3.1. Unpinned laminate simulation
We first show the results for the unpinned laminates in the DCB model. The following simulation results show the laminate separation for the unpinned configuration of the DCB test.

The following result show the in-plane principal stress distribution in the separated DCB beam.

The following result shows the material orientations plots on the deformed shape of the beam.

3.2. Z-pinned laminate simulation
Next, we test the condition for the Z-pins, where pins are inserted in the laminate layers of the adhesive material. The pin material is chosen copper, where the Young’s modulus is 130 GPa and Poisson’s ratio is 0.34. The following image shows the position of a pin inside the DCB laminate. The z-pin is inside the cohesive layer of the DCB setup.

The following image shows the simulation result when a Z-pin is tied to the cohesive laminate.

3.3. Comparison between standard test and model
This section of the report discusses the comparison between the standard DCB test and the model test. We compare here force vs displacement plot for both the unpinned and pinned laminate configurations. From the following plots, we see that for both the unpinned (left) and pinned (right) laminates, there is a slight discrepancy between the standard and model tests. This is due to the facts the model test has slightly different geometry, different material properties, variations in the loads and boundary conditions, choice of the solvers, and so forth. However, the profiles are similar in both cases.

3.4. Parametric study
In this part, we do the parametric study for the Z-pin location and count within the laminate through the pin pull out test. We chose two pin materials, copper, and steel, in order to see the effects of them on the displacements of the adhesive layers with respect to the applied force between the standard test and the current model results. The following two tables represent the parametric study for the two materials.

REFERENCES
[1] ABAQUS UNIFIED FEA (https://www.3ds.com/products-services/simulia/products/abaqus/)
[2] Blacklock, M, Joosten, MW, Pingkarawat, K, and Mouritz, AP, Prediction of mode I delamination resistance of z-pinned laminates using the embedded finite element technique, Composites: Part A 91 (2016) 283–291
[3] Standard Test Method for Mode I Interlaminar Fracture Toughness of Unidirectional Fiber-Reinforced Polymer Matrix Composites, Designation: D5528 – 13

#DoubleCantileverBeam   #FiniteElement  #FractureAnalysis  #ABAQUS  #LaminateSimulation