WHITEPAPER:
How to Choose an
Effective Grid System
for CFD Meshing
Abstract
Concurrent CFD is a new kind of CFD tool that enables mechanical engineers to
simulate the flow of fluid and heat transfer for today’s products using 3D CAD
models. One of the most critical steps in this process is meshing and
establishing an effective grid system for 3D simulation and analysis. This paper
discusses why automated adaptive meshing is advantageous and how new
designs can be meshed most effectively to dramatically reduce the time needed
for accurate analysis and to increase design productivity.
Contents
1
Needs and Choices ....................................................................................... 3
1.1
Why a Grid System in the First Place? ................................................... 3
1.2
What are the Choices of Grid System? .................................................. 4
2 Factors and Considerations Affecting the Choice of Grid System ................. 6
2.1
Cell Shape and Its Effect on “Grid Quality” ............................................. 6
2.2
Representation of Non-Rectangular Geometries .................................... 8
2.2.1
Patankar and co-workers (Ref 2) ..................................................... 9
2.2.2
Spalding and co-workers (Ref 3) ................................................... 10
2.2.3
Work at NASA Ames (Refs 4 and 5).............................................. 11
2.2.4
Work at University of Cambridge (Ref 6) ....................................... 12
2.3
Choice of Grid Arrangement - Structured or Unstructured? .................. 13
2.4
Grid Generation .................................................................................... 16
3 FloEFD’s Rectangular Adaptive Mesh Technology...................................... 19
3.1
Initial Mesh ........................................................................................... 19
3.2
Solution Adaptive Mesh ........................................................................ 21
4 REFERENCES ............................................................................................ 23
Appendix I: Diffusion Flux And Pressure Gradient In A Non-Orthogonal Grid .... 24
2
1 Needs and Choices
1.1 Why a Grid System in the First Place?
To begin with it is useful to consider the need for a grid system in any CFD
analysis:
All CFD analyses start from the differential equations governing fluid-dynamic
phenomena - the Navier-Stokes equations, and the associated conservation
equations for heat, etc.
As is well known, these equations are insoluble - at least by any analytical
means (except in cases which involve so many simplifications that they are of
virtually no practical interest).
Therefore the only way to solve them is by “discretisation”1:
Subdividing the region considered into many small volumes or “cells” - by
overlaying a conceptual grid system over the entire region of interest.
Making certain assumptions about the variation of the considered properties
(velocities, pressure, temperature, etc) within and between the volumes.
Thereby deriving approximations to the governing differential equations (
the so-called “finite-volume equations”) which are valid within the volumes
so long as each volume is small enough - and are therefore valid in
combination for the whole region of interest.
Then solving the resulting algebraic equations iteratively.
It is therefore clear that:
The grid is a means to an end - to the obtaining of a reasonably accurate
solution of the governing differential equations.
The chosen grid spacing or grid fineness will critically influence the accuracy
of the solution.
The choice of type of grid system - that is, the shape and arrangement of the
cells - is, in a sense, arbitrary. So long as it can easily be defined and yields
an accurate solution reliably and efficiently, any grid is as good as any other.
However, this “so long as …” is an important proviso. Experience shows that, for
any practical application, the choice of grid system for a CFD calculation can
radically affect:
User time in defining the problem, and in making subsequent
modifications
Ease of achieving good, accurate results.
Robustness and reliability of solution.
1
There are many excellent descriptions of this process in the literature, including Ref 1.
3
Computer speed and storage.
This is why the choice of grid systems for CFD calculations is such an
important one.
1.2 What are the Choices of Grid System?
There are two distinct aspects to the choice of grid system for CFD analyses:
(i) The shape of the grid cells, the main options being:
Cartesian - rectangular cuboid cells with the faces aligned with a Cartesian
x,y,z coordinate system.
Hexahedra - six-faced volumes which are distorted in some way from
Cartesian - these are sometimes referred to as “topologically Cartesian” (i.e.
like Cartesian but distorted), or “body-fitted” (i.e. derived - conceptually at least
- by distorting a Cartesian mesh around the surface of a body).
Tetrahedra - four faced volumes - in effect “triangular pyramids”
(ii) The arrangement of the grid cells, the main options being:
Structured - in which the grid cells are arranged in continuous lines through
the entire solution domain.
Unstructured - a completely arbitrary arrangement.
Partially unstructured - there are various intermediate, possibilities, usually
involving regions of structured grid combined with one another in some way.
Not all combinations of cell shape and grid arrangement are of practical interest.
The most widely used are:
Cartesian - both structured and partially unstructured - widely used for a wide
range of CFD applications.
Hexahedra - structured and partially unstructured (often referred to as “bodyfitted”) - most commonly used for “aerodynamic” applications (gas turbine
blades, aerofoils, streamlined bodies, etc) as a means to fit the grid to a
smoothly varying surface.
Fully unstructured hexahedra and/or tetrahedra - initially used in finite
element (rather than finite volume) CFD analyses, and now widely adopted for
the finite volume approach, often with prisms and square based pyramids
used to extrude and connect the surface mesh to the volume mesh.
These options are illustrated overleaf.
4
a) Cartesian Structured
b) Cartesian Partially Unstructured
(with Embedded Fine Grid Region)
c) Hexahedral Body Fitted
d) Fully Unstructured Hexahedra
e) Fully Unstructured Tetrahedra
Figure 1: Illustration of the Main Types of Grid System for CFD
5
A further comment is needed concerning the reference to Cartesian grids in the
above discussion. Strictly, many of the comments to be made about Cartesian
grids would apply equally to any “orthogonal” system - that is, one based on grid
lines aligned with coordinate directions which are everywhere at right angles to
each other. A Cartesian grid is the most common such system in practical use,
and is the one of relevance here. Orthogonal grids based on cylindrical
coordinates are also common, and others are in use, but are not generally
applicable. However, as will become apparent in the later discussion, it is the
“orthogonal” nature of the Cartesian system which leads to many of its
advantages over alternative (“non-orthogonal”) systems.
The remainder of this document considers these alternative approaches, in the
context particularly of the needs for CAD embedded CFD. It focuses mainly on
the first and the third in the earlier list - Cartesian, and fully unstructured
(hexahedra, tetrahedra and prisms). The second (structured hexahedra - body
fitted) is an intermediate approach, mainly suited to aerodynamic applications.
2 Factors and Considerations Affecting the Choice of Grid
System
2.1 Cell Shape and Its Effect on “Grid Quality”
A Cartesian cell shape is, in many respects, the “natural” choice. Why?
The governing equations are naturally derived and formulated in Cartesian
coordinates2.
The velocity components solved for are almost always those aligned in the
Cartesian coordinate directions.
This is the case whatever cell shape is used - or if it is not the case, then the
need to use a more general, and more complex non-orthogonal coordinate
system itself leads to difficulties of a similar kind to those described below.
The consequence is that a Cartesian grid leads to a “better quality grid” as
compared with any non-orthogonal shape - the greater the departure from
Cartesian (that is, the greater the degree of non-orthogonality), the greater the
degradation in “quality”.
The concept of “grid quality” is central to any consideration of alternative grid
systems for CFD. The cell shape (and particularly its departure from
2
Or in some other convenient orthogonal coordinate system
6
orthogonality) has severe implications on the assumptions made in the derivation
of the finite-volume equations from the differential equations, and on the resulting
solution method.
The central issue is explained in Appendix I. This considers the derivation of two
typical terms in the finite-volume equations - those representing diffusion flux (i.e.
heat conduction) across one cell face, and the pressure gradient which acts as a
source of velocity in one direction.
The derivation of these terms is considered for a highly non-orthogonal grid. The
important point to note is that, instead of resulting in a simple, single term (as for
a Cartesian system) the non-orthogonality leads to additional “secondary” terms.
In the two-dimensional case considered in the Appendix only two terms arise for
each of the processes considered (as compared with the single term arising for a
Cartesian system). However, in a fully three-dimensional system, the derivation
for a non-orthogonal grid leads to many times as many terms as for a Cartesian
system.
These additional secondary terms have a number of consequences:
Additional computer time - computation of the additional terms will clearly
have implications for computer time. As there may be several times as many
terms needed to represent a fully non-orthogonal system as a Cartesian one,
and as this calculation is repeated at every iteration of the solution, these
implications can be severe.
Additional computer storage - there can be major implications here. It is
usual to store (rather than continually re-calculate) the main geometric
parameters associated with each non-orthogonal grid cell. This is one reason
(the other is the need to store “connectivities” as explained later) why an
unstructured hexahedral or tetrahedral grid method can require substantially
more computer storage than a Cartesian grid method - and this can, in
practice, become a limitation on the use of such methods for large, complex,
calculations.
Reduced accuracy and reduced robustness of the iterative solution - the
evaluation and inclusion of these additional secondary terms introduce
additional “cross-linkages” into the system. That is to say, instead of values of
temperature at only two locations being used in the evaluation of a heat flux
(as in the primary term), values at many more, remote, locations will be
involved (in the secondary terms). There are two consequences:
Additional inaccuracies are introduced - which means that, all else being
equal, a highly non-orthogonal grid will have lower accuracy than an
7
orthogonal one of comparable spacing - or, to put it another way, to achieve
the same local numerical accuracy, a non-orthogonal grid will need to be
finer than an orthogonal one.
The second effect is on the stability of the convergence of the system of
finite-volume equations. Because of the less-direct (less implicit) manner in
which the secondary terms need to be handled in the iteration, as they
become more dominant, the iterative solution becomes progressively less
stable - leading to, at best, unreliable convergence or, at worst, divergence.
Of course the deficiencies in a non-orthogonal grid become more severe as the
grid becomes more distorted (i.e. less Cartesian) - and the consequences will
depend very much on the particular application in question. However, the effects
are clear and are well understood.
This is why:
CFD practitioners have sought, as far as possible, always to use Cartesian
grid systems, or other orthogonal systems.
Users of non-orthogonal systems are forced to go to great lengths to prevent
poor-quality grids, to the extent that (as explained later) grid generation usually involving some manual “adjustment” of any automatically-generated
grid - becomes the most time consuming part of the entire process of CFD
analysis.
2.2 Representation of Non-Rectangular Geometries
Why then, if the advantages of Cartesian grids are so clear, have CFD
practitioners made any use at all of non-orthogonal systems?
Clearly there is only one motivation - the apparent need to use such more
complex systems to represent physical shapes - particularly solid boundaries which are non-rectangular.
For these, non-orthogonal systems offer the (apparent) advantage that the grid
can be matched to (that is, fitted around) the physical shape of (say) an airfoil, so
that grid surfaces are forced to coincide with the physical boundaries.
There is, however, an alternative approach, of which there has been increasing,
successful experience in the last decade. In this a Cartesian grid is used, and
the non-rectangular solid shapes are allowed to cut through the grid in an
8
arbitrary way. The presence of the solid in the grid cells cut by the solid is
represented using appropriate “cut-cell” techniques.
The advantages of the approach are many:
Good grid quality is ensured, with the benefits explained earlier
The needs for any kind of “automatic” grid generation (with subsequent
manual adjustment) is avoided; and
For conjugate heat transfer problems, involving conductive heat transfer in
solid regions coupled to flow and heat transfer in the fluid (such as occur
commonly in electronics thermal applications), the grid system naturally covers
the fluid and solid regions, as needed for the complete, coupled solution.
There is now much experience of this approach, some for geometric shapes of
surprising complexity. Four examples are cited below.
2.2.1 Patankar and co-workers (Ref 2)
Figure 2 below shows work by Professor Patankar and co-workers.
Figure 2: Flow Over a Cylinder in Crossflow (Re = 26) Computed Using
Cartesian Grid and Body-Fitted Grid (Professor Patankar and Co-Workers,
Ref 2)
9
The figure demonstrates the quality of results obtained using a Cartesian grid
with a cut-cell representation of the fluid/solid cells, for a case which is
conceptually simple, but complex from the fluid-dynamics standpoint. Results for
flow around a cylinder in cross flow (at Re = 26) are compared with experimental
flow visualisation, and with results for a non-orthogonal body-fitted grid with a
comparable grid density.
Both sets of computational results show excellent correlation with the flow
visualisation, both for the predicted position of the separation point, and for the
predicted length and shape of the separated region. Other similar “simple” test
cases lead to essentially the same conclusion - that the Cartesian cut-cell
approach yields results just as good as alternative, more-complex nonorthogonal, body-fitted systems.
2.2.2 Spalding and co-workers (Ref 3)
Figure 3 shows work by Professor Spalding and co-workers (Ref 3).
Figure 3: Flow Around a Car Body Shape Computed Using a Cartesian Grid
With Embedded Sub Grids (Spalding and Co-Workers, Ref 3)
10
The case shown is turbulent flow around an automobile shape located in a wind
tunnel. In this case a Cartesian grid with embedded fine-grid regions is used,
giving a partially-unstructured grid (as discussed later).
The important conclusion is that the Cartesian grid gives results for pressure
variation over the surface of the vehicle which are in reasonable agreement with
measurements. Though results from alternative systems are not shown here, the
conclusion is that the Cartesian-grid results are of comparable quality with results
from body-fitted and other more-complex grid systems.
2.2.3 Work at NASA Ames (Refs 4 and 5)
Figure 4 refers to work at NASA Ames, primarily on the external aerodynamics of
aircraft and other airborne vehicles.
Figure 4: Cartesian Octree-Structured Grid for Computing Flow Around a
Military Helicopter (Aftosmis et al, Ref 4)
The illustration shows the application of a partially-unstructured Cartesian grid
(“octree-structured”) to the aerodynamics of a military helicopter (Ref 4). Such
11
grid systems are also being used at NASA Ames for computing flows around
airfoils and wing sections, complete aircraft fuselages, and multiple aircraft.
Other work at NASA Ames utilises Cartesian grids with embedded fine grid
regions (referred to as “overset structured grids”) in computing flows around and
behind flying bodies (Ref 5).
The authors have adopted these Cartesian-based techniques because of the
(relative) simplicity of grid generation and the superior numerical performance as
compared with alternative, non-orthogonal grid systems.
2.2.4 Work at University of Cambridge (Ref 6)
Professor Dawes paper reviews the development of CFD specifically for
turbomachinery simulations with a particular focus on application to problems
with complex geometry. Turbomachinery flows represent an extreme challenge
to modelling and simulation. Early turbomachinery CFD pioneered the use of
structured hexahedral meshes, e.g. for blade-blade flow analysis. This locked
the development trajectory of turbomachinery CFD into the “body-fitted”
paradigm that now underpins all the main general-purpose CFD software
systems. Professor Dawes argues that this is now holding back the use of CFD
and is effectively preventing its use in design due to time required to create the
mesh. A paradigm shift in mesh generation is needed, in which the geometry is
treated implicitly, rather than explicitly, where the volume mesh is fitted to the
surface.
Having made the case for an implicit geometry treatment, Professor Dawes
describes recent advances in computer graphics, where the development of
interactive volume sculpting and ‘physics-based animation’ have been driven by
the demands of the film industry. Level set techniques are used to accurately
represent multiply curved surfaces using a 3D distance field, storing the signed
distance to the nearest surface on an octree-structured Cartesian mesh. This
mesh is then used directly for the flow solver as shown below for external flow
around a turbine blade:
12
Figure 5: Tesselated geometry of a generic film-cooled turbine blade and octree
mesh used for flow solution around blade (Dawes, Ref 6)
Professor Dawes uses the example of changing one of the holes in the blade to
show how easy it is to change the geometry, as only mesh local to the hole
needs to be changed.
Generally, the conclusions from these and other studies are that:
Using appropriate cut-cell techniques, Cartesian grids can yield results for
extremely complex non-rectangular geometries which are of comparable
quality to the best obtained from more complex non-Cartesian systems; and
The use of Cartesian grids for such problems simplifies problem definition, and
ensures robust efficient solution - thereby ensuring user productivity and
optimum use of computer resources.
2.3 Choice of Grid Arrangement - Structured or Unstructured?
The second major choice in selecting a CFD grid system is the arrangement of
the grid cells - that is, are they in a tightly structured arrangement (in continuous
13
regular lines) such as that illustrated earlier in Fig 1a), or are they arranged in a
less structured or completely unstructured manner, as illustrated in Fig 1d) or
1e)?
Essentially the choice is really all about computer efficiency. An unstructured
grid (as shown in Fig 6 b)) can enable the user to concentrate fine grid only in
regions where it is required - a fully structured grid, with the same level of
fineness in the region of interest (as shown in Fig 6 a)), can involve apparently
“wasted” grid in the far field. The results from the two approaches would, all else
being equal, be identical - the only difference will be in the computer resources
required.
1
a) Structured Cartesian
b) Unstructured Tetrahedral
c) Cartesian with
Embedded Subgrid
Figure 6: Structured and Unstructured Grids
14
However, the adverse effect of the “wasted” grid is not as obvious as it at first
appears:
Solution on a fully unstructured grid such as that illustrated in Fig 6 b) requires
additional storage (of the “connectivities” which tell the solution which cells are
adjacent to which) and additional computation (to use the connectivities to
“unravel” the arbitrarily arranged data associated with the unstructured grid).
Furthermore, a non-orthogonal cell shape (usually hexahedral or tetrahedral which are almost always used with a fully unstructured grid) also leads to the
needs for additional storage, computational time, and grid fineness (as
compared with a Cartesian grid) due to the “grid quality” issues explained
earlier.
It is therefore far from self evident that the unstructured grid shown in Fig 6 b)
will lead to a more efficient solution than the fully structured grid in Fig 6 a).
Clearly the former has a smaller total number of grid cells - but it will require
substantially more computer storage and computer time per grid cell to obtain
a solution. The optimum choice will depend on the particular case in question.
Two further points are relevant:
Firstly, the advantages offered by unstructured grids are clearly the greatest
when the problem considered requires a very fine grid in one region (to resolve
detail in geometry of flow behaviour), surrounded by a large open region where a
much coarser grid can be used. Such cases are typical in external flow or
unconfined applications (the classic example being flow around a body in a free
stream). Two typical applications of this kind were illustrated in Section 2.2 – the
car-body shape in a (large) wind-tunnel (Fig 3), and the helicopter in free space
(Fig 4).
There are however many classes of problem (often “confined” flows - contained
within an enclosure) which do not exhibit a surrounding “large open region”. For
these the overheads associated with structured grids are much less. The interior
of a typical electronics enclosure is a classic example. The enclosure is densely
packed with components - the effects of all of which have to be modelled - so the
“wasted” grid from a local fine grid region is not usually wasted at all - it is used to
resolve necessary detail elsewhere in the flow domain. Similar comments apply
to pumps and valves which have complex internal structures that are difficult to
mesh using body-fitted techniques.
Secondly, there are extremely powerful intermediate approaches, which offer
virtually all of the flexibility of a fully unstructured system, while retaining virtually
all of the benefits (of robustness, speed, economy of computer storage) of a
Cartesian structured system. Two such approaches were referred to in the
examples cited in Section 2.2 above.
15
The most interesting of these3 is the use of embedded structured regions of fine
grid (or, in NASA’s terminology, overset structured grids). These enable large
numbers of regions of Cartesian grid to be combined with one another in
relatively arbitrary ways, with levels of refinement (regions within regions) as
required. So long as care is taken in handling the coupling between the regions
within the iterative solution, such methods can work extremely efficiently (with a
relatively small increase in computer time per cell as compared with a fully
structured grid) for as many as several hundred regions.
To conclude:
The use of structured vs. unstructured grids is entirely a question of computer
efficiency.
To judge computer efficiency simply by the total number of grid cells used to
solve the problem can be extremely misleading - for a structured Cartesian
system (for example) the overhead associated with “wasted” grid will often be
more than offset by the more efficient solution per grid cell.
Properly implemented, the use of embedded structured and octree grids in a
Cartesian system offers virtually all the flexibility of a fully unstructured
hexahedral or tetrahedral grid without any of the overheads (and, by using the
cut-cell techniques referred to earlier, can represent arbitrarily complex
geometries perfectly well).
2.4 Grid Generation
At some stage in setting up a CFD problem users need to be concerned with
“grid generation”. This has two aspects:
The mechanical setting of the data which define the grid - that is the x, y, z
locations of grid cell centres and/or vertices. This stage will often involve
some basic consideration of matching grid to geometric boundaries, both at
the edges and within the solution domain.
Ensuring that the grid is a “good” one - meaning:
That it will give results of the required accuracy - which involves ensuring
that the grid is sufficiently fine to resolve adequately the features of the
3
The alternative method referred to earlier is the octree-structured grid, which offers advantages
when used (as by NASA) for complex bodies such as aircraft fuselages, and (as by Cambridge
University) for turbomachinery applications. For such cases it is used in a “geometry adaptive”
manner - in which the grid is automatically refined locally based on the local geometric features of
the body.
16
solution of interest, and give results of at least the required “engineering
accuracy”.
That the iterative scheme will converge reliably. This relates particularly to
the question of “grid quality” referred to earlier.
For a Cartesian grid the first stage is trivial - the required data is simply the three
one-dimensional arrays, to set the x, y, and z locations of grid vertices (usually) in a 100,000 cell grid (roughly 46 x 46 x 46) this is 138 (46 x 3) numbers. These
could simply be set directly by the user, but this is usually not the most
convenient way. The point is that the fundamental simplicity of the required data
makes it possible to provide simple user controls to automate the setting and
manipulation of the grid, such as those available in FloEFD described later.
These make it relatively easy for even an inexperienced user to make any
adjustments needed to provide a “good” grid in the sense described in the
second point above.
In contrast, the grid setting (i.e. the first stage of the above) for an unstructured
non-orthogonal grid is an entirely different matter. Because of the absence of
any logical order or arrangement in the grid, it is necessary to set x, y and z
separately for every single grid vertex. In a 100,000 grid this would require
300,000 numbers to be set - which clearly cannot be done manually. This means
that some mechanical means has to be provided - using some form of algorithm.
This involves the creation of a 2D surface mesh whose faces are shared by the
3D volume mesh. The most usual approach is to use Delaunay Triangulation or
the Advancing Front Method which in effect “interpolates” between defined
surfaces in some geometric manner. This achieves the first stage of the grid
specification task. However, as the user has very little control over the resulting
grid (other than the specification of the defined surfaces), it is then virtually
always necessary to make further adjustments to ensure:
That the grid quality is good enough to ensure reasonably reliable
convergence. As a very localised region of poor quality grid (sometimes only
one grid cell) can disrupt the entire solution, this might involve manual redefinition of individual grid cells.
That the grid fineness is adequate in the various flow regions to give the
required accuracy. This is necessary because the interpolation method has
no way of anticipating the needs for fine grids in particular regions of the flow associated with high gradients in the solved for variables. The grid will
therefore need adjustment based on user knowledge or experience.
Since the process involves the use of a mechanical, algorithm-based method for
providing the grid locations it is conventionally (and misleadingly) referred to as
“automatic” grid generation. In fact it is anything but. The process takes no
17
account of the two critical issues without which the grid is useless – it’s quality
and fineness for the required solution accuracy. The complexity of the process
makes it difficult and time consuming for the user to make the subsequent
(usually manual) adjustments.
Furthermore, this complexity has implications for any geometric change in the
computational model. For example, if an object is re-located, the whole process
(often including the subsequent manual adjustments) has to be repeated making the performance of parametric design studies time consuming, error
prone and impossible to automate.
Professor Dawes (Ref 6) notes that a critical associated problem is the source of
the geometry itself as geometry exported from a CAD system is almost always
“dirty” (i.e. not water tight) even if exported direct from the solid modeling kernel
due to numerical tolerancing issues within the CAD system requiring very
substantial effort to clean up and condition this geometry representation so that
the body-fitted meshing software can run satisfactorily. He concludes that: “the
mesh generation may well fail and need careful nursing to produce an acceptable
mesh for a really complex geometry – and generating the associated viscous
layers remains a nightmare”. The latter point referring to the need to ensure that
the mesh near to surfaces is sufficiently fine to resolve near-wall flow boundary
layers.
Prof. Dawes also notes a key distinction between analysis and design, being that
analysis is aimed at gaining insight into the performance of a design, but design
involves changing geometry, so for design the flexibility and generality with which
the geometry can be changed is the critical enabling factor in the designer’s
properly explore the design space.
From the point of view of design, the critical factor is: how fast can the geometry
be changed and re-meshed?
To conclude:
Body-fitted meshes are time consuming to create, and often require manual
intervention
Body-fitted meshes are analysis centric, not design centric, making them
difficult to use for product design
18
3 FloEFD’s Rectangular Adaptive Mesh Technology
3.1 Initial Mesh
FloEFD uses an octree mesh. Where refinement is necessary, isotropic splitting
is used, resulting in 8 identical smaller cells. A cut-cell treatment is used at solidfluid boundaries.
In FloEFD the initial mesh (so-called as it’s created before the solution and any
solution-adaptive refinement) is defined first constructing a basic Cartesian mesh
which is then refined. Definition of the initial mesh can be fully automated using
the dialog below or it can be defined manually if the ‘Automatic settings’ check
box below is checked off.
Figure 7: FloEFD’s Initial Mesh dialog
The initial mesh is constructed from a near-uniform Cartesian basic mesh that is
subsequently refined according to a number of criteria. The ‘Level of Initial Mesh’
slider bar shown in the dialog controls the number of cells in the basic mesh.
19
The ‘Show basic mesh’ check box displays the basic mesh on the model as
shown in Figure 8 below. The basic mesh can be stretched to better capture
features of the model. The dialog settings shown in Figure 7 produce the basic
and initial meshes shown in Figure 8.
Figure 8: Basic Mesh and resulting default Initial Mesh for Ball Valve Tutorial
Case
The initial mesh is constructed by refining the basic mesh around the intersection
of the solid model, guided by settings for the ‘Minimum gap size’ and ‘Minimum
wall thickness’.
The ‘Level of initial mesh’ performs a number of functions in addition to refining
the basic mesh. It also determines how many times the basic mesh can be split
and sets levels and values for various refinement criteria. FloEFD has separate
refinement levels for solid, fluid, and cut cells. Small solid features, local
curvature, and narrow channels also have refinement levels together with an
associated dimension to denote the smallest size to which the cells can be split.
The ‘Level of initial mesh’ slider automatically sets values for all these refinement
levels to produce the automatic mesh.
Once the automatic mesh has been generated, the user can check off the
‘Automatic settings’ box and adjust the settings manually. This gives complete
control over the meshing process.
20
Figure 9: Manual refinement of partial cells (left) and fluid cells (right)
The initial mesh settings are applied to the entire computational domain. For
example, when specifying a mesh refinement in narrow channels, this is applied
to all regions having the same characteristics. However, the initial mesh can also
be refined locally, with the local region defined by a component (a part or
subassembly in assemblies, as well as a body in multibody parts), face, edge or
vertex, or a defined fluid region.
3.2 Solution Adaptive Mesh
The solution-adaptive meshing is a procedure for adapting the computational
mesh to the solution during the calculation. This is useful to capture flow
features, the location of which can not be predicted before solution, for example
to capture shocks in high Mach number flows. Cells that do not adequately
resolve the gradients of velocity, temperature, pressure, etc. on the initial or
previously adapted mesh are refined. Cells that are found to be finer than
required are correspondingly coarsened.
The octree-based mesh makes the procedure is very simple. Cells are refined
by splitting into 8 smaller cells and coarsened by merging 8 identical cells into
one. One of the validation cases supplied with FloEFD (Ref. 7) is suitable for
demonstrating this.
The case considers supersonic flow in a 2D convergent-divergent channel.
21
Figure 10: Schematic of Convergent-Divergent Channel showing location of
shocks
A uniform supersonic stream of air, having a Mach number of 3, a static
temperature of 293.2K, and a static pressure of 1atm, is specified at the channel
inlet between two parallel walls. In the convergent section the flow decelerates
through two oblique shocks. The shape of the convergent section has been
adjusted to the inlet Mach number, so the shape of the shocks matches the
geometry, as shown in Figure 10.
The initial grid is refined near to the walls, but is not well suited to capture the
above shocks. Adaptive mesh refinement is used to refine the mesh as the
solution proceeds. This reduces the overall cell count whilst concentrating the
mesh around the shocks. The initial fine grid and the result of the adaptive
meshing are shown in Figure 11.
Figure 11: Initial and Final (Solution Adapted) Mesh
The solution adapted mesh accurately captures the sharp shocks as shown in
the contour plot of Mach number below. Mach number values predicted with
FloEFD along the channel centerline (the reference points are marked by square
boxes with numbers) are also compared with the theoretical values.
22
Figure 12: Contour Plot of Mach Number and Agreement with Theory
4 REFERENCES
1. S V Patankar “Numerical Heat Transfer and Fluid Flow”, Hemisphere
Publishing, 1980.
2. S V Patankar, Unpublished Presentation at 6th International FloTHERM User
Conference, October 1997.
3. D B Spalding, “CAD to SFT, with Aeronautical Applications”, Plenary Lecture
at 38th Israel Annual Conference on Aerospace Sciences, February 1998.
4. M J Aftomis, M J Berger, and J E Melton, “Robust and Efficient Cartesian
Mesh Generation for Component-Based Geometry”, Paper no AIAA 97 - 0196
Presented at 35th AIAA Aerospace Sciences Meeting and Exhibit, January
1997.
5. R L Meakin, “On Adaptive Refinement and Overset Structured Grids, Paper
No AIAA - 97 - 1858, 1997.
6. W N Dawes, “Turbomachinery computational fluid dynamics: asymptotes and
paradigm shifts”, Phil. Trans. R. Soc. A, Vol. 365, No. 1859, pp. 2553-2585,
May 2007.
7. “EFD.Lab 8 Fundamentals”, Flomerics Ltd, 2007.
23
Appendix I: Diffusion Flux And Pressure Gradient In A NonOrthogonal Grid
For a non-orthogonal grid, the normal flux through a control volume face is not
aligned with the line joining the adjacent grid points. Therefore, calculation of
total normal flux through a face requires calculation of primary and secondary
fluxes. It is of interest to write the equation for calculation of diffusion flux for a
non-orthogonal grid. This is illustrated for a quadrilateral grid in two-dimensions.
However, the same arguments apply for triangular non-orthogonal grids
(departure from equilateral triangles in two dimensions).
X2
Tn
P
θ
E
X1
Ts
A non-orthogonal quadrilateral grid
In reference to the above figure, the total diffusion flux through a control volume
face is decomposed into primary and secondary fluxes as follows:
Q = − AK (
Q=(
AK
δ PE
.
∂T
)
∂n
AK Sinθ
1
)(TP − TE ) + (
.
)(T − T )
Cosθ
δsn Cosθ s n
Primary Coefficient
Secondary Coefficient
Note that for a conduction equation, the primary and secondary coefficients in the
discretization equations for the temperatures on the two sides of the control
volume face are directly proportional to the areas multiplying the temperature
gradient terms in the above equation. The behavior of these coefficients is
plotted in the following figure.
24
As the departure from the orthogonality increases, both the primary and
secondary coefficients become progressively large. It is the small difference
between the primary and secondary flux terms that creates the net flux. Note
that for a Cartesian or orthogonal grid, the primary coefficient (secondary
coefficient is zero) is inversely proportional to the distance between the grid
points on the two sides of the control volume face and it correctly represents the
physical “conductance” between the adjacent grid points. When the grid is
strongly non-orthogonal, the coefficients no longer reflect the physical
conductance.
The momentum equation for the velocity normal to the face (flow rate for
continuity equation) is given as follows:
∧
.
.
M = M+[
A
δ PE
A Sinθ
1
( PP − PE ) +
( P − Pn ) ]
Cosθ
δ sn Cosθ s
Again, the normal pressure gradient has to be decomposed into primary and
secondary gradients analogous to the temperature gradient calculation. When a
25
pressure-based solution procedure is used the handle the velocity-pressure
coupling, the coefficients in the pressure correction equation also behave
inappropriately.
26