complex mesh generation with openFOAM thchnical

www.usn.no
Faculty of Technology, Natural Sciences and Maritime Sciences
Campus Porsgrunn
FMH606 Master's Thesis 2021
Process Technology
Complex Mesh Generation with
OpenFOAM
Anne Marie Lande

www.usn.no
The University of South-Eastern Norway takes no responsibility for the results and
conclusions in this student report.
Summary:
In the course Computational Fluid Dynamics at the University of South-Eastern Norway there
have been some requests for more advanced geometry and meshing tools than the lectured
blockMesh dictionary and meshing tool in the open-source software OpenFOAM.
In this report, theory concerning mesh quality parameters and turbulence modeling is presented
and an evaluation of different open-source meshing tools is made. Salome is evaluated to be the
most user-friendly tool and is used to create and mesh a 3D model of a diverging converging
pipe with belly section. 3 meshes with a hexahedral OH-grid and different wall treatments are
constructed and imported to OpenFOAM. 4 different simulations are run with the steady-state
turbulent incompressible flow solver simpleFoam, applying the turbulence models standard
𝑘 − 𝜀 or 𝑘 − 𝜔 𝑆𝑆𝑇 to model the air flowing through the pipe. A student tutorial describing the
workflow of one of the cases is made.
An evaluation of basic fluid mechanics checkpoints, symmetry and residuals did not indicate
numerical errors in the solutions. The simulation cases generally obtained results that agreed
well with the analytical solutions, even though the complex flow field of turbulent, transitional
and laminar flow was modeled with turbulence models. The adjusted wall functions gave
slightly better results than the default wall functions for the 𝑘 − 𝜀 model. The 𝑘 − 𝜀 model on
Mesh B obtained pressure results that agreed well with the analytical solution. The 𝑘 − 𝜔 𝑆𝑆𝑇
model generally predicted the velocity field best, and also showed consistent results in terms of
pressure loss. Case A did not fulfill the wall function requirements and obtained diverging
pressure loss results. The OH-grid topology was evaluated to give good mesh optimality for the
full resolution approach and insufficient mesh optimality for the wall function approach.
Course: FMH606 Master's Thesis, 2021
Title: Complex Mesh generation with OpenFOAM
Number of pages: 125
Keywords: CFD, simpleFoam, Salome, diverging converging pipe with belly section, 3D,
mesh generation software, tutorial, hexahedral mesh, OH-grid (butterfly grid)
Student: Anne Marie Lande
Supervisor: Joachim Lundberg and Knut Vågsæther
External partner: -

Preface
3
Preface
This is a master’s thesis written at the University of South-Eastern Norway. The master’s thesis
is part of the last course at the master’s degree study in Process Technology and constitutes 30
credits.
I would like to thank my supervisor, associate professor in Process technology and laboratory
teacher in CFD, Joachim Lundberg. His guidance, help and assistance have been invaluable
throughout the work of this thesis.
Further, I would like to thank Olas Bil AS for letting me borrow a suitable computer for the
work on this thesis and providing me with the paid commercial software VMWare.
Avaldsnes, 18th
May 2021
Anne Marie Lande

Contents
4
Contents
Preface ...................................................................................................................3
Contents.................................................................................................................4
Nomenclature ........................................................................................................6
1 Introduction.......................................................................................................8
1.1 Previous work .........................................................................................................................9
1.2 Organization of thesis ..........................................................................................................10
2 Theory..............................................................................................................11
2.1 Mesh theory...........................................................................................................................11
2.1.1 Mesh structures ............................................................................................................11
2.1.2 Mesh quality aspects ....................................................................................................14
2.1.3 Mesh topologies for pipes............................................................................................17
2.2 Meshing tools........................................................................................................................19
2.2.1 Open-source meshing tools.........................................................................................19
2.2.2 Comparison of Salome and Gmsh ..............................................................................20
2.3 Turbulence boundary layer theory......................................................................................22
2.3.1 Estimation of 𝑦 +...........................................................................................................24
2.3.2 Wall treatment................................................................................................................25
2.4 Turbulence modeling............................................................................................................27
2.4.1 Turbulent flow characteristics.....................................................................................27
2.4.2 𝑘 − 𝜀 turbulence model ................................................................................................29
2.4.3 𝑘 − 𝜔 𝑆𝑆𝑇 turbulence model .........................................................................................30
2.4.4 Time step........................................................................................................................31
2.4.5 Pressure loss.................................................................................................................31
3 Case .................................................................................................................35
3.1 Geometry ...............................................................................................................................35
3.2 Meshes...................................................................................................................................36
3.3 Simulation cases...................................................................................................................40
3.4 Student tutorial .....................................................................................................................43
4 Results and discussion..................................................................................44
4.1 Evaluation of results.............................................................................................................44
4.1.1 Symmetry.......................................................................................................................45
4.1.2 Residuals .......................................................................................................................45
4.2 Boundary layer......................................................................................................................46
4.2.1 Increasing 𝑦 +................................................................................................................48
4.3 Pressure loss ........................................................................................................................50
4.4 Velocity ..................................................................................................................................53
4.5 Evaluation of models............................................................................................................56
4.5.1 Evaluation of mesh topology.......................................................................................56
4.5.2 Evaluation of flow models............................................................................................56
4.5.3 Evaluation of wall functions.........................................................................................57
4.5.4 Evaluation of analytical models...................................................................................57
5 Conclusion ......................................................................................................58
5.1 Further work ..........................................................................................................................59

Contents
5
References...........................................................................................................60
Appendices..........................................................................................................64

Nomenclature
6
Nomenclature
Latin symbols:
Symbol Description Unit
𝐴 Cross-sectional area of pipe [𝑚2]
𝐶𝑓 Skin friction coefficient [−]
𝐶𝜇 Turbulent viscosity constant [−]
𝐷 Pipe diameter [𝑚]
𝑓 Pipe friction factor [−]
𝑓, 𝑔 Functions [−]
𝑔 Gravitational acceleration [𝑚/𝑠2
]
𝑖𝑛 Location of pipe inlet [−]
𝐾 Obstruction loss factor [−]
𝑘 Turbulence kinetic energy [𝑚2
/𝑠2
]
𝐿 Length of a pipe section [𝑚]
𝑙 Turbulence length scale [𝑚]
𝑜𝑢𝑡 Location of pipe outlet [−]
𝑃 First computational interior node [−]
𝑝 Static pressure [𝑃𝑎]
𝑝0 Stagnation pressure [𝑃𝑎]
𝑝𝑘 Kinematic pressure [𝑚2
/𝑠2
]
𝑄 Volume flow [𝑚3
/𝑠]
𝑅𝑒 Reynolds number [−]
∆𝑡 Time step [𝑠]
𝑇 Temperature [℃]
𝑇𝑖 Turbulence intensity [−]
𝑈 Velocity [𝑚/𝑠]
𝑈𝑚𝑎𝑥 Maximum velocity [𝑚/𝑠]
𝑢𝜏 Friction velocity [𝑚/𝑠]
𝑢+
u plus [−]
∆𝑥 Length of a grid cell [𝑚]
𝑥𝑓𝑑,ℎ Hydrodynamic entry length [𝑚]
∆𝑦 Height of a grid cell [𝑚]
𝑦+
y plus [−]
𝑦 Distance from wall [𝑚]
∆𝑦𝑃 Distance from surface to nearest node P [𝑚]
𝑧 Elevation [𝑚]

Nomenclature
7
Greek symbols:
Symbol Description Unit
𝛼 Skewness angle [°]
𝛿 Boundary layer thickness [𝑚]
𝜀 Turbulence dissipation rate [𝑚2
/𝑠3
]
𝜖 Roughness height of the pipe wall [𝑚]
𝜇 Dynamic viscosity [𝑁𝑠/𝑚2
]
𝜇𝑡 Turbulent viscosity [𝑚2
/𝑠 ]
𝜈 Kinematic viscosity [𝑚2
/𝑠]
𝜌 Density [𝑘𝑔/𝑚3
]
𝜏 Shear stress [𝑃𝑎]
𝜏𝑤 Wall shear stress [𝑃𝑎]
𝜔 Turbulence dissipation rate [𝑠−1
]
Abbreviations:
1D One dimensional
2D Two dimensional
3D Three dimensional
AR Aspect ratio
CAD Computer-aided design
CFD Computational fluid dynamics
GUI Graphical user interface
HRN High-Reynolds-number
LRN Low-Reynolds-number
RANS Reynolds-averaged Navier-Stokes
RDT Rapid Distortion Theory
SIMPLE Semi-Implicit Method for Pressure-Linked Equations
SIMPLEC Semi-Implicit Method for Pressure-Linked Equations-Consistent
SST Shear Stress Transport
USN University of South-Eastern Norway
WF Wall functions

1 Introduction
8
1 Introduction
Computational Fluid Dynamics (CFD) is a course taught at the University of South-Eastern
Norway (USN). The CFD software used for the simulation part of the course is OpenFOAM
and the typical working method is to define the geometry, create the mesh, solve and post-
process. The students are taught how to program a simple 2D geometry and to generate a
mesh with the blockMesh meshing tool. However, over the past few years, there have been
requests from some students for a simple tool to mesh complex geometries for more applied
cases.
In this thesis, different tools for creating and meshing a 3D geometry are assessed, and the
user-friendliness of the different tools is evaluated. The recommended tool is used to create a
student tutorial. The tutorial describes the full workflow of modeling the geometry,
generating the mesh, importing the mesh to OpenFOAM, running a simulation and post-
processing.
The thesis is divided into two parts: one theory section and one method section. The theory
section explores different parameters for obtaining a good mesh, meshing tools and
turbulence boundary layer and modeling theory. The method section presents the case and the
results. The geometry, mesh and simulation cases are described, and the results of the
simulations are presented and discussed.
A relatively complex flow geometry is chosen for the case. The geometry is a 3D model of a
diverging converging pipe with belly section. The geometry is meshed with a hexahedral
OH-grid (butterfly grid). 3 meshes with different wall treatments are created. The physics
involved in the model is quite complex, because turbulent, transition and laminar flow occur.
The air flowing through the pipe is assumed to be steady state and incompressible and is
modeled with the turbulence models the standard 𝑘 − 𝜀 and the 𝑘 − 𝜔 𝑆𝑆𝑇 in the
simpleFoam solver in OpenFOAM. 4 cases with different meshes and wall treatments are
simulated.
The project topic description of the thesis is given in Appendix A.

1 Introduction
9
1.1 Previous work
A literature review has been performed and reveals that CFD simulations are a topic that is
extensively covered in the literature. However, the mesh generation stage is typically not
described. This claim is supported by Hernandez-Perez et al. [1]. In general, only a basic
description of the applied mesh is given, although sometimes additional information about
the quality and characteristics of the mesh is presented.
An in dept description of the full workflow from creating and meshing a geometry, importing
the mesh in OpenFOAM, to running a simulation has not been found in the literature.
However, there are meshing tutorials available on meshing platforms, web pages and
YouTube.
In a journal article Gao et. al [2] describes the steps of creating and meshing a neighborhood
of buildings in Salome.
In his master's thesis Nour [3] develops a 3D hexahedral butterfly mesh for a bent pipe
geometry in Gmsh. He describes the workflow of creating, programming and importing the
mesh to OpenFOAM. However, he does not explain how to make the mesh executable in
OpenFOAM by setting the correct boundaries and initial conditions in the case directory.
In her master's thesis Liestyarini [4] creates meshes for 3D straight, blind-tee and elbow pipes
in Salome and Gmsh. She explains that the meshing stage takes 60 % of the project time, but
does not present a description of the process. For the straight pipe geometry, the created mesh
is unstructured in the center of the pipe and structured in the rest of the pipe. For the blind-tee
and elbow geometries, the generated meshes are unstructured.

1 Introduction
10
1.2 Organization of thesis
The thesis is divided into 5 chapters.
Chapter 1 presents an introduction to the thesis with background information, objectives,
methods and scope. Additionally, a short literature review of similar work and the report
structure info is provided.
Chapter 2 describes theory about mesh structures and meshing tools. Furthermore, theory
about turbulence boundary layers and turbulence modeling are covered.
Chapter 3 presents the geometry, meshes, simulation cases and numerical setup for the CFD
analysis. In addition, some information about the student tutorial is given.
Chapter 4 contains comparisons of simulation results with analytical solutions, along with a
discussion of the results and models.
Chapter 5 concludes the thesis work. Further work is recommended.
Appendices provide additional information and figures that are not given in the report. The
student tutorial is located in the Appendices.

2 Theory
11
2 Theory
In this section, theory concerning meshes, meshing tools, turbulence boundary layers and
turbulence modeling are treated.
2.1 Mesh theory
The result of a CFD simulation is greatly influenced by the mesh or grid1
. The quality of the
mesh affects the convergence, numerical solution and stability of a simulation. The accuracy
of the results and solver convergence is established by a good mesh quality [1]. A good mesh
topology is essential for reducing discretization errors [5, p. 302]. Therefore, considerate
attention should be given to the mesh generation stage. The grid can determine whether a
simulation is a success or a failure. Consequently, research and advancement in the grid
generation field are important [6, p. 125].
Jasak [7, p. 245] describes the difference between mesh quality and mesh optimality in the
following manner: “[..] Mesh quality is a property of the mesh, specifying the amount of
mesh-induced errors expected from a certain mesh. Mesh optimality, on the other hand,
depends on the interaction between the mesh and the particular problem that is being solved.”
2.1.1 Mesh structures
There are many possible mesh structures. Mesh topologies can generally be divided into two
groups: structured (Figure 2.1) and unstructured (Figure 2.2) grids. A structured mesh
typically consists of elements that follow a regular cartesian pattern. In 2D domains the cells
usually consist of quadrilaterals, while in 3D domains hexahedral cells are typical. An
example of a hexahedral cell (hexahedron) is illustrated in Figure 2.3 [8]. In the 2D and 3D
domains of a structured mesh, the center cell is attached to four and six neighboring cells,
respectively. This pattern makes the computing, coupling and solution algorithms
straightforward.
1
The terms mesh and grid are considered to have the same meaning.

2 Theory
12
Figure 2.1: Structured mesh. Figure 2.2: Unstructured mesh.
A single-block structured mesh is a structured mesh that is meshed as a single block.
However, for complex geometries it may be difficult to create a high-quality structured grid
configuration without applying additional modifications to the interior geometry. A single-
block mesh for a complex geometry typically gives a low-quality mesh with high skewness
and non-orthogonality.
Many complex geometries require a block-structured grid to ensure a high-quality mesh. In
block-structured or multiblock meshes the geometry is divided into blocks or sub-regions that
are meshed separately. Thus, the topology of meshes in sub-regions can differ from each
other, and it is possible to refine the grid in desired areas, such as the near-wall area, and to
improve the quality of the mesh. However, if a satisfactory block division of the geometry is
not possible, the result may be various areas with highly skewed cells and bad mesh quality.
Moreover, the creation of fitting interior blocks can be difficult and requires expertise and
time. For even more complex geometries, a high-quality structured mesh may be impossible
to achieve and an unstructured grid is preferred [5, pp. 305, 309-310, 342]−[6, pp. 136, 139-
140].
Figure 2.3: 3D shapes [8].

2 Theory
13
An unstructured mesh is defined as a mesh where the elements do not follow a regular
pattern and every cell is considered to be a block. In 2D domains the cells usually consist of
triangles, while in 3D domains tetrahedral cells are typical. An example of a tetrahedral cell
(tetrahedron) is illustrated in Figure 2.3 [8]. Unlike the structured mesh, the center cell in an
unstructured mesh is attached to an inconsistent number of neighboring cells. This
complicates the solving of the numerical equations, such as the calculation of diffusion and
convection fluxes. More complex solver algorithms may be required, which increases the
required computing resources and time usage. In addition, difficulties may arise in generating
a high-quality mesh along the wall. Triangle and tetrahedral elements close to the wall
complicate the solving of the near-wall region and the solution of the boundary layers may be
inaccurate.
The major advantage of an unstructured mesh is that it can be used for all types of geometries
and is easy and fast to implement. Furthermore, it is easy to refine and adjust the unstructured
mesh in specific regions. It is also considered to use the computational resources for complex
flows in an efficient manner.
Figure 2.4: Hybrid mesh.
If the grid topology consists of a combination of different geometrical shapes, the grid is
called a hybrid mesh (Figure 2.4). Figure 2.3 [8] shows examples of different shapes that can
be used in various 3D mesh topologies. A hybrid mesh often consists of quadrilateral or
hexahedral cells along the wall for better resolution of the boundary layer, whilst triangular,
tetrahedral or polyhedral elements are generated on the rest of the geometry. This topology
typically improves convergence and accuracy of results [5, pp. 305, 311-312, ]−[6, pp. 139-
140, 342].

2 Theory
14
2.1.2 Mesh quality aspects
A low-quality mesh causes discretization errors. Mesh resolution, grading, aspect ratio,
skewness and orthogonality are important characteristics that affect the quality of a mesh and
the numerical stability and accuracy of results [6, p. 139]−[7].
It is important to make sure that the mesh is not too coarse. The mesh resolution directly
affects the accuracy of the solution, therefore the mesh must be constructed so that the
solution can be modeled accurately. A sufficiently fine grid ensures that the geometrical
shape and flow characteristics are captured. Too low mesh resolution may produce
unphysical results.
In addition, the distribution of the grid cells is important. A uniform grid is not always the
best arrangement for a given flow problem to ensure mesh optimality. Some regions of the
flow domain may need special attention. Problem areas may include regions of rapid
changes, high gradients, reattachment, separation or recirculation of the flow, as well as the
flow in the near-wall region. In order to resolve all the details in these areas, the mesh can be
refined locally. To accurately resolve the boundary layer towards the wall, a configuration of
quadrilateral or hexahedral elements is preferred.
If a mesh is refined in certain regions, smooth grading between coarse and fine mesh areas is
required to ensure the overall grid quality and accuracy of the solution [6, pp. 125, 133, 141-
143]−[7]. Figure 2.5 [9] illustrates the difference between a smooth and steep transition.
Figure 2.5: Smoothness [9, p. 311].
The aspect ratio (AR) is defined as the ratio between the longest and shortest length of a grid
cell, as shown in Equation (2.1). Figure 2.6 [10] illustrates the aspect ratio lengths, while
Figure 2.7 [11] demonstrates some examples of aspect ratios for different geometrical shapes.

2 Theory
15
𝐴𝑅 =
∆𝑥
∆𝑦
(2.1)
Where ∆𝑥 [𝑚] is the width of the grid cell and ∆𝑦 [𝑚] is the height of a grid cell.
Figure 2.6: Aspect ratio [10, p. 310]. Figure 2.7: Examples of aspect ratios [11].
The value of the aspect ratios of a mesh should be kept as low as possible, especially in
important areas of the flow geometry. High aspect ratios can increase the numerical diffusion,
decrease the accuracy of the numerical solution and cause convergence issues or divergence.
The erroneous effects are especially large if high gradients are present in the regions of high
aspect ratios. However, solver settings can influence the effects on the results [6, p. 149], [12,
p. 310].
Skewness or distortion describes the angle, 𝛼 [°], between the lines of a cell. The optimal
angle is 90°. A cell is considered to be highly skewed if the angle is smaller than 45° or larger
than 135°. Figure 2.8 shows an example of a skewed cell. A mesh with highly skewed cells
can cause stability issues and poor results. The calculation of the gradient and convective
terms are influenced. Moreover, the accuracy of face integrals is reduced to first order, which
creates a numerical diffusion error dependent on the degree of distortion. The introduction of
underrelaxation factors to the solution algorithm may improve the results of a mesh with
skewed cells [5, p. 308]−[6, p. 150]−[7], [12, p. 309].

2 Theory
16
Figure 2.8: Example of a skewed cell.
One of the drawbacks of an unstructured mesh is the skewness of the elements. The
unstructured mesh generally gives a zeroth-order of accuracy in OpenFOAM with the
standard divergence theorem (Green-Gauss) schemes. It is recommended to use the least-
squares gradient on highly skewed unstructured meshes to obtain second-order accuracy [13].
Orthogonality is another important mesh quality aspect. In an orthogonal mesh, the grid lines
at the junctions form a 90° angle, as shown in Figure 2.9. In a non-orthogonal mesh, on the
other hand, the angle of the grid lines at the junctions is not perpendicular. In non-orthogonal
meshes, diagonal equality is violated. The boundedness of the solution is affected and the
computational molecule increases in size. The calculation of the gradient and Laplacian terms
is affected and cross-diffusion effects are generated. As a result, there is a higher risk of
errors in the results. For highly non-orthogonal meshes, the introduction of non-orthogonal
correctors may be necessary [5, pp. 305, 342], [12, p. 308], [7].
Figure 2.9: Example of an orthogonal mesh.

2 Theory
17
2.1.3 Mesh topologies for pipes
Many different mesh topologies can be applied to a circular pipe geometry. A circular pipe
can be meshed with an unstructured or a structured grid. An example of an unstructured grid
topology for a pipe is illustrated in Figure 2.10. As previously mentioned, one weakness of
the unstructured mesh is that accurate solving of the boundary layers is difficult. A strength is
that it is easy to implement this mesh in many complex pipe geometries, like bends, elbows,
and pipes with expanding or contracting cross-sections.
Figure 2.10: Tetrahedral mesh for a circular pipe. Figure 2.11: H-grid for a circular pipe.
For structured grids, there are many possible pipe topologies. A structured grid can be created
with an H-grid, an OH-grid, an O-grid or an unstructured pave grid. All of these meshes
have advantages and disadvantages. Strengths and weaknesses of the topologies are related to
the complexity of the mesh-generation stage, expenditure and how the topology affects the
simulation and results. Here, only the H-grid and the OH-grid are explored. Further details
about O-grids and pave grids are available in [1].
Figure 2.11 shows an H-grid on a circular pipe geometry. The H-grid is a single-block mesh
and consists of orthogonal grid lines. A drawback is that there are 4 vertices at the wall with
highly skewed cells, as seen in Figure 2.11. If the number of cells is increased, the skewness
at the vertices increases and the mesh quality reduces [1].
The structured OH-grid or butterfly topology (Figure 2.12) is described as the ideal
configuration for hexahedral meshes in pipes [1]. It is a block-structured mesh where the
center of the mesh consists of a cartesian mesh, while the outer mesh is cylindrical. The grid

2 Theory
18
topology allows refinement of the mesh close to the wall. The high-quality hexahedral mesh
in the middle of the pipe allows accurate resolution of the flow along the centerline. The
topology is widely used in the literature. Some examples of publications with pipes modeled
with the OH-grid are the work by Gopalakrishnan and Disimile [14], Hernandez Perez [15],
Hernandez Perez et al. [1] and Zang et al. [16]. In [1] a comparison study of hexahedral mesh
topologies for a simulation of gas-liquid flow in a pipe was done, and the OH-grid obtained
the best results.
Figure 2.12: OH-grid for a circular pipe.
Of all the described structured grid topologies, the OH-grid employs the best mesh density,
orthogonality, skewness and aspect ratio. The main disadvantage with this mesh is that it can
be difficult and time-consuming to build, especially for inexperienced users. The geometry
must be divided into blocks, which can be a complicated task, especially for geometries that
are more complex than a straight pipe. However, some meshing tools have the ability to
automate the generation process of such a mesh [1].
The unstructured mesh and the H-grid are the simplest and fastest to create and are suitable
for complex geometries.

2 Theory
19
2.2 Meshing tools
This section explores different open-source meshing tools and compares the two meshing
tools Salome and Gmsh.
2.2.1 Open-source meshing tools
blockMeshDict is a dictionary file in OpenFOAM where a geometry and mesh can be
programmed. The mesh is generated with the blockMesh command. However, since there is
no graphical user interface (GUI) and only a basic hexahedral mesh algorithm, the use of this
utility is limited to simple geometries and meshes.
There exist many open-source meshing tools that are more advanced than blockMesh. Some
of the tools exist within OpenFOAM, like snappyHexMesh, some have a GUI, and others
have both a geometry and meshing module.
The meshing tool chosen for the student tutorial should be an approved and user-friendly
tool. Some essential features of the software to be used in the student tutorial are:
• GUI
• Geometry module
The two criteria are set to ensure the user-friendliness and simplicity of the tutorial. A GUI is
desired because it eliminates the need for programming and makes the tool accessible. A
geometry module is favorable because it enables geometry and mesh generation in the same
software. If a meshing tool does not have a geometry module, the geometry file (e.g.,
STEP/STL) must first be created and exported from a CAD software.
Different open-source meshing tools have been examined and their features have been
considered. Table 2.1 gives an overview of the assessment of the necessary features. As
shown in Table 2.1, only Salome, Gmsh and Netgen/NgSolve include both a geometry
module and a GUI, and are therefore the only software relevant for the student tutorial.

2 Theory
20
Table 2.1: Assessment of essential features available in open-source meshing tools.
Meshing tool Geometry module GUI
Salome X X
Gmsh X X
snappyHexMesh
cfMesh
Netgen/NgSolve X X
enGrid (with Netgen) X
Tetgen
2.2.2 Comparison of Salome and Gmsh
Salome, Gmsh and Netgen/NGSolve are determined to be the only meshing tool candidates
for the tutorial. However, Netgen/NgSolve is not evaluated further because Salome and Gmsh
are considered to be more popular and widespread software.
To determine the meshing software for the student tutorial, further evaluations of Salome and
Gmsh have been conducted. The same geometry2
was modeled and meshed with an
unstructured tetrahedral mesh algorithm in each software. A comparison of the software’s
user-friendliness and features was performed. The comparison key findings are summarized
in Table 2.2. The quality of the generated meshes was not evaluated and compared.
2
A diverging converging pipe with belly section, same geometry as in the tutorial.

2 Theory
21
Table 2.2: Comparison of Salome and Gmsh.
Salome-CFD 8.5 Gmsh 3.0.6
GUI yes yes
Object browser yes no
Complex geometry module yes no
Import of CAD-file yes yes
Edit geometry in GUI no no
Delete objects in GUI yes no
Undo command no yes3
Save as command yes no
Must change/choose settings no yes
Automatically saves file in correct format yes no
File extension .py .geo
Programming language python Gmsh's own
Easy modification of script file from GUI no yes
User forum yes no4
Easy to use advanced meshing tool yes no
Tetrahedral mesh algorithm Netgen Gmsh
As shown in Table 2.2, both software have advantages and disadvantages, and there is no
clear winner. However, after some evaluation, it was decided to use Salome in the tutorial.
Salome has a more user-friendly GUI with little need for simultaneous editing of the script,
because it has an object browser that lists all the created objects. Gmsh, on the other hand,
does not have an object browser, so there is no possibility to show or delete objects in the
GUI. As a consequence, simultaneous editing of the script is unavoidable.
3
Modules → Geometry → Remove last script.
4
It is possible to post issues to the developers at https://gitlab.onelab.info/Gmsh/Gmsh/-/issues.

2 Theory
22
Another advantage is that Salome uses the Python scripting language, which the students are
already familiar with, while Gmsh uses its own. In addition, Salome has a more advanced
geometry module that resembles a CAD software. The implementation of other geometries of
more applied cases is considered to be easier in Salome. Moreover, Salome has multiple
meshing algorithms and advanced meshing options.
However, for even more complex geometries, the Salome geometry module may not be
suitable. In these cases, the geometry can be drawn in an open-source drawing software, such
as FreeCAD or Blender, and exported to Salome.
2.3 Turbulence boundary layer theory
This section describes turbulence boundary layers, estimation of 𝑦+
and wall treatment.
Turbulent flow within solid smooth walls behaves significantly different than free stream
turbulent flow.
Equation (2.2) shows the law of the wall, which describes how the velocity of the flow
𝑈 [𝑚/𝑠] is dependent on the distance from the wall, 𝑦 [𝑚], the wall shear stress, 𝜏𝑤 [𝑃𝑎], the
dynamic viscosity, 𝜇 [𝑁𝑠/𝑚2
] and the density, 𝜌 [𝑘𝑔/𝑚3
]. It also describes the relationship
between the dimensionless groups 𝑦+
and 𝑢+
.
𝑢+
=
𝑈
𝑢𝜏
= 𝑓 (
𝜌𝑢𝜏𝑦
𝜇
) = 𝑓(𝑦+) (2.2)
Where 𝑓 symbolizes a function. The friction velocity, 𝑢𝜏 [𝑚/𝑠], is given by Equation (2.3):
𝑢𝜏 = √
𝜏𝑤
𝜌
(2.3)
The law of the wall is illustrated in Figure 2.13 [17].

2 Theory
23
Figure 2.13: Law of the wall [17].
The fluid velocity is zero at the wall. Closest to the wall, there is a thin layer where the fluid
flow is dominated by viscous effects. This region is called the viscous sub-layer or the linear
sub-layer and in this layer the values of 𝑦+
< 5. In this layer it is assumed that the wall shear
stress and the shear stress, 𝜏 [𝑃𝑎] are constant and equal.
Equation (2.4) shows that the viscous sub-layer has a linear relationship between the distance
from the wall and the velocity.
𝑈 =
𝜏𝑤𝑦
𝜇
(2.4)
Of this relationship follows Equation (2.5):
𝑦+
= 𝑢+ (2.5)
The buffer layer is the region outside the viscous sub-layer where 5 < 𝑦+
< 30. In this area,
the viscous and turbulent stresses are considered to be equal.

2 Theory
24
The log-law layer is located outside the viscous sub-layer and the buffer layer. It is defined as
the region where 30 < 𝑦+
< 500. In this region there is a logarithmic relation between 𝑢+
and 𝑦+
. Both turbulent and viscous effects influence the flow, but the turbulent stresses are
predominating.
In the outer layer, far from the wall, where 𝑦+
> 500, inertia forces dominate the flow and
the viscous forces are negligible. In this region the velocity-defect law or the law of the wake,
Equation (2.6), is valid.
𝑈𝑚𝑎𝑥 − 𝑈
𝑢𝜏
= 𝑔 (
𝑦
𝛿
) (2.6)
Where 𝛿 [𝑚] is the boundary layer thickness, 𝑈𝑚𝑎𝑥 [𝑚/𝑠] is the maximum velocity at the
pipe centerline and 𝑔 symbolizes a function [5, pp. 57-59].
2.3.1 Estimation of 𝑦+
𝑦+
is given by Equation (2.7) [5, p. 275]:
𝑦+
=
∆𝑦𝑃
𝜈
𝑢𝜏 =
∆𝑦𝑃
𝜈
√
𝜏𝑤
𝜌
(2.7)
Where ∆𝑦𝑃 [𝑚] is the distance from the nearest node 𝑃 to the wall and 𝜈 [𝑚2
/𝑠] is the
kinematic viscosity.
If 𝑦+
≤ 11.63 the flow near the wall is considered to be entirely dominated by viscous
effects and is assumed to be laminar. If 𝑦+
≥ 11.63 the flow is considered turbulent and wall
functions (WF) must be used to model the flow. The intersection between the linear profile
and the log law curve occurs at the value of 𝑦+
= 11.63, as illustrated in Figure 2.13 [5, p.
275].
The wall shear stress, 𝜏𝑤, is defined by Equation (2.8) [18, p. 362]:

2 Theory
25
𝜏𝑤 =
𝐶𝑓𝜌𝑈2
2
(2.8)
Where 𝐶𝑓 is the skin friction coefficient. Several different formulas for the approximation of
the skin friction coefficient based on boundary layer theory for flat plates are available in the
literature. White [19, p. 473] proposes Equation (2.9):
𝐶𝑓 =
0.027
𝑅𝑒
1
7
(2.9)
Where 𝑅𝑒 [−] is the Reynolds number.
Since the friction velocity is not known before running a simulation, Equation (2.7) only
approximates the 𝑦+
. The actual 𝑦+
must be determined after running a simulation [12, p.
855].
2.3.2 Wall treatment
Wall functions are used to model the flow in the near-wall area. The first wall function was
formulated by Spalding in 1961 [20]. In the literature, wall functions are covered by among
others Kalitzin et al. [21], Bredberg [22], Liu [23] and Liu [24].
The standard wall functions are based on the law of the wall and are valid in the log-law
region. Thus, wall functions should be used when the node closest to the wall is placed in the
log-law region, where 30 < 𝑦+
< 500. However, a value of 𝑦+
> 11.63 might be acceptable
[5, p. 283]. Some advantages of the wall function approach are that it allows for a coarse grid,
which reduces the requirements of the computer and the computational cost, along with
improved convergence and numerical stability.
The wall function approach is expected to give less accurate results, as it may not model the
flow adjacent to the wall adequately. The wall function method requires a high-Reynolds-
number (HRN) turbulence model.
To accurately resolve the flow in the boundary layer, the mesh near the wall must be very
fine. The node closest to the wall must be placed in the viscous region where 𝑦+
< 5.
However, a value of 𝑦+
≤ 1 is recommended. In the viscous layer, the log-law is not valid,

2 Theory
26
so wall functions are inaccurate and should not be used. The appropriate turbulence model for
this condition is a low-Reynolds-number (LRN) model. An LRN-model is a model that can be
integrated towards the wall. The disadvantage with this approach is that the requirements of
the computer and the computational cost increase with a finer mesh.
In the buffer layer, there are rapid fluctuations in the turbulent source terms, and it is
challenging to predict and model the flow behavior. If the first node is located in the buffer
layer, neither the wall function approach nor the full resolution approach is fitting. Therefore,
it is recommended not to place the first node in the buffer layer. The general practice is to
either position the first node in the viscous sub-layer and use an LRN-model, or place it in the
log-law layer and use an HRN-model [5, pp. 85, 106, 275-276, 283], [22].
If 𝑦+
< 30 and wall functions are used, the flow predicted by the wall functions may be
inaccurate or erroneous [5, p. 279]. However, in complex flows and geometries, it may be
challenging to fulfill the 𝑦+
requirement at certain locations in the domain. As a
consequence, the flow downstream of a 𝑦+
violation can be affected by an inaccurate solution
upstream[5, p. 292].
In the design phase of a mesh it is important to keep in mind the desired turbulence model,
wall treatment and 𝑦+
. The equations in Chapter 2.3.1 can give an estimate of the 𝑦+
and the
required distance to the first computational interior node.

2 Theory
27
2.4 Turbulence modeling
This section describes turbulent flow characteristics, the turbulence models 𝑘 − 𝜀 and
𝑘 − 𝜔 𝑆𝑆𝑇, simulation time step and pressure loss.
2.4.1 Turbulent flow characteristics
The volume flow, 𝑄 [𝑚3
/𝑠], is given by Equation (2.10):
𝑄 = 𝑈𝐴 (2.10)
Where 𝐴 [𝑚2] is the cross-sectional area of the pipe and is calculated as shown in Equation
(2.11):
𝐴 =
𝜋𝐷2
4
(2.11)
The continuity equation for an incompressible fluid flowing through a pipe is given by
Equation (2.12) [18, p. 109]:
𝑄 = 𝑈𝑖𝑛𝐴𝑖𝑛 = 𝑈𝑜𝑢𝑡𝐴𝑜𝑢𝑡 (2.12)
Where the subscripts 𝑖𝑛 is the location of the inlet and 𝑜𝑢𝑡 is the location of the outlet.
The critical Reynolds number for a circular tube is approximately 2300. The flow is laminar
for Reynolds numbers below this value. For Reynolds numbers between 2300 and 4000 the
flow is transitional. The Reynolds number must be 4000 to achieve fully developed turbulent
flow [25].
The Reynolds number for a pipe is given by Equation (2.13):
𝑅𝑒 =
𝑈𝐷
𝜈
(2.13)

2 Theory
28
Where 𝐷 [𝑚] is the diameter.
The kinematic viscosity is calculated by dividing the dynamic viscosity with the fluid density,
as displayed in Equation (2.14):
𝜈 =
𝜇
𝜌
(2.14)
Fully developed turbulent flow occurs when the velocity profile does not change in the
direction of the flow. The hydrodynamic entry length, 𝑥𝑓𝑑,ℎ [𝑚], is defined as the length from
the inlet until fully developed flow occurs. The hydrodynamic entry length is dependent on
many factors and an approximation is shown in Equation (2.15) [26]:
10 ≲
𝑥𝑓𝑑,ℎ
𝐷
≳ 60 (2.15)
The maximum velocity occurs at the centerline of the pipe and is a function of the mean
velocity. The maximum velocity for laminar flow, 𝑈𝑚𝑎𝑥,𝑙𝑎𝑚, is given by Equation (2.16) [18,
p. 264]:
𝑈𝑚𝑎𝑥,𝑙𝑎𝑚 = 2𝑈 (2.16)
The maximum velocity for turbulent flow, 𝑈𝑚𝑎𝑥,𝑡𝑢𝑟𝑏, is given by Equation (2.17) [18, pp.
277-278]:
𝑈𝑚𝑎𝑥,𝑡𝑢𝑟𝑏 = (1 + 1.44√𝑓𝑡𝑢𝑟𝑏 )𝑈 (2.17)
Where 𝑓𝑡𝑢𝑟𝑏 [−] is the turbulent friction factor.
The turbulent velocity profile is predicted by Equation (2.18) [18, pp. 277-278]:
𝑈 = (1 + 1.44√𝑓𝑡𝑢𝑟𝑏 )𝑈 − 2.15√𝑓𝑡𝑢𝑟𝑏𝑈 ∙ 𝑙𝑜𝑔10
𝑟0
𝑟0 − 𝑟
(2.18)

2 Theory
29
Where 𝑟0 [𝑚] is the radius of the pipe and 𝑟 [𝑚] is any radius.
2.4.2 𝑘 − 𝜀 turbulence model
The 𝑘 − 𝜀 model is the most widespread and verified turbulence model and is extensively
used in engineering applications in the industry [5, pp. 78, 97]. It is a Reynolds-averaged
Navier-Stokes (RANS) turbulence model. The 𝑘 − 𝜀 model in OpenFOAM (kEpsilon) is
based on the standard model by Launder and Spalding [27] and on the Rapid Distortion
Theory (RDT) compression term by El Tahry [28]. It is a two-equation model, with one
equation for 𝑘 and one for 𝜀. The standard 𝑘 − 𝜀 model is an HRN-model and needs wall
functions. Some disadvantages with the model are that it predicts too high quantities of shear
stresses, as well as turbulence in stagnation locations. Some advantages are that it is
computationally efficient and gives good results for many industrial flow problems [1], [5,
pp. 88, 97], [29].
In a CFD simulation inlet values of 𝑘 and 𝜀 must be provided as boundary conditions.
Measurements of these values for a given CFD case are frequently not available in the
literature. However, formulas based on the turbulence length scale, 𝑙, and the turbulence
intensity, 𝑇𝑖, can give an approximation [5, p. 76].
The turbulence length scale, 𝑙 [𝑚], for a circular pipe is given by Equation (2.19):
𝑙 = 0.07𝐷 (2.19)
The turbulence intensity, 𝑇𝑖 [−], is given by Equation (2.20) [30, Eq. (6.68)].
𝑇𝑖 = 0.16𝑅𝑒−
1
8 (2.20)
The turbulence kinetic energy, 𝑘 [𝑚2
/𝑠2
], and turbulence dissipation rate, 𝜀 [𝑚2
/𝑠3
], are
given by Equations (2.21) - (2.22):
𝑘 =
3
2
(𝑇𝑖𝑈)2 (2.21)

2 Theory
30
𝜀 =
𝐶𝜇
3
4
𝑘
3
2
𝑙
(2.22)
Where 𝐶𝜇 is a constant equal to 0.09 [5, pp. 76-77].
2.4.3 𝑘 − 𝜔 𝑆𝑆𝑇 turbulence model
The 𝑘 − 𝜔 turbulence model is a RANS model and is the most common alternative to the
𝑘 − 𝜀 model. The 𝑘 − 𝜔 Shear Stress Transport (SST) turbulence model in OpenFOAM
(kOmegaSST) is based on the model by Menter and Esch [31] and the updated model by
Menter et al. [32]. It is a two-equation model, with one equation for 𝑘 and one for 𝜔. It is a
hybrid model; in the near-wall region, the 𝑘 − 𝜔 model is used and in the fully turbulent
region 𝑘 − 𝜀 is used. Advantages of the hybrid model are that the 𝑘 − 𝜔 model performs
better than 𝑘 − 𝜀 in the near-wall area, while the 𝑘 − 𝜀 model is more robust in the fully
turbulent region. As a result, the solution is numerically stable and robust. The model also has
the capacity to model flow separation. The model can solve the flow in the near-wall area and
can be used without wall functions in LRN applications. One disadvantage is that the model
does not model the interactions between the mean flow and turbulent stresses accurately [5,
pp. 90-92], [33].
The turbulence dissipation rate, 𝜔 [𝑠−1
] is given by Equation (2.23) [33].
𝜔 =
√𝑘
𝐶𝜇
1
4
𝑙
(2.23)
The turbulence kinetic energy, 𝑘, is calculated as for the 𝑘 − 𝜀 model, by Equation (2.21).

2 Theory
31
2.4.4 Time step
The appropriate time step of a simulation can be estimated with the Courant number. The
courant number expresses how much information is transferred in one time-step through one
cell. An appropriate courant number helps ensure numerical stability and convergence of the
simulation. A courant number of 1 is often considered to give a good result. The definition of
the Courant number in 1D is shown in Equation (2.24):
𝐶𝑜𝑢𝑟𝑎𝑛𝑡 𝑛𝑢𝑚𝑏𝑒𝑟 =
𝑈∆𝑡
∆𝑥
(2.24)
Where ∆𝑡 [𝑠] is the time step and ∆𝑥 [𝑚] is the length of a grid cell [12, pp. 616-618].
The courant number is of significant importance in transient simulations. However, in steady
state simulations, the courant number should not notably affect the simulation, and the time
step is considered to be an iteration counter [34].
2.4.5 Pressure loss
The static pressure, 𝑝 [𝑃𝑎], is defined as the fluid pressure in a moving fluid.
The pressure results in OpenFOAM for incompressible solvers like simpleFoam, are given as
the kinematic pressure, 𝑝𝑘 [𝑚2
/𝑠2
]. The static pressure is calculated by multiplying the
kinematic pressure with the fluid density, as shown in Equation (2.25).
𝑝 = 𝑝𝑘⋅𝜌 (2.25)
Stagnation pressure, 𝑝0 [𝑃𝑎], is defined as the sum of the static pressure and the dynamic
pressure, 𝜌
𝑈2
2
[𝑃𝑎], as shown in Equation (2.26), and is valid for incompressible fluids [18,
p. 139].
𝑝0 = 𝑝 + 𝜌
𝑈2
2
(2.26)

2 Theory
32
The steady flow energy balance for an incompressible fluid along a streamline is given by
Equation (2.27) [18, p. 145]:
1
2
𝜌𝑈𝑖𝑛
2
+ 𝑝𝑖𝑛 + 𝜌𝑔𝑧𝑖𝑛 − 𝑝𝑙𝑜𝑠𝑠 =
1
2
𝜌𝑈𝑜𝑢𝑡
2
+ 𝑝𝑜𝑢𝑡 + 𝜌𝑔𝑧𝑜𝑢𝑡
(2.27)
Where 𝑝 [𝑃𝑎] is the gage pressure, 𝑧 [𝑚] is the elevation, 𝑔 [𝑚/𝑠2
] is the gravitational
acceleration and 𝑝𝑙𝑜𝑠𝑠 [𝑃𝑎] is the total pressure loss.
For a pipe with no change in elevation between inlet and outlet, 𝑧𝑖𝑛 = 𝑧𝑜𝑢𝑡. When the
pressure at the discharge is the same as that of the surrounding pressure, the gage pressure at
the outlet is zero, 𝑝𝑜𝑢𝑡 = 0. Then, Equation (2.27) reduces to Equation (2.28):
1
2
𝜌𝑈𝑖𝑛
2
+ 𝑝𝑖𝑛 − 𝑝𝑙𝑜𝑠𝑠 =
1
2
𝜌𝑈𝑜𝑢𝑡
2 (2.28)
The total pressure loss is the sum of the pressure loss due to friction, 𝑝𝑓𝑟𝑖𝑐𝑡𝑖𝑜𝑛, and the
pressure loss due to obstruction, 𝑝𝑜𝑏𝑠𝑡𝑟𝑢𝑐𝑡𝑖𝑜𝑛, and is given by Equation (2.29):
𝑝𝑙𝑜𝑠𝑠 = ∑ 𝑝𝑓𝑟𝑖𝑐𝑡𝑖𝑜𝑛 + ∑ 𝑝𝑜𝑏𝑠𝑡𝑟𝑢𝑐𝑡𝑖𝑜𝑛 (2.29)
The pressure loss due to friction is given by Equation (2.30) [18, p. 261]:
𝑝𝑓𝑟𝑖𝑐𝑡𝑖𝑜𝑛 = 𝑓
𝐿
𝐷
1
2
𝜌𝑈2 (2.30)
Where 𝐿 [𝑚] is the length of the pipe section.
For laminar flow in a pipe, the friction factor, 𝑓𝑙𝑎𝑚 [−], is given by Equation (2.31) [18, p.
265]:
𝑓𝑙𝑎𝑚 =
64
𝑅𝑒
(2.31)

2 Theory
33
For turbulent flow in a pipe, the friction factor, 𝑓𝑡𝑢𝑟𝑏 [−], can be approximated by the
Swamee-Jain equation, Equation (2.32) [35, Eq. 19], which is based on the Darcy-Weisbach
equation and the Colebrook-White equation.
𝑓𝑡𝑢𝑟𝑏 =
0.25
[log10 (
1
3.7 (
𝐷
𝜖
)
+
5.74
𝑅𝑒0.9)]
2
(2.32)
Where 𝜖 [𝑚] is the roughness height of the pipe wall. Equation (2.32) is valid for
5000 < 𝑅𝑒 < 108
and 10−6
<
𝜖
𝐷
< 10−2
.
For smooth walls, the roughness height of the pipe wall is zero [18, p. 284]. The friction
factor for smooth walls can be approximated by Equation (2.33) by Blasius [36]:
𝑓𝑡𝑢𝑟𝑏 =
0.316
𝑅𝑒0.25
(2.33)
Equation (2.33) is valid for 3000 < 𝑅𝑒 < 105
.
The pressure loss due to obstruction is given by Equation (2.34) [37, p. 69]:
𝑝𝑜𝑏𝑠𝑡𝑟𝑢𝑐𝑡𝑖𝑜𝑛 = 𝐾 ⋅
𝜌
2
𝑈2 (2.34)
Where 𝐾 [−] is the obstruction loss factor.
A table with obstruction loss factors for different obstructions is available in [37, Tab. 2.1].
Some relevant obstruction loss factors are listed in Table 2.3.

2 Theory
34
Table 2.3: Obstruction loss factors [37, Tab. 2.1].
Obstruction K
Tank exit 0.5
Tank entry 1.0
Conical enlargement:
(total included angle)
6° 0.13
10° 0.16
15° 0.30
25° 0.55
Sudden contractions:
Area ratio (A2/A1)
0.2 0.41
0.4 0.30
0.6 0.18
0.8 0.06

3 Case
35
3 Case
In this section the flow geometry, meshes, simulation cases, numerical setup and student
tutorial are presented. The software used in the cases is listed in Appendix B.
3.1 Geometry
A relatively complex flow geometry is chosen for the case. The geometry is a 3D model of a
diverging converging pipe with belly section. Figure 3.1 shows the geometry with
measurements. The inlet section has a diameter of 20 mm, the diameter of the belly section is
60 mm, and the diameter of the outlet section is 10 mm. The length of the inlet section is 300
mm (15𝐷), the diverging, belly and converging sections have a length of 50 mm each, and
the outlet section is 300 mm (30𝐷) long.
A technical drawing of the pipe is available in Appendix C.
Figure 3.1: Geometry.
The geometry is modeled in the geometry module in Salome. Based on the theory presented
in Section 2.1.3, it is decided to create an OH-grid, and the interior geometry is designed to
enable the meshing of this grid. The pipe consists of a divided disk with five quadrangles
extruded along the pipe length, as shown in Figure 3.2. The quadrilateral design is a template
for the hexahedral OH-grid. When the pipe is divided into quadrangles, the quadrangle
mapping algorithm in Salome can create a fully hexahedral mesh without highly skewed
cells.
Another option for creating a block-structured mesh is to use the HexaBlock module in
Salome. This module creates the geometry in the form of blocks, which makes a basis for
hexahedral mesh construction in the mesh module [38].

3 Case
36
The method of creating the geometry is described in the student tutorial in Appendix N.
Figure 3.2: Sub-regions for the OH-grid.
3.2 Meshes
The meshes are created in the mesh module in Salome. The mesh type is hexahedral, created
with the 3D Hexahedron, 2D Quadrangle Mapping and 1D Wire Discretization algorithms.
The 1D algorithm discretizes lines in the domain, the 2D algorithm creates 2D surfaces and
domains, and the 3D algorithm creates volume meshes from the 2D meshes.
Furthermore, sub-meshes in the axial direction are created to ensure the desired distribution
and number of cells. For some of the meshes, sub-meshes with grading in the radial direction
are created on the outer quadrangles to control the distance from the wall to the first interior
node. In addition, the mesh groups inlet, outlet and wall are created for the simulation in
OpenFOAM.
The result is an OH-grid with quadrangle surfaces and hexahedron volumes, as shown in
Figure 3.3. The OH-grid is extruded along the pipe length; the grid expands radially outwards

3 Case
37
in the diverging section of the pipe and contracts radially inwards in the converging section
of the pipe.
Figure 3.3: Mesh.
3 different meshes are created for the pipe geometry to account for different wall treatments.
The meshes are built with the same pattern in the axial direction and in the center quadrangle,
but differ in the four quadrangles towards the wall. The python script for the meshes is
available in Appendix D.
Descriptions of the meshes are given in Table 3.1.
Mesh A (Figure 3.4) is the original mesh and was created without considering the value of
𝑦+
, only the general mesh quality. Mesh B (Figure 3.5) is created to be used with wall
functions and aims for a 𝑦+
of 30 at the inlet. Mesh C (Figure 3.6) is created to be used with
the full resolution approach and aims for a 𝑦+
less than 1. Mesh B and Mesh C are graded
towards the wall.
The equations presented in Chapter 2.3.1 are used for the calculations of 𝑦+
.

3 Case
38
Figure 3.4: Mesh A. Figure 3.5: Mesh B.
Figure 3.6: Mesh C.
Table 3.1 shows that the non-orthogonality of the three meshes is quite similar. The
maximum non-orthogonality appears in Mesh A. Likewise; the maximum skewness also
appears in Mesh A. However, the maximum aspect ratio is significantly larger in Mesh C
than in the other meshes because of the thin layers of cells near the wall. Mesh B has the
lowest non-orthogonality, skewness and aspect ratio.

3 Case
39
Table 3.1: Mesh cases.
Mesh A B C
∆𝒚𝑷 [𝒎𝒎] 0.33 2.36 0.041
Calculated 𝒚+
at inlet 4.24 30.33 0.53
Appropriate turbulence model LRN5
HRN LRN
Mesh description original 𝑦+
≈ 30 𝑦+
≤ 1
Number of cells 375 000 135 000 675 000
Max aspect ratio 7.04 6.63 44.41
Mesh non-orthogonality:
Max 35.00 28.36 33.92
Average 8.47 7.31 7.75
Max skewness 2.04 1.26 1.62
Desired turbulence model kEpsilon kEpsilon kOmegaSST
Wall treatment Wall functions Wall functions Full resolution
Visualizations of the aspect ratios and skewness of the circular cross-sections are available in
Appendix F. Mesh A has the highest aspect ratio just outside the corners of the middle
quadrangle. The highest aspect ratios of Mesh B occur in the layer of cells closest to the wall
and from the outer corners of the middle quadrangle towards the wall. Mesh C has the highest
aspect ratios in the thin layers of cells closest to the wall, although the figure does not display
the colors visibly. The maximum skewness in Mesh A and Mesh C occur in the cells in the
regions outside the corners of the middle quadrangle. The cells of Mesh B have the largest
skewness in the corner areas in the layer outside the middle quadrangle.
The procedure to create Mesh B is described in the student tutorial in Appendix N. The
procedure to create Mesh A and Mesh C is explained in Appendix M.
The method to import a mesh created in Salome to OpenFOAM is described in Appendix E.
5
𝑦+
< 5 places the first node in the viscous region, but for LRN models the value should ideally be 𝑦+
≤ 1.

3 Case
40
The checkMesh command did not detect any errors in any of the meshes.
3.3 Simulation cases
The case is a complex internal pipe flow problem. Air enters the pipe inlet at a velocity of
3 m/s at a Reynolds number of 4000, thus fully turbulent flow. The physics involved in the
model is quite complex, because turbulent, transition and laminar flow occur. When the
cross-section of the pipe expands to the belly section, the flow transitions to laminar flow.
When the pipe contracts to the narrower outlet section, the flow transitions back to turbulent.
The turbulent air flow continues through the outlet section at and leaves the pipe at the outlet.
The flow medium is air at 20 ℃. The flow is 3D, isothermal and without gravity forces. The
flow is modeled with the RANS turbulence models standard 𝑘 − 𝜀 and 𝑘 − 𝜔 𝑆𝑆𝑇. The
simpleFoam solver in OpenFOAM is used to calculate the pipe flow. simpleFoam is a solver
for steady-state turbulent incompressible flow, which uses the semi-implicit method for
pressure-linked equations (SIMPLE) algorithm or the semi-implicit method for pressure-
linked equations-consistent (SIMPLEC) for the solution of the momentum and continuity
equations.
To ensure the user-friendliness of the student tutorial, the case is based on a tutorial available
in OpenFOAM6
, pitzDaily [39]. The contents of the pitzDaily directory can be copied to a
new working directory and only small changes need to be made.
The initial and boundary conditions are adjusted to fit the current case and the boundaries and
patches are changed to correspond to the imported mesh. Furthermore, the turbulent
properties 𝑘, 𝜀 and 𝜔 are calculated with the equations given in Section 2.4.2 and 2.4.3 and
the kinematic viscosity of air is adjusted. Constants and boundary conditions are listed in
Appendix H.
Table 3.2 summarizes the numerical setup of the 4 simulation cases.
6
Path: /opt/openfoam8/tutorials/incompressible/simpleFoam/pitzDaily

3 Case
41
Table 3.2: Numerical setup for the simulation cases.
Case A B1 B2 C
Mesh A B B C
Turbulence model kEpsilon with
default WF
kEpsilon with
default WF
kEpsilon with
adjusted WF
kOmegaSST
Solution algorithm SIMPLE SIMPLEC SIMPLEC SIMPLEC
Number of iterations 688 476 390 1472
Simulation time7 [min] 11 3 3 129
residualControl:
p 1E-05 1E-03 1E-03 1E-05
U 1E-05 1E-03 1E-03 1E-05
k|epsilon|omega 1E-05 1E-04 1E-04 1E-05
relaxationFactors:
p 0.6 0.8 0.7 0.7
U 0.7 0.8 0.7 0.5
k|epsilon|omega 0.7 0.8 0.7 0.7
The relaxation factors, tolerances and algorithms are chosen based on simulation tests and
residual plots to assess the best factors. The values of the solution tolerances and residual
controls are decreased from default to increase the accuracy of the solution. The relaxation
factors are decreased to ensure numerical stability and convergence. SIMPLEC showed better
stability for Cases B1-C. The numerical schemes remain default.
The time step is decreased to 0.0001. The timestep is calculated by setting the Courant
number to 1, velocity to 10 m/s and ∆x to 1 mm. This gives an approximate value for the
whole flow domain, but is not considered to notably influence the simulation in steady state.
7
Simulation time is not fixed, but depends on available computer power.

3 Case
42
Case A is the original case and was made without considering 𝑦+
. Case B1 and Case B2 aim
for a 𝑦+
of 30, and an HRN-turbulence model, the 𝑘 − 𝜀 with wall functions. Case C aims for
a 𝑦+
less than 1, and an LRN-turbulence model, the 𝑘 − 𝜔 𝑆𝑆𝑇.
An overview of different wall functions in OpenFOAM and their properties is given in
Appendix G.
Table 3.3 shows the wall functions used in the 𝑘 − 𝜀 models. Case A and Case B1 use the
default wall functions in the pitzDaily tutorial. The 𝜀 wall function is valid in both the viscous
and log-law layers. The wall functions for 𝑘 and the turbulent viscosity, 𝜇𝑡 [𝑚2
/𝑠 ], (nut) are
only valid in the log-law layer.
Case B2 utilizes other wall functions for 𝑘 and 𝜇𝑡 , specifically the kLowReWallFunction and
the nutUSpaldingWallFunction. The kLowReWallFunction is chosen because it is valid in both
the viscous and log-law layers. The nutUSpaldingWallFunction is chosen because it is valid in
all layers. The intention is that these wall functions can give better accuracy in areas where
𝑦+
< 30.
Table 3.3: Wall functions 𝑘 − 𝜀 models.
Case k epsilon nut
A kqRWallFunction epsilonWallFunction nutkWallFunction
B1 kqRWallFunction epsilonWallFunction nutkWallFunction
B2 kLowReWallFunction epsilonWallFunction nutUSpaldingWallFunction
Table 3.4 shows the wall treatment used in the 𝑘 − 𝜔 𝑆𝑆𝑇 model. The wall treatment is
chosen based on the recommended wall treatment for resolved boundary layer models in [12,
p. 853] and [40].
Table 3.4: Wall treatment 𝑘 − 𝜔 𝑆𝑆𝑇 model.
Case k omega nut
C 0 omegaWallFunction nutLowReWallFunction

3 Case
43
3.4 Student tutorial
A focus of the student tutorial has been to describe a user-friendly, accessible and general
approach to creating and meshing a geometry.
Case B1 is the case chosen for the student tutorial based on the following points:
• Differs the least from the pitzDaily tutorial.
• 𝑘 − 𝜀 is the most validated turbulence model.
• Implements wall functions → short simulation time.
• Demonstrates how to adjust the mesh in the boundary layer region.
• Shows consistent results.
The student tutorial is available in Appendix N.

4 Results and discussion
44
This section presents the results. Basic fluid mechanics checkpoints, symmetry and residuals
are evaluated, and the simulated pressure loss and velocity field are compared to the
analytical solution. Uncertainties and weaknesses of the models are discussed.
4.1 Evaluation of results
In a given CFD simulation there is a risk of errors and uncertainties. Possible errors include
numerical errors caused by errors in roundoff, iterative convergence or discretization.
Additionally, errors can be of the type coding errors and user errors. Uncertainties can be
caused by wrong assumptions, approximations, simplifications and boundary conditions, or
uncertainties related to the physical model [5, pp. 286, 292]. Consequently, it is important to
evaluate the results of a simulation.
Versteeg and Malalasekera [5, pp. 301-302] list some checkpoints for evaluating the results
of a simulation which include:
1. Fluid flows from high to low pressure (in pressure-driven flows)
2. Static pressure decreases when velocity increases (Bernoulli’s theorem for inviscid flows)
3. Friction losses cause a decrease of total pressure in the direction of flow (viscous flow) […]
4. The speed of a fluid near a stationary wall is smaller than the speed further away from
the wall (boundary layer formation)
5. Flow adopts a fully developed state after a sufficiently long distance in a straight duct
with constant cross-section [...]
6. A flow emerging into a large expanse of fluid from a small hole generally forms a jet [...]
An evaluation of each checkpoint is given below:
1. Yes. For all the simulation cases, the outlet static pressure is 0, as seen in the cut plane
visualizations in Appendix I.
2. Yes. If one compares the velocity and static pressure plots in Appendix I, one can see
that they show opposite behavior. The inlet and mid sections show high static pressure
and low velocity, while the outlet section show low static pressure and high velocity.
3. Yes. The total pressure is decreasing in the direction of the flow, as seen in the total
pressure visualizations in Appendix I.
4. Yes. The velocity near the wall is small in all simulation cases, as seen in velocity
distribution visualizations in Appendix I.
5. Yes. As seen in Figure 4.4, all the simulations show signs of fully developed flow at
the end of the outlet section which is 30𝐷 long.

45
6. Yes. The velocity distributions shown in Appendix I show that in all the cases, the
flow emerging from the smaller inlet section to the wider belly section forms a jet.
The simulation results in this report are considered to satisfy all of the listed checkpoints.
4.1.1 Symmetry
In all the cases, the geometry, inlet boundary conditions and flow are symmetrical about the
centerline of the pipe. Thus, in the steady-state model, the simulation results are expected to
be symmetrical. Consequently, unsymmetrical results are a clear indication of numerical
errors.
The solution of the velocity, stagnation pressure (total pressure in OpenFOAM) and static
pressure fields for all the cases are visualized in ParaView with a 2D slice on the Z normal.
The visualizations are shown in Appendix I. The results appear to be symmetrical and
indicate that the simulation cases show symmetrical solutions about the centerline of the pipe.
4.1.2 Residuals
Residuals can be monitored live during the simulation as described in [41, p. 202] or they can
be created after the simulation as described in [42] and demonstrated in the student tutorial in
Appendix N. For both methods, a log file with the terminal output must be created during the
simulations to enable the creation of plots.
The generated residual plots for the simulation cases are shown in Appendix J. All the plots
show relatively stable residuals which decrease or stabilize along a straight line, showing
signs of monotonic convergence. Ergo, steady behavior is indicated, even though some of the
quantities show small oscillations.
In Case B1, B2 and C the pressure is generally the most oscillating quantity. Case A gives the
most stable plot for all the quantities. The fact that Case A shows the most stable residuals
and small solution tolerances demonstrates that a good residual plot does not guarantee a
consistent solution. Nor is a convergent solution necessarily an accurate solution. An unstable
and fluctuating residual plot may indicate that the solution is amiss, but a stable plot does not
subsequently indicate the opposite.

46
4.2 Boundary layer
The 𝑦+
values of a simulation are a direct measure of mesh optimality. In OpenFOAM, 𝑦+
is computed with the post-processing utility. The 𝑦+
field is calculated by typing the
following command in the terminal:
simpleFoam -postProcess -func yPlus
The computed minimum, maximum and average values of 𝑦+
are displayed in the terminal,
and the entire 𝑦+
field can be visualized in ParaView.
Table 4.1 shows the computed 𝑦+
values from the simulations.
Visualizations of the 𝑦+
distributions of the cases are available in Appendix K and they show
that the 𝑦+
distributions of the respective cases do not follow the same pattern. Case A and
Case B1 have the lowest values along the inlet and diverging sections. Case B2 has the
lowest values along the mid section (the diverging, belly and converging sections). Case C
has the lowest values of 𝑦+
along the diverging section, at the intersection of the belly and
converging section, and at the middle part of the converging section.
Case C has a maximum 𝑦+
value of 1.88. The average value is 0.55 and the 𝑦+
visualization
shows that 𝑦+
is mostly lower than 1. Regardless, a 𝑦+
of 1.88 places the first node in the
viscous sub-layer. Thus, Mesh C is considered to be successful in the 𝑦+
distribution for this
flow case and gives good mesh optimality.

47
Table 4.1: Computed 𝑦+
values.
Case A B1 B2 C
Turbulence
model
kEpsilon
(default WF)
kEpsilon
(default WF)
kEpsilon
(adjusted WF)
kOmegaSST
(full resolution)
Required 𝒚+
𝑦+
> 30 𝑦+
> 30 𝑦+
> 30 𝑦+
≤ 1
Calculated 𝑦+ 4.24 30.33 30.33 0.53
Simulation 𝑦+
:
average 3.7 29 27 0.55
max 11 58 50 1.88
min 0.7 8.6 1.6 0.05
Section where
low 𝒚+
occur:
inlet X X
div. X X X X
belly X
conv. X X
outlet
When Mesh A was originally constructed, 𝑦+
was not taken into consideration. However, it
was already decided to use the standard 𝑘 − 𝜀 model. The estimated and computed average
𝑦+
for Case A of less than 5, places the first interior node in the viscous sub-layer.
Consequently, the utilization of wall functions and the standard 𝑘 − 𝜀 model, an HRN-model,
are assumed to give erroneous results.
Case B1 has an average value of 𝑦+
of 29. However, the minimum value of 8.6 places the
first computational node in the buffer layer, where the log-law is not valid. The visualization
of the 𝑦+
distribution shows that the lowest values occur in the region closest to the inlet.
Along the inlet and diverging section the values of 𝑦+
are mostly lower than 30.

48
Case B2 has an average 𝑦+
value of 27. However, the minimum value of 1.6 places the first
near-wall node in the viscous layer. The minimum 𝑦+
value of Case B2 is considerably
smaller than for Case B1. Along the mid section, the lowest 𝑦+
values occur and are mostly
below 20. The 𝑦+
distribution places the first interior nodes in all the sub-layers: viscous,
buffer, log-law.
The intersection between the linear profile and the log law curve occurs at the value of
𝑦+
= 11.63. According to Versteeg and Malalasekera [5, p. 275], one can consider the flow
as turbulent and use wall functions when 𝑦+
≥ 11.63. However, wall functions should
preferably be used when 𝑦+
> 30 [5, p. 283].
The 𝑦+
and wall function dependency does not seem to be covered in the OpenFOAM
documentation. In his master’s thesis, Furbo [43] investigates the 𝑘 − 𝜀 model both with and
without wall functions for HRN and LRN applications for many different meshes with 𝑦+
ranging from around 1 to above 30. The simulations gave varying results. He also points out
that the pitzDaily tutorial in OpenFOAM uses a mesh with 𝑦+
in the range 0.7 to 26, while
using wall functions, thus not fulfilling the wall function requirement.
Since cases B1 and B2 have a large part of the 𝑦+
values larger than 11.63, the wall functions
may give acceptable results. Case A, on the other hand, has a maximum 𝑦+
value of 11,
therefore unsatisfactory results can be expected from the wall function approach.
The 𝑦+
computations confirm that the 𝑦+
estimates must be checked after a simulation.
Moreover, 𝑦+
estimations limited to only one geometrical flow domain (inlet section in this
case) can fail to predict the entire 𝑦+
distribution.
4.2.1 Increasing 𝑦+
Some mesh and simulation tests were carried out to investigate if it was possible to increase
the 𝑦+
values in Case B1. Reducing the number of mesh cells in the outer quadrangles to
only 1 in each quadrangle gives a ∆𝑦𝑃 of 3.3 mm and is demonstrated in Figure 4.1.
Nonetheless, the visualization of the 𝑦+
distribution showed that the 𝑦+
values along the inlet
section do not reach 30.
Consequently, ∆𝑦𝑃 must be even longer to increase the 𝑦+
to 30. However, it is not possible
to increase the ∆𝑦𝑃 more, because the pipe is divided into 5 quadrangles by the divided disk
utility in Salome. An alternative is to create the quadrangles manually.

49
Therefore, no further attempts to increase ∆𝑦𝑃 were made. For this specific geometry and
flow problem, increasing the 𝑦+
even more is considered to give a too coarse and bad-quality
mesh. It would be expected to merely capture basic characteristics of the flow and give low
accuracy of the solution.
Figure 4.1: Coarser mesh, ∆𝑦𝑃 = 3.3 𝑚𝑚.

50
4.3 Pressure loss
The best way to test a CFD computation is to compare the computed results with
experimental results. The model is recognized as validated if the difference in results is
satisfactorily small [5]. However, for this specific work there is no experimental data
available, therefore the solution is compared with the analytical solution.
The analytical solution is calculated with the equations and coefficients given in Section 2.4.
The pressure friction losses are calculated for turbulent flow in the inlet and outlet sections,
and laminar flow for the belly section. In the diverging and converging sections, the
appropriate friction factor is chosen based on the calculated Reynolds number at each point.
The obstruction pressure losses are calculated for the diverging and converging sections of
the pipe. The angle of the divergent section is determined to be 22°. The corresponding value
of the obstruction loss factor for conical enlargement is calculated with linear interpolation.
The converging section is regarded as a sudden contraction. However, the area ratio of 0.03
is considerably smaller than the ratios listed in [37, Tab. 2.1], as shown in Table 2.3, so
interpolation is not considered to give a credible result. As a result, the value of the
obstruction factor is instead approximated to be that of a tank exit.
However, the table values for the obstruction loss factor do not take into account special flow
phenomena, but consider a uniform and homogenous inflow into a given geometrical domain.
The velocity field in the converging section is not uniform, but resembles the shape of a jet; it
has a higher velocity in the area along the centerline than in the area closer to the wall. In
addition, the pressure field is not homogeneous and the flow is transitioning from laminar to
turbulent flow, which further complicate the flow field. These flow phenomena are assumed
to increase the influence of vena contracta8
and the pressure drop. Due to these factors, an
additional 0.5 is added to the obstruction loss factor. An increased obstruction loss factor also
agrees better with the simulation data.
For the friction loss calculations, the correct value of the wall roughness height must be
determined. However, roughness information is not found in the OpenFOAM documentation.
Lipej et al. [44] claim that most CFD analyses are based on hydraulically smooth walls.
Furthermore, in the analyses in [45], [46] and [47] it is assumed that the default wall
roughness in OpenFOAM is smooth. Moreover, on the SimScale platform which uses
OpenFOAM, and in ANSYS, the default wall roughness is smooth [44], [48]. In addition,
there are specific wall functions available in OpenFOAM which account for wall roughness,
8
More information about vena contracta is available in [18, pp. 506-507].

51
namely the nutkRoughWallFunction and the nutURoughWallFunction. Thus, it is assumed
that the default roughness in OpenFOAM is smooth.
The simulated cross-sectional average stagnation pressure loss for the simulation cases, along
with the analytical solution is shown in Figure 4.2.
The method to compute the average stagnation pressure in OpenFOAM is described in
Appendix L.
The values and results of the calculations are shown in Appendix L.
Figure 4.2: Stagnation pressure loss.
The results displayed in Figure 4.2 show that the analytical solution agrees quite well with
Cases B1, B2 and C. Case A, on the other hand, show results diverging from the analytical
solution; the pressure loss is larger, especially along the outlet section.
Since Case A does not satisfy the required 𝑦+
range for standard wall functions, inaccurate
results can be expected. The deviations in Case A support the theory concerning turbulence
boundary layers and wall functions.
0
50
100
150
200
250
300
0 0,05 0,1 0,15 0,2 0,25 0,3 0,35 0,4 0,45 0,5 0,55 0,6 0,65 0,7 0,75
Stagnation
pressure
[Pa]
Pipe length [m]
Pressure loss
Case A Case B1 Case B2 Case C Analytical

52
Even though Case B1 and Case B2 have a considerable amount of 𝑦+
< 30, their results are
consistent with the analytical solution. This can be explained by the fact that most of the
𝑦+
> 11.63. The adjusted wall functions in Case B2 create a small change in pressure from
Case B1, and the overall pressure loss in Case B2 agrees best with the analytical solution of
all the cases.
It should also be noted that Cases B1 and B2 which employ the HRN 𝑘 − 𝜀 models with wall
functions have a grid with considerably less number of cells and shorter simulation time than
Case C with the full resolution approach. Case C runs for more than 2 hours, while Case B1
and Case B2 converge in 3 minutes. Yet, the results are very similar. If anything, Cases B1
and B2 show slightly better agreement with the analytical result in terms of average pressure
loss.
The pressure results support the claim that wall functions are faster and more economical and
can give good approximations of the flow. Although, in this particular case, a simulation time
of 2 hours for the LRN model was not problematic. But in other flow applications, the
simulation time may play a bigger role, especially in simulation cases that take days or
weeks.

53
4.4 Velocity
Figure 4.3 shows the simulated cross-sectional average velocity compared with the calculated
velocity. The calculated velocity is calculated with the continuity equation for each point.
Figure 4.3: Average velocity along pipe length.
The velocities overlap, and it is not possible to observe deviations on the plot, except for in
the region 45-47 mm from the inlet. The analytical solution gives a velocity of 12 m/s when
the pipe diameter is 10 mm at 45 mm from the inlet, thus upholding the continuity equation.
The simulated velocities, on the other hand, can be claimed to violate the continuity equation
in this area because the velocity is lower than predicted. Energy loss cannot be the reason,
because the velocities increase to 12 m/s at 47 mm from the inlet, even though the diameter
has a constant cross-section from 45 mm.
Another interesting result is that Case A, which did not give consistent stagnation pressure
results, matched the other three simulations in terms of average velocity. A reason for this
may be that the computed velocities are more accurate than the computed pressures in Case
A.
Figure 4.4 shows the centerline velocity compared with the calculated centerline velocity.
The analytical maximum velocities are calculated with the equations in section 2.4.1.
Laminar flow is assumed for Reynolds numbers below 4000. For the calculation of the
turbulent centerline velocity, fully developed flow is assumed to be reached at 10𝐷 for the
0
2
4
6
8
10
12
14
0 0,05 0,1 0,15 0,2 0,25 0,3 0,35 0,4 0,45 0,5 0,55 0,6 0,65 0,7 0,75
Velocity
[m/s]
Pipe length [m]
Average velocity

54
inlet section and 15𝐷 for the outlet section, and the centerline velocity 45 mm from the inlet
is assumed to be 13.5 m/s. These approximations make deviations from the calculated
centerline velocity expected. In addition, the standard laminar flow predictions do not take
into account a flow regime with a jet along the axis of the pipe.
Fully developed turbulent flow is achieved when the velocity along the centerline does not
change. Along the inlet pipe section, which is 15𝐷 long, simulation data shows that fully
developed flow is not achieved for all the simulations. However, along the outlet pipe
section, which is 30𝐷 long, simulation data shows that fully developed flow is achieved at
29𝐷 (74 mm from the inlet) for all cases, except Case C. However, the behavior of Case C
indicates that fully developed flow would be achieved downstream if the outlet section had
been slightly longer.
Figure 4.4: Centerline velocity along pipe length.
Figure 4.4 shows that Case C generally agrees best with the analytical solution in the pipe
sections with turbulent flow (inlet and outlet). Cases B1 and B2 display larger deviations
from the analytical solution, especially along the outlet section. They generally show similar
0
2
4
6
8
10
12
14
16
0 0,05 0,1 0,15 0,2 0,25 0,3 0,35 0,4 0,45 0,5 0,55 0,6 0,65 0,7 0,75
Velocity
[m/s]
Pipe length [m]
Centerline velocity

55
behaviour, although Case B2 agrees slightly better with the analytical solution. Case A is
quite consistent with the calculated velocity at the outlet. It should be noted that the analytical
solution in the laminar flow regime is considered to give poor results because of the actual
formation of a jet along the middle section of the pipe.
Figure 4.5 shows the turbulent velocity profile and analytical solution 74 mm from the inlet.
The analytical solution fails to model the velocity at the pipe center and predicts a sharp point
at the center of the pipe, although the profile should be rounded [18, p. 276].
Figure 4.5: Velocity profile 74 mm from the inlet.
Case A and Case C show results consistent with the analytical solution. Case A predicts the
velocity in the area close to the axis best, while Case C predicts the maximum velocity best.
Case B1 and Case B2 diverge from the analytical solution in the area near the wall, which can
be explained by the wall functions. Case B2 shows slightly better agreement with the
analytical solution than Case B1.
0
2
4
6
8
10
12
14
16
-5 -4 -3 -2 -1 0 1 2 3 4 5
Velocity
[m/s]
Pipe radius [mm]
Turbulent velocity profile

56
Comparison of velocities with the analytical solutions show that Case C generally predicts
the velocity field best. Case C is most successful in predicting both the maximum velocity at
the centerline and the turbulent velocity profile. This can be explained by the full boundary
layer resolution approach. LRN models resolve the flow in the boundary layers, while HRN
models with wall functions model the flow in the near-wall area.
4.5 Evaluation of models
This section evaluates the applied mesh topology, flow models, wall functions and analytical
models.
4.5.1 Evaluation of mesh topology
For this particular flow geometry and problem, the OH-grid is not considered to give good
mesh optimality for standard wall functions. When the circular cross-section of the pipe is
expanding or contracting, the aspect ratio of the OH-grid in the radial direction stays
constant. This makes it difficult to control the height of the first node in all the sections of the
pipe. Moreover, it was not possible to increase the 𝑦+
> 30 in most areas without getting too
low mesh quality.
However, for the full resolution approach, the OH-grid gives good mesh optimality, and it is
even possible to decrease the values of 𝑦+
more by refining the mesh in the near-wall area.
The drawback of the fine grid close to the wall is that the cells there attain a large aspect
ratio, which reduces the mesh quality.
4.5.2 Evaluation of flow models
According to Kalitzin et al. [21] RANS models are unable to predict transitional flow
satisfactorily. Turbulence models should generally not be used to model transitional and
laminar flows because it can cause erroneous results.
In this case, turbulence models were applied to a complex geometry with turbulent, transition
and laminar flow regimes. However, the models overall seem to have predicted the general
flow behavior quite consistent with the analytical solution.
In the discussion forums, some claim that the 𝑘 − 𝜔 𝑆𝑆𝑇 model performs better in laminar
flow than the 𝑘 − 𝜀 model. However, there is no clear indication that this is the case here, and

57
any discrepancy from the 𝑘 − 𝜀 model is more likely caused by the difference in wall
treatment.
4.5.3 Evaluation of wall functions
Assessment of the pressure and velocity results show that the adjusted wall functions applied
in Case B2 seem to have predicted the flow slightly better than the default wall functions
utilized in Case B1. Thus, the intention of better accuracy with the adjusted wall functions
was achieved.
4.5.4 Evaluation of analytical models
The analytical solutions presented are based on approximations and simplifications and
generally do not take into account the specific flow phenomena occurring in this particular
model. Therefore, it can be difficult to know for sure what cases obtained the best result in a
given comparison, especially if the cases do not show large deviations from each other.

5 Conclusion
58
5 Conclusion
Theory concerning mesh quality parameters and turbulence modeling have been presented
and an evaluation of different open-source meshing tools has been made. Salome was
evaluated to be the most user-friendly tool and was used to create and mesh a 3D model of a
diverging converging pipe with belly section. 3 meshes with a hexahedral OH-grid and
different wall treatments were constructed and imported to OpenFOAM.
4 simulations of air flowing through the pipe were run with the steady-state turbulent
incompressible flow solver simpleFoam. Case A and Case B1 applied Mesh A and Mesh B,
respectively, with the standard 𝑘 − 𝜀 model and default wall functions. Case B2 used Mesh
B with the standard 𝑘 − 𝜀 model and adjusted wall functions. Case C utilized Mesh C with
the 𝑘 − 𝜔 𝑆𝑆𝑇 model and full boundary layer resolution.
The computed average 𝑦+
values were 3.7, 29, 27 and 0.55 for Cases A, B1, B2 and C,
respectively. Case A did not fulfill the wall function requirements. The OH-grid topology
was evaluated to give good mesh optimality for the full resolution approach and
unsatisfactory mesh optimality for the wall function approach. An evaluation of basic fluid
mechanics checkpoints, symmetry and residuals did not indicate numerical errors in the
solutions.
The stagnation pressure loss agreed quite well with the analytical solution for Cases B1, B2
and C. Case B2 showed the most accurate result, while Case A showed results diverging from
the analytical solution and obtained too large pressure loss.
All the cases showed consistent average velocity results compared with the analytical
solution, except for in the inlet region of the outlet section, where all the simulations showed
a lower velocity than predicted. Comparisons of maximum velocities along the centerline
with the analytical solution showed that Case C achieved the best agreement with the
analytical solution. Cases B1 and B2 displayed some deviations from the analytical solution.
Assessment of the turbulence velocity profile demonstrated that Case A and Case C obtained
results quite consistent with the analytical solution. Case B1 and Case B2 diverged from the
analytical solution in the area near the wall, which can be explained by the wall functions.
The simulation cases generally obtained results that agreed well with the analytical solutions,
even though the complex flow field of turbulent, transitional and laminar flow was modeled
with turbulence models. The adjusted wall functions gave slightly better results than the
default wall functions for the 𝑘 − 𝜀 model. The 𝑘 − 𝜀 model on Mesh B obtained pressure
results that agreed well with the analytical solution. The 𝑘 − 𝜔 𝑆𝑆𝑇 model generally
predicted the velocity field best, and also showed consistent results in terms of pressure loss.

5 Conclusion
59
A student tutorial describing the workflow of case B1 was made.
5.1 Further work
Possible further work on the simulation cases could be to make additional assessments of the
results. Additional parameters could be checked, and force plots could be implemented. For
the 𝑘 − 𝜔 𝑆𝑆𝑇 model, a grid independence study could be performed to check if the mesh
resolution influences the results. Furthermore, the length of the inlet and outlet sections could
be increased to 60𝐷 to achieve fully turbulent flow for all cases and to get a better overview
of the flow development.
The student tutorial has many areas of improvement. The main weakness of the tutorial is that
it only provides a step-by-step explanation of the workflow. It may be a good idea to add
some theory about weaknesses of the model, mesh quality, boundary layers, wall functions
and calculation formulas for 𝑘 and 𝜀. Furthermore, descriptions of some steps could be more
detailed, tables and figures could be referred to, and the post-processing in ParaView could
be described.
When learning to use a new meshing software, it can be difficult to follow and understand the
steps of a written tutorial. Further work could involve making a supplementary video of the
tutorial. It would also be a good idea to provide the hdf-file of the complete geometry and
mesh in Salome to the students for download.

References
60
References
[1] V. Hernandez-Perez, M. Abdulkadir, and B. J. Azzopardi, "Grid Generation Issues in
the CFD Modelling of Two-Phase Flow in a Pipe," The Journal of Computational
Multiphase Flows, vol. 3, no. 1, pp. 13-26, 2011. [Online]. Available: doi:
10.1260/1757-482X.3.1.13
[2] Z. Gao, R. Bresson, Y. Qu, M. Milliez, C. de Munck, and B. Carissimo, "High
resolution unsteady RANS simulation of wind, thermal effects and pollution
dispersion for studying urban renewal scenarios in a neighborhood of Toulouse,"
Urban climate, vol. 23, pp. 114-130, 2018. [Online]. Available: doi:
10.1016/j.uclim.2016.11.002
[3] S. M. Nour, "CFD simulations of flow in bent pipe at high Reynolds numbers
conditions," Master's Thesis, Faculty of Mathematics and Natural Sciences,
University of Oslo, Oslo, 2014. [Online]. Available: http://urn.nb.no/URN:NBN:no-
46977
[4] U. C. Liestyarini, "CFD Analysis of Internal Pipe Flows," Master's Thesis, Faculty of
Science and Technology, University of Stavanger, Stavanger, 2016. [Online].
Available: http://hdl.handle.net/11250/2411432
[5] H. K. Versteeg and W. Malalasekera, An Introduction to Computational Fluid
Dynamics: The Finite Volume Method, 2. ed. Harlow: Pearson Education Limited,
2007, pp. 57-59, 76-78, 85, 88, 90-92, 97, 106, 151, 264, 275-279, 283, 286, 292, 296,
301-302, 305, 308-312, 342.
[6] J. Tu, G. H. Yeoh, and C. Liu, Computational Fluid Dynamics: A Practical
Approach, 3 ed. Butterworth-Heinemann, 2018, pp. 125, 133, 136, 139-143, 149-150.
[7] H. Jasak, "Error Analysis and Estimation for the Finite Volume Method with
Applications to Fluid Flows," Ph.D. Thesis, Department of Mechanical Engineering,
Imperial College of Science, Technology and Medicine, London, 1996. [Online].
Available: https://spiral.imperial.ac.uk/bitstream/10044/1/8335/1/Hrvoje_Jasak-1996-
PhD-Thesis.pdf
[8] Shyam2791, Basic three-dimensional cell shapes, Licenced under CC BY-SA 3.0 /
Modified, Nov. 15, 2012. Accessed on: Apr. 17, 2021. [Online figure]. Available:
https://en.wikipedia.org/wiki/Types_of_mesh
[9] J. Guerrero, Mesh quality metrics. Smoothness, Licenced under CC BY-SA 4.0, Wolf
Dynamics, 2020. Accessed on: Apr. 9, 2021. [Online figure]. Available:
http://www.wolfdynamics.com/training/introOF8/all.pdf
[10] J. Guerrero, Mesh quality metrics. Mesh aspect ratio AR, Licenced under CC BY-SA
4.0, Wolf Dynamics, 2020. Accessed on: Apr. 9, 2021. [Online figure]. Available:
[11] Shyam2791, Types of mesh, Licenced under CC BY-SA 3.0, Nov. 15, 2012. Accessed
on: Apr. 17, 2021. [Online figure]. Available:
https://en.wikipedia.org/wiki/Types_of_mesh

References
61
[12] J. Guerrero, OpenFOAM® Introductory Training Online session – 2020 Edition,
Wolf Dynamics, 2020. Accessed on: Apr. 9, 2021. [Online]. Available:
[13] A. Syrakos, S. Varchanis, Y. Dimakopoulos, A. Goulas, and J. Tsamopoulos, "A
critical analysis of some popular methods for the discretisation of the gradient
operator in finite volume methods," Physics of Fluids, vol. 29, no. 12, p. 127103,
2017. [Online]. Available: doi: 10.1063/1.4997682
[14] R. N. Gopalakrishnan and P. J. Disimile, "CFD Analysis of Twin Turbulent
Impinging Round Jets at Different Impingement Angles," Fluids, vol. 3, no. 4, 79,
2018. [Online]. Available: doi: 10.3390/fluids3040079
[15] V. Hernandez Perez, "Gas-liquid two-phase flow in inclined pipes," Ph.D. Thesis,
Department of Chemical and Environmental Engineering, University of Nottingham,
2008. [Online]. Available: http://eprints.nottingham.ac.uk/11764/1/Hernandez-
Perez.pdf
[16] P. Zhang, R. M. Roberts, and A. Bénard, "Computational guidelines and an empirical
model for particle deposition in curved pipes using an Eulerian-Lagrangian
approach," Journal of Aerosol Science, vol. 53, pp. 1-20, 2012. [Online]. Available:
doi: 10.1016/j.jaerosci.2012.05.007
[17] Aokomoriuta, Law of the wall, Licenced under CC BY-SA 3.0, July 1, 2011.
Accessed on: March. 17, 2021. [Online figure]. Available:
https://en.wikipedia.org/wiki/Law_of_the_wall
[18] J. B. Franzini and E. J. Finnemore, Fluid Mechanics with Engineering Applications,
10 ed. New York: McGraw-Hill, 2002, pp. 109, 139, 145, 261, 265, 284, 362.
[19] F. M. White, Fluid Mechanics, 7th ed. New York: McGraw-Hill, 2011, p. 473.
[20] D. B. Spalding, "A Single Formula for the “Law of the Wall”," Journal of Applied
Mechanics, vol. 28, no. 3, pp. 455-458, 1961. [Online]. Available: doi:
10.1115/1.3641728
[21] G. Kalitzin, G. Medic, G. Iaccarino, and P. Durbin, "Near-wall behavior of RANS
turbulence models and implications for wall functions," Journal of Computational
Physics, vol. 204, no. 1, pp. 265-291, 2005. [Online]. Available: doi:
10.1016/j.jcp.2004.10.018
[22] J. Bredberg, "On the Wall Boundary Condition for Turbulence Models," Chalmers
University of Technology, Department of Thermo and Fluid Dynamics, Technical
Report 00/4, 2000. Accessed on: Apr. 4, 2021. [Online]. Available:
http://www.tfd.chalmers.se/~lada/postscript_files/jonas_report_WF.pdf
[23] F. Liu, "Thorough Description Of How Wall Functions Are Implemented In
OpenFOAM," in "In Proceedings of CFD with OpenSource Software," edited by: H.
Nilsson and M. Irannezhad, Chalmers University of Technology, Göteborg, Project
Report, 2016. Accessed on: Apr. 4, 2021. [Online]. Available:
http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2016/FangqingLiu/openfoamFinal
.pdf
[24] S. N. Liu, "Implementation of a Complete Wall Function for the Standard k−epsilon
Turbulence Model in OpenFOAM 4.0," in "In Proceedings of CFD with OpenSource

References
62
Software," edited by: H. Nilsson and M. Arabnejad, University of Stavanger,
Stavanger, Project Work, 2016. Accessed on: Apr. 4, 2021. [Online]. Available:
http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2016/ShengnanLiu/FinalReport-
Shengnan.pdf
[25] G. Chen, Q. Xiong, P. J. Morris, E. G. Paterson, A. Sergeev, and Y.-C. Wang,
"OpenFOAM for Computational Fluid Dynamics," Notices of the American
Mathematical Society, vol. 61, no. 4, pp. 354-363, 2014. [Online]. Available: doi:
10.1090/noti1095
[26] F. P. Incropera, D. P. DeWitt, T. L. Bergman, and A. S. Lavine, Incropera's
Principles of Heat and Mass Transfer, 8. Global. ed. Singapore: Wiley, 2017, pp.
467-477.
[27] B. E. Launder and D. B. Spalding, "The numerical computation of turbulent flows,"
Computer Methods in Applied Mechanics and Engineering, vol. 3, no. 2, pp. 269-289,
1974. [Online]. Available: doi: 10.1016/0045-7825(74)90029-2
[28] S. H. E. Tahry, "k-epsilon Equation for Compressible Reciprocating Engine Flows,"
Journal of Energy, vol. 7, no. 4, pp. 345-353, 1983. [Online]. Available: doi:
10.2514/3.48086
[29] OpenFOAM, k-epsilon, OpenFOAM: User Guide v2006, OpenCFD Ltd. Accessed
on: Apr. 4, 2021. [Online]. Available:
https://www.openfoam.com/documentation/guides/latest/doc/guide-turbulence-ras-k-
epsilon.html
[30] ANSYS, Inc., "ANSYS Fluent User's Guide, Release 19.0," ANSYS, Inc., 2018.
[31] F. Menter and T. Esch, "Elements of Industrial Heat Transfer Prediction," presented at
the 16th Brazilian Congr. of Mechanical Engineering (COBEM), Nov. 2001.
[32] F. Menter, M. Kuntz, and R. Langtry, "Ten Years of Industrial Experience with the
SST Turbulence Model," in Proc. of the 4th Int. Symp. on Turbulence, Heat and Mass
Transfer, Antalya, Turkey, Begell House, 2003, pp. 625–632.
[33] OpenFOAM, k-omega Shear Stress Transport (SST), OpenFOAM: User Guide
v2012, OpenCFD Ltd. Accessed on: Apr. 24, 2021. [Online]. Available:
https://www.openfoam.com/documentation/guides/latest/doc/guide-turbulence-ras-k-
omega-sst.html
[34] OpenFOAM®, Steady turbulent flow over a backward-facing step, Tutorial Guide,
OpenCFD Ltd. Accessed on: May 6, 2021. [Online]. Available:
https://www.openfoam.com/documentation/tutorial-guide/3-compressible-flow/3.1-
steady-turbulent-flow-over-a-backward-facing-step
[35] P. K. Swamee and A. Jain, "Explicit Equations for Pipe-Flow Problems," Journal of
Hydraulic Division, vol. 102, no. 5, pp. 657-664, 1976. [Online]. Available: doi:
10.1061/JYCEAJ.0004542
[36] H. Blasius, "Das Aehnlichkeitsgesetz bei Reibungsvorgängen in Flüssigkeiten," VDI
Forsch. Gebiete Ingenieurw., vol. 131, pp. 1-39, 1913. [Online]. Available: doi:
10.1007/978-3-662-02239-9_1
[37] T. Al-Shemmeri, Engineering Fluid Mechanics, 1. ed. Bookboon, 2012, p. 69.
[Online]. Available: https://bookboon.com/nb/engineering-fluid-mechanics-ebook

References
63
[38] SALOME, Introduction to HEXABLOCK, CEA/DEN, EDF R&D. Accessed on: Apr.
6, 2021. [Online]. Available: https://docs.salome-
platform.org/latest/gui/HEXABLOCK/general.html
[39] R. W. Pitz and J. W. Daily, "Combustion in a turbulent mixing layer formed at a
rearward-facing step," AIAA Journal, vol. 21, no. 11, pp. 1565-1570, 1983. [Online].
Available: doi: 10.2514/3.8290
[40] SimScale, Turbulent Pipe Flow, 2019. Accessed on: Nov. 23, 2019. [Online].
Available:
https://www.simscale.com/docs/validation/TurbulentPipeFlow/TurbulentPipeFlow.ht
ml
[41] C. J. Greenshields, "OpenFOAM User Guide version 8," OpenFOAM Foundation
Ltd., CFD Direct Ltd., July 22, 2020.
[42] D. A. Jones, M. Chapuis, M. Liefvendahl, D. Norrison, and R. Widjaja, "RANS
Simulations using OpenFOAM Software," Australian Government: Department of
Defence: Defence Science and Technology Group, Technical Report DST-Group-TR-
3204, Jan. Jan., 2016. Accessed on: Mar. 22, 2021. [Online]. Available:
https://apps.dtic.mil/sti/pdfs/AD1002391.pdf
[43] E. Furbo, "Evaluation of RANS turbulence models for flow problems with signigicant
impact of boundary layers," Master's Thesis, Department of Information Technology,
Uppsala University, Uppsala, 2010. [Online]. Available: http://uu.diva-
portal.org/smash/record.jsf?pid=diva2%3A379743
[44] A. Lipej, S. Muhič, and D. Mitruševski, "Wall Roughness Influence on the Efficiency
Characteristics of Centrifugal Pump," Strojniški vestnik - Journal of Mechanical
Engineering, vol. 63, no. 9, pp. 529-536, 2017. [Online]. Available: doi: 10.5545/sv-
jme.2017.4526
[45] J. S. Jayakumar and R. Manuraj, "Estimation of local wall shear stress in curved pipes
using cgns mesh in OpenFOAM," presented at the 5th Int. and 41st Nat. Conf. on
Fluid Mechanics and Fluid Power (FMFP) 2014, Indian Institute of Technology
Kanpur, 2014. Accessed on: Apr. 29, 2021. [Online]. Available:
https://ijcrt.org/papers/IJCRT_193642.pdf
[46] OpenFOAM, Turbulent plane channel flow with smooth walls, OpenFOAM: User
Guide v2012, OpenCFD Ltd. Accessed on: Apr. 25, 2021. [Online]. Available:
https://www.openfoam.com/documentation/guides/latest/doc/verification-validation-
turbulent-plane-channel-flow.html
[47] J. C. Puig, Laminar flow through a circular pipe, OPENFOAM GUIDE FOR
BEGINNERS, UPC Sch. of Prof. & Exec. Dev., ESEIAAT. Accessed on: Apr. 25,
2021. [Online]. Available: http://files.the-foam-house5.webnode.es/200000363-
59a695aa6c/Chapter4_Pipe.pdf
[48] SimScale, How to Model Wall Roughness in CFD?, 2020. Accessed on: Apr. 29,
2021. [Online]. Available: https://www.simscale.com/knowledge-base/how-to-model-
wall-roughness-in-cfd/

Appendices
Appendices
Appendix A - Project topic description......................................................... A.1
Appendix B - Software.................................................................................... B.1
Appendix C - Technical drawing geometry................................................... C.1
Appendix D - Python script for Mesh A, B and C ......................................... D.1
Appendix E - Importing mesh to OpenFOAM ............................................... E.1
Appendix F - Cross-sectional mesh properties.............................................F.1
Appendix G - Wall functions in OpenFOAM .................................................G.1
Appendix H - Constants and boundary conditions...................................... H.1
Appendix I - Symmetry planes........................................................................I.1
Appendix J - Residual plots............................................................................J.1
Appendix K - Visualization of 𝐲 + distribution.............................................. K.1
Appendix L - Pressure loss calculation.........................................................L.1
Appendix M - Wall treatment procedures .....................................................M.1
Appendix N - Student tutorial ........................................................................ N.1
64

Appendices
A.1
Appendix A -Project topic description

Appendices
B.1
Appendix B - Software
The software used for the cases are listed below:
• Oracle VM VirtualBox 6.1-18
• Ubuntu 20.04.2 LTS (focal)
• Salome 9.6.0
• openfoam8
• paraviewopenfoam56
• 40 GB RAM and 4 cores assigned to the virtual machine

Appendices
C.1
Appendix C - Technical drawing geometry

Appendices
D.1
Appendix D -Python script for Mesh A, B and C
#!/usr/bin/env python
### This file is generated automatically by SALOME v9.6.0 with dump python functionality
###
import sys
import salome
salome.salome_init()
import salome_notebook
notebook = salome_notebook.NoteBook()
sys.path.insert(0, r'/home/virtualbox/Documents/salome_files_FINAL')
###
### GEOM component
###
import GEOM
from salome.geom import geomBuilder
import math
import SALOMEDS
geompy = geomBuilder.New()
O = geompy.MakeVertex(0, 0, 0)
OX = geompy.MakeVectorDXDYDZ(1, 0, 0)
OY = geompy.MakeVectorDXDYDZ(0, 1, 0)
OZ = geompy.MakeVectorDXDYDZ(0, 0, 1)
geomObj_1 = geompy.MakeMarker(0, 0, 0, 1, 0, 0, 0, 1, 0)
sk = geompy.Sketcher2D()
sk.addPoint(0.000000, 0.000000)
sk.addSegmentAbsolute(300.000000, 0.000000)
Sketch_1 = sk.wire(geomObj_1)
[Edge_1,Edge_2,Edge_3,Edge_4,Edge_5] = geompy.ExtractShapes(Sketch_1, geompy.ShapeType["EDG
E"], True)
[Vertex_1,Vertex_2,Vertex_3,Vertex_4,Vertex_5,Vertex_6] = geompy.ExtractShapes(Sketch_1, ge
ompy.ShapeType["VERTEX"], True)
Wire_1 = geompy.MakeWire([Edge_1, Edge_2, Edge_3, Edge_4, Edge_5], 1e-07)
Divided_Disk_1 = geompy.MakeDividedDiskPntVecR(Vertex_1, Edge_1, 10, GEOM.SQUARE)
[Face_1, Face_2, Face_3] = geompy.Propagate(Divided_Disk_1)
[Face_1,Face_2,Face_3,Face_4,Face_5] = geompy.ExtractShapes(Divided_Disk_1, geompy.ShapeTyp
e["FACE"], True)
[Face_6,Face_7,Face_8,Face_9,Face_10] = geompy.ExtractShapes(Divided_Disk_2, geompy.ShapeTy
pe["FACE"], True)
[Face_11,Face_12,Face_13,Face_14,Face_15] = geompy.ExtractShapes(Divided_Disk_3, geompy.Sha
peType["FACE"], True)

Appendices
D.2
Pipe_1 = geompy.MakePipeWithDifferentSectionsBySteps([Face_1, Face_6, Face_11, Face_16, Fac
e_21, Face_26], [Vertex_1, Vertex_2, Vertex_3, Vertex_4, Vertex_5, Vertex_6], Wire_1)
Pipe_5 = geompy.MakePipeWithDifferentSectionsBySteps([Face_5, Face_10, Face_15, Face_20, Fa
ce_25, Face_30], [Vertex_1, Vertex_2, Vertex_3, Vertex_4, Vertex_5, Vertex_6], Wire_1)
Compound_1 = geompy.MakeCompound([Pipe_1, Pipe_2, Pipe_3, Pipe_4, Pipe_5])
Glue_1 = geompy.MakeGlueFaces(Compound_1, 1e-07)
[corners, flowedges_inlet_outlet, flowedges_belly, Compound_5, Compound_6, Compound_7, Comp
ound_8, Compound_9] = geompy.Propagate(Glue_1)
flowedges_inlet_outlet = geompy.UnionListOfGroups([Compound_5, Compound_9])
flowedges_belly = geompy.UnionListOfGroups([Compound_6, Compound_7, Compound_8])
inlet = geompy.CreateGroup(Glue_1, geompy.ShapeType["FACE"])
geompy.UnionIDs(inlet, [296, 136, 205, 32, 254])
outlet = geompy.CreateGroup(Glue_1, geompy.ShapeType["FACE"])
geompy.UnionIDs(outlet, [310, 190, 114, 288, 239])
wall = geompy.CreateGroup(Glue_1, geompy.ShapeType["FACE"])
geompy.UnionIDs(wall, [158, 171, 128, 145, 184, 101, 41, 14, 61, 81, 280, 243, 256, 264, 27
2, 304, 298, 292, 301, 307])
[corners, Compound_5, Compound_6, Compound_7, Compound_8, Compound_9, flowedges_inlet_outle
t, flowedges_belly, inlet, outlet, wall] = geompy.GetExistingSubObjects(Glue_1, False)
geompy.addToStudy( O, 'O' )
geompy.addToStudy( OX, 'OX' )
geompy.addToStudy( OY, 'OY' )
geompy.addToStudy( OZ, 'OZ' )
geompy.addToStudy( Sketch_1, 'Sketch_1' )
geompy.addToStudyInFather( Sketch_1, Edge_1, 'Edge_1' )
geompy.addToStudyInFather( Sketch_1, Vertex_1, 'Vertex_1' )
geompy.addToStudy( Wire_1, 'Wire_1' )
geompy.addToStudy( Divided_Disk_1, 'Divided Disk_1' )
geompy.addToStudyInFather( Divided_Disk_1, Face_1, 'Face_1' )

Appendices
D.3
geompy.addToStudy( Pipe_1, 'Pipe_1' )
geompy.addToStudy( Compound_1, 'Compound_1' )
geompy.addToStudy( Glue_1, 'Glue_1' )
geompy.addToStudyInFather( Glue_1, corners, 'corners' )
geompy.addToStudyInFather( Glue_1, flowedges_inlet_outlet, 'flowedges_inlet_outlet' )
geompy.addToStudyInFather( Glue_1, flowedges_belly, 'flowedges_belly' )
geompy.addToStudyInFather( Glue_1, Compound_5, 'Compound_5' )
geompy.addToStudyInFather( Glue_1, inlet, 'inlet' )
geompy.addToStudyInFather( Glue_1, outlet, 'outlet' )
geompy.addToStudyInFather( Glue_1, wall, 'wall' )
###
### SMESH component
###
import SMESH, SALOMEDS
from salome.smesh import smeshBuilder
smesh = smeshBuilder.New()
MeshA = smesh.Mesh(Glue_1)
Regular_1D = MeshA.Segment()
Number_of_Segments_10 = Regular_1D.NumberOfSegments(10)
Quadrangle_2D = MeshA.Quadrangle(algo=smeshBuilder.QUADRANGLE)
Hexa_3D = MeshA.Hexahedron(algo=smeshBuilder.Hexa)
inlet_1 = MeshA.GroupOnGeom(inlet,'inlet',SMESH.FACE)
outlet_1 = MeshA.GroupOnGeom(outlet,'outlet',SMESH.FACE)
wall_1 = MeshA.GroupOnGeom(wall,'wall',SMESH.FACE)
isDone = MeshA.Compute()

Appendices
D.4
[ smeshObj_1, smeshObj_2, smeshObj_3, smeshObj_4, smeshObj_5, smeshObj_6, smeshObj_7, smesh
Obj_8, inlet_1, outlet_1, wall_1 ] = MeshA.GetGroups()
Regular_1D_1 = MeshA.Segment(geom=flowedges_inlet_outlet)
Number_of_Segments_300 = Regular_1D_1.NumberOfSegments(100)
Regular_1D_2 = MeshA.Segment(geom=flowedges_belly)
Number_of_Segments_50 = Regular_1D_2.NumberOfSegments(50)
Number_of_Segments_300.SetNumberOfSegments( 300 )
isDone = MeshA.Compute()
MeshB = smesh.Mesh(Glue_1)
status = MeshB.AddHypothesis(Number_of_Segments_10)
Regular_1D_3 = MeshB.Segment()
Quadrangle_2D_1 = MeshB.Quadrangle(algo=smeshBuilder.QUADRANGLE)
Hexa_3D_1 = MeshB.Hexahedron(algo=smeshBuilder.Hexa)
inlet_2 = MeshB.GroupOnGeom(inlet,'inlet',SMESH.FACE)
outlet_2 = MeshB.GroupOnGeom(outlet,'outlet',SMESH.FACE)
wall_2 = MeshB.GroupOnGeom(wall,'wall',SMESH.FACE)
Regular_1D_4 = MeshB.Segment(geom=flowedges_inlet_outlet)
status = MeshB.AddHypothesis(Number_of_Segments_300,flowedges_inlet_outlet)
Regular_1D_5 = MeshB.Segment(geom=flowedges_belly)
status = MeshB.AddHypothesis(Number_of_Segments_50,flowedges_belly)
[ smeshObj_9, smeshObj_10, smeshObj_11, smeshObj_12, smeshObj_13, smeshObj_14, smeshObj_15,
smeshObj_16, inlet_2, outlet_2, wall_2 ] = MeshB.GetGroups()
Regular_1D_6 = MeshB.Segment(geom=corners)
Number_of_Segments_2 = Regular_1D_6.NumberOfSegments(2,0.4,[])
[ smeshObj_9, smeshObj_10, smeshObj_11, smeshObj_12, smeshObj_13, smeshObj_14, smeshObj_15,
smeshObj_16, inlet_2, outlet_2, wall_2 ] = MeshB.GetGroups()
Number_of_Segments_2.SetNumberOfSegments( 2 )
Number_of_Segments_2.SetScaleFactor( 0.4 )
Number_of_Segments_2.SetReversedEdges( [ 9, 13, 40, 60, 80, 100, 123, 127, 144, 157, 170, 1
83 ] )
isDone = MeshB.Compute()
[ inlet_2, outlet_2, wall_2 ] = MeshB.GetGroups()
MeshC = smesh.Mesh(Glue_1)
status = MeshC.AddHypothesis(Number_of_Segments_10)
Regular_1D_7 = MeshC.Segment()
Quadrangle_2D_2 = MeshC.Quadrangle(algo=smeshBuilder.QUADRANGLE)
Hexa_3D_2 = MeshC.Hexahedron(algo=smeshBuilder.Hexa)
inlet_3 = MeshC.GroupOnGeom(inlet,'inlet',SMESH.FACE)
outlet_3 = MeshC.GroupOnGeom(outlet,'outlet',SMESH.FACE)
wall_3 = MeshC.GroupOnGeom(wall,'wall',SMESH.FACE)
Regular_1D_8 = MeshC.Segment(geom=flowedges_inlet_outlet)
status = MeshC.AddHypothesis(Number_of_Segments_300,flowedges_inlet_outlet)
Regular_1D_9 = MeshC.Segment(geom=flowedges_belly)
status = MeshC.AddHypothesis(Number_of_Segments_50,flowedges_belly)
[ smeshObj_17, smeshObj_18, smeshObj_19, smeshObj_20, smeshObj_21, smeshObj_22, smeshObj_23
, smeshObj_24, inlet_3, outlet_3, wall_3 ] = MeshC.GetGroups()
Regular_1D_10 = MeshC.Segment(geom=corners)
Regular_1D_11 = MeshC.Segment(geom=corners)
Number_of_Segments_20 = Regular_1D_10.NumberOfSegments(20,10,[ 9, 13, 40, 60, 80, 100, 123,
127, 144, 157, 170, 183 ])
isDone = MeshC.Compute()
[ smeshObj_17, smeshObj_18, smeshObj_19, smeshObj_20, smeshObj_21, smeshObj_22, smeshObj_23
, smeshObj_24, inlet_3, outlet_3, wall_3 ] = MeshC.GetGroups()
flowedges_inlet_outlet_1 = Regular_1D_1.GetSubMesh()
flowedges_belly_1 = Regular_1D_2.GetSubMesh()

Appendices
D.5
corners_1 = Regular_1D_6.GetSubMesh()
corners_2 = Regular_1D_10.GetSubMesh()
## Set names of Mesh objects
smesh.SetName(Regular_1D.GetAlgorithm(), 'Regular_1D')
smesh.SetName(Hexa_3D.GetAlgorithm(), 'Hexa_3D')
smesh.SetName(Quadrangle_2D.GetAlgorithm(), 'Quadrangle_2D')
smesh.SetName(Number_of_Segments_300, 'Number of Segments=300')
smesh.SetName(inlet_1, 'inlet')
smesh.SetName(outlet_1, 'outlet')
smesh.SetName(wall_1, 'wall')
smesh.SetName(flowedges_inlet_outlet_2, 'flowedges_inlet_outlet')
smesh.SetName(flowedges_belly_2, 'flowedges_belly')
smesh.SetName(corners_1, 'corners')
smesh.SetName(MeshA.GetMesh(), 'MeshA')
smesh.SetName(MeshC.GetMesh(), 'MeshC')
smesh.SetName(MeshB.GetMesh(), 'MeshB')
smesh.SetName(corners_2, 'corners')
if salome.sg.hasDesktop():
salome.sg.updateObjBrowser()

Appendices
E.1
Appendix E - Importing mesh to OpenFOAM
A mesh created in Salome can be imported to OpenFOAM with the following procedure:
In the mesh module in Salome, right-click on the mesh and export it as an unv-file.
Copy the unv-file to an OpenFOAM case directory. Delete the existing polyMesh or
blockMesh file. Open the terminal and import the mesh with the command:
ideasUnvToFoam mesh_name.unv
OpenFOAM uses the SI system, but the mesh made in Salome does not have a length unit.
The mesh is transformed from 𝑚 to 𝑚𝑚 with the transformPoints command:
transformPoints -scale '(1e-3 1e-3 1e-3)'
In addition, the correct boundaries and patches must be set in the polyMesh directory.

Appendices
F.1
Appendix F - Cross-sectional mesh properties
Aspect ratio
Figure F.1: Aspect ratio Mesh A.
Figure F.2: Aspect ratio Mesh B.

Appendices
F.2
Figure F.3: Aspect ratio Mesh C.
Skewness
Figure F.4: Skewness Mesh A.

Appendices
F.3
Figure F.5: Skewness Mesh B.
Figure F.6: Skewness Mesh C.

Appendices
G.1
Appendix G -Wall functions in OpenFOAM
Available wall functions in OpenFOAMv8 are listed and described by typing the following
command in the terminal:
foamInfo wallFunction
𝑘 wall functions
Table G.1: 𝑘 wall functions.
Wall function Suitable for turbulence model
HRN LRN
kqRWallFunction X
kLowReWallFunction X X
𝜀 wall functions
Table G.2: 𝜀 wall functions.
HRN LRN
epsilonWallFunction X
𝜔 wall functions
Table G.3: 𝜔 wall functions.
HRN LRN
omegaWallFunction X X

Appendices
G.2
𝜇𝑡 wall functions
Table G.4: 𝜇𝑡 wall functions [1].
HRN LRN All regions
nutkWallFunction X
nutLowReWallFunction X X
nutUSpaldingWallFunction X
nutUTabulatedWallFunction X
nutURoughWallFunction X
nutUWallFunction X
nutkRoughWallFunction X
nutkAtmRoughWallFunction X
References
[1] S. N. Liu, "Implementation of a Complete Wall Function for the Standard k−epsilon
Turbulence Model in OpenFOAM 4.0," in "In Proceedings of CFD with OpenSource
Software," edited by: H. Nilsson and M. Arabnejad, University of Stavanger,
Stavanger, Project Work, 2016. Accessed on: Apr. 4, 2021. [Online]. Available:
http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2016/ShengnanLiu/FinalReport-
Shengnan.pdf

Appendices
H.1
Appendix H -Constants and boundary conditions
Table H.1: Air properties [1, p. 733].
𝑻 [℃] 𝝂 [𝒎𝟐
/𝒔] 𝝆 [𝒌𝒈/𝒎𝟑
] 𝝁 [𝑵𝒔/𝒎𝟐
]
20 1.5 ∙ 10−5
1.205 1.81 ∙ 10−5
Table H.2: Constants and calculated boundary conditions at inlet.
𝑫 [m] 0.02
𝒍 [m] 0.0014
𝑼 [m/s] 3
𝑹𝒆 [−] 4000
𝑻𝒊 [−] 0.057
𝒌 [𝒎𝟐
/𝒔𝟐
] 0.043457
𝜺 [𝒎𝟐
/𝒔𝟑
] 1.06327
𝝎 [𝒔−𝟏
] 271.857
Table H.3: Initial and boundary conditions 𝑈 and 𝑝 for all cases.
Type 𝑼 [𝒎/𝒔] 𝒑 [𝒎𝟐
/𝒔𝟐
]
internalField uniform (0 0 0) uniform 0
inlet fixedValue
uniform (3 0 0)
zeroGradient
outlet zeroGradient fixedValue
uniform 0
wall noSlip zeroGradient

Appendices
H.2
Table H.4: Initial and boundary conditions Case A and Case B1.
Type 𝒌 [𝒎𝟐
/𝒔𝟐
] 𝒆𝒑𝒔𝒊𝒍𝒐𝒏 [𝒎𝟐
/𝒔𝟑
] 𝒏𝒖𝒕 [𝒎𝟐
/𝒔]
internalField uniform 0.043457 uniform 1.06327 uniform 0
inlet fixedValue
uniform 0.043457
fixedValue
uniform 1.06327
calculated
uniform 0
outlet zeroGradient zeroGradient calculated
uniform 0
wall kqRWallFunction
uniform 0.043457
epsilonWallFunction
uniform 1.06327
nutkWallFunction
uniform 0
Table H.5: Initial and boundary conditions Case B2.
Type 𝒌 [𝒎𝟐
/𝒔𝟐
/𝒔𝟑
/𝒔]
inlet fixedValue
uniform 0.043457
fixedValue
uniform 1.06327
calculated
uniform 0
uniform 0
wall kLowReWallFunction
uniform 0.043457
epsilonWallFunction
uniform 1.06327
nutUSpaldingWallFunction
uniform 0
Table H.6: Initial and boundary conditions Case C.
Type 𝒌 [𝒎𝟐
/𝒔𝟐
] 𝒐𝒎𝒆𝒈𝒂 [𝒔−𝟏
/𝒔]
inlet fixedValue
uniform 0.043457
fixedValue
uniform 271.857
calculated
uniform 0
uniform 0
wall fixedValue
uniform 0
omegaWallFunction
uniform 271.857
nutLowReWallFunction
uniform 0

Appendices
H.3
References
[1] J. B. Franzini and E. J. Finnemore, Fluid Mechanics with Engineering Applications,
10 ed. New York: McGraw-Hill, 2002, p. 733.

Appendices
I.1
Appendix I - Symmetry planes
Velocity
Figure I.1: Velocity Case A.
Figure I.2: Velocity Case B1.

Appendices
I.2
Figure I.3: Velocity Case B2.
Figure I.4: Velocity Case C.

Appendices
I.3
Stagnation pressure
Figure I.5: Stagnation pressure Case A.
Figure I.6: Stagnation pressure Case B1.

Appendices
I.4
Figure I.7: Stagnation pressure Case B2.
Figure I.8: Stagnation pressure Case C.

Appendices
I.5
Static pressure
The static pressure can be calculated in OpenFOAM with the same post-processing procedure
as in Appendix L for total pressure. Just change all the occurrences of
totalPressureIncompressible to staticPressure, and total(p) to static(p), and the correct
density will be used in the calculations.
Figure I.9: Static pressure Case A.
Figure I.10: Static pressure Case B1.

Appendices
I.6
Figure I.11: Static pressure Case B2.
Figure I.12: Static pressure Case C.

Appendices
J.1
Appendix J - Residual plots
Figure J.1: Residuals Case A.
Figure J.2: Residuals Case B1.

Appendices
J.2
Figure J.3: Residuals Case B2.
Figure J.4: Residuals Case C.

Appendices
K.1
Appendix K - Visualization of y+
distribution
Visualization of the 𝑦+
field in ParaView of the four simulations.
Figure K.1: Case A.
Figure K.2: Case B1.

Appendices
K.2
Figure K.3: Case B2.
Figure K.4: Case C.

Appendices
L.1
Appendix L - Pressure loss calculation
Calculating total pressure in OpenFOAM
The default density for incompressible solvers in OpenFOAM is 1.2. In order for
OpenFOAM to calculate the total pressure with a chosen density, the density must be
provided in an additional file.
The density for calculating the stagnation pressure in OpenFOAM is added by creating an
additional file named totalPressureIncompressible1 in the system directory containing the
correct density:
#includeEtc "caseDicts/postProcessing/pressure/totalPressureIncompressible.cfg"
pRef 0.0;
rhoInf 1.205; //1.2;
The function must be added in the controlDict dictionary with the following lines:
functions
{
#includeFunc totalPressureIncompressible1
}
The total pressure for each time step is then calculated by typing in the terminal:
simpleFoam -postProcess -fields "(p U)" -func totalPressureIncompressible1
The average values of the inlet and outlet patches can be calculated by the command:
postProcess -func 'patchAverage(name=inlet,p,U,total(p))' -latestTime
and
postProcess -func 'patchAverage(name=outlet,p,U,total(p))' -latestTime

Appendices
L.2
The total pressure for all fields can be viewed in ParaView. To find the value of the average
pressure over an area:
• make a slice on the X Normal on the desired X coordinate.
• Integrate variables. Attruibute Cell Data. To get the total pressure: manually divide
the result of the integrated variable by the area, or use the calculator filter.
• (Alternatively: Export data to spreadsheet. Several CSV-files can be imported to
Excel in one batch and divided by Area in Excel for simplicity and data storage)
Stagnation pressure loss calculations
Pipe section Inlet Diverging Belly Converging Outlet
𝐿 [𝑚𝑚] 300 50 50 50 300
𝐷 [𝑚𝑚] 20 * 60 * 10
𝐴 [𝑚2
] 3.14E-04 * 2.83E-03 * 7.85E-05
𝑄 [𝑚3
/𝑠] 9.42E-04 9.42E-04 9.42E-04 9.42E-04 9.42E-04
𝑈𝑐𝑎𝑙𝑐𝑢𝑙𝑎𝑡𝑒𝑑 3 * 0.33 * 12
𝑅𝑒 4000 * 1333 * 8000
𝑓𝑡𝑢𝑟𝑏 0.040 * - * 0.033
𝑓𝑙𝑎𝑚 - * 0.048 * -
𝐾 - 0.4381
- 12
-
𝑝𝑙𝑜𝑠𝑠 [𝑃𝑎]3
3.24 1.06 0.003 96.76 87.19
1
Conical enlargement 22°
2
Sudden contraction 0.03 → tank exit 0.5 + 0.5 extra
3
The sum of the pressure losses is 188.25 Pa
* Calculated at each point

M.1
Right-click on MeshC and click Create Sub-mesh.
Name edges
Mesh MeshC
Geometry edges
Algorithm Wire Discretisation
Hypothesis Number of Segments Name Number of Segments=20
Number of Segments 20
Type of distribution Scale distribution
Scale factor 10
Helper Check the box:
Propagation chains.
Mark Chain 1 (24 edges)
and click Add.
Appendices
Appendix M - Wall treatment procedures
Mesh B
The procedure for creating Mesh B is explained in the student tutorial in Appendix N.
Mesh A
To create Mesh A the procedure is the same as in the student tutorial, but the step Sub-mesh
for edges must be omitted.
Mesh C
To create Mesh C, the procedure is the same as in the student tutorial, but the step Sub-mesh
for edges must be replaced with the following sub-mesh:

Appendices
N.1
Appendix N -Student tutorial
Contents
Introduction
This tutorial describes how to use the meshing software Salome. We will create and mesh a
3D model of a diverging converging pipe with belly section with a hexahedral OH-grid. We
will import the mesh to OpenFOAM and run the simpleFoam solver, applying the turbulence
model standard 𝐤 − 𝛆 with wall functions.
Figure N.1: Diverging converging pipe with belly section.

Appendices
N.2
Figure N.2: Cross-section of pipe.
Workflow:
• Install the meshing software Salome
• Draw a diverging converging pipe with belly section in 3D
• Create boundary groups
• Generate mesh
• Improve mesh for better mesh quality and optimality
• Export mesh
• Import mesh to OpenFOAM
• Set appropriate boundary conditions and patches
• Run a simulation
• Post-process
The aim of this tutorial is to show the students a complete workflow from creating and
meshing a complex geometry in Salome to importing it to OpenFOAM, running a simulation
and post-processing. The intention is that the students can use what they have learned in this
tutorial to create their own geometries and meshes for more applied cases.

Appendices
N.3
Installation of Salome in Ubuntu
First, some additional packages in Ubuntu need to be installed. Open the terminal and run the
command:
sudo apt install net-tools
and:
sudo apt install libopengl0 -y
To download Salome, go to the following website:
https://www.salome-platform.org/downloads/current-version
Download:
Universal Linux binary
Move the downloaded file to the directory you want Salome to be located in, e.g., Home.
Open the terminal window from the directory. In the terminal, list the contents in the
directory by typing:
ls
Copy the name of the Salome tar-file (e.g., SALOME-x.x.x.tar.gz). Then paste the filename
after the untar-command:
tar -zxvf SALOME-x.x.x.tar.gz
The output of the untar-process is seen in the terminal. Go to the untared directory by typing:
cd SALOME-x.x.x
To run Salome, type:
./salome.
Installation problems
If there are problems opening Salome, try updating and upgrading the ubuntu software:
sudo apt-get update
and:
sudo apt-get upgrade

Appendices
N.4
How to use Salome
Open the Salome directory, right-click and click Open in Terminal.
Launch Salome by typing in the terminal window:
./salome
Tips & tricks in Salome
Save as
Save the hdf-file with the Save as command many times during the process. Salome might
crash, or you might have made the wrong input. If you have saved previous versions of the
file, you can go back, and do not need to start over again.
Marking multiple objects in the object browser:
• Hold down Shift-key to mark objects adjacent to each other.
• Hold down Ctrl-key to mark objects not adjacent to each other.
Eye symbol
Click on the eye symbol in the Object Browser to show or hide an object.
Show only
If you do not know where an object listed in the object browser is located on the geometry,
right-click on the object in the object tree and choose Show Only.

Appendices
N.5
Geometry module in Salome
Go to the scrolldown-menu and click Geometry to open the geometry module.
Check that vectors are present in the object browser.
Click the arrow in the object browser in front of geometry.
If the vectors OX, OY and OZ do not appear, open settings with command Ctrl + P, and check
the box Auto create under the heading Origin and base vectors.

Appendices
N.6
Create 2D sketch
Go to New Entity -> Basic -> 2D Sketch
Make a 2D sketch with the following coordinates. Click Apply after adding each point. Close.
X Y
0 0
300 0
350 0
400 0
450 0
750 0

Appendices
N.8
Explode sketch into edges and vertices
Go to New Entity -> Explode
Main Object: Sketch_1
Sub-shapes Type: Edge
Click Apply
Change Sub-shapes Type to Vertex
Click Apply and Close
Click on the arrow next to Sketch_1 in the Object Browser to see the created (exploded)
edges and vertices. There should be 5 edges and 6 vertices.

Appendices
N.9
Build wire
Go to New Entity -> Build -> Wire
Select Object Type as Edge.
Click the blue arrow next to Edge and select all the five edges in Sketch_1 by holding down
the Shift-key. Click Apply and Close.
A wire is created based on all the edges.

Appendices
N.10
Create divided disks
Go to New Entity -> Blocks -> Divided Disk
Go to the second constructor.
Division pattern: Square
Fill in the following Arguments by pushing the blue arrow to mark the argument in the Object
Browser. Click Apply for each divided disk.
Name Center Point Vector Radius
Divided Disk_1 Vertex_1 Edge_1 10

Appendices
N.11
Explode disks
Go to New Entity -> Explode. Each disk should be divided into faces, as displayed in the
table below. Click Apply for each divided disk. Each divided disk will be exploded into 5
faces.
Name Sub-shapes Type
Divided Disk_1 Face
Divided Disk_2 Face
Divided Disk_3 Face
Divided Disk_4 Face
Divided Disk_5 Face
Divided Disk_6 Face

Appendices
N.12
Generate pipe with different sections
Go to New Entity -> Generation -> Extrusion Along Path
Go to the third pipe constructor. Choose Arguments by clicking the blue arrow, holding down
the Ctrl-key and marking the Base Objects in the Object Browser. Hold down the Shift-key to
mark the Locations. Do this for each argument. Choose Step-by-step generation. Click Apply
after adding each pipe. 5 pipe sections will be created.
Name Base Object Locations Path Object
Pipe_1 Face_1, Face_6,
Face_11, Face_16,
Face_21, Face_26
Vertex_1, Vertex_2,
Vertex_3, Vertex_4,
Vertex_5, Vertex_6
(6_objects)
Wire_1
Face_12, Face_17,
Face_22, Face_27
Face_13, Face_18,
Face_23, Face_28
Face_14, Face_19,
Face_24, Face_29
Face_15, Face_20,
Face_25, Face_30

Appendices
N.13
Build compound
Go to New Entity -> Build -> Compound. Fill in the information in the table below.
Choose all the pipe sections and click Apply and Close. A compound with all the pipe
sections has been created.
Name Objects
Compund_1 Pipe_1, Pipe_2, Pipe_3, Pipe_4, Pipe_5
(5_objects)

Appendices
N.14
Glue faces
Go to Repair -> Glue Faces. Select shape Compound_1 and click Apply and Close. Glue_1 has
been created.

Appendices
N.15
Create edges groups
Go to Operations -> Blocks -> Propagate. Choose object Glue_1. Click Apply and Close.
Groups Compound_2 - Compound_9 have been created.
Rename the created groups in the object browser by clicking F2 after selecting a group. To
differentiate the groups, right-click on a group in the object browser and click Show Only.
Name Rename to
Compound_2 corners
Delete Compound_3 and Compound_4.
Go to New Entity -> Group -> Union Groups
The group union and names are shown in the table below:
Groups Name
Compound_5, Compound_9 flowedges_inlet_outlet
Compound_6, Compund_7, Compound_8 flowedges_belly

Appendices
N.16
Create faces groups
Go to New Entity -> Group -> Create Group. Click on the third constructor (face). Main
Shape: Glue_1. Mark the inlet, outlets, or walls, respectively, by holding down the Shift key
and clicking on all the parts of the respective face group. The marked faces get white lines at
the intersection of faces. Click Add. Click Apply.
Name Main Shape Selection Numbers
inlet 296, 136, 205, 32, 254
outlet 310, 190, 114, 288, 239
wall 158, 171, 128, 145, 184, 101, 41, 14, 61, 81,
280, 243, 256, 264, 272, 304, 298, 292, 301,
307
Check that the groups are created correctly by only displaying one of them and moving the
viewpoint (especially for the wall).

Appendices
N.17
Mesh module in Salome
Open the Mesh module from the dropdown menu:
Mesh_1
Go to Mesh ->Create Mesh. Fill in the following settings:
Name Mesh_1
Geometry Glue_1
Mesh Type Hexahedral
Create all Groups on
Geometry
Check the box
Algorithm 3D Hexahedron (i,j,k)
2D Quadrangle Mapping
1D Wire Discretisation
Hypothesis 1D Number of
Segments
Name Number of Segments=10
Number
of
Segments
10

Appendices
N.18
Click Apply and Close.
Right-click on Mesh_1 in the Object Browser and click Compute.

Appendices
N.19
Sub-mesh flowedges_inlet_outlet
Right-click on Mesh_1 and click Create Sub-mesh.
Name flowedges_inlet_outlet
Mesh Mesh_1
Geometry flowedges_inlet_outlet
Click Apply and Close. Right-click on Mesh_1 and click Compute.
Sub-mesh flowedges_belly
Name flowedges_belly
Mesh Mesh_1
Geometry flowedges_belly

Appendices
N.20
Sub-mesh for edges
Name edges
Mesh Mesh_1
Geometry edges
Type of distribution Scale distribution
Scale factor 0.4
Helper Check the box:
Propagation chains.
Mark Chain 1 (24 edges)
and click Add.

Appendices
N.22
Mesh information
The final mesh should have the following Mesh Info:

Appendices
N.23
Delete Edges Groups
During the creation of Mesh_1, groups on geometry were created (Create all Groups on
Geometry box was checked). However, all Groups of Edges must be deleted because they
will create error messages in OpenFOAM.
Mark all Groups on Edges in the Object Browser, right-click and click Delete.
In contrast, The Groups of Faces (inlet, outlet, wall) are important, as they will be the
boundaries of the mesh in the OpenFOAM simulation.
Export the mesh
The hdf-file is useless in OpenFOAM. The mesh must be exported to an unv-file. Righ-click
on Mesh_1, click Export -> UNV file. Choose directory, and click Save.

Appendices
N.24
Simulation in OpenFOAM
Copy the directory pitzDaily from opt/openfoam8/tutorials/incompressible/simpleFoam/.
Paste the directory in the wanted directory and rename it to pipeBelly. Copy the exported
mesh, Mesh_1.unv, into the pipeBelly directory.
Import mesh to OpenFOAM
Open the terminal in the pipeBelly case directory (0, constant, system).
To import the mesh to OpenFOAM-format, write the command:
ideasUnvToFoam Mesh_1.unv
OpenFOAM uses the SI system, but the geometry made in Salome does not have a length
unit. Transform points to mm by writing:
transformPoints -scale '(1e-3 1e-3 1e-3)'
Next, check the mesh:
checkMesh
Constant directory
polyMesh
The polyMesh directory contains the imported mesh. Open the boundary file. Change the
wall type from patch to wall and save:
wall
{
type wall;
nFaces 30000;
startFace 390180;
}

Appendices
N.25
transportProperties
Change nu (the kinematic viscosity) to:
nu [0 2 -1 0 0 0 0] 1.5e-05;
0 directory
Delete f, nuTilda, omega and v2 (we will not need them in the simulation).
Must change the boundaryField in all the files. We need to have the same groups we created
in Salome:
• inlet
• outlet
• wall
In all the files:
• Delete lowerWall, frontAndBack and its contents.
• Change name from upperWall to wall.
P
Don not make any changes.
nut
Do not make any changes.
U
Change velocity from 10 m/s to 3 m/s:
value uniform (3 0 0);

Appendices
N.26
k
Change the value of k to 0.043457:
internalField uniform 0.043457;
boundaryField
{
inlet
{
type fixedValue;
value uniform 0.043457;
}
outlet
{
type zeroGradient;
}
wall
{
type kqRWallFunction;
}
}
epsilon
Change the value of epsilon to 1.06327:
boundaryField
{
inlet
{
type fixedValue;
}
outlet
{
type zeroGradient;
}
wall
{
type epsilonWallFunction;
}
}

Appendices
N.27
Table N.1 gives an overview of the boundary and initial conditions.
Table N.1: Boundary and initial conditions.
Type 𝑼 [𝒎/𝒔] 𝒑 [𝒎𝟐
/𝒔𝟐
] 𝒌 [𝒎𝟐
/𝒔𝟐
/𝒔𝟑
/𝒔]
internal
Field
uniform
(0 0 0)
uniform 0 uniform 0.043457 uniform 1.06327 uniform 0
inlet fixedValue
uniform
(3 0 0)
zeroGradient fixedValue
uniform 0.043457
fixedValue
uniform 1.06327
calculated
uniform 0
outlet
zeroGradient
fixedValue
uniform 0
zeroGradient zeroGradient calculated
uniform 0
wall noSlip zeroGradient kqRWallFunction
uniform 0.043457
epsilonWallFunction
uniform 1.06327
nutkWallFunction
uniform 0
System directory
Delete blockMeshDict and streamlines.
controlDict
Change deltaT to 0.0001 and writeInterval to 50:
deltaT 0.0001;
writeInterval 50;
Delete the following lines:
cacheTemporaryObjects
(
kEpsilon:G
);
functions
{
#includeFunc streamlines
#includeFunc writeObjects(kEpsilon:G)
}

Appendices
N.28
fvSchemes
do not make any changes.
fvSolution
Change to the values in the lines marked yellow:
solvers
{
p
{
solver GAMG;
tolerance 1e-09;
relTol 0.01;
smoother GaussSeidel;
}
"(U|k|epsilon|omega|f|v2)"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-09;
relTol 0.1;
}
}
SIMPLE
{
nNonOrthogonalCorrectors 0;
consistent yes;
residualControl
{
p 1e-3;
U 1e-3;
"(k|epsilon|omega|f|v2)" 1e-4;
}
}

Appendices
N.29
relaxationFactors
{
equations
{
U 0.8; // 0.9 is more stable but 0.95 more convergent
“.*” 0.8; // 0.9 is more stable but 0.95 more convergent
}
}
Residuals script
Open the text editor in Ubuntu and paste the following lines:
set term png
set output “residuals.png”
set logscale y
set title “Residuals”
set ylabel ‘Residual’
set xlabel ‘Iteration’
plot “<cat log | grep ‘Solving for Ux’ | cut -d ' ’ -f9 | tr -d ‘,'"
title 'Ux'
with lines,
"<cat log | grep 'Solving for Uy' | cut -d ' ' -f9 | tr -d ','"
title 'Uy'
with lines,
"<cat log | grep 'Solving for Uz' | cut -d ' ' -f9 | tr -d ','"
title 'Uz'
with lines,
"<cat log | grep 'Solving for p' | cut -d ' ' -f9 | tr -d ','"
title 'p'
with lines,
"<cat log | grep 'Solving for k' | cut -d ' ' -f9 | tr -d ','"
title 'k'
with lines,
"<cat log | grep 'Solving for epsilon' | cut -d ' ' -f9 | tr -d ','"
title 'epsilon'
with lines,
Save the file in the pipeBelly case directory and name it residuals.

Appendices
N.30
Case directory
Open the Allrun file and change the contents to:
#!/bin/sh
cd ${0%/*} || exit 1 # Run from this directory
simpleFoam > log &
tail -200f log
#------------------------------------------------------------------------------
Run the script
Open the terminal from the case directory and run the command:
./Allrun
The solution is converged when the following line appears:
SIMPLE solution converged in 0.0476 iterations
When the solution converges, stop the process with the command:
Ctr+C
To create the residual plot: write in the terminal:
gnuplot residuals -
Check 𝑦+
:
simpleFoam -postProcess -func yPlus
To post-process, open ParaView:
paraFoam

Appendices
N.31
Trouble shooting
Salome
It is recommended to make use of the Salome forum [1] when creating a mesh in Salome.
Using the search bar, one may find discussions and answers to problems, meshes and
geometries similar to your own case. Frequently, people will post answers in the form of a
python script. It is a good idea to download the script and evaluate it both in a text editor
program as well as to load it in the Salome GUI. Examining both the Python script and the
objects in the GUI, it should be possible to understand what is done. Then it may be easier to
implement the same method in your own case. In addition, an extensive collection of pre-
made example scripts is available in the Salome documentation. The Salome documentation
is available for download as an extra package on the Salome download page. There are also
many videos available on YouTube, in addition to the written documentation.
OpenFOAM
When creating a simulation in OpenFOAM it is recommended to take a good look at the
OpenFOAM User Guide [2] located on the path OpenFOAM /opt/openfoam8/doc/Guides and
look here first if you have questions.
It is also a good idea to make use of the CFD Online Forum [3] if the information you are
looking for is not easily available in the literature. There are discussions about many topics,
and it is possible to search for specific problems. However, one must remember to not trust
blindly in claims made in online discussion forums, but try to find more reliable sources to
back up the information. Still, it might be a good help for convergence problems, simulation
setup and for information about checking and validating the simulation. One tip is to create
an account in the forum early on in the CFD learning process, because attached files and
images in the forum are not available for non-users.
References
[1] SALOME, SALOME forum, OPEN CASCADE, 2005-2021. Accessed on: Jan.-Apr.,
2021. [Online]. Available: https://www.salome-platform.org/forum
[2] C. J. Greenshields, "OpenFOAM User Guide version 8," OpenFOAM Foundation
Ltd., CFD Direct Ltd., July 22, 2020.
[3] CFD Online Forum, CFD online, 1994-2021. Accessed on: Jan.-Apr., 2021. [Online].
Available: https://www.cfd-online.com/Forums/

complex mesh generation with openFOAM thchnical

More Related Content

Similar to complex mesh generation with openFOAM thchnical (20)

More from ssusercf6d0e (20)

Recently uploaded (20)

complex mesh generation with openFOAM thchnical