A Comparison of Free and Mapped Meshes for Static Structural Analysis

Finite Element Analysis (FEA) is a numerical method used to provide approximate solutions for problems that lack closed-form analytical solutions (Kurowski, 2022). The core principle of Finite Element Modelling (FEM) involves creating a mathematical representation that closely mimics the geometry of real-world structures, generating responses that are deemed equivalent when appropriate modeling techniques are applied (Hoppe, 2023). In essence, FEA enables detailed analysis of complex engineering and physical systems by discretizing them into smaller elements. The accuracy of the results depends on the fidelity of the mathematical model with respect to the physical reality, and on the careful application of numerical techniques throughout the simulation process.

Discretization of the problem domain involves generating a mesh model, which serves as a bridge between the computer aided design (CAD) model and the Finite Element (FE) solver. When the mesh is submitted to the FE solver, it is inherently assumed to accurately represent the component’s geometry. Therefore, the quality of the mesh plays a pivotal role in determining the accuracy of solution (Schröder et al., 2021).

Two distinct types of meshing strategies are commonly employed: the “free mesh,” also known as an unstructured mesh, and the “mapped mesh,” also referred to as a structured or regular mesh. A free mesh forgoes the constraints of a predefined pattern or grid structure, allowing for irregular arrangement of mesh element – typically triangles in 2D, or tetrahedra in 3D. This flexibility proves invaluable when modeling intricate geometries, where imposing a structured mesh might prove impractical. A mapped mesh, on the other hand, employs a structured pattern, akin to a grid. This mesh type predominantly relies on quadrilateral and hexahedral elements for 2D and 3D bodies, respectively (Papadimitrakis et al., 2022). The mapped mesh’s structured nature offers simplicity in both generation and manipulation, particularly in applications where the geometry exhibits well-behaved characteristics and can be effectively represented by a structured grid (Pietroni et al., 2022).

In physics simulations, the choice between free and mapped meshes hinges on the specific nature of the problem at hand. Factors such as computational efficiency, accuracy requirements, the geometry of the problem, and the nature of the physical system being simulated play pivotal roles in this decision-making process (Sher et al., 2020). Neither meshing technique is inherently superior; each has its own strengths and weaknesses, contingent upon such factors as the geometric intricacies of the problem, the underlying physics, and the targeted level of precision (Liu et al., 2021).

A free mesh, with its flexibility and adaptability to complex, dynamic, more deformable geometries, is particularly advantageous in simulations involving complex shapes. A mapped mesh, in contrast, characterized by adherence to the geometry of the simulation domain, is resource-efficient and well-suited for scenarios featuring stable and well-defined geometries, such as structural analyses. In many cases, a hybrid meshing approach can be judiciously employed to strategically exploit the strengths of both free and mapped meshes across different sections of the simulation domain. This hybrid approach becomes particularly relevant when dealing with multifaceted simulation domains exhibiting varying geometric characteristics (Jiang et al., 2021).

Engineers and researchers typically undertake mesh sensitivity analyses to assess how meshing choices affect both simulation outcomes and computational efficiency, iteratively refining the mesh to optimize its efficacy for the specific problem at hand. Stress analysts, for instance, commonly rely on the automatic mesh generators integrated into commercial software platforms, owing to the inherent convenience they offer in the meshing process (Smitha 2021). Nevertheless, the decision to opt for either free or mapped mesh types, particularly in conjunction with the automatic mesh generators found in Finite Element Analysis (FEA) software such as Ansys^® and MSC Patran^®, requires careful consideration on the part of the analyst (Okereke et al., 2018).

Ansys and MSC Patran are prominent FEA software solutions, each offering a suite of tools that include numerous checks to ensure the creation of a sound mesh model. Note, however, that while these software packages provide safeguards against a poor mesh, they do not inherently prevent analysts from inaccurately representing the problem domain (Ereiz et al., 2022). Thus, the responsibility ultimately rests with the analyst to exercise due diligence in making informed decisions regarding meshing strategies and ensuring a faithful representation of simulation domain (Park et al., 2019).

This growing inclination among Finite Element (FE) analysts to prefer free meshes over mapped meshes is primarily fueled by a belief or assumption that both types of meshes will produce comparable results, as long as proper mesh convergence is attained (Marcé-Nogué et al., 2020). This belief has led to the unfortunate misconception that the choice between using a free or mapped mesh is a noncritical factor in Finite Element (FE) analysis, erroneously implying that free and mapped meshes have a negligible influence on the accuracy of FE results, once mesh convergence is achieved (Ruggiero et al., 2019).

While achieving mesh convergence is undoubtedly critical for ensuring solution accuracy, the selection between free and mapped meshes nevertheless involves more nuanced considerations (Jalammanavar et al., 2018) The geometry of the problem, the nature of the physics involved, and the specific requirements of the simulation can significantly impact the appropriateness of one mesh type over the other.

While certain convenient benchmarks for mesh convergence have been established (De Mooij et al., 2019), a notable gap exists in literature in terms of comprehensive comparisons between free meshes utilizing tetrahedral elements and mapped meshes employing wedge/hexahedral elements in a broader context. Additionally, there appears to have been insufficient reviews regarding the impact of the automatic mesh generators available in Finite Element Analysis (FEA) software (İrsel, 2019). The absence of a comparative analysis between free meshes with tetrahedral elements and mapped meshes with wedge/hexahedral elements suggests a potential gap in understanding the performance of these meshing strategies across diverse simulation scenarios. Such a comparison is nevertheless crucial for discerning the strengths and limitations of each approach in different problem domains and could contribute valuable insights into optimizing mesh selection based on specific requirements. Furthermore, the influence of automatic mesh generators in FEA software underscores the need for a comprehensive examination of their efficacy in producing accurate and reliable meshes. Investigating the comparative performance of different automatic mesh generators could also enhance the overall reliability and accuracy of numerical simulations.

The primary aim of this study, therefore, is to assess and compare the performance of structured/mapped mesh and unstructured/free mesh in the context of static structural analysis for a solid model using two prominent Finite Element Analysis (FEA) software tools, namely Ansys and Patran.

The study involves conducting Finite Element (FE) Analysis on a three-dimensional solid model representing a structural component of an aircraft wing. The analysis begins by assigning appropriate material properties to the CAD model. The problem domain is then discretized using both free and mapped meshes, in both Ansys and Patran. A static structural analysis of the component then is carried out under specific design load conditions, with fixed boundary conditions. The analysis focuses on evaluating equivalent stress results generated using the different FE models with both mesh types. A thorough comparison of the equivalent stress results obtained from these diverse FE models is then carried out.

This research aims to provide meaningful insights and formulate guidelines for selecting the appropriate mesh type when performing static structural analysis of components subjected to design loads. By systematically comparing the performance of structured/mapped mesh and unstructured/free mesh in the specific context of Ansys and Patran, this study aims to provide valuable recommendations and guidelines that can aid engineers and analysts in making informed decisions regarding mesh selection for similar structural analyses.

Static structural analysis of an aircraft wing’s structural member, the wing tulip, was carried out using two prominent FE software tools: Ansys and MSC Patran. The CAD model was generated using SpaceClaim Design Modeller^®, with the material properties assigned as linear elastic and isotropic.

Meshing was performed in Ansys and MSC Patran, generating both free and mapped meshes. Tetrahedral elements were utilized for the free mesh, while wedge and hexahedral elements are employed for the mapped mesh (Sabat & Kundu, 2020). Both types of elements employed featured quadratic shape functions, meaning nodes were positioned at the corners and mid-sides of the element, allowing for a parabolic approximation of the solution. Quadratic elements can capture more complex variations in the solution field and typically offer higher accuracy than linear elements, albeit at a higher computational cost.

A fixed boundary condition, constraining all 6 degrees of freedom, was applied at the attachment bolt holes. Utilizing the default solver settings, a static structural analysis of the wing tulip was carried out under the design load. Successive mesh refinements were carried out until discretization errors reached acceptable limits (Arndt et al., 2021). A grid-independent solution was considered to be achieved when the percent change in equivalent stress between two successive mesh refinements was less than 5% (Nemade & Shikalgar 2020).

Maximum deformation results were also analyzed, where deformation refers specifically to the relative displacement of points within the structure, excluding rigid body translations. Finally, the study finally compared the results from both free and mapped mesh models to identify any significant differences.

This study examined the performance of free meshes based on quadratic tetrahedral elements versus mapped meshes based on quadratic wedge / hexahedral elements, generated in two FEA software tools: Ansys and MSC Patran. Comparing the FE results from these two leading tools was performed to verify the preferences of FE analysts for particular software based on meshing performance and simulation accuracy (Magomedov and Sebaeva 2020).

Both free and mapped meshes were used for static structural analysis of a wing tulip component under the design load. Table 2 summarizes the key differences and similarities between the free and mapped mesh models across both software platforms. Equivalent mesh elements were used in each case: the solid Tet10 element in Patran corresponds to the Tetrahedral (Solid 72) element in Ansys, while CPENTA / CHEXA elements in Patran are equivalent to Wed6 / Hex8 (Solid 182) elements in Ansys, respectively. Both element types preserve midside nodes to enforce a quadratic shape function. A mesh convergence study was carried out to determine appropriate mesh with no effect of discretization on the solution.

Free mesh generation from the CAD model was straightforward in both FEA software platforms. However, in Patran, mesh elements and global mesh density parameters can only be adjusted globally, without the option for local mesh refinement at areas of interest, such as stress concentration zones. In contrast, Ansys provides full control over meshing parameters, including element type, shape function, mesh density, and the ability to refine local and global mesh densities.

Generating the mapped mesh required considerable time and effort from the analyst in both software tools. In particular, edge and element sizing had to be creatively managed, especially at transition zones between wedge and hexahedral elements.

Comparing the deformation and stress fringe plots for different meshes in both FEA software platforms reveals that all mesh models consistently identified the same location of maximum deformation and maximum equivalent stress. The maximum deformation was observed at the flange of the model and the maximum stress at the location of the bolt holes. Contrary to the work of Shah et al. (2022), therefore, this study identified same stress hot spots in both commercially available software

In Patran, the maximum stress observed was 49.6 MPa for the free mesh of 4,295 elements. As the mesh density increased, value of maximum stress also increased. With a mesh of 82,998 elements, no further increase in maximum stress was observed. The maximum stress value increased by 11 times its initial value as the mesh density increased – aligning with previous findings on mesh convergency reported by Halliday (2023).

For the mapped mesh in Patran, the maximum stress value was 665 MPa for 5,510 elements, increasing to 787 MPa as the number of elements increased to 7,481. A 17.8% increase in stress value was observed with increasing mesh density. Mesh convergence was achieved with a fairly small increment in mapped mesh density – a finding also noted by Jalammanavar et al. (2018).

In Ansys, the maximum stress was 494 MPa for a free mesh of 2,731 elements. As the mesh density increased, the maximum stress value also increased. With a mesh of 72,321 elements, no further increase in maximum stress was observed. Note that the maximum stress value increased by 37.4% of its initial value with increasing mesh density. For the mapped mesh, the maximum stress was 739 MPa for 5,400 elements, increasing to 782 MPa as the number of elements increased to 7294. Here only a 6% increase in stress value was observed with increasing mesh density.

This 6% increase observed in our study contradicts with Svetlichny’s (2022) prediction of an increase of 24% in maximum stress. This discrepancy can likely be attributed to differences in the modeling approach. Svetlichny’s model incorporated such factors as different boundary conditions and material properties, which may account for the higher stress increase. Further investigation into these differences in maximum value of stress with different boundary conditions and material properties could be a fruitful avenue of new research in this field.

A significant increase in maximum stress was observed with larger density of the free mesh in Patran. This is likely because Patran does not provide control over the local mesh density in regions of geometrical transition and stress gradients, resulting in underpredicted stress values due to discretization errors arising from a coarse mesh. In the case of free mesh in Ansys, in contrast, the increase in maximum stress is not as high as for Patran, likely because of the local mesh refinement in the areas of geometric transition and stress gradients.

For the mapped meshes, the increase in maximum stress value was not large at higher mesh density. Static structural analysis of the model yielded Factor of Safety (FOS) calculations ranging from 1.06 to 1.38 across the different mesh models

This study addressed a critical research question in numerical simulations: whether free and mapped meshes provide consistent results for grid-independent solutions. The expectation was that as the mesh refines, the solution should converge to a consistent value, reflecting insensitivity to the mesh. The study added further complexity to this by comparing free and mapped meshes across two prominent FEA software platforms, Ansys and Patran.

Contrary to the initial hypothesis, the results revealed that free and mapped meshes do not yield identical results, even with proper mesh convergence. Mapped meshes demonstrated superior accuracy over free meshes, highlighting the significant impact the choice of mesh type can have on simulation accuracy.

Equivalent 3D solid elements in Patran and Ansys, used for static structural analysis, showed consistent results in identifying maximum deformation and stress locations in free and mapped mesh models. However, during free mesh convergence studies in both software platforms, there was a notable increase in maximum stress with successive refinement, indicating sensitivity to mesh density – especially in Patran. Ansys exhibited a smaller increase compared to Patran, demonstrating better stability.

Mapped meshes proved to be more efficient, requiring fewer elements than free meshes for numerical approximation, and the solution becomes mesh-independent at a coarser level. In both Patran and Ansys, maximum stress was higher in mapped meshes than in free meshes. Notably, both software platforms provided the same maximum stress value for the mapped meshes, resulting in consistent Factors of Safety (FOS).

This emphasizes the need for a detailed exploration and understanding of the specific problem at hand when selecting a mesh type. Mapped meshes, with their structured nature, prove advantageous in regular geometries, enhancing efficiency and accuracy. Conversely, free meshes provide flexibility for irregular geometries but demand finer resolutions. Integrating machine learning techniques into automated mesh generation algorithms could optimize mesh quality.

The performance of different mesh types may be sensitive to simulation parameters and specific solver settings, potentially influencing observed results. The observed superiority of mapped meshes may be specific to certain simulations or physical phenomena. Additionally, mapped meshes may entail higher computational costs in terms of mesh generation and simulation time. Evaluating and balancing the trade-off between accuracy and computational efficiency is crucial in this context.

For greater robustness, additional validation against experimental data or benchmark cases is recommended to ensure result reliability. As FEA software continues to improve, particularly in generating similar outcomes for both free and mapped meshes, the conclusions of this study may evolve.

Future research should investigate the underlying reasons for the observed differences in convergence rates and computational efficiency. Understanding the conditions under which mapped meshes outperform free meshes, and examining the impact of element shapes and connectivity on solution accuracy, would provide valuable insights for meshing strategies.

Extending this study’s application to interdisciplinary fields, such as fluid-structure interaction, heat transfer, and electromagnetics, could help verify whether the observed trends are consistent across diverse physical phenomena. Exploring hybrid meshing strategies, combining the strengths of free and mapped meshes, could be a promising direction for advancing FEA practices.