The prediction of the overall effective properties of fibre-reinforced piezocomposites has drawn much interest from investigators recently. In this work, an algorithm used in two-dimensional (2D) analysis for calculating transversely isotropic material properties is developed. Since the finite element (FE) meshing patterns on the opposite areas are the same, constraint equations can be applied directly to generate appropriate load. The numerical results derived using this model have found a good agreement with those in the literature. The 2D algorithm is then modified and improved in such a way that it is valid for three-dimensional (3D) analysis in the case of random distributed shorts and inclusions. Linear interpolation of displacement field is employed to establish constraint equations of nodal displacements between two adjacent elements.
Piezoelectric materials have unique features of converting mechanical field into electric field or vice versa. Being the most widely used “smart” material, it has drawn an increasing attention in the past several decades and much effort has been devoted to the research of the fabrications and applications of piezoelectric materials [
Since piezoelectric composites are heterogeneous on a microscopic level, the definition and study of the material properties are hard to impose on a specific area. Historically, homogenization approach [
Besides, in using RVE to evaluate materials effective properties, the condition of the periodicity of a unit cell should be considered. To this end, the periodic boundary condition is to be applied to impose a uniform deformation field and subsequently the same stress field. In this case, no gaps or overlaps should exist between adjacent cells. The general periodic boundary condition given by Havner [
It should be mentioned that the cost of the fabrication of laminated fibre composite is considerably high because of precise requirements and restrictions to the reaction conditions. On the other hand, random distributed short fibre or particle inclusions provide approximate advantages as fibre laminates such as high specific strength and light weight while the cost is much lower for mass production [
In this study, we aim to develop a practical algorithm for the analysis of 3D piezocomposites with random inclusions. A 2D FE model is first evaluated and verified as an introduction of the modelling and processing actions adopted by ANSYS Parametric Design Language (APDL). For 3D modeling, periodic boundary conditions for a free-meshed unit cell is defined so that it is suitable for any composite unit cell with random configuration or inclusion such as particle, fibre reinforced, or microdefects which can also be generated using different algorithms.
For the transversely isotropic composite studied here (see Figure
(a) Schematic diagrams of periodic 1–3 composite laminate and (b) unit cell (the fibre laminates are poled in
The prediction of effective coefficients appeared in (
As the homogeneous medium consists of periodic unit cells, periodic boundary conditions are required to apply on the boundaries of the RVE. The general periodic conditions expressed by Havner [
Based on the boundary condition (
In (
Figure
SOLID226 in ANSYS element library is used, which is a 20-node hexagonal shaped element type with 3D displacement degree of freedom (DoF) and additional voltage degree of freedom. This element type is easy for the implementation of periodic boundary conditions. And in the later development of 3D model, this element type will be suitable as the meshing method used for irregular model is only valid with tetrahedral element.
The material properties inputs are based on Berger et al. [
Composite constituent’s properties [
|
|
|
|
|
|
|
|
|
|
|
|
---|---|---|---|---|---|---|---|---|---|---|---|
PZT-5 | 12.1 | 7.54 | 7.52 | 11.1 | 2.11 | 2.28 | 12.3 | 5.4 | 15.8 | 8.11 | 7.35 |
Polymer | 0.386 | 0.257 | 0.257 | 0.386 | 0.064 | 0.064 | — | — | — | 0.07965 | 0.07965 |
For meshing, the area geometry is generated first and then sweep mesh is used to further generate the volume. In this way, the meshing result on
Different meshing density when volume fraction is 0.666. The RVE edge line is set into (a) 20 and (b) 40 divisions.
As for periodic boundary condition, specific boundary conditions will be assigned to the exact opposite positions, namely,
The boundary conditions are shown in Figure
Application of periodic boundary conditions from a coordinate’s view.
Since the meshing scheme has ensured that there exists a pair of corresponding nodes at the opposite positions, the problem lies in developing a method to apply constraint equations on each pair of node for overcoming the problem of time-consuming over the node pair selection by graphical users’ interface. An internal programme has thus been designed for accomplishing the task. The procedures of the implementation are described as follows. Define the areas Start from the first node in master array; get the node number Use the coordinates ( Given the node number of the nodes on opposite location, constraint equations could be established.
The same procedures are adopted on
When integrating the constraint equations in three directions, special care has been taken to avoid overconstraint over the edges that connect areas
Overconstraint situations for 2D model.
Proper boundary conditions with strain load are specified pertaining to the calculation of different coefficients. For example, for the calculation of
Summary of the numerical calculation of coefficients.
Coefficient | Non-zero term | Loading | Boundary conditions | Derivation |
---|---|---|---|---|
|
|
|
|
|
|
||||
|
|
|
|
|
|
||||
|
|
|
|
|
|
||||
|
|
|
|
|
|
||||
|
|
|
|
|
|
|
|||
|
|
|||
|
||||
|
|
|
Same as conditions in |
|
|
||||
|
|
|
|
|
The numerical results obtained are shown in Figure
Numerical results of effective coefficients.
The other observation is that, as for piezoelectric and permittivity tensors, the trend matches with that presented in the literature well.
The 2D model developed in Section
(a) Random distributed and (b) transversely distributed short fibre composite RVE generated by RSA and FE mesh in Kari et al. [
The most noticeable variation to the 2D model is the meshing method adopted. As in the model to be used for 3D analysis, sweep meshing method is not allowed for the irregular geometry. As a result, free mesh will be used which meshes the volume depending on the geometry of the inclusion inside the volume and the geometry patterns on the surfaces. In the free mesh method, SOLID227 is selected as the subsequent element type, which is a 10-node tetrahedral shaped element with 3D displacement DoFs and additional electric DoF as used in SOLID226 for the 2D model. The material properties of PZT and polymer are the same as that in 2D model. The geometry of the RVE is designed to be the same as the one used for applying out-of-plane loading. As discussed in Section
(a) Geometry and (b) meshing of the RVE.
The most principal part of 3D model generation is the application of periodic boundary conditions in order to maintain periodicity on exact opposite location of an RVE. The nature of the 2D model offers the privilege that, at each pair of opposite locations, there exist a pair of nodes generated from sweep meshing, whereas, for 3D model, the mesh patterns on opposite areas are different. There are three scenarios:
Three possible results when projecting node from one area to the other.
The method of linking the existing node on one area to the hypothetical projected node on the opposite area is developed and illustrated in Figure
Method for applying constraint equations for opposite areas with dissimilar mesh patterns.
Furthermore, since the projected node is always on the surface of the RVE, it means that the displacement result of the projected node is regardless of the fourth corner node inside the RVE as shown in Figure
Simplification to triangular element with 3-dimensional DoFs.
After free meshing of the RVE, elements and corresponding nodes are generated subsequently. The same presteps described in Section
As illustrated in Figure
Selection and definition of element field.
A
Element selected by crossing the defined path.
Some of the testing results have manifested that, in ANSYS when dealing with entity selection, such as element selection in this case, tolerance is one of the most significant factors affecting the results and needs to be considered. To be specific, if the path node falls slightly away from the edge of elements as illustrated in Figure
Effect of tolerance on the element selection. If the path node falls in the tolerance domain, Elements I and II and others may be selected.
Due to the fact that the description for manipulating the tolerance when using path to select element is vague, at this stage there has not been a way developed to ensure the exact element that the path node falls in is selected; as a result, problematic cases such as those illustrated in Figure
Problematic case of element selection viewing from
In the first graph of Figure
When an element is selected to be the domain for linear interpolation, corner nodes or corner nodes on the RVE face are further selected due to the reason that the displacement components of the node on the boundary of the RVE could be determined without considering the fourth node inside the RVE. The three-node triangle element which is called Turner triangle is shown in Figure
(a) Turner triangle geometry and (b) displacement interpolation.
It should be noted that the area given by (
The coefficients
By substituting (
The simplified linear interpolation relations are given when the unknown point lands on the edge of the triangle element. In this case, the displacement is only depending on the two nodes at the ends of the edge and can be determined through
The relations are used when the path node locates on the edge of an element, or in the selected element, there are two nodes on the RVE face instead of three.
It is desirable that the 3D RVE model could be verified with the random inclusions generated using algorithms such as RSA and MC. However, since these algorithms are currently unavailable, one way available to verify the model is to recalculate the transversely isotropic matrix derived using the 2D model in the previous sections. Using regular geometry of inclusion, but free meshing to generate irregular meshing patterns similar to that of random inclusions, the stiffness tensors are recalculated afterwards. If similar results could be obtained, it can be proved that the algorithm for generating 3D model is suitably developed.
In the conducted 2D analysis, when calculating the elastic tensors
Figures
RVE nodal solutions for
The results are listed in Table
Comparison of the results calculated by 2D and 3D models.
Volume fraction | ||||||
---|---|---|---|---|---|---|
0.111 | 0.222 | 0.333 | 0.444 | 0.555 | 0.666 | |
|
|
|
|
|
|
|
|
|
|
|
|
|
|
Error (%) |
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
Error (%) | 2.697% | 6.247% | 2.421% | 1.757% | 4.086% | 4.597% |
Comparison between the results derived from 2D and 3D models for
There are several points that should be noted. First of all, the employment of the 10-node tetrahedral element type (Solid227) is a compromise over the irregular inclusion configuration. Theoretically, 20-node hexagonal shaped element type (Solid226) presents a more complex order of shape function along its element edges and more accurate DoFs interpolation than Solid227, so Solid226 is more capable of generating accurate stress and strain field results.
In addition, the 3D analysis requires a much larger number of elements, and the use of Solid227 has again increased the total elements involved; therefore an efficient algorithm is crucial pertaining to the computation capability. To the best knowledge of the author, the final version of both algorithms has been improved, if not optimized. However, as previously mentioned, the number of the division of the RVE edge still has to be controlled under 15 divisions per RVE edge.
An algorithm using ANSYS Parametric Design Language to predict effective properties of piezoelectric composite materials has been developed in this work. In the first part, the fibre inclusion within the RVE is of regular geometry and the analysis is simplified as two-dimensional models with effective coefficients. The conclusions can be drawn as follows. With regular geometry, sweep meshing could be adopted to generate the same meshing patterns on opposite areas. The developed algorithm for applying constraint equations on exact opposite node pairs is easy to use. The calculated transversely isotropic effective coefficients are in good agreement with those in the literatures. The FE results for longitudinal elastic tensor
In the second part, the RVE model is developed in such a way that 3D analysis can be conducted for predicting effective properties of composite with random inclusions. Element shape functions are used to interpolate the degree of freedom, so that constraint equations could be applied indirectly. The algorithms for generating random inclusions are not currently available; as a result, the geometry of the RVE in this case is still regular; however, with the use of free meshing, dissimilar meshing patterns are produced for verifying the improved algorithm. It is found that the nodal solution patterns have found distortion. The distortion has been investigated that it is due to the problematic element solution before implementing linear interpolation. Since numerical results have shown validation of the model, the problematic element solution is not supposed to affect the calculation at this stage.
The authors declare that there is no conflict of interests regarding the publication of this paper.