A Comparison of Free and Mapped Meshes for Static Structural Analysis.pdf

A COMPARISON OF FREE AND MAPPED MESHES
FOR STATIC STRUCTURALANALYSIS
Aun Haider
Institute of Aeronautics and Avionics, Air University Islamabad,
E-9/4 E-9, Islamabad, Islamabad Capital Territory 44000, Pakistan.
aunbutta@gmail.com
Abstract
This study addresses the challenge faced by Finite Element Analysts when choosing
between free and mapped meshes, especially in terms of convergence stability and
solution accuracy. The investigation focuses on 3D solid models under static structural
loading, analyzed using Ansys® and MSC Patran®. Both free and mapped mesh types,
employing equivalent 3D solid elements, are used to assess an aircraft structural
component under design load conditions, with fixed boundaries. For free meshes, Tet10
elements in Patran (equivalent to Solid 72 in Ansys) are used, whereas for mapped
meshes, CPENTA / CHEXA elements in Patran (equivalent to Wed6 / Hex8 in Ansys)
are employed. Mesh convergence studies ensure that discretization does not affect the
numerical solution. Notably, a significant stress increase is observed with successive
refinement of free meshes, while mapped meshes achieve mesh independence at coarser
refinement levels. Comparison of fringe plots indicates the same location for maximum
deformation and equivalent stress in both free and mapped mesh models. The findings
demonstrate that free meshes tend to underpredict maximum deformation and equivalent
stress compared to mapped meshes, with both meshes showing deformation and stress
at consistent locations. The findings underscore the importance of carefully choosing
the appropriate mesh type, particularly when analyzing critical structural components,
to ensure reliability and accuracy in FEA simulations.
Keywords: mesh convergence, mesh independence, discretization scheme, Finite
Element Analysis, FE Software.
Article category: research article
DOI: 10.2478/fas-2023-0007
FATIGUE OF AIRCRAFT STRUCTURES
Volume 2023: Issue 15, pp. 115–132

Introduction
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.
Methodology
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.
Results
CAD Model of Component
CAD model of the component was developed in SpaceClaim Design Modeler®.
Figure 1 shows the CAD model, which is imported in IGES format to both MSC Patran
and Ansys®. Using this CAD model as a template, both free (unstructured) and mapped
(structured) mesh is generated in each software package. The component was made of
alloy 30CrMnSiA, which has a modulus of elasticity (E) of 196 GPa, a yield strength
(σy) of 835 MPa, and a Poisson ratio (µ) of 0.3.
Fig. 1. CAD Model of Component.
Loads on Component
Table 1 outlines the design loads applied to the component, specified as force and
moment vectors. Finite element analysis were conducted under these design load
conditions using both free and mapped meshes in Patran and Ansys.
Table 1. Design loads for model
Force Magnitude (N) Moment Magnitude (Nm)
Fx 30,100 Mx 718
Fy 9,510 My 36.8
Fz 37,300 Mz 1.0

FEAwith Free Mesh in Patran
The CAD model was imported into Patran in IGES format. MSC Patran, serving as
a pre / post processing tool for the FE Solver Nastran®, was used to apply loads and
boundary condition as shown in Figure 2. The solid CAD model was meshed using
Tet10 3D solid elements – tetrahedral elements with 10 nodes – to create the free mesh.
Midside nodes on each element side are present to ensure quadratic shape functions.
Patran affords the analyst flexibility in varying the global mesh density. A mesh
convergence study was carried out to establish a numerical model independent of mesh
density.
Fig. 2. Loads and Constraints for Free Mesh in Patran.
Fig. 3. Free Mesh Convergence Study.
Figure 3 illustrates that the maximum stress value became independent of mesh
density at 82,998 elements. A further increase in number of elements did not change the
magnitude of equivalent stress.
The free mesh model is shown in Figure 4. After the FE model was developed in
Patran, it was submitted to the solver. Post processing of the solution file provides
deformation and stress fringe plots.

Deformation field of model under the applied load is displayed in Figure 5.
A maximum deformation of 0.287 mm is observed at the point of interest, i.e., the flange
of the model. Note that in this context, deformation refers specifically to the relative
movement of points within the structure, excluding rigid body translations. Furthermore,
the model is fully constrained to prevent any rigid body motion.
The stress field of the model under the applied load is given in Figure 6. Maximum
stress (606 MPa) is observed at the bolt hole. Based on the material’s yield strength, the
calculated Factor of Safety (FOS) for the free mesh in Patran is 1.38.
Fig. 4. Free Mesh in Patran.
Fig. 5. Deformation with Free Mesh in Patran.

Fig. 6. Stress with Free Mesh in Patran.
FEAwith Free Mesh inAnsys
The CAD model of the component was also imported into Ansys in the IGES format.
Figure 7 shows the applied loads and boundary condition for the Ansys model. A similar
mesh convergence study was performed to generate an FE model with stress field
independent of mesh density. Figure 3 shows that the solution becomes independent of
mesh size at 72,321 elements.
Fig. 7. Loads and Constraints for Free Mesh inAnsys.
Tetrahedral elements (Solid72) with midside nodes were used for meshing in Ansys.
The presence of midside nodes provides a quadratic shape function, improving the
interpolation of deformation values between the corners. To accurately capture stress
gradients, local mesh refinement was carried out at areas of stress concentration and
geometric transition.
Figure 8 shows the free mesh model in Ansys. The deformation field of the model
under the applied loads is given in Figure 9, with the maximum deformation of 0.13 mm
observed at the flange of the model.

The equivalent stress on the model under the design load is given in Figure 10.
Maximum stress 674 MPa is observed at the bolt holes of the model. Based on the
material’s yield strength, the Factor of Safety was calculated to be 1.24.
Fig. 8. Free Mesh inAnsys.
Fig. 9. Deformation with Free Mesh inAnsys.
Fig. 10. Stress with Free Mesh inAnsys.

FEAwith Mapped Mesh in Patran
A mapped mesh for the model was generated in MSC Patran for the Nastran solver,
using wedge-shaped (CPENTA) and brick-shaped (CHEXA) solid elements. Both
CPENTA and CHEXA elements are quadratic, containing midside nodes—CPENTA
elements have 15 nodes, while CHEXAelements have 20 nodes. These elements preserve
six degrees of freedom (DOFs) at each node, allowing for more accurate representation of
complex stress and strain distributions within the structure.
RBE2 multipoint constraints (MPC 184) were applied at the bolt holes of the model,
effectively constraining both translation and rotation in these areas. Figure 11 illustrates
the mapped mesh and applied constraints on the model.
Fig. 11. Constraints on FE Model in Patran.
Figure 12 shows the applied design load applied as equivalent nodal forces on the
finite elements of the model. A mesh convergence study was carried out for the mapped
mesh. Figure 13 shows that the solution became independent of mesh density at 7,481
elements.
Fig. 12. Loads on Mapped Mesh in Patran.

Once the finite element analysis was performed in Nastran, the solution file was post-
processed in Patran to obtain fringe plots for deformation and stress. The deformation
field of the model under the applied load is given in Figure 14. Maximum deformation
of 0.275 mm was observed at the flange of the model.
Fig. 13. Mapped Mesh Convergence Study.
Fig. 14. Deformation for Mapped Mesh in Patran.
Equivalent stress field of the model is given in Figure 15, with maximum stress of
787 MPa observed at bolt hole of the model. Based on the material’s yield strength, the
Factor of Safety (FOS) for the mapped mesh in Patran was calculated to be 1.06.

Fig. 15. Stress for Mapped Mesh in Patran.
FEAwith mapped mesh inAnsys
The CAD model was imported into Ansys, where mapped meshing was applied using
edge and element sizing. Figure 16 shows the applied loads and boundary conditions on
the model. The mapped mesh convergence study, shown in Figure 13, identifies that the
solution becomes independent of mesh size at 7,264 elements.
Wed6 and Hex8 Solid 182 elements are used for meshing the model. Both elements
have midside nodes to enforce quadratic shape functions. The mapped mesh generated in
Ansys is shown in Figure 17.
FE analysis of the model was carried out under the applied load and boundary
conditions. The deformation field for the model the applied load is given in Figure 18,
with a maximum deformation of 0.32 mm observed at the flange of the model.
The stress field on the model under the applied load is shown in Figure 19, with the m
aximum equivalent stress of 782 MPa observed at the bolt holes of the model.
Fig. 16. Loads and Constraints for Mapped Mesh inAnsys.

Fig. 17. Mapped Mesh inAnsys.
Fig. 18. Deformation with Mapped Mesh inAnsys.
Fig. 19. Stress with Mapped Mesh inAnsys.

Discussion
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 FEAsoftware
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.
Table 2. Comparison of Free and Mapped Mesh in Patran andAnsys.
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.
Quantity Patran Mesh Ansys Mesh
Free Mapped Free Mapped
Element Type Tet10 CPENTA/CHEXA Solid72 Solid182
Element Shape Tetra Wedge/Brick Tetra Wedge/Brick
Nodes per Element 10 15/20 10 15/20
Shape Function Quadratic
Total Elements 82998 7481 72321 7264
Deformation (mm) 0.287 0.275 0.13 0.32
Stress (MPa) 606 787 674 782
FOS 1.38 1.06 1.24 1.07

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
Conclusion
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 FEApractices.

References
Arndt, D., Bangerth, W., & Davydov, D. (2021). Finite element library: Design, features,
and insights. Computers & Mathematics with Applications, 81, 407-422.
https://doi.org/10.1016/j.camwa.2020.02.022
De Mooij, C., Martinez, M., & Benedictus, R. (2019). iFEM benchmark problems for
solid elements. Smart Materials and Structures, 28(6), 065003. https://doi.org/
10.1088/1361-665X/ab136f
Ereiz, S., Duvnjak, I., & Jiménez-Alonso, J. F. (2022). Review of finite element model
updating methods for structural applications. Structures, 41, 684-723.
https://doi.org/10.1016/j.istruc.2022.05.041
Halliday, A., Vulpe, C., & Fourie, A. (2023). A comparison of finite element software
for use in tailings applications. In 91st Annual ICOLD Meeting, ICOLD.
Hoppe, H. (2023). Progressive meshes. In Seminal Graphics Papers: Pushing the
Boundaries, 2, 111-120. https://doi.org/10.1145/3596711.3596725
İrsel, G. (2019). The effect of using shell and solid models in structural stress analysis.
Vibroengineering PROCEDIA, 27, 115-120. https://doi.org/10.21595/vp.2019.20977
Jalammanavar, K., Pujar, N., & Raj, R. V. (2018). Finite element study on mesh
discretization error estimation. 2018 International Conference on Computational
Techniques, Electronics and Mechanical Systems (CTEMS), 344-350.
https://doi.org/10.1109/CTEMS.2018.8769258
Jiang, Z., Zhang, Z., & Hu, Y. (2021). Bijective and coarse high-order tetrahedral
meshes. ACM Transactions on Graphics (TOG), 40(4), 1-16. https://doi.org/10.1145/
3450626.3459840
Kurowski, P. M. (2022). Finite element analysis for design engineers. Pennsylvania:
SAE International.
Liu, Z., Chen, J., & Xia, Y. (2021). Automatic sizing functions for unstructured mesh
generation. Engineering Computations, 38(10), 3995-4023. https://doi.org/10.1108/EC-
12-2020-0700
Magomedov, I., & Sebaeva, Z. (2020). Comparative study of finite element analysis
software packages. Journal of Physics: Conference Series, 1515(2020), 032073.
https://doi.org/10.1088/1742-6596/1515/3/032073
Marcé-Nogué, J., Fortuny, J., Gil, L., & Sánchez, M. (2020). On improving mesh
generation in finite element analysis. Spanish Journal of Palaeontology, 30(1), 117-
132. https://doi.org/10.7203/sjp.30.1.17227
Nemade, A., & Shikalgar, A. (2020). The mesh quality significance in finite element
analysis. IOSR Journal of Mechanical and Civil Engineering (IOSR-JMCE), 17(2), 44-
48. https://doi.org/10.9790/1684-1702054448

Okereke, M., & Keates, S. (2018). Finite element mesh generation. In Finite element
applications: A practical guide to FEM process (p. 165-186). https://doi.org/10.1007/
978-3-319-67125-3_6
Papadimitrakis, D., Armstrong, C. G., & Robinson, T. T. (2022). Investigating
singularities in hex meshing. In Mesh generation and adaptation: Cutting-edge
techniques (p. 41-67). https://doi.org/10.1007/978-3-030-92540-6_3.
Park, M., Kleb, W., Jones, W., Krakos, J., Todd, M., Loseille, A., Haimes, R., &
Dannenhoffer, J. (2019). Geometry modeling for unstructured mesh adaptation. AIAA
Aviation 2019 Forum. https://doi.org/10.2514/6.2019-2946.
Pietroni, N., Campen, M., Sheffer, A., Cherchi, G., Bommes, D., Gao, X., Scateni, R.,
Ledoux, F., Remacle, J. & Livesu, M. (2022). Hex-mesh generation and processing:
A survey. ACM Transactions on Graphics, 42(2), 1-44.
Ruggiero, A., D’Amato, R., & Affatato, S. (2019). Comparison of meshing strategies
in finite element modelling. Materials, 12(14), 2332. https://doi.org/10.3390/
ma12142332
Sabat, L., & Kundu, C. K. (2020). History of Finite Element Method: A Review. In
Recent Developments in Sustainable Infrastructure (pp. 395–404). Springer Singapore.
https://doi.org/10.1007/978-981-15-4577-1_32
Schröder, J., Wick, T., & Reese, S. (2021). A selection of benchmark problems in solid
mechanics and applied mathematics. Archives of Computational Methods in
Engineering, 28(2), 713-751. https://doi.org/10.1007/s11831-020-09477-3
Shah, M., Yunus, M., & Rani, M. (2022). A comparison of FE modelling techniques of
composite structure using MSC Patran/Nastran and Ansys software. AIP Conference
Proceedings, 2545(1), 7. https://doi.org/10.1063/5.0103287
Sher, R. J., Irfan-ul-Hassan, M., & Ghafoor, M. T. (2020). Analysis and design of box
girder and t-beam bridge superstructure; A comparative study. Mehran University
Research Journal of Engineering & Technology, 39(3), 453-465. https://doi.org/10.22581/
muet1982.2003.01
Smitha, T. (2021). A study on various mesh generation techniques used for engineering
applications. Journal of Innovative Image Processing, 3(2), 75-84. https://doi.org/10.36548/
jiip.2021.2.001
Svetlichny, J. (2022). Overview of Ansys meshing pre-processor capabilities to create
high quality meshes. Open Information and Computer Integrated Technologies, 5(95),
83-113. https://doi.org/10.32620/oikit.2022.95.07

A Comparison of Free and Mapped Meshes for Static Structural Analysis.pdf

More Related Content

Similar to A Comparison of Free and Mapped Meshes for Static Structural Analysis.pdf (20)

More from Aun Haider (16)

Recently uploaded (20)

A Comparison of Free and Mapped Meshes for Static Structural Analysis.pdf