User Guide

User Manual: Pdf

Open the PDF directly: View PDF .
Page Count: 1

Download
Open PDF In Browser	View PDF

Open∇FOAM

The Open Source CFD Toolbox

User Guide

Version 1.6
24th July 2009

U-2
c 2000, 2001, 2002, 2003, 2004, 2005, 2006, 2007, 2008, 2009 OpenCFD
Copyright °
Limited.
Permission is granted to copy, distribute and/or modify this document under the terms
of the GNU Free Documentation License, Version 1.2 published by the Free Software
Foundation; with no Invariant Sections, no Back-Cover Texts and one Front-Cover Text:
“Available free from openfoam.org.” A copy of the license is included in the section
entitled “GNU Free Documentation License”.
This document is distributed in the hope that it will be useful, but WITHOUT ANY
WARRANTY; without even the implied warranty of MERCHANTABILITY or FITNESS
FOR A PARTICULAR PURPOSE.
Typeset in LATEX.

Open∇FOAM-1.6

U-3

GNU Free Documentation License
Version 1.2, November 2002
c
Copyright °2000,2001,2002
Free Software Foundation, Inc.
59 Temple Place, Suite 330, Boston, MA 02111-1307 USA
Everyone is permitted to copy and distribute verbatim copies of this license document, but
changing it is not allowed.

Preamble
The purpose of this License is to make a manual, textbook, or other functional and useful
document “free” in the sense of freedom: to assure everyone the effective freedom to copy and
redistribute it, with or without modifying it, either commercially or noncommercially. Secondarily, this License preserves for the author and publisher a way to get credit for their work,
while not being considered responsible for modifications made by others.
This License is a kind of “copyleft”, which means that derivative works of the document
must themselves be free in the same sense. It complements the GNU General Public License,
which is a copyleft license designed for free software.
We have designed this License in order to use it for manuals for free software, because free
software needs free documentation: a free program should come with manuals providing the
same freedoms that the software does. But this License is not limited to software manuals; it
can be used for any textual work, regardless of subject matter or whether it is published as a
printed book. We recommend this License principally for works whose purpose is instruction or
reference.

1. APPLICABILITY AND DEFINITIONS

This License applies to any manual or other work, in any medium, that contains a notice placed
by the copyright holder saying it can be distributed under the terms of this License. Such a
notice grants a world-wide, royalty-free license, unlimited in duration, to use that work under
the conditions stated herein. The “Document”, below, refers to any such manual or work.
Any member of the public is a licensee, and is addressed as “you”. You accept the license if
you copy, modify or distribute the work in a way requiring permission under copyright law.
A “Modified Version” of the D8(e)-053.1098(e)-437.503(D)8.811(m)0.0828044(e)-0.233867(n)0653867(h

U-4
document straightforwardly with generic text editors or (for images composed of pixels) generic
paint programs or (for drawings) some widely available drawing editor, and that is suitable for
input to text formatters or for automatic translation to a variety of formats suitable for input to
text formatters. A copy made in an otherwise Transparent file format whose markup, or absence
of markup, has been arranged to thwart or discourage subsequent modification by readers is not
Transparent. An image format is not Transparent if used for any substantial amount of text. A
copy that is not “Transparent” is called “Opaque”.
Examples of suitable formats for Transparent copies include plain ASCII without markup,
Texinfo input format, LaTeX input format, SGML or XML using a publicly available DTD,
and standard-conforming simple HTML, PostScript or PDF designed for human modification.
Examples of transparent image formats include PNG, XCF and JPG. Opaque formats include
proprietary formats that can be read and edited only by proprietary word processors, SGML or
XML for which the DTD and/or processing tools are not generally available, and the machinegenerated HTML, PostScript or PDF produced by some word processors for output purposes
only.
The “Title Page” means, for a printed book, the title page itself, plus such following pages
as are needed to hold, legibly, the material this License requires to appear in the title page. For
works in formats which do not have any title page as such, “Title Page” means the text near
the most prominent appearance of the work’s title, preceding the beginning of the body of the
text.
A section “Entitled XYZ” means a named subunit of the Document whose title either is
precisely XYZ or contains XYZ in parentheses following text that translates XYZ in another
language. (Here XYZ stands for a specific section name mentioned below, such as “Acknowledgements”, “Dedications”, “Endorsements”, or “History”.) To “Preserve the Title” of such a section when you modify the Document means that it remains a section “Entitled
XYZ” according to this definition.
The Document may include Warranty Disclaimers next to the notice which states that this
License applies to the Document. These Warranty Disclaimers are considered to be included by
reference in this License, but only as regards disclaiming warranties: any other implication that
these Warranty Disclaimers may have is void and has no effect on the meaning of this License.

2. VERBATIM COPYING
You may copy and distribute the Document in any medium, either commercially or noncommercially, provided that this License, the copyright notices, and the license notice saying this
License applies to the Document are reproduced in all copies, and that you add no other conditions whatsoever to those of this License. You may not use technical measures to obstruct or
control the reading or further copying of the copies you make or distribute. However, you may
accept compensation in exchange for copies. If you distribute a large enough number of copies
you must also follow the conditions in section 3.
You may also lend copies, under the same conditions stated above, and you may publicly
display copies.

3. COPYING IN QUANTITY
If you publish printed copies (or copies in media that commonly have printed covers) of the
Document, numbering more than 100, and the Document’s license notice requires Cover Texts,
you must enclose the copies in covers that carry, clearly and legibly, all these Cover Texts:
Front-Cover Texts on the front cover, and Back-Cover Texts on the back cover. Both covers
must also clearly and legibly identify you as the publisher of these copies. The front cover must
present the full title with all words of the title equally prominent and visible. You may add
other material on the covers in addition. Copying with changes limited to the covers, as long as
they preserve the title of the Document and satisfy these conditions, can be treated as verbatim
copying in other respects.
Open∇FOAM-1.6

U-5
If the required texts for either cover are too voluminous to fit legibly, you should put the first
ones listed (as many as fit reasonably) on the actual cover, and continue the rest onto adjacent
pages.
If you publish or distribute Opaque copies of the Document numbering more than 100, you
must either include a machine-readable Transparent copy along with each Opaque copy, or state
in or with each Opaque copy a computer-network location from which the general network-using
public has access to download using public-standard network protocols a complete Transparent
copy of the Document, free of added material. If you use the latter option, you must take
reasonably prudent steps, when you begin distribution of Opaque copies in quantity, to ensure
that this Transparent copy will remain thus accessible at the stated location until at least one
year after the last time you distribute an Opaque copy (directly or through your agents or
retailers) of that edition to the public.
It is requested, but not required, that you contact the authors of the Document well before
redistributing any large number of copies, to give them a chance to provide you with an updated
version of the Document.

4. MODIFICATIONS
You may copy and distribute a Modified Version of the Document under the conditions of
sections 2 and 3 above, provided that you release the Modified Version under precisely this
License, with the Modified Version filling the role of the Document, thus licensing distribution
and modification of the Modified Version to whoever possesses a copy of it. In addition, you
must do these things in the Modified Version:
A. Use in the Title Page (and on the covers, if any) a title distinct from that of the Document,
and from those of previous versions (which should, if there were any, be listed in the
History section of the Document). You may use the same title as a previous version if the
original publisher of that version gives permission.
B. List on the Title Page, as authors, one or more persons or entities responsible for authorship of the modifications in the Modified Version, together with at least five of the
principal authors of the Document (all of its principal authors, if it has fewer than five),
unless they release you from this requirement.
C. State on the Title page the name of the publisher of the Modified Version, as the publisher.
D. Preserve all the copyright notices of the Document.
E. Add an appropriate copyright notice for your modifications adjacent to the other copyright
notices.
F. Include, immediately after the copyright notices, a license notice giving the public permission to use the Modified Version under the terms of this License, in the form shown
in the Addendum below.
G. Preserve in that license notice the full lists of Invariant Sections and required Cover Texts
given in the Document’s license notice.
H. Include an unaltered copy of this License.
I. Preserve the section Entitled “History”, Preserve its Title, and add to it an item stating
at least the title, year, new authors, and publisher of the Modified Version as given on the
Title Page. If there is no section Entitled “History” in the Document, create one stating
the title, year, authors, and publisher of the Document as given on its Title Page, then
add an item describing the Modified Version as stated in the previous sentence.
Open∇FOAM-1.6

U-6
J. Preserve the network location, if any, given in the Document for public access to a Transparent copy of the Document, and likewise the network locations given in the Document
for previous versions it was based on. These may be placed in the “History” section. You
may omit a network location for a work that was published at least four years before the
Document itself, or if the original publisher of the version it refers to gives permission.
K. For any section Entitled “Acknowledgements” or “Dedications”, Preserve the Title of the
section, and preserve in the section all the substance and tone of each of the contributor
acknowledgements and/or dedications given therein.
L. Preserve all the Invariant Sections of the Document, unaltered in their text and in their
titles. Section numbers or the equivalent are not considered part of the section titles.
M. Delete any section Entitled “Endorsements”. Such a section may not be included in the
Modified Version.
N. Do not retitle any existing section to be Entitled “Endorsements” or to conflict in title
with any Invariant Section.
O. Preserve any Warranty Disclaimers.
If the Modified Version includes new front-matter sections or appendices that qualify as
Secondary Sections and contain no material copied from the Document, you may at your option
designate some or all of these sections as invariant. To do this, add their titles to the list of
Invariant Sections in the Modified Version’s license notice. These titles must be distinct from
any other section titles.
You may add a section Entitled “Endorsements”, provided it contains nothing but endorsements of your Modified Version by various parties–for example, statements of peer review or
that the text has been approved by an organization as the authoritative definition of a standard.
You may add a passage of up to five words as a Front-Cover Text, and a passage of up to
25 words as a Back-Cover Text, to the end of the list of Cover Texts in the Modified Version.
Only one passage of Front-Cover Text and one of Back-Cover Text may be added by (or through
arrangements made by) any one entity. If the Document already includes a cover text for the
same cover, previously added by you or by arrangement made by the same entity you are acting
on behalf of, you may not add another; but you may replace the old one, on explicit permission
from the previous publisher that added the old one.
The author(s) and publisher(s) of the Document do not by this License give permission to
use their names for publicity for or to assert or imply endorsement of any Modified Version.

5. COMBINING DOCUMENTS
You may combine the Document with other documents released under this License, under
the terms defined in section 4 above for modified versions, provided that you include in the
combination all of the Invariant Sections of all of the original documents, unmodified, and list
them all as Invariant Sections of your combined work in its license notice, and that you preserve
all their Warranty Disclaimers.
The combined work need only contain one copy of this License, and multiple identical Invariant Sections may be replaced with a single copy. If there are multiple Invariant Sections
with the same name but different contents, make the title of each such section unique by adding
at the end of it, in parentheses, the name of the original auth
Invariant Sections im thlieense notich of thr combined wo

U-7
6. COLLECTIONS OF DOCUMENTS
You may make a collection consisting of the Document and other documents released under
this License, and replace the individual copies of this License in the various documents with a
single copy that is included in the collection, provided that you follow the rules of this License
for verbatim copying of each of the documents in all other respects.
You may extract a single document from such a collection, and distribute it individually
under this License, provided you insert a copy of this License into the extracted document, and
follow this License in all other respects regarding verbatim copying of that document.

7. AGGREGATION WITH INDEPENDENT WORKS
A compilation of the Document or its derivatives with other separate and independent documents or works, in or on a volume of a storage or distribution medium, is called an “aggregate”
if the copyright resulting from the compilation is not used to limit the legal rights of the compilation’s users beyond what the individual works permit. When the Document is included in
an aggregate, this License does not apply to the other works in the aggregate which are not
themselves derivative works of the Document.
If the Cover Text requirement of section 3 is applicable to these copies of the Document,
then if the Document is less than one half of the entire aggregate, the Document’s Cover Texts
may be placed on covers that bracket the Document within the aggregate, or the electronic
equivalent of covers if the Document is in electronic form. Otherwise they must appear on
printed covers that bracket the whole aggregate.

8. TRANSLATION
Translation is considered a kind of modification, so you may distribute translations of the
Document under the terms of section 4. Replacing Invariant Sections with translations requires
special permission from their copyright holders, but you may include translations of some or
all Invariant Sections in addition to the original versions of these Invariant Sections. You
may include a translation of this License, and all the license notices in the Document, and any
Warranty Disclaimers, provided that you also include the original English version of this License
and the original versions of those notices and disclaimers. In case of a disagreement between
the translation and the original version of this License or a notice or disclaimer, the original
version will prevail.
If a section in the Document is Entitled “Acknowledgements”, “Dedications”, or “History”,
the requirement (section 4) to Preserve its Title (section 1) will typically require changing the
actual title.

9. TERMINATION
You may not copy, modify, sublicense, or distribute the Document except as expressly provided
for under this License. Any other attempt to copy, modify, sublicense or distribute the Document
is void, and will automatically terminate your rights under this License. However, parties who
have received copies, or rights, from you under this License will not have their licenses terminated
so long as such parties remain in full compliance.

10. FUTURE REVISIONS OF THIS LICENSE
The Free Software Foundation may publish new, revised versions of the GNU Free Documentation License from time to time. Such new versions will be similar in spirit to the present version,
but may differ in detail to address new problems or concerns. See http://www.gnu.org/copyleft/.
Each version of the License is given a distinguishing version number. If the Document
specifies that a particular numbered version of this License “or any later version” applies to it,
you have the option of following the terms and conditions either of that specified version or of
Open∇FOAM-1.6

U-8
any later version that has been published (not as a draft) by the Free Software Foundation. If
the Document does not specify a version number of this License, you may choose any version
ever published (not as a draft) by the Free Software Foundation.

Open∇FOAM-1.6

U-9
Trademarks
ANSYS is a registered trademark of ANSYS Inc.
CFX is a registered trademark of Ansys Inc.
CHEMKIN is a registered trademark of Reaction Design Corporation
EnSight is a registered trademark of Computational Engineering International Ltd.
Fieldview is a registered trademark of Intelligent Light
Fluent is a registered trademark of Ansys Inc.
GAMBIT is a registered trademark of Ansys Inc.
Icem-CFD is a registered trademark of Ansys Inc.
I-DEAS is a registered trademark of Structural Dynamics Research Corporation
JAVA is a registered trademark of Sun Microsystems Inc.
Linux is a registered trademark of Linus Torvalds
OpenFOAM is a registered trademark of OpenCFD Ltd
ParaView is a registered trademark of Kitware
STAR-CD is a registered trademark of Computational Dynamics Ltd.
UNIX is a registered trademark of The Open Group

Open∇FOAM-1.6

U-10

Open∇FOAM-1.6

Contents
Copyright Notice

U-2

GNU Free Documentation Licence
1. APPLICABILITY AND DEFINITIONS . . . . . . .
2. VERBATIM COPYING . . . . . . . . . . . . . . .
3. COPYING IN QUANTITY . . . . . . . . . . . . . .
4. MODIFICATIONS . . . . . . . . . . . . . . . . . .
5. COMBINING DOCUMENTS . . . . . . . . . . . .
6. COLLECTIONS OF DOCUMENTS . . . . . . . . .
7. AGGREGATION WITH INDEPENDENT WORKS
8. TRANSLATION . . . . . . . . . . . . . . . . . . . .
9. TERMINATION . . . . . . . . . . . . . . . . . . . .
10. FUTURE REVISIONS OF THIS LICENSE . . . .

U-3
U-3
U-4
U-4
U-5
U-6
U-7
U-7
U-7
U-7
U-7

.
.
.
.
.
.
.
.
.
.

Trademarks

U-9

Contents

U-11

1 Introduction

U-17

2 Tutorials
2.1 Lid-driven cavity flow . . . . . . . . . . . . . . . . . . . . . . .
2.1.1 Pre-processing . . . . . . . . . . . . . . . . . . . . . . .
2.1.1.1 Mesh generation . . . . . . . . . . . . . . . .
2.1.1.2 Boundary and initial conditions . . . . . . . .
2.1.1.3 Physical properties . . . . . . . . . . . . . . .
2.1.1.4 Control . . . . . . . . . . . . . . . . . . . . .
2.1.1.5 Discretisation and linear-solver settings . . . .
2.1.2 Viewing the mesh . . . . . . . . . . . . . . . . . . . . .
2.1.3 Running an application . . . . . . . . . . . . . . . . . .
2.1.4 Post-processing . . . . . . . . . . . . . . . . . . . . . .
2.1.4.1 Isosurface and contour plots . . . . . . . . . .
2.1.4.2 Vector plots . . . . . . . . . . . . . . . . . . .
2.1.4.3 Streamline plots . . . . . . . . . . . . . . . .
2.1.5 Increasing the mesh resolution . . . . . . . . . . . . . .
2.1.5.1 Creating a new case using an existing case . .
2.1.5.2 Creating the finer mesh . . . . . . . . . . . .
2.1.5.3 Mapping the coarse mesh results onto the fine
2.1.5.4 Control adjustments . . . . . . . . . . . . . .
2.1.5.5 Running the code as a background process . .
2.1.5.6 Vector plot with the refined mesh . . . . . . .

U-19
U-19
U-20
U-20
U-22
U-23
U-23
U-25
U-25
U-26
U-28
U-28
U-30
U-30
U-30
U-32
U-32
U-32
U-33
U-33
U-33

. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
. . .
mesh
. . .
. . .
. . .

U-12

Contents

2.1.5.7 Plotting graphs . . . . . . . . . . . . . . . . . .
Introducing mesh grading . . . . . . . . . . . . . . . . .
2.1.6.1 Creating the graded mesh . . . . . . . . . . . .
2.1.6.2 Changing time and time step . . . . . . . . . .
2.1.6.3 Mapping fields . . . . . . . . . . . . . . . . . .
2.1.7 Increasing the Reynolds number . . . . . . . . . . . . . .
2.1.7.1 Pre-processing . . . . . . . . . . . . . . . . . .
2.1.7.2 Running the code . . . . . . . . . . . . . . . . .
2.1.8 High Reynolds number flow . . . . . . . . . . . . . . . .
2.1.8.1 Pre-processing . . . . . . . . . . . . . . . . . .
2.1.8.2 Running the code . . . . . . . . . . . . . . . . .
2.1.9 Changing the case geometry . . . . . . . . . . . . . . . .
2.1.10 Post-processing the modified geometry . . . . . . . . . .
Stress analysis of a plate with a hole . . . . . . . . . . . . . . .
2.2.1 Mesh generation . . . . . . . . . . . . . . . . . . . . . .
2.2.1.1 Boundary and initial conditions . . . . . . . . .
2.2.1.2 Mechanical properties . . . . . . . . . . . . . .
2.2.1.3 Thermal properties . . . . . . . . . . . . . . . .
2.2.1.4 Control . . . . . . . . . . . . . . . . . . . . . .
2.2.1.5 Discretisation schemes and linear-solver control
2.2.2 Running the code . . . . . . . . . . . . . . . . . . . . . .
2.2.3 Post-processing . . . . . . . . . . . . . . . . . . . . . . .
2.2.4 Exercises . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.2.4.1 Increasing mesh resolution . . . . . . . . . . . .
2.2.4.2 Introducing mesh grading . . . . . . . . . . . .
2.2.4.3 Changing the plate size . . . . . . . . . . . . .
Breaking of a dam . . . . . . . . . . . . . . . . . . . . . . . . .
2.3.1 Mesh generation . . . . . . . . . . . . . . . . . . . . . .
2.3.2 Boundary conditions . . . . . . . . . . . . . . . . . . . .
2.3.3 Setting initial field . . . . . . . . . . . . . . . . . . . . .
2.3.4 Fluid properties . . . . . . . . . . . . . . . . . . . . . . .
2.3.5 Turbulence modelling . . . . . . . . . . . . . . . . . . . .
2.3.6 Time step control . . . . . . . . . . . . . . . . . . . . . .
2.3.7 Discretisation schemes . . . . . . . . . . . . . . . . . . .
2.3.8 Linear-solver control . . . . . . . . . . . . . . . . . . . .
2.3.9 Running the code . . . . . . . . . . . . . . . . . . . . . .
2.3.10 Post-processing . . . . . . . . . . . . . . . . . . . . . . .
2.3.11 Running in parallel . . . . . . . . . . . . . . . . . . . . .
2.3.12 Post-processing a case run in parallel . . . . . . . . . . .
2.1.6

2.2

2.3

3 Applications and libraries
3.1 The programming language of OpenFOAM
3.1.1 Language in general . . . . . . . .
3.1.2 Object-orientation and C++ . . . .
3.1.3 Equation representation . . . . . .
3.1.4 Solver codes . . . . . . . . . . . . .
3.2 Compiling applications and libraries . . . .
3.2.1 Header .H files . . . . . . . . . . . .
3.2.2 Compiling with wmake . . . . . . .
3.2.2.1 Including headers . . . . .
3.2.2.2 Linking to libraries . . . .
Open∇FOAM-1.6

.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

U-34
U-36
U-37
U-38
U-39
U-39
U-39
U-39
U-40
U-41
U-42
U-43
U-46
U-46
U-47
U-49
U-51
U-51
U-51
U-52
U-54
U-54
U-55
U-55
U-56
U-56
U-56
U-56
U-58
U-58
U-59
U-60
U-60
U-61
U-62
U-62
U-63
U-63
U-67

.
.
.
.
.
.
.
.
.
.

U-69
U-69
U-69
U-70
U-70
U-71
U-71
U-71
U-73
U-73
U-74

U-13

Contents

3.3
3.4

3.5
3.6
3.7

3.2.2.3 Source files to be compiled . . . . . . . . . . . .
3.2.2.4 Running wmake . . . . . . . . . . . . . . . . . .
3.2.2.5 wmake environment variables . . . . . . . . . .
3.2.3 Removing dependency lists: wclean and rmdepall . . . . .
3.2.4 Compilation example: the pisoFoam application . . . . .
3.2.5 Debug messaging and optimisation switches . . . . . . .
3.2.6 Linking new user-defined libraries to existing applications
Running applications . . . . . . . . . . . . . . . . . . . . . . . .
Running applications in parallel . . . . . . . . . . . . . . . . . .
3.4.1 Decomposition of mesh and initial field data . . . . . . .
3.4.2 Running a decomposed case . . . . . . . . . . . . . . . .
3.4.3 Distributing data across several disks . . . . . . . . . . .
3.4.4 Post-processing parallel processed cases . . . . . . . . . .
3.4.4.1 Reconstructing mesh and data . . . . . . . . .
3.4.4.2 Post-processing decomposed cases . . . . . . . .
Standard solvers . . . . . . . . . . . . . . . . . . . . . . . . . . .
Standard utilities . . . . . . . . . . . . . . . . . . . . . . . . . .
Standard libraries . . . . . . . . . . . . . . . . . . . . . . . . . .

4 OpenFOAM cases
4.1 File structure of OpenFOAM cases . . . . . . . . . . . . .
4.2 Basic input/output file format . . . . . . . . . . . . . . . .
4.2.1 General syntax rules . . . . . . . . . . . . . . . . .
4.2.2 Dictionaries . . . . . . . . . . . . . . . . . . . . . .
4.2.3 The data file header . . . . . . . . . . . . . . . . .
4.2.4 Lists . . . . . . . . . . . . . . . . . . . . . . . . . .
4.2.5 Scalars, vectors and tensors . . . . . . . . . . . . .
4.2.6 Dimensional units . . . . . . . . . . . . . . . . . . .
4.2.7 Dimensioned types . . . . . . . . . . . . . . . . . .
4.2.8 Fields . . . . . . . . . . . . . . . . . . . . . . . . .
4.2.9 Directives and macro substitutions . . . . . . . . .
4.3 Time and data input/output control . . . . . . . . . . . .
4.4 Numerical schemes . . . . . . . . . . . . . . . . . . . . . .
4.4.1 Interpolation schemes . . . . . . . . . . . . . . . . .
4.4.1.1 Schemes for strictly bounded scalar fields
4.4.1.2 Schemes for vector fields . . . . . . . . . .
4.4.2 Surface normal gradient schemes . . . . . . . . . .
4.4.3 Gradient schemes . . . . . . . . . . . . . . . . . . .
4.4.4 Laplacian schemes . . . . . . . . . . . . . . . . . .
4.4.5 Divergence schemes . . . . . . . . . . . . . . . . . .
4.4.6 Time schemes . . . . . . . . . . . . . . . . . . . . .
4.4.7 Flux calculation . . . . . . . . . . . . . . . . . . . .
4.5 Solution and algorithm control . . . . . . . . . . . . . . . .
4.5.1 Linear solver control . . . . . . . . . . . . . . . . .
4.5.1.1 Solution tolerances . . . . . . . . . . . . .
4.5.1.2 Preconditioned conjugate gradient solvers
4.5.1.3 Smooth solvers . . . . . . . . . . . . . . .
4.5.1.4 Geometric-algebraic multi-grid solvers . .
4.5.2 Solution under-relaxation . . . . . . . . . . . . . .
4.5.3 PISO and SIMPLE algorithms . . . . . . . . . . . .
4.5.3.1 Pressure referencing . . . . . . . . . . . .

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

U-74
U-75
U-75
U-75
U-76
U-79
U-80
U-80
U-81
U-81
U-83
U-84
U-85
U-85
U-85
U-85
U-88
U-94

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

U-101
U-101
U-102
U-102
U-102
U-103
U-104
U-105
U-105
U-106
U-106
U-107
U-108
U-110
U-112
U-113
U-113
U-114
U-114
U-115
U-115
U-116
U-117
U-117
U-117
U-118
U-119
U-119
U-119
U-120
U-121
U-121

Open∇FOAM-1.6

U-14

Contents

4.5.4

Other parameters . . . . . . . . . . . . . . . . . . . . . . . .

5 Mesh generation and conversion
5.1 Mesh description . . . . . . . . . . . . . . . . . . . . . . . .
5.1.1 Mesh specification and validity constraints . . . . . .
5.1.1.1 Points . . . . . . . . . . . . . . . . . . . . .
5.1.1.2 Faces . . . . . . . . . . . . . . . . . . . . .
5.1.1.3 Cells . . . . . . . . . . . . . . . . . . . . . .
5.1.1.4 Boundary . . . . . . . . . . . . . . . . . . .
5.1.2 The polyMesh description . . . . . . . . . . . . . . . .
5.1.3 The cellShape tools . . . . . . . . . . . . . . . . . . .
5.1.4 1- and 2-dimensional and axi-symmetric problems . .
5.2 Boundaries . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.2.1 Specification of patch types in OpenFOAM . . . . . .
5.2.2 Base types . . . . . . . . . . . . . . . . . . . . . . . .
5.2.3 Primitive types . . . . . . . . . . . . . . . . . . . . .
5.2.4 Derived types . . . . . . . . . . . . . . . . . . . . . .
5.3 Mesh generation with the blockMesh utility . . . . . . . . . .
5.3.1 Writing a blockMeshDict file . . . . . . . . . . . . . .
5.3.1.1 The vertices . . . . . . . . . . . . . . . .
5.3.1.2 The edges . . . . . . . . . . . . . . . . . .
5.3.1.3 The blocks . . . . . . . . . . . . . . . . . .
5.3.1.4 The patches . . . . . . . . . . . . . . . . .
5.3.2 Multiple blocks . . . . . . . . . . . . . . . . . . . . .
5.3.3 Creating blocks with fewer than 8 vertices . . . . . .
5.3.4 Running blockMesh . . . . . . . . . . . . . . . . . . .
5.4 Mesh generation with the snappyHexMesh utility . . . . . . .
5.4.1 The mesh generation process of snappyHexMesh . . .
5.4.2 Creating the background hex mesh . . . . . . . . . .
5.4.3 Cell splitting at feature edges and surfaces . . . . . .
5.4.4 Cell removal . . . . . . . . . . . . . . . . . . . . . . .
5.4.5 Cell splitting in specified regions . . . . . . . . . . . .
5.4.6 Snapping to surfaces . . . . . . . . . . . . . . . . . .
5.4.7 Mesh layers . . . . . . . . . . . . . . . . . . . . . . .
5.4.8 Mesh quality controls . . . . . . . . . . . . . . . . . .
5.5 Mesh conversion . . . . . . . . . . . . . . . . . . . . . . . . .
5.5.1 fluentMeshToFoam . . . . . . . . . . . . . . . . . . .
5.5.2 starToFoam . . . . . . . . . . . . . . . . . . . . . . .
5.5.2.1 General advice on conversion . . . . . . . .
5.5.2.2 Eliminating extraneous data . . . . . . . . .
5.5.2.3 Removing default boundary conditions . . .
5.5.2.4 Renumbering the model . . . . . . . . . . .
5.5.2.5 Writing out the mesh data . . . . . . . . . .
5.5.2.6 Problems with the .vrt file . . . . . . . . . .
5.5.2.7 Converting the mesh to OpenFOAM format
5.5.3 gambitToFoam . . . . . . . . . . . . . . . . . . . . . .
5.5.4 ideasToFoam . . . . . . . . . . . . . . . . . . . . . . .
5.5.5 cfx4ToFoam . . . . . . . . . . . . . . . . . . . . . . .
5.6 Mapping fields between different geometries . . . . . . . . .
5.6.1 Mapping consistent fields . . . . . . . . . . . . . . . .
5.6.2 Mapping inconsistent fields . . . . . . . . . . . . . . .
Open∇FOAM-1.6

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

U-122
U-123
U-123
U-123
U-124
U-124
U-124
U-125
U-125
U-126
U-126
U-128
U-128
U-130
U-132
U-132
U-132
U-134
U-135
U-135
U-136
U-137
U-138
U-139
U-140
U-140
U-141
U-142
U-143
U-144
U-145
U-146
U-146
U-148
U-148
U-149
U-150
U-151
U-151
U-152
U-152
U-153
U-154
U-154
U-154
U-155
U-155
U-155
U-156
U-156

U-15

Contents

5.6.3

Mapping parallel cases . . . . . . . . . . . . . . . . . . . . .

U-156

6 Post-processing
6.1 paraFoam . . . . . . . . . . . . . . . . . . . . .
6.1.1 Overview of paraFoam . . . . . . . . . .
6.1.2 The Properties panel . . . . . . . . . . .
6.1.3 The Display panel . . . . . . . . . . . . .
6.1.4 The button toolbars . . . . . . . . . . .
6.1.5 Manipulating the view . . . . . . . . . .
6.1.5.1 View settings . . . . . . . . . .
6.1.5.2 General settings . . . . . . . .
6.1.6 Contour plots . . . . . . . . . . . . . . .
6.1.6.1 Introducing a cutting plane . .
6.1.7 Vector plots . . . . . . . . . . . . . . . .
6.1.7.1 Plotting at cell centres . . . . .
6.1.8 Streamlines . . . . . . . . . . . . . . . .
6.1.9 Image output . . . . . . . . . . . . . . .
6.1.10 Animation output . . . . . . . . . . . . .
6.2 Post-processing with Fluent . . . . . . . . . . .
6.3 Post-processing with Fieldview . . . . . . . . . .
6.4 Post-processing with EnSight . . . . . . . . . . .
6.4.1 Converting data to EnSight format . . .
6.4.2 The ensight74FoamExec reader module .
6.4.2.1 Configuration of EnSight for the
6.4.2.2 Using the reader module . . . .
6.5 Sampling data . . . . . . . . . . . . . . . . . . .
6.6 Monitoring and managing jobs . . . . . . . . . .
6.6.1 The foamJob script for running jobs . . .
6.6.2 The foamLog script for monitoring jobs .

. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
. . . .
reader
. . . .
. . . .
. . . .
. . . .
. . . .

. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .
module
. . . . .
. . . . .
. . . . .
. . . . .
. . . . .

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

U-159
U-159
U-159
U-160
U-161
U-163
U-163
U-163
U-163
U-164
U-164
U-164
U-164
U-164
U-165
U-165
U-166
U-167
U-167
U-168
U-168
U-168
U-168
U-169
U-172
U-173
U-173

7 Models and physical properties
7.1 Thermophysical models . . . . .
7.1.1 Thermophysical property
7.2 Turbulence models . . . . . . .
7.2.1 Model coefficients . . . .
7.2.2 Wall functions . . . . . .

.
.
.
.
.

U-175
U-175
U-177
U-178
U-179
U-179

Index

. . .
data
. . .
. . .
. . .

.
.
.
.
.

U-181

Open∇FOAM-1.6

U-16

Open∇FOAM-1.6

Contents

Chapter 1
Introduction
This guide accompanies the release of version 1.6 of the Open Source Field Operation
and Manipulation (OpenFOAM) C++ libraries. It provides a description of the basic
operation of OpenFOAM, first through a set of tutorial exercises in chapter 2 and later
by a more detailed description of the individual components that make up OpenFOAM.
OpenFOAM is first and foremost a C++ library, used primarily to create executables, known as applications. The applications fall into two categories: solvers, that are
each designed to solve a specific problem in continuum mechanics; and utilities, that are
designed to perform tasks that involve data manipulation. The OpenFOAM distribution
contains numerous solvers and utilities covering a wide range of problems, as described
in chapter 3.
One of the strengths of OpenFOAM is that new solvers and utilities can be created
by its users with some pre-requisite knowledge of the underlying method, physics and
programming techniques involved.
OpenFOAM is supplied with pre- and post-processing environments. The interface
to the pre- and post-processing are themselves OpenFOAM utilities, thereby ensuring
consistent data handling across all environments. The overall structure of OpenFOAM is
shown in Figure 1.1. The pre-processing and running of OpenFOAM cases is described
Open Source Field Operation and Manipulation (OpenFOAM) C++ Library

Pre-processing

Utilities

Meshing
Tools

Solving

User
Standard
Applications Applications

Post-processing

ParaView

Others
e.g.EnSight

Figure 1.1: Overview of OpenFOAM structure.
in chapter 4 In chapter 5, we cover both the generation of meshes using the mesh generator supplied with OpenFOAM and conversion of mesh data generated by third-party
products. Post-processing is described in chapter 6.

U-18

Open∇FOAM-1.6

Introduction

Chapter 2
Tutorials
In this chapter we shall describe in detail the process of setup, simulation and postprocessing for some OpenFOAM test cases, with the principal aim of introducing a user to
the basic procedures of running OpenFOAM. The $FOAM TUTORIALS directory contains
many more cases that demonstrate the use of all the solvers and many utilities supplied
with OpenFOAM. Before attempting to run the tutorials, the user must first make sure
that they have installed OpenFOAM correctly.
The tutorial cases describe the use of the blockMesh pre-processing tool, case setup
and running OpenFOAM solvers and post-processing using paraFoam. Those users with
access to third-party post-processing tools supported in OpenFOAM have an option:
either they can follow the tutorials using paraFoam; or refer to the description of the use
of the third-party product in chapter 6 when post-processing is required.
Copies of all tutorials are available from the tutorials directory of the OpenFOAM
installation. The tutorials are organised into a set of directories according to the type
of flow and then subdirectories according to solver. For example, all the icoFoam cases
are stored within a subdirectory incompressible/icoFoam, where incompressible indicates
the type of flow. If the user wishes to run a range of example cases, it is recommended
that the user copy the tutorials directory into their local run directory. They can be easily
copied by typing:

mkdir -p $FOAM RUN
cp -r $FOAM TUTORIALS $FOAM RUN

2.1

Lid-driven cavity flow

This tutorial will describe how to pre-process, run and post-process a case involving
isothermal, incompressible flow in a two-dimensional square domain. The geometry is
shown in Figure 2.1 in which all the boundaries of the square are walls. The top wall
moves in the x-direction at a speed of 1 m/s while the other 3 are stationary. Initially,
the flow will be assumed laminar and will be solved on a uniform mesh using the icoFoam
solver for laminar, isothermal, incompressible flow. During the course of the tutorial, the
effect of increased mesh resolution and mesh grading towards the walls will be investigated.
Finally, the flow Reynolds number will be increased and the pisoFoam solver will be used
for turbulent, isothermal, incompressible flow.

U-20

Tutorials

Ux = 1 m/s

d = 0.1 m
y
x
Figure 2.1: Geometry of the lid driven cavity.

2.1.1

Pre-processing

Cases are setup in OpenFOAM by editing case files. Users should select an xeditor of
choice with which to do this, such as emacs, vi, gedit, kate, nedit, etc. Editing files is
possible in OpenFOAM because the I/O uses a dictionary format with keywords that
convey sufficient meaning to be understood by even the least experienced users.
A case being simulated involves data for mesh, fields, properties, control parameters,
etc. As described in section 4.1, in OpenFOAM this data is stored in a set of files within
a case directory rather than in a single case file, as in many other CFD packages. The
case directory is given a suitably descriptive name, e.g. the first example case for this
tutorial is simply named cavity. In preparation of editing case files and running the first
cavity case, the user should change to the case directory
cd $FOAM RUN/tutorials/incompressible/icoFoam/cavity
2.1.1.1

Mesh generation

OpenFOAM always operates in a 3 dimensional Cartesian coordinate system and all
geometries are generated in 3 dimensions. OpenFOAM solves the case in 3 dimensions
by default but can be instructed to solve in 2 dimensions by specifying a ‘special’ empty
boundary condition on boundaries normal to the (3rd) dimension for which no solution
is required.
The cavity domain consists of a square of side length d = 0.1 m in the x-y plane. A
uniform mesh of 20 by 20 cells will be used initially. The block structure is shown in
Figure 2.2. The mesh generator supplied with OpenFOAM, blockMesh, generates meshes
from a description specified in an input dictionary, blockMeshDict located in the constant/polyMesh directory for a given case. The blockMeshDict entries for this case are as
follows:
1
2
3
4
5
6
7
8
9
10

Open∇FOAM-1.6

U-21

2.1 Lid-driven cavity flow

2
7

y
0

x
z

1
5

Figure 2.2: Block structure of the mesh for the cavity.
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63

format
class
object

ascii;
dictionary;
blockMeshDict;

}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 0.1;
vertices
(
(0 0
(1 0
(1 1
(0 1
(0 0
(1 0
(1 1
(0 1
);

0)
0)
0)
0)
0.1)
0.1)
0.1)
0.1)

blocks
(
hex (0 1 2 3 4 5 6 7) (20 20 1) simpleGrading (1 1 1)
);
edges
(
);
patches
(
wall movingWall
(
(3 7 6 2)
)
wall fixedWalls
(
(0 4 7 3)
(2 6 5 1)
(1 5 4 0)
)
empty frontAndBack
(
(0 3 2 1)
(4 5 6 7)
)
);
mergePatchPairs
(
);
// ************************************************************************* //

The file first contains header information in the form of a banner (lines 1-7), then file
information contained in a FoamFile sub-dictionary, delimited by curly braces ({...}).
Open∇FOAM-1.6

U-22

Tutorials

For the remainder of the manual:
For the sake of clarity and to save space, file headers, including the banner and
FoamFile sub-dictionary, will be removed from verbatim quoting of case files
The file first specifies coordinates of the block vertices; it then defines the blocks
(here, only 1) from the vertex labels and the number of cells within it; and finally, it defines
the boundary patches. The user is encouraged to consult section 5.3 to understand the
meaning of the entries in the blockMeshDict file.
The mesh is generated by running blockMesh on this blockMeshDict file. From within
the case directory, this is done, simply by typing in the terminal:
blockMesh
The running status of blockMesh is reported in the terminal window. Any mistakes in
the blockMeshDict file are picked up by blockMesh and the resulting error message directs
the user to the line in the file where the problem occurred. There should be no error
messages at this stage.
2.1.1.2

Boundary and initial conditions

Once the mesh generation is complete, the user can look at this initial fields set up for
this case. The case is set up to start at time t = 0 s, so the initial field data is stored in
a 0 sub-directory of the cavity directory. The 0 sub-directory contains 2 files, p and U,
one for each of the pressure (p) and velocity (U) fields whose initial values and boundary
conditions must be set. Let us examine file p:
17
18
19
20
21
22
23
24
25
26
27
28
29
30

dimensions

[0 2 -2 0 0 0 0];

internalField

uniform 0;

boundaryField
{
movingWall
{
type
}

31
32
33
34
35
36
37
38
39

}

zeroGradient;

fixedWalls
{
type
}

zeroGradient;

frontAndBack
{
type
}

empty;

// ************************************************************************* //

There are 3 principal entries in field data files:
dimensions specifies the dimensions of the field, here kinematic pressure, i.e. m2 s−2 (see
section 4.2.6 for more information);
internalField the internal field data which can be uniform, described by a single value;
or nonuniform, where all the values of the field must be specified (see section 4.2.8
for more information);
boundaryField the boundary field data that includes boundary conditions and data for
all the boundary patches (see section 4.2.8 for more information).
Open∇FOAM-1.6

2.1 Lid-driven cavity flow

U-23

For this case cavity, the boundary consists of walls only, split into 2 patches named: (1)
fixedWalls for the fixed sides and base of the cavity; (2) movingWall for the moving top
of the cavity. As walls, both are given a zeroGradient boundary condition for p, meaning
“the normal gradient of pressure is zero”. The frontAndBack patch represents the front
and back planes of the 2D case and therefore must be set as empty.
In this case, as in most we encounter, the initial fields are set to be uniform. Here the
pressure is kinematic, and as an incompressible case, its absolute value is not relevant, so
is set to uniform 0 for convenience.
The user can similarly examine the velocity field in the 0/U file. The dimensions are
those expected for velocity, the internal field is initialised as uniform zero, which in the
case of velocity must be expressed by 3 vector components, i.e.uniform (0 0 0) (see
section 4.2.5 for more information).
The boundary field for velocity requires the same boundary condition for the frontAndBack patch. The other patches are walls: a no-slip condition is assumed on the
fixedWalls, hence a fixedValue condition with a value of uniform (0 0 0). The top
surface moves at a speed of 1 m/s in the x-direction so requires a fixedValue condition
also but with uniform (1 0 0).
2.1.1.3

Physical properties

The physical properties for the case are stored in dictionaries whose names are given the
suffix . . . Properties, located in the Dictionaries directory tree. For an icoFoam case,
the only property that must be specified is the kinematic viscosity which is stored from
the transportProperties dictionary. The user can check that the kinematic viscosity is
set correctly by opening the transportProperties dictionary to view/edit its entries. The
keyword for kinematic viscosity is nu, the phonetic label for the Greek symbol ν by which
it is represented in equations. Initially this case will be run with a Reynolds number of
10, where the Reynolds number is defined as:
Re =

d|U|
ν

(2.1)

where d and |U| are the characteristic length and velocity respectively and ν is the
kinematic viscosity. Here d = 0.1 m, |U| = 1 m s−1 , so that for Re = 10, ν = 0.01 m2 s−1 .
The correct file entry for kinematic viscosity is thus specified below:
17
18
19
20
21

nu [ 0 2 -1 0 0 0 0 ] 0.01;

// ************************************************************************* //

2.1.1.4

Control

Input data relating to the control of time and reading and writing of the solution data are
read in from the controlDict dictionary. The user should view this file; as a case control
file, it is located in the system directory.
The start/stop times and the time step for the run must be set. OpenFOAM offers
great flexibility with time control which is described in full in section 4.3. In this tutorial
we wish to start the run at time t = 0 which means that OpenFOAM needs to read field
data from a directory named 0 — see section 4.1 for more information of the case file
structure. Therefore we set the startFrom keyword to startTime and then specify the
startTime keyword to be 0.
For the end time, we wish to reach the steady state solution where the flow is circulating around the cavity. As a general rule, the fluid should pass through the domain 10
Open∇FOAM-1.6

U-24

Tutorials

times to reach steady state in laminar flow. In this case the flow does not pass through
this domain as there is no inlet or outlet, so instead the end time can be set to the time
taken for the lid to travel ten times across the cavity, i.e. 1 s; in fact, with hindsight, we
discover that 0.5 s is sufficient so we shall adopt this value. To specify this end time, we
must specify the stopAt keyword as endTime and then set the endTime keyword to 0.5.
Now we need to set the time step, represented by the keyword deltaT. To achieve
temporal accuracy and numerical stability when running icoFoam, a Courant number of
less than 1 is required. The Courant number is defined for one cell as:
δt|U|
δx

Co =

(2.2)

where δt is the time step, |U| is the magnitude of the velocity through that cell and δx
is the cell size in the direction of the velocity. The flow velocity varies across the domain
and we must ensure Co < 1 everywhere. We therefore choose δt based on the worst case:
the maximum Co corresponding to the combined effect of a large flow velocity and small
cell size. Here, the cell size is fixed across the domain so the maximum Co will occur next
to the lid where the velocity approaches 1 m s−1 . The cell size is:
δx =

0.1
d
=
= 0.005 m
n
20

(2.3)

Therefore to achieve a Courant number less than or equal to 1 throughout the domain
the time step deltaT must be set to less than or equal to:
δt =

Co δx
1 × 0.005
=
= 0.005 s
|U|
1

(2.4)

As the simulation progresses we wish to write results at certain intervals of time that
we can later view with a post-processing package. The writeControl keyword presents
several options for setting the time at which the results are written; here we select the
timeStep option which specifies that results are written every nth time step where the
value n is specified under the writeInterval keyword. Let us decide that we wish to
write our results at times 0.1, 0.2,. . . , 0.5 s. With a time step of 0.005 s, we therefore
need to output results at every 20th time time step and so we set writeInterval to 20.
OpenFOAM creates a new directory named after the current time, e.g. 0.1 s, on each
occasion that it writes a set of data, as discussed in full in section 4.1. In the icoFoam
solver, it writes out the results for each field, U and p, into the time directories. For this
case, the entries in the controlDict are shown below:
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39

application

icoFoam;

startFrom

startTime;

startTime

stopAt

endTime;

endTime

0.5;

deltaT

0.005;

writeControl

timeStep;

writeInterval

20;

purgeWrite

writeFormat

ascii;

writePrecision

Open∇FOAM-1.6

U-25

2.1 Lid-driven cavity flow
40
41
42
43
44
45
46
47
48
49

writeCompression uncompressed;
timeFormat

general;

timePrecision

runTimeModifiable yes;
// ************************************************************************* //

2.1.1.5

Discretisation and linear-solver settings

The user specifies the choice of finite volume discretisation schemes in the fvSchemes
dictionary in the system directory. The specification of the linear equation solvers and
tolerances and other algorithm controls is made in the fvSolution dictionary, similarly in
the system directory. The user is free to view these dictionaries but we do not need to
discuss all their entries at this stage except for pRefCell and pRefValue in the PISO
sub-dictionary of the fvSolution dictionary. In a closed incompressible system such as the
cavity, pressure is relative: it is the pressure range that matters not the absolute values.
In cases such as this, the solver sets a reference level by pRefValue in cell pRefCell. In
this example both are set to 0. Changing either of these values will change the absolute
pressure field, but not, of course, the relative pressures or velocity field.

2.1.2

Viewing the mesh

Before the case is run it is a good idea to view the mesh to check for any errors. The mesh
is viewed in paraFoam, the post-processing tool supplied with OpenFOAM. The paraFoam
post-processing is started by typing in the terminal from within the case directory
paraFoam
Alternatively, it can be launched from another directory location with an optional
-case argument giving the case directory, e.g.
paraFoam -case $FOAM RUN/tutorials/incompressible/icoFoam/cavity
This launches the ParaView window as shown in Figure 6.1. In the Pipeline Browser,
the user can see that ParaView has opened cavity.OpenFOAM, the module for the cavity
case. Before clicking the Apply button, the user needs to select some geometry from
the Region Status and panel. Because the case is small, it is easiest to select all the data
by checking the box adjacent to the Region Status panel title, which automatically checks
all individual components within the respective panel. The user should then click the
Apply button to load the geometry into ParaView.
some general settings are applied as described in section 6.1.5.1. Please consult this
section about these settings.
The user should then open the Display panel that controls the visual representation of
the selected module. Within the Display panel the user should do the following as shown
in Figure 2.3: (1) set Color by Solid Color; (2) click Set Solid Color and select an appropriate colour e.g. black (for a white background); (3) in the Style panel, select Wireframe
from the Representation menu. The background colour can be set by selecting View
Settings... from Edit in the top menu panel.
Especially the first time the user starts ParaView, it is recommended that they
manipulate the view as described in section 6.1.5. In particular, since this is a 2D case,
it is recommended that Use Parallel Projection is selected in the General panel of View
Open∇FOAM-1.6

U-26

Tutorials

Open Display panel
Select Color by Solid Color
Set Solid Color, e.g. black
Select Wireframe

Figure 2.3: Viewing the mesh in paraFoam.
Settings window selected from the Edit menu. The Orientation Axes can be toggled on
and off in the Annotation window or moved by drag and drop with the mouse.

2.1.3

Running an application

Like any UNIX/Linux executable, OpenFOAM applications can be run in two ways: as
a foreground process, i.e. one in which the shell waits until the command has finished
before giving a command prompt; as a background process, one which does not have to
be completed before the shell accepts additional commands.
On this occasion, we will run icoFoam in the foreground. The icoFoam solver is executed either by entering the case director034(h)-0.310405(e)-6.37 amwie

U-27

2.1 Lid-driven cavity flow

Open Display panel
Select Color by interpolated p
Rescale to Data Range
Select Surface

Figure 2.4: Displaying pressure contours for the cavity case.

Figure 2.5: Pressures in the cavity case.

Open∇FOAM-1.6

U-28

2.1.4

Tutorials

Post-processing

As soon as results are written to time directories, they can be viewed using paraFoam.
Return to the paraFoam window and select the Properties panel for the cavity.OpenFOAM
case module. If the correct window panels for the case module do not seem to be present
at any time, please ensure that: cavity.OpenFOAM is highlighted in blue; eye button
alongside it is switched on to show the graphics are enabled;
To prepare paraFoam to display the data of interest, we must first load the data at
the required run time of 0.5 s. If the case was run while ParaView was open, the output
data in time directories will not be automatically loaded within ParaView. To load the
data the user should select Update GUI in the Properties window and then click the green
Apply button. The time data will be loaded into ParaView.

2.1.4.1

Isosurface and contour plots

To view pressure, the user should open the Display panel since it that controls the visual
representation of the selected module. To make a simple plot of pressure, the user should
select the following, as described in detail in Figure 2.4: in the Style panel, select Surface
from the Representation menu; in the Color panel, select Color by
and Rescale to
Data Range. Now in order to view the solution at t = 0.5 s, the user can use the VCR
Controls or Current Time Controls to change the current time to 0.5. These are
located in the toolbars below the menus at the top of the ParaView window, as shown in
Figure 6.4. The pressure field solution has, as expected, a region of low pressure at the
top left of the cavity and one of high pressure at the top right of the cavity as shown in
Figure 2.5.
With the point icon ( ) the pressure field is interpolated across each cell to give a
continuous appearance. Instead if the user selects the cell icon,
, from the Color by
menu, a single value for pressure will be attributed to each cell so that each cell will be
denoted by a single colour with no grading.
A colour bar can be included by either by clicking the Toggle Color Legend Visibility
button in the Active Variable Controls toolbar, or by selecting Show Color Legend
from the View menu. Clicking the Edit Color Map button, either in the Active Variable
Controls toolbar or in the Color panel of the Display window, the user can set a range
of attributes of the colour bar, such as text size, font selection and numbering format for
the scale. The colour bar can be located in the image window by drag and drop with the
mouse.
New versions of ParaView default to using a colour scale of blue to white to red rather
than the more common blue to green to red (rainbow). Therefore the first time that the
user executes ParaView, they may wish to change the colour scale. This can be done by
selecting Choose Preset in the Color Scale Editor and selecting Blue to Red Rainbow. After
clicking the OK confirmation button, the user can click the Make Default button so that
ParaView will always adopt this type of colour bar.
If the user rotates the image, they can see that they have now coloured the complete
geometry surface by the pressure. In order to produce a genuine contour plot the user
should first create a cutting plane, or ‘slice’, through the geometry using the Slice filter
as described in section 6.1.6.1. The cutting plane should be centred at (0.05, 0.05, 0.005)
and its normal should be set to (0, 0, 1). Having generated the cutting plane, the contours
can be created using by the Contour filter described in section 6.1.6.
Open∇FOAM-1.6

U-29

2.1 Lid-driven cavity flow

Open Parameters panel
Specify Set Scale Factor 0.005
Select Scale Mode off
Select Glyph Type Arrow

Figure 2.6: Properties panel for the Glyph filter.

Figure 2.7: Velocities in the cavity case.

Open∇FOAM-1.6

U-30
2.1.4.2

Tutorials

Vector plots

Before we start to plot the vectors of the flow velocity, it may be useful to remove other
modules that have been created, e.g. using the Slice and Contour filters described above.
These can: either be deleted entirely, by highlighting the relevant module in the Pipeline
Browser and clicking Delete in their respective Properties panel; or, be disabled by toggling
the eye button for the relevant module in the Pipeline Browser.
We now wish to generate a vector glyph for velocity at the centre of each cell. We
first need to filter the data to cell centres as described in section 6.1.7.1. With the
cavity.OpenFOAM module highlighted in the Pipeline Browser, the user should select Cell
Centers from the Filter menu and then click Apply.
With these Centers highlighted in the Pipeline Browser, the user should then select
Glyph from the Filter menu. The Properties window panel should appear as shown in
Figure 2.6. In the resulting Properties panel, the velocity field, U, is automatically selected
in the vectors menu, since it is the only vector field present. By default the Scale Mode
for the glyphs will be Vector Magnitude of velocity but, since the we may wish to view
the velocities throughout the domain, the user should instead select off and Set Scale
Factor to 0.005. On clicking Apply, the glyphs appear but, probably as a single colour,
e.g. white. The user should colour the glyphs by velocity magnitude which, as usual, is
controlled by setting Color by U in the Display panel. The user should also select Show
Color Legend in Edit Color Map. The output is shown in Figure 2.7, in which uppercase
Times Roman fonts are selected for the Color Legend headings and the labels are specified
to 2 fixed significant figures by deselecting Automatic Label Format and entering %-#6.2f
in the Label Format text box. The background colour is set to white in the General panel
of View Settings as described in section 6.1.5.1.
2.1.4.3

Streamline plots

Again, before the user continues to post-process in ParaView, they should disable modules
such as those for the vector plot described above. We now wish to plot a streamlines of
velocity as described in section 6.1.8.
With the cavity.OpenFOAM module highlighted in the Pipeline Browser, the user
should then select Stream Tracer from the Filter menu and then click Apply. The
Properties window panel should appear as shown in Figure 2.8. The Seed points should
be specified along a Line Source running vertically through the centre of the geometry,
i.e. from (0.05, 0, 0.005) to (0.05, 0.1, 0.005). For the image in this guide we used: a point
Resolution of 21; Max Propagation by Length 0.5; Initial Step Length by Cell Length 0.01;
and, Integration Direction BOTH. The Runge-Kutta 2 IntegratorType was used with
default parameters.
On clicking Apply the tracer is generated. The user should then select Tube from the
Filter menu to produce high quality streamline images. For the image in this report, we
used: Num. sides 6; Radius 0.0003; and, Radius factor 10. The streamtubes are coloured
by velocity magnitude. On clicking Apply the image in Figure 2.9 should be produced.

2.1.5

Increasing the mesh resolution

The mesh resolution will now be increased by a factor of two in each direction. The results
from the coarser mesh will be mapped onto the finer mesh to use as initial conditions for
the problem. The solution from the finer mesh will then be compared with those from
the coarser mesh.
Open∇FOAM-1.6

U-31

2.1 Lid-driven cavity flow

Open Parameters panel
Set Max Propagation to Length 0.5
Set Initial Step Length to Cell Length 0.01
Set Integration Direction to BOTH
Specify Line Source and set points and resolution

Figure 2.8: Properties panel for the Stream Tracer filter.

Figure 2.9: Streamlines in the cavity case.

Open∇FOAM-1.6

U-32
2.1.5.1

Tutorials

Creating a new case using an existing case

We now wish to create a new case named cavityFine that is created from cavity. The user
should therefore clone the cavity case and edit the necessary files. First the user should
create a new case directory at the same directory level as the cavity case, e.g.
cd $FOAM RUN/tutorials/incompressible/icoFoam
mkdir cavityFine
The user should then copy the base directories from the cavity case into cavityFine, and
then enter the cavityFine case.
cp -r cavity/constant cavityFine
cp -r cavity/system cavityFine
cd cavityFine
2.1.5.2

Creating the finer mesh

We now wish to increase the number of cells in the mesh by using blockMesh. The user
should open the blockMeshDict file in an editor and edit the block specification. The blocks
are specified in a list under the blocks keyword. The syntax of the block definitions is
described fully in section 5.3.1.3; at this stage it is sufficient to know that following hex
is first the list of vertices in the block, then a list (or vector) of numbers of cells in each
direction. This was originally set to (20 20 1) for the cavity case. The user should now
change this to (40 40 1) and save the file. The new refined mesh should then be created
by running blockMesh as before.
2.1.5.3

Mapping the coarse mesh results onto the fine mesh

The mapFields utility maps one or more fields relating to a given geometry onto the corresponding fields for another geometry. In our example, the fields are deemed ‘consistent’
because the geometry and the boundary types, or conditions, of both source and target fields are identical. We use the -consistent command line option when executing
mapFields in this example.
The field data that mapFields maps is read from the time directory specified by
startFrom/startTime in the controlDict of the target case, i.e. those into which the
results are being mapped. In this example, we wish to map the final results of the coarser
mesh from case cavity onto the finer mesh of case cavityFine. Therefore, since these results are stored in the 0.5 directory of cavity, the startTime should be set to 0.5 s in the
controlDict dictionary and startFrom should be set to startTime.
The case is ready to run mapFields. Typing mapFields -help quickly shows that mapFields requires the source case directory as an argument. We are using the -consistent
option, so the utility is executed from withing the cavityFine directory by
mapFields ../cavity -consistent
The utility should run with output to the terminal including:
Source: ".." "cavity"
Target: "." "cavityFine"
Create databases as time
Source time: 0.5

Open∇FOAM-1.6

U-33

2.1 Lid-driven cavity flow
Target time: 0.5
Create meshes
Source mesh size: 400

Target mesh size: 1681

Consistently creating and mapping fields for time 0.5
interpolating p
interpolating U
End

2.1.5.4

Control adjustments

To maintain a Courant number of less that 1, as discussed in section 2.1.1.4, the time
step must now be halved since the size of all cells has halved. Therefore deltaT should
be set to to 0.0025 s in the controlDict dictionary. Field data is currently written out at
an interval of a fixed number of time steps. Here we demonstrate how to specify data
output at fixed intervals of time. Under the writeControl keyword in controlDict, instead
of requesting output by a fixed number of time steps with the timeStep entry, a fixed
amount of run time can be specified between the writing of results using the runTime
entry. In this case the user should specify output every 0.1 and therefore should set
writeInterval to 0.1 and writeControl to runTime. Finally, since the case is starting
with a the solution obtained on the coarse mesh we only need to run it for a short period
to achieve reasonable convergence to steady-state. Therefore the endTime should be set
to 0.7 s. Make sure these settings are correct and then save the file.
2.1.5.5

Running the code as a background process

The user should experience running icoFoam as a background process, redirecting the
terminal output to a log file that can be viewed later. From the cavityFine directory, the
user should execute:
icoFoam > log &
cat log
2.1.5.6

Vector plot with the refined mesh

The user can open multiple cases simultaneously in ParaView; essentially because each new
case is simply another module that appears in the Pipeline Browser. There is one minor
inconvenience when opening a new case in ParaView because there is a prerequisite that
the selected data is a file with a name that has an extension. However, in OpenFOAM,
each case is stored in a multitude of files with no extensions within a specific directory
structure. The solution, that the paraFoam script performs automatically, is to create
a dummy file with the extension .OpenFOAM — hence, the cavity case module is called
cavity.OpenFOAM.
However, if the user wishes to open another case directly from within ParaView, they
need to create such a dummy file. For example, to load the cavityFine case the file would
be created by typing at the command prompt:
cd $FOAM RUN/tutorials/incompressible/icoFoam
touch cavityFine/cavityFine.OpenFOAM
Now the cavityFine case can be loaded into ParaView by selecting Open from the File
menu, and having navigated the directory tree, selecting cavityFine.OpenFOAM. The user
Open∇FOAM-1.6

U-34

Tutorials

Open Display panel
Select Ux from Line Series
Select arc length
Select Scatter Plot

Figure 2.10: Selecting fields for graph plotting.
can now make a vector plot of the results from the refined mesh in ParaView. The plot can
be compared with the cavity case by enabling glyph images for both case simultaneously.
2.1.5.7

Plotting graphs

The user may wish to visualise the results by extracting some scalar measure of velocity
and plotting 2-dimensional graphs along lines through the domain. OpenFOAM is well
equipped for this kind of data manipulation. There are numerous utilities that do specialised data manipulations, and some, simpler calculations are incorporated into a single
utility foamCalc. As a utility, it is unique in that it is executed by
foamCalc
The calculator operation is specified in ; at the time of writing, the following
operations are implemented: addSubtract; randomise; div; components; mag; magGrad;
magSqr; interpolate. The user can obtain the list of by deliberately calling
one that does not exist, so that foamCalc throws up an error message and lists the types
available, e.g.
>> foamCalc xxxx
Selecting calcType xxxx
unknown calcType type xxxx, constructor not in hash table
Valid calcType selections are:
8
(
randomise

Open∇FOAM-1.6

U-35

2.1 Lid-driven cavity flow
magSqr
magGrad
addSubtract
div
mag
interpolate
components
)

The components and mag calcTypes provide usefu l scalar measures of velocity. When
“foamCalc components U” is run on a case, say cavity, it reads in the velocity vector field
from each time directory and, in the corresponding time directories, writes scalar fields
Ux, Uy and Uz representing the x, y and z components of velocity. Similarly “foamCalc
mag U” writes a scalar field magU to each time directory representing the magnitude of
velocity.
The user can run foamCalc with the components calcType on both cavity and cavityFine
cases. For example, for the cavity case the user should execute the following command:
foamCalc components U -case $FOAM RUN/tutorials1.5/icoFoam/cavity
The individual components can be plotted as a graph in ParaView. It is quick, convenient and has reasonably good control over labelling and formatting, so the printed
output is a fairly good standard. However, to produce graphs for publication, users may
prefer to write raw data and plot it with a dedicated graphing tool, such as gnuplot or
Grace/xmgr. To do this, we recommend using the sample utility, described in section 6.5
and section 2.2.3.
Before commencing plotting, the user needs to load the newly generated Ux, Uy and Uz
fields into ParaView. To do this, the user should check the Update GUI button at the top
of the Properties panel of the base module they are working on, e.g.cavity.OpenFOAM.
Clicking Apply will then cause the new fields to be loaded into ParaView which will appear
in the Vol Field Status window. Ensure the new fields are selected and the changes
are applied, i.e. click Apply again if necessary. Also, data is interpolated incorrectly at
boundaries if the boundary regions are selected in the Region Status panel. Therefore the
user should deselect the patches in the Region Status panel, i.e.movingWall, fixedWall
and frontAndBack, and apply the changes.
Now, in order to display a graph in ParaView the user should select the module of interest, e.g.cavity.OpenFOAM and apply the Plot Over Line filter from the Filter->Data
Analysis menu. This opens up a new XY Plot window beside the existing 3D View window. A ProbeLine module is created in which the user can specify the end points of the
line in the Properties panel. In this example, the user should position the line vertically
up the centre of the domain, i.e. from (0.05, 0, 0.005) to (0.05, 0.1, 0.005), in the Point1
and Point2 text boxes. The Resolution can be set to 100.
On clicking Apply, a graph is generated in the XY Plot window. In the Display panel,
the user should choose Scatter Plot from the Plot Type menu, with Attribute Mode
Point Data. The Use Data Array option can be selected for the X Axis Data, taking the
arc length option so that the x-axis of the graph represents distance from the base of
the cavity.
The user can choose the fields to be displayed in the Line Series panel of the Display
window. From the list of scalar fields to be displayed, it can be seen that the magnitude
and components of vector fields are available by default, e.g. displayed as U:X, so that
it was not necessary to create Ux using foamCalc. Nevertheless, the user should deselect
all series except Ux (or U:x). A square colour box in the adjacent column to the selected
series indicates the line colour. The user can edit this most easily by a double click of the
mouse over that selection.
Open∇FOAM-1.6

U-36

Tutorials

Figure 2.11: Plotting graphs in paraFoam.
In order to format the graph, the user should move over to the XY Plot itself. Now,
with the cursor over the graph, the user can click the right mouse-button and select
Properties from the small floating menu produced. A Chart Options window appears
with General settings for title and legend and menus for each axis. The menu for each
axis can be expanded by a double click to reveal individual menus for Layout and Title,
one for each axis. The user can set font, colour and alignment of the axes titles, and has
several options for axis range and labels in linear or logarithmic scales.
Figure 2.11 is a graph produced using ParaView. The user can produce a graph however he/she wishes. For information, the graph in Figure 2.11 was produced with the
options for axes of: Standard type of Notation; Specify Axis Range selected; titles in
Sans Serif 12 font. The graph is displayed as a set of points rather than a line by activating the Enable Line Series button in the Display window. Note: if this button appears to
be inactive by being “greyed out”, it can be made active by selecting and deselecting the
sets of variables in the Line Series panel. Once the Enable Line Series button is selected,
the Line Style and Marker Style can be adjusted to the user’s preference.

2.1.6

Introducing mesh grading

The error in any solution will be more pronounced in regions where the form of the
true solution differ widely from the form assumed in the chosen numerical schemes. For
example a numerical scheme based on linear variations of variables over cells can only
generate an exact solution if the true solution is itself linear in form. The error is largest
in regions where the true solution deviates greatest from linear form, i.e. where the change
in gradient is largest. Error decreases with cell size.
It is useful to have an intuitive appreciation of the form of the solution before setting
up any problem. It is then possible to anticipate where the errors will be largest and
to grade the mesh so that the smallest cells are in these regions. In the cavity case the
large variations in velocity can be expected near a wall and so in this part of the tutorial
the mesh will be graded to be smaller in this region. By using the same number of cells,
greater accuracy can be achieved without a significant increase in computational cost.
A mesh of 20 × 20 cells with grading towards the walls will be created for the liddriven cavity problem and the results from the finer mesh of section 2.1.5.2 will then be
mapped onto the graded mesh to use as an initial condition. The results from the graded
mesh will be compared with those from the previous meshes. Since the changes to the
blockMeshDict dictionary are fairly substantial, the case used for this part of the tutorial,
Open∇FOAM-1.6

U-37

2.1 Lid-driven cavity flow

cavityGrade, is supplied in the $FOAM RUN/tutorials/incompressible/icoFoam directory.
2.1.6.1

Creating the graded mesh

The mesh now needs 4 blocks as different mesh grading is needed on the left and right and
top and bottom of the domain. The block structure for this mesh is shown in Figure 2.12.
The user can view the blockMeshDict file in the constant/polyMesh subdirectory of cavi6

7
15

8
16

2
3

17
3

4
12

5
13

y
0

x
z

14
1

2
10

Figure 2.12: Block structure of the graded mesh for the cavity (block numbers encircled).
tyGrade; for completeness the key elements of the blockMeshDict file are also reproduced
below. Each block now has 10 cells in the x and y directions and the ratio between largest
and smallest cells is 2.
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56

convertToMeters 0.1;
vertices
(
(0 0 0)
(0.5 0 0)
(1 0 0)
(0 0.5 0)
(0.5 0.5 0)
(1 0.5 0)
(0 1 0)
(0.5 1 0)
(1 1 0)
(0 0 0.1)
(0.5 0 0.1)
(1 0 0.1)
(0 0.5 0.1)
(0.5 0.5 0.1)
(1 0.5 0.1)
(0 1 0.1)
(0.5 1 0.1)
(1 1 0.1)
);
blocks
(
hex
hex
hex
hex
);

(0
(1
(3
(4

1
2
4
5

4
5
7
8

3
4
6
7

9 10 13 12) (10 10 1) simpleGrading (2 2 1)
10 11 14 13) (10 10 1) simpleGrading (0.5 2 1)
12 13 16 15) (10 10 1) simpleGrading (2 0.5 1)
13 14 17 16) (10 10 1) simpleGrading (0.5 0.5 1)

edges
(
);
patches
(
wall movingWall
(

Open∇FOAM-1.6

U-38

Tutorials
(6 15 16 7)
(7 16 17 8)

57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85
86

);

)
wall fixedWalls
(
(3 12 15 6)
(0 9 12 3)
(0 1 10 9)
(1 2 11 10)
(2 5 14 11)
(5 8 17 14)
)
empty frontAndBack
(
(0 3 4 1)
(1 4 5 2)
(3 6 7 4)
(4 7 8 5)
(9 10 13 12)
(10 11 14 13)
(12 13 16 15)
(13 14 17 16)
)

mergePatchPairs
(
);
// ************************************************************************* //

Once familiar with the blockMeshDict file for this case, the user can execute blockMesh
from the command line. The graded mesh can be viewed as before using paraFoam as
described in section 2.1.2.
2.1.6.2

Changing time and time step

The highest velocities and smallest cells are next to the lid, therefore the highest Courant
number will be generated next to the lid, for reasons given in section 2.1.1.4. It is therefore
useful to estimate the size of the cells next to the lid to calculate an appropriate time
step for this case.
When a nonuniform mesh grading is used, blockMesh calculates the cell sizes using a
geometric progression. Along a length l, if n cells are requested with a ratio of R between
the last and first cells, the size of the smallest cell, δxs , is given by:
r−1
αr − 1
where r is the ratio between one cell size and the next which is given by:
δxs = l

r = R n−1

(2.5)

(2.6)

and
(
R
α=
1 − r−n + r−1

for R > 1,
for R < 1.

(2.7)

For the cavityGrade case the number of cells in each direction in a block is 10, the ratio
between largest and smallest cells is 2 and the block height and width is 0.05 m. Therefore
the smallest cell length is 3.45 mm. From Equation 2.2, the time step should be less than
3.45 ms to maintain a Courant of less than 1. To ensure that results are written out
at convenient time intervals, the time step deltaT should be reduced to 2.5 ms and the
writeInterval set to 40 so that results are written out every 0.1 s. These settings can
be viewed in the cavityGrade/system/controlDict file.
The startTime 6(e)0.04.2450]TJ /R386(yF.049408307((e)0.04.245089(t)-)0.21(a)-0.252204(vi)-0.04

U-39

2.1 Lid-driven cavity flow

2.1.6.3

Mapping fields

As in section 2.1.5.3, use mapFields to map the final results from case cavityFine onto the
mesh for case cavityGrade. Enter the cavityGrade directory and execute mapFields by:
cd $FOAM RUN/tutorials/incompressible/icoFoam/cavityGrade
mapFields ../cavityFine -consistent
Now run icoFoam from the case directory and monitor the run time information. View
the converged results for this case and compare with other results using post-processing
tools described previously in section 2.1.5.6 and section 2.1.5.7.

2.1.7

Increasing the Reynolds number

The cases solved so far have had a Reynolds number of 10. This is very low and leads
to a stable solution quickly with only small secondary vortices at the bottom corners of
the cavity. We will now increase the Reynolds number to 50, at which point the solution
takes a noticeably longer time to converge. The coarsest mesh in case cavity will be used
initially. The user should make a copy of the cavity case and name it cavityHighRe by
typing:
cd $FOAM_RUN/tutorials/incompressible/icoFoam
cp -r cavity cavityHighRe
2.1.7.1

Pre-processing

Enter the the cavityHighRe case and edit the transportProperties dictionary. Since the
Reynolds number is required to be increased by a factor of 10, decrease the kinematic
viscosity by a factor of 10, i.e. to 1 × 10−3 m2 s−1 . We can now run this case by restarting
from the solution at the end of the cavity case run. To do this we can use the option of
setting the startFrom keyword to latestTime so that icoFoam takes as its initial data
the values stored in the directory corresponding to the most recent time, i.e. 0.5. The
endTime should be set to 2 s.
2.1.7.2

Running the code

Run icoFoam for this case from the case directory and view the run time information.
When running a job in the background, the following UNIX commands can be useful:
nohup enables a command to keep running after the user who issues the command has
logged out;
nice changes the priority of the job in the kernel’s scheduler; a niceness of -20 is the
highest priority and 19 is the lowest priority.
This is useful, for example, if a user wishes to set a case running on a remote machine
and does not wish to monitor it heavily, in which case they may wish to give it low
priority on the machine. In that case the nohup command allows the user to log out of a
remote machine he/she is running on and the job continues running, while nice can set
the priority to 19. For our case of interest, we can execute the command in this manner
as follows:
Open∇FOAM-1.6

U-40

Tutorials

cd $FOAM RUN/tutorials/incompressible/icoFoam/cavityHighRe
nohup nice -n 19 icoFoam > log &
cat log
In previous runs you may have noticed that icoFoam stops solving for velocity U quite
quickly but continues solving for pressure p for a lot longer or until the end of the run.
In practice, once icoFoam stops solving for U and the initial residual of p is less than
the tolerance set in the fvSolution dictionary (typically 10−6 ), the run has effectively
converged and can be stopped once the field data has been written out to a time directory.
For example, at convergence a sample of the log file from the run on the cavityHighRe
case appears as follows in which the velocity has already converged after 1.62 s and
initial pressure residuals are small; No Iterations 0 indicates that the solution of U has
stopped:
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34

Time = 1.63
Courant Number mean: 0.108642 max: 0.818175
DILUPBiCG: Solving for Ux, Initial residual = 7.86044e-06, Final residual = 7.86044e-06,
No Iterations 0
DILUPBiCG: Solving for Uy, Initial residual = 9.4171e-06, Final residual = 9.4171e-06,
No Iterations 0
DICPCG: Solving for p, Initial residual = 3.54721e-06, Final residual = 7.13506e-07,
No Iterations 4
time step continuity errors : sum local = 6.46788e-09, global = -9.44516e-19,
cumulative = 1.04595e-17
DICPCG: Solving for p, Initial residual = 2.15824e-06, Final residual = 9.95068e-07,
No Iterations 3
time step continuity errors : sum local = 8.67501e-09, global = 7.54182e-19,
cumulative = 1.12136e-17
ExecutionTime = 1.02 s ClockTime = 1 s
Time = 1.635
Courant Number mean: 0.108643 max: 0.818176
DILUPBiCG: Solving for Ux, Initial residual = 7.6728e-06, Final residual = 7.6728e-06,
No Iterations 0
DILUPBiCG: Solving for Uy, Initial residual = 9.19442e-06, Final residual = 9.19442e-06,
No Iterations 0
DICPCG: Solving for p, Initial residual = 3.13107e-06, Final residual = 8.60504e-07,
No Iterations 4
time step continuity errors : sum local = 8.15435e-09, global = -5.84817e-20,
cumulative = 1.11552e-17
DICPCG: Solving for p, Initial residual = 2.16689e-06, Final residual = 5.27197e-07,
No Iterations 14
time step continuity errors : sum local = 3.45666e-09, global = -5.62297e-19,
cumulative = 1.05929e-17
ExecutionTime = 1.02 s ClockTime = 1 s

2.1.8

High Reynolds number flow

View the results in paraFoam and display the velocity vectors. The secondary vortices in
the corners have increased in size somewhat. The user can then increase the Reynolds
number further by decreasing the viscosity and then rerun the case. The number of
vortices increases so the mesh resolution around them will need to increase in order to
resolve the more complicated flow patterns. In addition, as the Reynolds number increases
the time to convergence increases. The user should monitor residuals and extend the
endTime accordingly to ensure convergence.
The need to increase spatial and temporal resolution then becomes impractical as
the flow moves into the turbulent regime, where problems of solution stability may also
occur. Of course, many engineering problems have very high Reynolds numbers and it
is infeasible to bear the huge cost of solving the turbulent behaviour directly. Instead
Reynolds-averaged stress (RAS) turbulence models are used to solve for the mean flow
behaviour and calculate the statistics of the fluctuations. The standard k − ε model
with wall functions will be used in this tutorial to solve the lid-driven cavity case with
a Reynolds number of 104 . Two extra variables are solved for: k, the turbulent kinetic
energy; and, ε, the turbulent dissipation rate. The additional equations and models for
turbulent flow are implemented into a OpenFOAM solver called pisoFoam.
Open∇FOAM-1.6

U-41

2.1 Lid-driven cavity flow

2.1.8.1

Pre-processing

Change directory to the cavity case in the $FOAM RUN/tutorials/incompressible/pisoFoam/ras directory (N.B: the pisoFoam/ras directory). Generate the mesh by running blockMesh
as before. Mesh grading towards the wall is not necessary when using the standard k − ε
model with wall functions since the flow in the near wall cell is modelled, rather than
having to be resolved.
From version 1.6 onwards, a range of wall function models is available in OpenFOAM
that are applied as boundary conditions on individual patches. This enables different
wall function models to be applied to different wall regions. The choice of wall function
models are specified through the turbulent viscosity field, νt in the 0/nut file:
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41

dimensions

[0 2 -1 0 0 0 0];

internalField

uniform 0;

boundaryField
{
movingWall
{
type
value
}
fixedWalls
{
type
value
}
frontAndBack
{
type
}
}

nutWallFunction;
uniform 0;
nutWallFunction;
uniform 0;
empty;

// ************************************************************************* //

This case uses standard wall functions, specified by the nutWallFunction keyword entry
one the movingWall and fixedWalls patches. Other wall function models include the
rough wall functions, specified though the nutRoughWallFunction keyword.
The user should now open the field files for k and ε (0/k and 0/epsilon) and examine
their boundary conditions. For a wall boundary condition, ε is assigned a epsilonWallFunction boundary condition and a kqRwallFunction boundary condition is assigned to k.
The latter is a generic boundary condition that can be applied to any field that are of a
turbulent kinetic energy type, e.g. k, q or Reynolds Stress R. The initial values for k and
ε are set using an estimated fluctuating component of velocity U′ and a turbulent length
scale, l. k and ε are defined in terms of these parameters as follows:
1
k = U′ • U′
2
Cµ0.75 k 1.5
ε=
l

(2.8)
(2.9)

where Cµ is a constant of the k − ε model equal to 0.09. For a Cartesian coordinate
system, k is given by:
1
k = (Ux′ 2 + Uy′ 2 + Uz′ 2 )
2

(2.10)

where Ux′ 2 , Uy′ 2 and Uz′ 2 are the fluctuating components of velocity in the x, y and z
directions respectively. Let us assume the initial turbulence is isotropic, i.e. Ux′ 2 = Uy′ 2 =
Uz′ 2 , and equal to 5% of the lid velocity and that l, is equal to 20% of the box width, 0.1
Open∇FOAM-1.6

U-42

Tutorials

m, then k and ε are given by:
5
1 m s−1
Ux′ = Uy′ = Uz′ =
100
µ
¶2
3
5
⇒k=
m2 s−2 = 3.75 × 10−3 m2 s−2
2 100
Cµ0.75 k 1.5
≈ 7.65 × 10−4 m2 s−3
ε=
l

(2.11)
(2.12)
(2.13)

These form the initial conditions for k and ε. The initial conditions for U and p are
(0, 0, 0) and 0 respectively as before.
Prior to version 1.6 of OpenFOAM, the type of turbulence modelling method, e.g.
RAS or large-eddy simulation (LES), was declared within each solver. This resulted in
a lot of duplication of code in solver applications, where for most solvers that used RAS
turbulence modelling, there would be an equivalent LES solver.
From version 1.6 however, the choice of turbulence modelling method is selectable at
run-time through the simulationType keyword in turbulenceProperties dictionary. The
user can view this file in the constant directory:
17
18
19
20
21

simulationType

RASModel;

// ************************************************************************* //

The options for simulationType are laminar, RASmodel and LESmodel. With RASmodel
selected in this case, the choice of RAS modelling is specified in a RASProperties file, also
in the constant directory. The turbulence model is selected by the RASModel entry from a
long list of available models that are listed in Table 3.9. The kEpsilon model should be
selected which is is the standard k −ε model; the user should also ensure that turbulence
calculation is switched on.
The coefficients for each turbulence model are stored within the respective code with
a set of default values. Setting the optional switch called printCoeffs to on will make
the default values be printed to standard output, i.e. the terminal, when the model
is called at run time. The coefficients are printed out as a subdictionary whose name
is that of the model name with the word Coeffs appended, e.g. kEpsilonCoeffs in
the case of the kEpsilon model. The coefficients of the model, e.g. kEpsilon, can be
modified by optionally including that subdictionary within the RASProperties dictionary
and adjusting values accordingly.
The user should next set the laminar kinematic viscosity in the transportProperties
dictionary. To achieve a Reynolds number of 104 , a kinematic viscosity of 10−5 m is
required based on the Reynolds number definition given in Equation 2.1.
Finally the user should set the startTime, stopTime, deltaT and the writeInterval
in the controlDict. Set deltaT to 0.005 s to satisfy the Courant number restriction and
the endTime to 10 s.
2.1.8.2

Running the code

Execute pisoFoam by entering the case directory and typing “pisoFoam”. In this case,
where the viscosity is low, the boundary layer next to the moving lid is very thin and
the cells next to the lid are comparatively large so the velocity at their centres are much
less than the lid velocity. In fact, after ≈

2.1 Lid-driven cavity flow

U-43

the solution time by increasing the time step to a level where the Courant number is
much closer to 1. Therefore reset deltaT to 0.02 s and, on this occasion, set startFrom
to latestTime. This instructs pisoFoam to read the start data from the latest time
directory, i.e.10.0. The endTime should be set to 20 s since the run converges a lot slower
than the laminar case. Restart the run as before and monitor the convergence of the
solution. View the results at consecutive time steps as the solution progresses to see if
the solution converges to a steady-state or perhaps reaches some periodically oscillating
state. In the latter case, convergence may never occur but this does not mean the results
are inaccurate.

2.1.9

Changing the case geometry

A user may wish to make changes to the geometry of a case and perform a new simulation.
It may be useful to retain some or all of the original solution as the starting conditions
for the new simulation. This is a little complex because the fields of the original solution
are not consistent with the fields of the new case. However the mapFields utility can map
fields that are inconsistent, either in terms of geometry or boundary types or both.
As an example, let us go to the cavityClipped case in the icoFoam directory which
consists of the standard cavity geometry but with a square of length 0.04 m removed from
the bottom right of the cavity, according to the blockMeshDict below:
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67

convertToMeters 0.1;
vertices
(
(0 0 0)
(0.6 0 0)
(0 0.4 0)
(0.6 0.4 0)
(1 0.4 0)
(0 1 0)
(0.6 1 0)
(1 1 0)
(0 0 0.1)
(0.6 0 0.1)
(0 0.4 0.1)
(0.6 0.4 0.1)
(1 0.4 0.1)
(0 1 0.1)
(0.6 1 0.1)
(1 1 0.1)
);
blocks
(
hex (0 1 3 2 8 9 11 10) (12 8 1) simpleGrading (1 1 1)
hex (2 3 6 5 10 11 14 13) (12 12 1) simpleGrading (1 1 1)
hex (3 4 7 6 11 12 15 14) (8 12 1) simpleGrading (1 1 1)
);
edges
(
);
patches
(
wall lid
(
(5 13 14 6)
(6 14 15 7)
)
wall fixedWalls
(
(0 8 10 2)
(2 10 13 5)
(7 15 12 4)
(4 12 11 3)
(3 11 9 1)
(1 9 8 0)
)

Open∇FOAM-1.6

U-44

Tutorials

68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83

);

empty frontAndBack
(
(0 2 3 1)
(2 5 6 3)
(3 6 7 4)
(8 9 11 10)
(10 11 14 13)
(11 12 15 14)
)

mergePatchPairs
(
);
// ************************************************************************* //

Generate the mesh with blockMesh. The patches are set accordingly as in previous cavity
cases. For the sake of clarity in describing the field mapping process, the upper wall patch
is renamed lid, previously the movingWall patch of the original cavity.
In an inconsistent mapping, there is no guarantee that all the field data can be mapped
from the source case. The remaining data must come from field files in the target case
itself. Therefore field data must exist in the time directory of the target case before
mapping takes place. In the cavityClipped case the mapping is set to occur at time 0.5 s,
since the startTime is set to 0.5 s in the controlDict. Therefore the user needs to copy
initial field data to that directory, e.g. from time 0:
cd $FOAM RUN/tutorials/incompressible/icoFoam/cavityClipped
cp -r 0 0.5
Before mapping the data, the user should view the geometry and fields at 0.5 s.
Now we wish to map the velocity and pressure fields from cavity onto the new fields
of cavityClipped. Since the mapping is inconsistent, we need to edit the mapFieldsDict
dictionary, located in the system directory. The dictionary contains 2 keyword entries:
patchMap and cuttingPatches. The patchMap list contains a mapping of patches from
the source fields to the target fields. It is used if the user wishes a patch in the target
field to inherit values from a corresponding patch in the source field. In cavityClipped, we
wish to inherit the boundary values on the lid patch from movingWall in cavity so we
must set the patchMap as:
patchMap
(
lid movingWall
);
The cuttingPatches list contains names of target patches whose values are to be
mapped from the source internal field through which the target patch cuts. In this case
we will include the fixedWalls to demonstrate the interpolation process.
cuttingPatches
(
fixedWalls
);
Now the user should run mapFields, from within the cavityClipped directory:
mapFields ../cavity
Open∇FOAM-1.6

U-45

2.1 Lid-driven cavity flow

Figure 2.13: cavity solution velocity field mapped onto cavityClipped.

Figure 2.14: cavityClipped solution for velocity field.

Open∇FOAM-1.6

U-46

Tutorials

The user can view the mapped field as shown in Figure 2.13. The boundary patches
have inherited values from the source case as we expected. Having demonstrated this,
however, we actually wish to reset the velocity on the fixedWalls patch to (0, 0, 0). Edit
the U field, go to the fixedWalls patch and change the field from nonuniform to uniform
(0, 0, 0). The nonuniform field is a list of values that requires deleting in its entirety. Now
run the case with icoFoam.

2.1.10

Post-processing the modified geometry

Velocity glyphs can be generated for the case as normal, first at time 0.5 s and later at
time 0.6 s, to compare the initial and final solutions. In addition, we provide an outline of
the geometry which requires some care to generate for a 2D case. The user should select
Extract Block from the Filter menu and, in the Parameter panel, highlight the patches
of interest, namely the lid and fixedWalls. On clicking Apply, these items of geometry can
be displayed by selecting Wireframe in the Display panel. Figure 2.14 displays the patches
in black and shows vortices forming in the bottom corners of the modified geometry.

2.2

Stress analysis of a plate with a hole

This tutorial describes how to pre-process, run and post-process a case involving linearelastic, steady-state stress analysis on a square plate with a circular hole at its centre.
The plate dimensions are: side length 4 m and radius R = 0.5 m. It is loaded with a
uniform traction of σ = 10 kPa over its left and right faces as shown in Figure 2.15. Two
symmetry planes can be identified for this geometry and therefore the solution domain
need only cover a quarter of the geometry, shown by the shaded area in Figure 2.15.

y
symmetry plane

R = 0.5 m

σ = 10 kPa

symmetry plane

σ = 10 kPa

4.0 m
Figure 2.15: Geometry of the plate with a hole.
The problem can be approximated as 2-dimensional since the load is applied in the
plane of the plate. In a Cartesian coordinate system there are two possible assumptions
to take in regard to the behaviour of the structure in the third dimension: (1) the plane
Open∇FOAM-1.6

2.2 Stress analysis of a plate with a hole

U-47

stress condition, in which the stress components acting out of the 2D plane are assumed
to be negligible; (2) the plane strain condition, in which the strain components out of
the 2D plane are assumed negligible. The plane stress condition is appropriate for solids
whose third dimension is thin as in this case; the plane strain condition is applicable for
solids where the third dimension is thick.
An analytical solution exists for loading of an infinitely large, thin plate with a circular
hole. The solution for the stress normal to the vertical plane of symmetry is
¶
 µ
2
4
σ 1 + R + 3R
for |y| ≥ R
2y 2
2y 4
(σxx )x=0 =


U-48

Tutorials

right

left
4
x2
9

left

x2
0

5
hole

x1
2

right

1
x2
0

x2
x1
down

down

Figure 2.16: Block structure of the mesh for the plate with a hole.

52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85
86
87
88
89
90

);
edges
(
arc
arc
arc
arc
arc
arc
arc
arc
);

0 5 (0.469846 0.17101 0)
5 10 (0.17101 0.469846 0)
1 4 (0.939693 0.34202 0)
4 9 (0.34202 0.939693 0)
11 16 (0.469846 0.17101 0.5)
16 21 (0.17101 0.469846 0.5)
12 15 (0.939693 0.34202 0.5)
15 20 (0.34202 0.939693 0.5)

patches
(
symmetryPlane left
(
(8 9 20 19)
(9 10 21 20)
)
patch right
(
(2 3 14 13)
(3 6 17 14)
)
symmetryPlane down
(
(0 1 12 11)
(1 2 13 12)
)
patch up
(
(7 8 19 18)
(6 7 18 17)
)
patch hole
(
(10 5 16 21)

Open∇FOAM-1.6

2.2 Stress analysis of a plate with a hole
91
92
93
94
95
96
97
98
99
100
101
102
103
104
105
106
107
108
109
110
111
112

);

U-49

(5 0 11 16)
)
empty frontAndBack
(
(10 9 4 5)
(5 4 1 0)
(1 4 3 2)
(4 7 6 3)
(4 9 8 7)
(21 16 15 20)
(16 11 12 15)
(12 13 14 15)
(15 14 17 18)
(15 18 19 20)
)

mergePatchPairs
(
);
// ************************************************************************* //

Until now, we have only specified straight edges in the geometries of previous tutorials but
here we need to specify curved edges. These are specified under the edges keyword entry
which is a list of non-straight edges. The syntax of each list entry begins with the type
of curve, including arc, simpleSpline, polyLine etc., described further in section 5.3.1.
In this example, all the edges are circular and so can be specified by the arc keyword
entry. The following entries are the labels of the start and end vertices of the arc and a
point vector through which the circular arc passes.
The blocks in this blockMeshDict do not all have the same orientation. As can be seen
in Figure 2.16 the x2 direction of block 0 is equivalent to the −x1 direction for block 4.
This means care must be taken when defining the number and distribution of cells in each
block so that the cells match up at the block faces.
6 patches are defined: one for each side of the plate, one for the hole and one for the
front and back planes. The left and down patches are both a symmetry plane. Since this
is a geometric constraint, it is included in the definition of the mesh, rather than being
purely a specification on the boundary condition of the fields. Therefore they are defined
as such using a special symmetryPlane type as shown in the blockMeshDict.
The frontAndBack patch represents the plane which is ignored in a 2D case. Again
this is a geometric constraint so is defined within the mesh, using the empty type as shown
in the blockMeshDict. For further details of boundary types and geometric constraints,
the user should refer to section 5.2.1.
The remaining patches are of the regular patch type. The mesh should be generated
using blockMesh and can be viewed in paraFoam as described in section 2.1.2. It should
appear as in Figure 2.17.
2.2.1.1

Boundary and initial conditions

Once the mesh generation is complete, the initial field with boundary conditions must be
set. For a stress analysis case without thermal stresses, only displacement D needs to be
set. The 0/D is as follows:
17
18
19
20
21
22
23
24
25
26
27
28

dimensions

[0 1 0 0 0 0 0];

internalField

uniform (0 0 0);

boundaryField
{
left
{
type
}
right
{

symmetryPlane;

Open∇FOAM-1.6

U-50

Tutorials

Figure 2.17: Mesh of the hole in a plate problem.

type
traction
pressure
value

29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58

}

}
down
{
type
}
up
{
type
traction
pressure
value
}
hole
{
type
traction
pressure
value
}
frontAndBack
{
type
}

tractionDisplacement;
uniform ( 10000 0 0 );
uniform 0;
uniform (0 0 0);
symmetryPlane;

tractionDisplacement;
uniform ( 0 0 0 );
uniform 0;
uniform (0 0 0);
tractionDisplacement;
uniform ( 0 0 0 );
uniform 0;
uniform (0 0 0);
empty;

// ************************************************************************* //

Firstly, it can be seen that the displacement initial conditions are set to (0, 0, 0) m. The
left and down patches must be both of symmetryPlane type since they are specified
as such in the mesh description in the constant/polyMesh/boundary file. Similarly the
frontAndBack patch is declared empty.
The other patches are traction boundary conditions, set by a specialist traction boundary type. The traction boundary conditions are specified by a linear combination of: (1)
a boundary traction vector under keyword traction; (2) a pressure that produces a traction normal to the boundary surface that is defined as negative when pointing out of
the surface, under keyword pressure. The up and hole patches are zero traction so the
boundary traction and pressure are set to zero. For the right patch the traction should
be (1e4, 0, 0) Pa and the pressure should be 0 Pa.
Open∇FOAM-1.6

U-51

2.2 Stress analysis of a plate with a hole

2.2.1.2

Mechanical properties

The physical properties for the case are set in the mechanicalProperties dictionary in the
constant directory. For this problem, we need to specify the mechanical properties of
steel given in Table 2.1. In the mechanical properties dictionary, the user must also set
planeStress to yes.
Property
Units
Density
kg m−3
Young’s modulus
Pa
Poisson’s ratio
—

Keyword
Value
rho
7854
E
2 × 1011
nu
0.3

Table 2.1: Mechanical properties for steel

2.2.1.3

Thermal properties

The temperature field variable T is present in the solidDisplacementFoam solver since the
user may opt to solve a thermal equation that is coupled with the momentum equation
through the thermal stresses that are generated. The user specifies at run time whether
OpenFOAM should solve the thermal equation by the thermalStress switch in the thermalProperties dictionary. This dictionary also sets the thermal properties for the case,
e.g. for steel as listed in Table 2.2.
Property
Specific heat capacity
Thermal conductivity
Thermal expansion coeff.

Units
Jkg−1 K−1
Wm−1 K−1
K−1

Keyword
Value
C
434
k
60.5
alpha
1.1 × 10−5

Table 2.2: Thermal properties for steel
In this case we do not want to solve for the thermal equation. Therefore we must set
the thermalStress keyword entry to no in the thermalProperties dictionary.
2.2.1.4

Control

As before, the information relating to the control of the solution procedure are read in
from the controlDict dictionary. For this case, the startTime is 0 s. The time step is
not important since this is a steady state case; in this situation it is best to set the time
step deltaT to 1 so it simply acts as an iteration counter for the steady-state case. The
endTime, set to 100, then acts as a limit on the number of iterations. The writeInterval
can be set to 20.
The controlDict entries are as follows:
17
18
19
20
21
22
23
24
25
26
27
28
29
30

application

solidDisplacementFoam;

startFrom

startTime;

startTime

stopAt

endTime;

endTime

100;

deltaT

writeControl

timeStep;

Open∇FOAM-1.6

U-52
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51

Tutorials

writeInterval

20;

purgeWrite

writeFormat

ascii;

writePrecision

writeCompression uncompressed;
timeFormat

general;

timePrecision

graphFormat

raw;

runTimeModifiable yes;
// ************************************************************************* //

2.2.1.5

Discretisation schemes and linear-solver control

Let us turn our attention to the fvSchemes dictionary. Firstly, the problem we are
analysing is steady-state so the user should select SteadyState for the time derivatives
in timeScheme. This essentially switches off the time derivative terms. Not all solvers,
especially in fluid dynamics, work for both steady-state and transient problems but solidDisplacementFoam does work, since the base algorithm is the same for both types of
simulation.
The momentum equation in linear-elastic stress analysis includes several explicit terms
containing the gradient of displacement. The calculations benefit from accurate and
smooth evaluation of the gradient. Normally, in the finite volume method the discretisation is based on Gauss’s theorem The Gauss method is sufficiently accurate for most
purposes but, in this case, the least squares method will be used. The user should therefore open the fvSchemes dictionary in the system directory and ensure the leastSquares
method is selected for the grad(U) gradient discretisation scheme in the gradSchemes
sub-dictionary:
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50

d2dt2Schemes
{
default
}

steadyState;

gradSchemes
{
default
grad(D)
grad(T)
}

leastSquares;
leastSquares;
leastSquares;

divSchemes
{
default
div(sigmaD)
}

none;
Gauss linear;

laplacianSchemes
{
default
none;
laplacian(DD,D) Gauss linear corrected;
laplacian(DT,T) Gauss linear corrected;
}
interpolationSchemes
{
default
linear;
}
snGradSchemes
{
default

Open∇FOAM-1.6

none;

2.2 Stress analysis of a plate with a hole
51
52
53
54
55
56
57
58
59
60
61

U-53

}
fluxRequired
{
default
D
T
}

no;
yes;
no;

// ************************************************************************* //

The fvSolution dictionary in the system directory controls the linear equation solvers and
algorithms used in the solution. The user should first look at the solvers sub-dictionary
and notice that the choice of solver for D is GAMG. The solver tolerance should be set to
10−6 for this problem. The solver relative tolerance, denoted by relTol, sets the required
reduction in the residuals within each iteration. It is uneconomical to set a tight (low)
relative tolerance within each iteration since a lot of terms in each equation are explicit
and are updated as part of the segregated iterative procedure. Therefore a reasonable
value for the relative tolerance is 0.01, or possibly even higher, say 0.1, or in some cases
even 0.9 (as in this case).
17
18
19
20
21
22
23
24
25
26
27
28
29

solvers
{
D
{

}

30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53

solver
GAMG;
tolerance
1e-06;
relTol
0.9;
smoother
GaussSeidel;
cacheAgglomeration true;
nCellsInCoarsestLevel 20;
agglomerator
faceAreaPair;
mergeLevels
1;

T
{

}

solver
GAMG;
tolerance
1e-06;
relTol
0.9;
smoother
GaussSeidel;
cacheAgglomeration true;
nCellsInCoarsestLevel 20;
agglomerator
faceAreaPair;
mergeLevels
1;

}

stressAnalysis
{
compactNormalStress yes;
nCorrectors
1;
D
1e-06;
}
// ************************************************************************* //

The fvSolution dictionary contains a sub-dictionary, stressAnalysis that contains some control parameters specific to the application solver. Firstly there is nCorrectors which
specifies the number of outer loops around the complete system of equations, including
traction boundary conditions within each time step. Since this problem is steady-state,
we are performing a set of iterations towards a converged solution with the ’time step’
acting as an iteration counter. We can therefore set nCorrectors to 1.
The D keyword specifies a convergence tolerance for the outer iteration loop, i.e. sets
a level of initial residual below which solving will cease. It should be set to the desired
solver tolerance specified earlier, 10−6 for this problem.
Open∇FOAM-1.6

U-54

2.2.2

Tutorials

Running the code

The user should run the code here in the background from the command line as specified
below, so he/she can look at convergence information in the log file afterwards.
cd $FOAM RUN/tutorials/stressAnalysis/solidDisplacementFoam/plateHole
solidDisplacementFoam > log &
The user should check the convergence information by viewing the generated log file which
shows the number of iterations and the initial and final residuals of the displacement in
each direction being solved. The final residual should always be less than 0.9 times the
initial residual as this iteration tolerance set. Once both initial residuals have dropped
below the convergence tolerance of 10−6 the run has converged and can be stopped by
killing the batch job.

2.2.3

Post-processing

Post processing can be performed as in section 2.1.4. The solidDisplacementFoam solver
outputs the stress field σ as a symmetric tensor field sigma. This is consistent with the
way variables are usually represented in OpenFOAM solvers by the mathematical symbol
by which they are represented; in the case of Greek symbols, the variable is named
phonetically.
For post-processing individual scalar field components, σxx , σxy etc., can be generated
by running the foamCalc utility as before in section 2.1.5.7, this time on sigma:
foamCalc components sigma
Components named sigmaxx, sigmaxy etc. are written to time directories of the case.
The σxx stresses can be viewed in paraFoam as shown in Figure 2.18.
30

σxx (kPa)

25
20
15
10
5
0
Figure 2.18: σxx stress field in the plate with hole.
We would like to compare the analytical solution of Equation 2.14 to our solution.
We therefore must output a set of data of σxx along the left edge symmetry plane of
our domain. The user may generate the required graph data using the sample utility.
The utility uses a sampleDict dictionary located in the system directory, whose entries are
summarised in Table 6.3. The sample line specified in sets is set between (0.0, 0.5, 0.25)
and (0.0, 2.0, 0.25), and the fields are specified in the fields list:
Open∇FOAM-1.6

U-55

2.2 Stress analysis of a plate with a hole

Stress (σxx )x=0 (kPa)

35
30
25
20
15
10
5
0
0.6

0.8

1.0

1.2

1.4

1.6

1.8

2.0

Distance, y (m)
Numerical prediction

Analytical solution

Figure 2.19: Normal stress along the vertical symmetry (σxx )x=0
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39

interpolationScheme cellPoint;
setFormat
sets
(
leftPatch
{
type
axis
start
end
nPoints
}
);

raw;

uniform;
y;
( 0 0.5 0.25 );
( 0 2 0.25 );
100;

surfaces

();

fields

( sigmaxx );

// ************************************************************************* //

The user should execute sample as normal. The writeFormat is raw 2 column format.
The data is written into files within time subdirectories of a sets directory, e.g. the data
at t = 100 s is found within the file sets/100/leftPatch sigmaxx.xy. In an application such
as GnuPlot, one could type the following at the command prompt would be sufficient to
plot both the numerical data and analytical solution:
plot [0.5:2] [0:] ’sets/100/leftPatch sigmaxx.xy’,
1e4*(1+(0.125/(x**2))+(0.09375/(x**4)))
An example plot is shown in Figure 2.19.

2.2.4

Exercises

The user may wish to experiment with solidDisplacementFoam by trying the following
exercises:
2.2.4.1

Increasing mesh resolution

Increase the mesh resolution in each of the x and y directions. Use mapFields to map the
final coarse mesh results from section 2.2.3 to the initial conditions for the fine mesh.
Open∇FOAM-1.6

U-56

Tutorials

2.2.4.2

Introducing mesh grading

Grade the mesh so that the cells near the hole are finer than those away from the hole.
Design the mesh so that the ratio of sizes between adjacent cells is no more than 1.1
and so that the ratio of cell sizes between blocks is similar to the ratios within blocks.
Mesh grading is described in section 2.1.6. Again use mapFields to map the final coarse
mesh results from section 2.2.3 to the initial conditions for the graded mesh. Compare
the results with those from the analytical solution and previous calculations. Can this
solution be improved upon using the same number of cells with a different solution?
2.2.4.3

Changing the plate size

The analytical solution is for an infinitely large plate with a finite sized hole in it. Therefore this solution is not completely accurate for a finite sized plate. To estimate the error,
increase the plate size while maintaining the hole size at the same value.

2.3

Breaking of a dam

In this tutorial we shall solve a problem of simplified dam break in 2 dimensions using
the interFoam.The feature of the problem is a transient flow of two fluids separated by
a sharp interface, or free surface. The two-phase algorithm in interFoam is based on the
volume of fluid (VOF) method in which a specie transport equation is used to determine
the relative volume fraction of the two phases, or phase fraction α1 , in each computational
cell. Physical properties are calculated as weighted averages based on this fraction. The
nature of the VOF method means that an interface between the species is not explicitly
computed, but rather emerges as a property of the phase fraction field. Since the phase
fraction can have any value between 0 and 1, the interface is never sharply defined, but
occupies a volume around the region where a sharp interface should exist.
The test setup consists of a column of water at rest located behind a membrane on
the left side of a tank. At time t = 0 s, the membrane is removed and the column of
water collapses. During the collapse, the water impacts an obstacle at the bottom of the
tank and creates a complicated flow structure, including several captured pockets of air.
The geometry and the initial setup is shown in Figure 2.20.

2.3.1

Mesh generation

The user should go to the damBreak case in their $FOAM RUN/tutorials/multiphase/interFoam/laminar directory. Generate the mesh running blockMesh as described previously.
The damBreak mesh consist of 5 blocks; the blockMeshDict entries are given below.
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35

convertToMeters 0.146;
vertices
(
(0 0 0)
(2 0 0)
(2.16438 0 0)
(4 0 0)
(0 0.32876 0)
(2 0.32876 0)
(2.16438 0.32876 0)
(4 0.32876 0)
(0 4 0)
(2 4 0)
(2.16438 4 0)
(4 4 0)
(0 0 0.1)
(2 0 0.1)
(2.16438 0 0.1)

Open∇FOAM-1.6

2.3 Breaking of a dam

U-57

U-58
83
84
85
86
87
88
89
90
91
92

Tutorials

);

)

(9 21 22 10)
(10 22 23 11)

mergePatchPairs
(
);
// ************************************************************************* //

2.3.2

Boundary conditions

The user can examine the boundary geometry generated by blockMesh by viewing the
boundary file in the constant/polyMesh directory. The file contains a list of 5 boundary
patches: leftWall, rightWall, lowerWall, atmosphere and defaultFaces. The user
should notice the type of the patches. The atmosphere is a standard patch, i.e. has no
special attributes, merely an entity on which boundary conditions can be specified. The
defaultFaces patch is empty since the patch normal is in the direction we will not solve
in this 2D case. The leftWall, rightWall and lowerWall patches are each a wall. Like
the plain patch, the wall type contains no geometric or topological information about the
mesh and only differs from the plain patch in that it identifies the patch as a wall, should
an application need to know, e.g. to apply special wall surface modelling.
A good example is that the interFoam solver includes modelling of surface tension at
the contact point between the interface and wall surface. The models are applied by
specifying the alphaContactAngle boundary condition on the alpha1 (α1 ) field. With it,
the user must specify the following: a static contact angle, theta0 θ0 ; leading and trailing
edge dynamic contact angles, thetaA θA and thetaR θR respectively; and a velocity scaling
function for dynamic contact angle, uTheta.
In this tutorial we would like to ignore surface tension effects between the wall and
interface. We can do this by setting the static contact angle, θ0 = 90◦ and the velocity
scaling function to 0. However, the simpler option which we shall choose here is to specify
a zeroGradient type on alpha1, rather than use the alphaContactAngle boundary condition.
The top boundary is free to the atmosphere and so is given an atmosphere boundary
type; the defaultFaces representing the front and back planes of the 2D problem, is, as
usual, an empty type.

2.3.3

Setting initial field

Unlike the previous cases, we shall now specify a non-uniform initial condition for the
phase fraction α1 where
(
1 for the liquid phase
α1 =
(2.15)
0 for the gas phase
This will be done by running the setFields utility. It requires a setFieldsDict dictionary,
located in the system directory, whose entries for this case are shown below.
17
18
19
20
21
22
23
24
25
26
27
28

defaultFieldValues
(
volScalarFieldValue alpha1 0
);
regions
(
boxToCell
{
box (0 0 -1) (0.1461 0.292 1);
fieldValues

Open∇FOAM-1.6

U-59

2.3 Breaking of a dam
29
30

(

31
32
33
34
35
36

);

}

volScalarFieldValue alpha1 1

// ************************************************************************* //

The defaultFieldValues sets the default value of the fields, i.e. the value the field
takes unless specified otherwise in the regions sub-dictionary. That sub-dictionary contains a list of subdictionaries containing fieldValues that override the defaults in a
specified region. The region is expressed in terms of a topoSetSource that creates a set
of points, cells or faces based on some topological constraint. Here, boxToCell creates
a bounding box within a vector minimum and maximum to define the set of cells of the
liquid region. The phase fraction α1 is defined as 1 in this region.
The user should execute setFields as any other utility is executed. Using paraFoam,
check that the initial alpha1 field corresponds to the desired distribution as in Figure 2.21.

Phase fraction, α1
1.0
0.9
0.8
0.7
0.6
0.5
0.4
0.3
0.2
0.1
0.0
Figure 2.21: Initial conditions for phase fraction alpha1.

2.3.4

Fluid properties

Let us examine the transportProperties file in the constant directory. It dictionary contains the material properties for each fluid, separated into two subdictionaries phase1
and phase2. The transport model for each phase is selected by the transportModel
keyword. The user should select Newtonian in which case the kinematic viscosity is single valued and specified under the keyword nu. The viscosity parameters for the other
models, e.g.CrossPowerLaw, are specified within subdictionaries with the generic name
Coeffs, i.e.CrossPowerLawCoeffs in this example. The density is specified under
the keyword rho.
The surface tension between the two phases is specified under the keyword sigma.
The values used in this tutorial are listed in Table 2.3.
Gravitational acceleration is uniform across the domain and is specified in a file named
g in the constant directory. Unlike a normal field file, e.g. U and p, g is a uniformDimensionedVectorField and so simply contains a set of dimensions and a value that represents
(0, 9.81, 0) m s−2 for this tutorial:
Open∇FOAM-1.6

U-60

Tutorials

phase1 properties
Kinematic viscosity
Density

m2 s−1
kg m−3

nu
rho

1.0 × 10−6
1.0 × 103

phase2 properties
Kinematic viscosity
Density

m2 s−1
kg m−3

nu
rho

1.48 × 10−5
1.0

sigma

0.07

Properties of both phases
Surface tension
N m−1

Table 2.3: Fluid properties for the damBreak tutorial

17
18
19
20
21
22

dimensions
value

[0 1 -2 0 0 0 0];
( 0 -9.81 0 );

// ************************************************************************* //

2.3.5

Turbulence modelling

As in the cavity example, the choice of turbulence modelling method is selectable at runtime through the simulationType keyword in turbulenceProperties dictionary. In this
example, we wish to run without turbulence modelling so we set laminar:
17
18
19
20
21

simulationType

laminar;

// ************************************************************************* //

2.3.6

Time step control

Time step control is an important issue in free surface tracking since the surface-tracking
algorithm is considerably more sensitive to the Courant number Co than in standard fluid
flow calculations. Ideally, we should not exceed an upper limit Co ≈ 0.5 in the region
of the interface. In some cases, where the propagation velocity is easy to predict, the
user should specify a fixed time-step to satisfy the Co criterion. For more complex cases,
this is considerably more difficult. interFoam therefore offers automatic adjustment of the
time step as standard in the controlDict. The user should specify adjustTimeStep to be
on and the the maximum Co, maxCo to be 0.5. The upper limit on time step maxDeltaT
can be set to a value that will not be exceeded in this simulation, e.g. 1.0.
By using automatic time step control, the steps themselves are never rounded to a
convenient value. Consequently if we request that OpenFOAM saves results at a fixed
number of time step intervals, the times at which results are saved are somewhat arbitrary.
However even with automatic time step adjustment, OpenFOAM allows the user to specify
that results are written at fixed times; in this case OpenFOAM forces the automatic time
stepping procedure to adjust time steps so that it ‘hits’ on the exact times specified for
write output. The user selects this with the adjustableRunTime option for writeControl
in the controlDict dictionary. The controlDict dictionary entries should be:
17
18
19
20
21

application

interFoam;

startFrom

startTime;

Open∇FOAM-1.6

U-61

2.3 Breaking of a dam
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55

startTime

stopAt

endTime;

endTime

deltaT

0.001;

writeControl

adjustableRunTime;

writeInterval

0.05;

purgeWrite

writeFormat

ascii;

writePrecision

writeCompression uncompressed;
timeFormat

general;

timePrecision

runTimeModifiable yes;
adjustTimeStep

yes;

maxCo

0.5;

maxDeltaT

// ************************************************************************* //

2.3.7

Discretisation schemes

The free surface treatment in OpenFOAM does not account for the effects of turbulence.
This is a consequence of the fact that the Reynolds averaged approach to turbulence
modelling does not match the notion of an infinitesimally thin interface between air and
water. As a consequence, all free surface simulations can be viewed as a direct numerical
simulation (DNS) of fluid flow. DNS is associated with certain requirements on the mesh
size, far beyond the mesh resolution of our test case.
This solver uses the multidimensional universal limiter for explicit solution (MULES)
method, created by OpenCFD, to maintain boundedness of the phase fraction independent of underlying numerical scheme, mesh structure, etc. The choice of schemes for
convection are therfore not restricted to those that are strongly stable or bounded, e.g.
upwind differencing.
The convection schemes settings are made in the divSchemes sub-dictionary of the
fvSchemes dictionary. In this example, the convection term in the momentum equation
(∇ • (ρUU)), denoted by the div(rho*phi,U) keyword, uses Gauss limitedLinearV
1.0 to produce good accuracy. The limited linear schemes require a coefficient φ as
described in section 4.4.1. Here, we have opted for best stability with φ = 1.0. The
∇ • (Uα1 ) term, represented by the div(phi,alpha) keyword uses the vanLeer scheme.
The ∇ • (Urb α1 ) term, represeniv(

U-62

Tutorials
default
grad(U)
grad(alpha1)

25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
61

Gauss linear;
Gauss linear;
Gauss linear;

}
divSchemes
{
div(rho*phi,U) Gauss limitedLinearV 1;
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss interfaceCompression;
}
laplacianSchemes
{
default
}

Gauss linear corrected;

interpolationSchemes
{
default
linear;
}
snGradSchemes
{
default
}
fluxRequired
{
default
p;
pcorr;
alpha1;
}

corrected;

no;

// ************************************************************************* //

2.3.8

Linear-solver control

In the fvSolution, the PISO sub-dictionary contains elements that are specific to interFoam.
There are the usual correctors to the momentum equation but also correctors to a PISO
loop around the α1 phase equation. Of particular interest are the nAlphaSubCycles and
cAlpha keywords. nAlphaSubCycles represents the number of sub-cycles within the α1
equation; sub-cycles are additional solutions to an equation within a given time step. It
is used to enable the solution to be stable without reducing the time step and vastly
increasing the solution time. Here we specify 2 sub-cycles, which means that the α1
equation is solved in 2× half length time steps within each actual time step.
The cAlpha keyword is a factor that controls the compression of the interface where: 0
corresponds to no compression; 1 corresponds to conservative compression; and, anything
larger than 1, relates to enhanced compression of the interface. We generally recommend
a value of 1.0 which is employed in this example.

2.3.9

Running the code

Running of the code has been described in detail in previous tutorials. Try the following,
that uses tee, a command that enables output to be written to both standard output and
files:
cd $FOAM RUN/tutorials/multiphase/interFoam/laminar/damBreak
interFoam | tee log
The code will now be run interactively, with a copy of output stored in the log file.
Open∇FOAM-1.6

U-63

2.3 Breaking of a dam

2.3.10

Post-processing

Post-processing of the results can now be done in the usual way. The user can monitor
the development of the phase fraction alpha1 in time; Figure 2.22.

2.3.11

Running in parallel

The results from the previous example are generated using a fairly coarse mesh. We now
wish to increase the mesh resolution and re-run the case. The new case will typically
take a few hours to run with a single processor so, should the user have access to multiple
processors, we can demonstrate the parallel processing capability of OpenFOAM.
The user should first make a copy of the damBreak case, e.g. by
cd $FOAM RUN/tutorials/multiphase/interFoam/laminar
mkdir damBreakFine
cp -r damBreak/0 damBreakFine
cp -r damBreak/system damBreakFine
cp -r damBreak/constant damBreakFine
Enter the new case directory and change the blocks description in the blockMeshDict
dictionary to
blocks
(
hex
hex
hex
hex
hex
);

(0
(2
(4
(5
(6

1
3
5
6
7

5 4 12 13 17 16) (46 10 1) simpleGrading (1 1
7 6 14 15 19 18) (40 10 1) simpleGrading (1 1
9 8 16 17 21 20) (46 76 1) simpleGrading (1 2
10 9 17 18 22 21) (4 76 1) simpleGrading (1 2
11 10 18 19 23 22) (40 76 1) simpleGrading (1

1)
1)
1)
1)
2 1)

Here, the entry is presented as printed from the blockMeshDict file; in short the user must
change the mesh densities, e.g. the 46 10 1 entry, and some of the mesh grading entries
to 1 2 1. Once the dictionary is correct, generate the mesh.
As the mesh has now changed from the damBreak example, the user must re-initialise
the phase field alpha1 in the 0 time directory since it contains a number of elements that
is inconsistent with the new mesh. Note that there is no need to change the U and p
fields since they are specified as uniform which is independent of the number of elements

U-64

Tutorials

Phase fraction, α1
1.0
0.9
0.8
0.7
0.6
0.5
0.4
0.3
0.2
0.1
0.0
(a) At t = 0.25 s.

Phase fraction, α1
1.0
0.9
0.8
0.7
0.6
0.5
0.4
0.3
0.2
0.1
0.0
(b) At t = 0.50 s.

Figure 2.22: Snapshots of phase α1 .

Open∇FOAM-1.6

U-65

2.3 Breaking of a dam

case is therefore to decompose the domain using the decomposePar utility. There is a
dictionary associated with decomposePar named decomposeParDict which is located in
the system directory of the tutorial case; also, like with many utilities, a default dictionary can be found in the directory of the source code of the specific utility, i.e. in
$FOAM UTILITIES/parallelProcessing/decomposePar for this case.
The first entry is numberOfSubdomains which specifies the number of subdomains into
which the case will be decomposed, usually corresponding to the number of processors
available for the case.
In this tutorial, the method of decomposition should be simple and the corresponding
simpleCoeffs should be edited according to the following criteria. The domain is split
into pieces, or subdomains, in the x, y and z directions, the number of subdomains in
each direction being given by the vector n. As this geometry is 2 dimensional, the 3rd
direction, z, cannot be split, hence nz must equal 1. The nx and ny components of n
split the domain in the x and y directions and must be specified so that the number
of subdomains specified by nx and ny equals the specified numberOfSubdomains, i.e.
nx ny = numberOfSubdomains. It is beneficial to keep the number of cell faces adjoining
the subdomains to a minimum so, for a square geometry, it is best to keep the split
between the x and y directions should be fairly even. The delta keyword should be set
to 0.001.
For example, let us assume we wish to run on 4 processors. We would set numberOfSubdomains to 4 and n = (2, 2, 1). When running decomposePar, we can see from the
screen messages that the decomposition is distributed fairly even between the processors.
The user should consult section 3.4 for details of how to run a case in parallel; in
this tutorial we merely present an example of running in parallel. We use the openMPI
implementation of the standard message-passing interface (MPI). As a test here, the user
can run in parallel on a single node, the local host only, by typing:
mpirun -np 4 interFoam -parallel > log &
The user may run on more nodes over a network by creating a file that lists the host
names of the machines on which the case is to be run as described in section 3.4.2. The
case should run in the background and the user can follow its progress by monitoring the
log file as usual.

Figure 2.23: Mesh of processor 2 in parallel processed case.

Open∇FOAM-1.6

U-66

Tutorials

Phase fraction, α1
1.0
0.9
0.8
0.7
0.6
0.5
0.4
0.3
0.2
0.1
0.0
(a) At t = 0.25 s.

Phase fraction, α1
1.0
0.9
0.8
0.7
0.6
0.5
0.4
0.3
0.2
0.1
0.0
(b) At t = 0.50 s.

Figure 2.24: Snapshots of phase α1 with refined mesh.

Open∇FOAM-1.6

2.3 Breaking of a dam

2.3.12

U-67

Post-processing a case run in parallel

Once the case has completed running, the decomposed fields and mesh must be reassembled for post-processing using the reconstructPar utility. Simply execute it from the command line. The results from the fine mesh are shown in Figure 2.24. The user can see
that the resolution of interface has improved significantly compared to the coarse mesh.
The user may also post-process a segment of the decomposed domain individually by
simply treating the individual processor directory as a case in its own right. For example
if the user starts paraFoam by
paraFoam -case processor1
then processor1 will appear as a case module in ParaView. Figure 2.23 shows the mesh
from processor 1 following the decomposition of the domain using the simple method.

Open∇FOAM-1.6

U-68

Open∇FOAM-1.6

Tutorials

Chapter 3
Applications and libraries
We should reiterate from the outset that OpenFOAM is a C++ library used primarily to
create executables, known as applications. OpenFOAM is distributed with a large set of
precompiled applications but users also have the freedom to create their own or modify
existing ones. Applications are split into two main categories:
solvers that are each designed to solve a specific problem in computational continuum
mechanics;
utilities that perform simple pre-and post-processing tasks, mainly involving data manipulation and algebraic calculations.
OpenFOAM is divided into a set of precompiled libraries that are dynamically linked
during compilation of the solvers and utilities. Libraries such as those for physical models
are supplied as source code so that users may conveniently add their own models to the
libraries.
This chapter gives an overview of solvers, utilities and libraries, their creation, modification, compilation and execution. The actual writing of code for solvers and utilities
is not described here but is within the Programmer’s Guide. The Programmer’s Guide is
currently under development so, if users have any queries, further information may also
available at the OpenFOAM web site.

3.1

The programming language of OpenFOAM

In order to understand the way in which the OpenFOAM library works, some background
knowledge of C++, the base language of OpenFOAM, is required; the necessary information will be presented in this chapter. Before doing so, it is worthwhile addressing the
concept of language in general terms to explain some of the ideas behind object-oriented
programming and our choice of C++ as the main programming language of OpenFOAM.

3.1.1

Language in general

The success of verbal language and mathematics is based on efficiency, especially in
expressing abstract concepts. For example, in fluid flow, we use the term “velocity field”,
which has meaning without any reference to the nature of the flow or any specific velocity
data. The term encapsulates the idea of movement with direction and magnitude and
relates to other physical properties. In mathematics, we can represent velocity field by
a single symbol, e.g. U, and express certain concepts using symbols, e.g. “the field of
velocity magnitude” by |U|. The advantage of mathematics over verbal language is its
greater efficiency, making it possible to express complex concepts with extreme clarity.

U-70

Applications and libraries

The problems that we wish to solve in continuum mechanics are not presented in
terms of intrinsic entities, or types, known to a computer, e.g. bits, bytes, integers. They
are usually presented first in verbal language, then as partial differential equations in 3
dimensions of space and time. The equations contain the following concepts: scalars,
vectors, tensors, and fields thereof; tensor algebra; tensor calculus; dimensional units.
The solution to these equations involves discretisation procedures, matrices, solvers, and
solution algorithms. The topics of tensor mathematics and numerics are the subjects of
chapter 1 and chapter 2 of the Programmer’s Guide.

3.1.2

Object-orientation and C++

Progamming languages that are object-oriented, such as C++, provide the mechanism
— classes — to declare types and associated operations that are part of the verbal and
mathematical languages used in science and engineering. Our velocity field introduced
earlier can be represented in programming code by the symbol U and “the field of velocity
magnitude” can be mag(U). The velocity is a vector field for which there should exist,
in an object-oriented code, a vectorField class. The velocity field U would then be an
instance, or object, of the vectorField class; hence the term object-oriented.
The clarity of having objects in programming that represent physical objects and
abstract entities should not be underestimated. The class structure concentrates code
development to contained regions of the code, i.e. the classes themselves, thereby making
the code easier to manage. New classes can be derived or inherit properties from other
classes, e.g. the vectorField can be derived from a vector class and a Field class. C++
provides the mechanism of template classes such that the template class Field can
represent a field of any , e.g.scalar, vector, tensor. The general features of the
template class are passed on to any class created from the template. Templating and
inheritance reduce duplication of code and create class hierarchies that impose an overall
structure on the code.

3.1.3

Equation representation

A central theme of the OpenFOAM design is that the solver applications, written using the
OpenFOAM classes, have a syntax that closely resembles the partial differential equations
being solved. For example the equation
∂ρU
+ ∇ • φU − ∇ • µ∇U = −∇p
∂t
is represented by the code
solve
(
fvm::ddt(rho, U)
+ fvm::div(phi, U)
- fvm::laplacian(mu, U)
==
- fvc::grad(p)
);
This and other requirements demand that the principal programming language of OpenFOAM has object-oriented features such as inheritance, template classes, virtual functions
Open∇FOAM-1.6

3.2 Compiling applications and libraries

U-71

and operator overloading. These features are not available in many languages that purport to be object-orientated but actually have very limited object-orientated capability,
such as FORTRAN-90. C++, however, possesses all these features while having the additional advantage that it is widely used with a standard specification so that reliable
compilers are available that produce efficient executables. It is therefore the primary
language of OpenFOAM.

3.1.4

Solver codes

Solver codes are largely procedural since they are a close representation of solution algorithms and equations, which are themselves procedural in nature. Users do not need a
deep knowledge of object-orientation and C++ programming to write a solver but should
know the principles behind object-orientation and classes, and to have a basic knowledge
of some C++ code syntax. An understanding of the underlying equations, models and
solution method and algorithms is far more important.
There is often little need for a user to immerse themselves in the code of any of the
OpenFOAM classes. The essence of object-orientation is that the user should not have
to; merely the knowledge of the class’ existence and its functionality are sufficient to use
the class. A description of each class, its functions etc. is supplied with the OpenFOAM
distribution in HTML documentation generated with

U-72

Applications and libraries

nc class

Main code
newApp.C
#include "nc.H"
int main()
{
...
...
return(0);
}

Header file
-I option

nc.H
Definition...

nc.C
#include "nc.H"
Code...
Compiled

Compiled
newApp
Executable

Linked
-l option

nc.so
Library

Figure 3.1: Header files, source files, compilation and linking.
of header files for all the classes on which the top level .C code ultimately depends; these
.H files are known as the dependencies. With a dependency list, a compiler can check
whether the source files have been updated since their last compilation and selectively
compile only those that need to be.
Header files are included in the code using # include statements, e.g.
# include "otherHeader.H";
causes the compiler to suspend reading from the current file to read the file specified.
Any self-contained piece of code can be put into a header file and included at the relevant location in the main code in order to improve code readability. For example, in
most OpenFOAM applications the code for creating fields and reading field input data is
included in a file createFields.H which is called at the beginning of the code. In this way,
header files are not solely used as class declarations. It is wmake that performs the task
of maintaining file dependency lists amongst other functions listed below.
• Automatic generation and maintenance of file dependency lists, i.e. lists of files
which are included in the source files and hence on which they depend.
• Multi-platform compilation and linkage, handled through appropriate directory
structure.
• Multi-language compilation and linkage, e.g. C, C++, Java.
• Multi-option compilation and linkage, e.g. debug, optimised, parallel and profiling.
• Support for source code generation programs, e.g. lex, yacc, IDL, MOC.
• Simple syntax for source file lists.
• Automatic creation of source file lists for new codes.
• Simple handling of multiple shared or static libraries.
• Extensible to new machine types.
Open∇FOAM-1.6

U-73

3.2 Compiling applications and libraries

• Extremely portable, works on any machine with: make; sh, ksh or csh; lex, cc.
• Has been tested on Apollo, SUN, SGI, HP (HPUX), Compaq (DEC), IBM (AIX),
Cray, Ardent, Stardent, PC Linux, PPC Linux, NEC, SX4, Fujitsu VP1000.

3.2.2

Compiling with wmake

OpenFOAM applications are organised using a standard convention that the source code
of each application is placed in a directory whose name is that of the application. The
top level source file takes the application name with the .C extension. For example, the
source code for an application called newApp would reside is a directory newApp and the
top level file would be newApp.C as shown in Figure 3.2. The directory must also contain
newApp
newApp.C
otherHeader.H
Make
files
options
Figure 3.2: Directory structure for an application
a Make subdirectory containing 2 files, options and files, that are described in the following
sections.
3.2.2.1

Including headers

The compiler searches for the included header files in the following order, specified with
the -I option in wmake:
1. the $WM PROJECT DIR/src/OpenFOAM/lnInclude directory;
2. a local lnInclude directory, i.e.newApp/lnInclude;
3. the local directory, i.e.newApp;
4. platform dependent paths set in files in the $WM PROJECT DIR/wmake/rules/$WM ARCH/ directory, e.g./usr/X11/include and $(MPICH ARCH PATH)/include;
5. other directories specified explicitly in the Make/options file with the -I option.
The Make/options file contains the full directory paths to locate header files using the
syntax:
EXE INC = \
-I \
-I \
...
\
-I
Notice first that the directory names are preceeded by the -I flag and that the syntax
uses the \ to continue the EXE INC across several lines, with no \ after the final entry.
Open∇FOAM-1.6

U-74
3.2.2.2

Applications and libraries

Linking to libraries

The compiler links to shared object library files in the following directory paths, specified
with the -L option in wmake:
1. the $FOAM LIBBIN directory;
2. platform dependent paths set in files in the $WM DIR/rules/$WM ARCH/ directory,
e.g./usr/X11/lib and $(MPICH ARCH PATH)/lib;
3. other directories specified in the Make/options file.
The actual library files to be linked must be specified using the -l option and removing
the lib prefix and .so extension from the library file name, e.g.libnew.so is included with
the flag -lnew. By default, wmake loads the following libraries:
1. the libOpenFOAM.so library from the $FOAM LIBBIN directory;
2. platform dependent libraries specified in set in files in the $WM DIR/rules/$WM ARCH/
directory, e.g.libm.so from /usr/X11/lib and liblam.so from $(LAM ARCH PATH)/lib;
3. other libraries specified in the Make/options file.
The Make/options file contains the full directory paths and library names using the syntax:
EXE LIBS = \
-L \
-L \
...
\
-L \
-l
\
-l
\
...
\
-l
Let us reiterate that the directory paths are preceeded by the -L flag, the library names
are preceeded by the -l flag.
3.2.2.3

Source files to be compiled

The compiler requires a list of .C source files that must be compiled. The list must contain
the main .C file but also any other source files that are created for the specific application
but are not included in a class library. For example, users may create a new class or
some new functionality to an existing class for a particular application. The full list of
.C source files must be included in the Make/files file. As might be expected, for many
applications the list only includes the name of the main .C file, e.g.newApp.C in the case
of our earlier example.
The Make/files file also includes a full path and name of the compiled executable,
specified by the EXE = syntax. Standard convention stipulates the name is that of the application, i.e.newApp in our example. The OpenFOAM release offers two useful choices for
path: standard release applications are stored in $FOAM APPBIN; applications developed
by the user are stored in $FOAM USER APPBIN.
If the user is developing their own applications, we recommend they create an applications subdirectory in their $WM PROJECT USER DIR directory containing the source
Open∇FOAM-1.6

U-75

3.2 Compiling applications and libraries

code for personal OpenFOAM applications. As with standard applications, the source
code for each OpenFOAM application should be stored within its own directory. The
only difference between a user application and one from the standard release is that the
Make/files file should specify that the user’s executables are written into their $FOAM USER APPBIN directory. The Make/files file for our example would appear as follows:
newApp.C
EXE = $(FOAM_USER_APPBIN)/newApp
3.2.2.4

Running wmake

The wmake script is executed by typing:
wmake
The is the directory path of the application that is being compiled. Typically, wmake is executed from within the directory of the application being
compiled, in which case can be omitted.
If a user wishes to build an application executable, then no
are required. However may be specified for building libraries etc.
as described in Table 3.1.
Argument
lib
libso
libo
jar
exe

Type of compilation
Build a statically-linked library
Build a dynamically-linked library
Build a statically-linked object file library
Build a JAVA archive
Build an application independent of the specified project

Table 3.1: Optional compilation arguments to wmake.

3.2.2.5

wmake environment variables

For information, the environment variable settings used by wmake are listed in Table 3.2.

3.2.3

Removing dependency lists: wclean and rmdepall

On execution, wmake builds a dependency list file with a .dep file extension, e.g.newApp.dep
in our example, and a list of files in a Make/$WM OPTIONS directory. If the user wishes
to remove these files, perhaps after making code changes, the user can run the wclean
script by typing:
wclean
Again, the is a path to the

re applicat ta.216461840.20

U-76

Applications and libraries

Main paths
$WM PROJECT INST DIR
$WM PROJECT
$WM PROJECT
$WM PROJECT
$WM PROJECT

Full
path
to
installation
directory,
e.g.$HOME/OpenFOAM
Name of the project being compiled: OpenFOAM
VERSION Version of the project being compiled: 1.6
DIR
Full path to locate binary executables of OpenFOAM
release, e.g.$HOME/OpenFOAM/OpenFOAM-1.6
USER DIR Full path to locate binary executables of the user
e.g.$HOME/OpenFOAM/${USER}-1.6

Other paths/settings
$WM ARCH
$WM
$WM
$WM
$WM
$WM
$WM
$WM
$WM

$WM
$WM

Machine architecture: cray decAlpha dec ibm linux
linuxPPC sgi3 sgi32 sgi64 sgiN32 solaris sx4 t3d
COMPILER
Compiler being used: Gcc3 - gcc 4.3.3, KAI - KAI
COMPILER DIR
Compiler installation directory
COMPILER BIN
Compiler installation binaries $WM COMPILER BIN/bin
COMPILER LIB
Compiler installation libraries $WM COMPILER BIN/lib
COMPILE OPTION
Compilation option: Debug - debugging, Opt optimisation.
DIR
Full path of the wmake directory
JAVAC OPTION
Compilation option for JAVA: Debug - debugging, Opt
optimisation.
LINK LANGUAGE
Compiler used to link libraries and executables. In multilanguage projects a $WM LINK LANGUAGE is set to the
primary language.
MPLIB
Parallel communications library: LAM, MPI, MPICH, PVM
OPTIONS
= $WM ARCH$WM COMPILER...
...$WM COMPILE OPTION$WM MPLIB
e.g.linuxGcc3OptMPICH
PROJECT LANGUAGE Programming language of project, e.g.c++
SHELL
Shell used for the wmake scripts bash, csh, ksh, tcsh
Table 3.2: Environment variable settings for wmake.

If a user wishes to remove the dependency files and files from the Make directory, then
no are required. However if lib is specified in
a local lnInclude directory will be deleted also.
An additional script, rmdepall removes all dependency .dep files recursively down the
directory tree from the point at which it is executed. This can be useful when updating
OpenFOAM libraries.

3.2.4

Compilation example: the pisoFoam application

The source code for application pisoFoam is in the $FOAM APP/solvers/incompressible/pisoFoam
directory and the top level source file is named pisoFoam.C. The pisoFoam.C source code
is:
1
2
3
4

/*---------------------------------------------------------------------------*\
=========
|
\\
/ F ield
| OpenFOAM: The Open Source CFD Toolbox
\\
/
O peration
|

Open∇FOAM-1.6

U-77

3.2 Compiling applications and libraries
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85
86
87
88

\\ /
A nd
| Copyright (C) 1991-2009 OpenCFD Ltd.
\\/
M anipulation |
------------------------------------------------------------------------------License
This file is part of OpenFOAM.
OpenFOAM is free software; you can redistribute it and/or modify it
under the terms of the GNU General Public License as published by the
Free Software Foundation; either version 2 of the License, or (at your
option) any later version.
OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License
for more details.
You should have received a copy of the GNU General Public License
along with OpenFOAM; if not, write to the Free Software Foundation,
Inc., 51 Franklin St, Fifth Floor, Boston, MA 02110-1301 USA
Application
pisoFoam
Description
Transient solver for incompressible flow.
Turbulence modelling is generic, i.e. laminar, RAS or LES may be selected.
\*---------------------------------------------------------------------------*/
#include "fvCFD.H"
#include "singlePhaseTransportModel.H"
#include "turbulenceModel.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
int main(int argc, char *argv[])
{
#include "setRootCase.H"
#include
#include
#include
#include

"createTime.H"
"createMesh.H"
"createFields.H"
"initContinuityErrs.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Info<< "\nStarting time loop\n" << endl;
while (runTime.loop())
{
Info<< "Time = " << runTime.timeName() << nl << endl;
#include "readPISOControls.H"
#include "CourantNo.H"
// Pressure-velocity PISO corrector
{
// Momentum predictor
fvVectorMatrix UEqn
(
fvm::ddt(U)
+ fvm::div(phi, U)
+ turbulence->divDevReff(U)
);
UEqn.relax();
if (momentumPredictor)
{
solve(UEqn == -fvc::grad(p));
}
// --- PISO loop
for (int corr=0; corrcorrect();
runTime.write();

}

Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
<< " ClockTime = " << runTime.elapsedClockTime() << " s"
<< nl << endl;

Info<< "End\n" << endl;
}

return 0;

// ************************************************************************* //

The code begins with a brief description of the application contained within comments
over 1 line (//) and multiple lines (/*...*/). Following that, the code contains several
# include statements, e.g.# include "fvCFD.H", which causes the compiler to suspend
reading from the current file, pisoFoam.C to read the fvCFD.H.
pisoFoam resources the cfdTools, incompressibleRASModels and incompressibleTransportModels libraries and therefore requires the necessary header files, specified by the EXE INC
= -I... option, and links to the libraries with the EXE LIBS = -l... option. The
Make/options therefore contains the following:
1
2
3
4
5
6
7
8
9
10
11
12

EXE_INC = \
-I$(LIB_SRC)/turbulenceModels/incompressible/turbulenceModel \
-I$(LIB_SRC)/transportModels \
-I$(LIB_SRC)/transportModels/incompressible/singlePhaseTransportModel \
-I$(LIB_SRC)/finiteVolume/lnInclude
EXE_LIBS = \
-lincompressibleRASModels \
-lincompressibleLESModels \
-lincompressibleTransportModels \
-lfiniteVolume \
-lmeshTools

Open∇FOAM-1.6

3.2 Compiling applications and libraries

U-79

pisoFoam contains only the pisoFoam.C source and the executable is written to the $FOAM APPBIN
directory as all standard applications are. The Make/files therefore contains:
1
2
3

pisoFoam.C
EXE = $(FOAM_APPBIN)/pisoFoam

The user can compile pisoFoam by going to the $FOAM CFD/pisoFoam directory and
typing:
wmake
The code should compile and produce a message similar to the following
Making dependency list for source file pisoFoam.C
SOURCE DIR=.
SOURCE=pisoFoam.C ;
g++ -DFOAM EXCEPTION -Dlinux -DlinuxOptMPICH
-DscalarMachine -DoptSolvers -DPARALLEL -DUSEMPI -Wall -O2 -DNoRepository
-ftemplate-depth-17 -I.../OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude
-IlnInclude
-I.
......
-lmpich -L/usr/X11/lib -lm
-o .../OpenFOAM/OpenFOAM-1.6/applications/bin/linuxOptMPICH/pisoFoam

The user can now try recompiling and will receive a message similar to the following to
say that the executable is up to date and compiling is not necessary:
make: Nothing to be done for ‘allFiles’.
make: ‘Make/linuxOptMPICH/dependencies’ is up to date.
make: ‘.../OpenFOAM/OpenFOAM-1.6/applications/bin/linuxOptMPICH/pisoFoam’
is up to date.

The user can compile the application from scratch by removing the dependency list with
wclean
and running wmake.

3.2.5

Debug messaging and optimisation switches

OpenFOAM provides a system of messaging that is written during runtime, most of which
are to help debugging problems encountered during running of a OpenFOAM case. The
switches are listed in the $WM PROJECT DIR/etc/controlDict file; should the user wish
to change the settings they should make a copy to their $HOME directory, i.e.$HOME/.OpenFOAM/1.6/controlDict file. The list of possible switches is extensive and can be
viewed by running the foamDebugSwitches

U-80

Applications and libraries

fileModificationSkew. OpenFOAM scans the write time of data files to check for modification. When running over a NFS with some disparity in the clock settings on different
machines, field data files appear to be modified ahead of time. This can cause a problem
if OpenFOAM views the files as newly modified and attempting to re-read this data. The
fileModificationSkew keyword is the time in seconds that OpenFOAM will subtract
from the file write time when assessing whether the file has been newly modified.
High level debugging switches - sub-dictionary DebugSwitches
level
Overall level of debugging messaging for OpenFOAM- - 3 levels 0,
1, 2
lduMatrix
Messaging for solver convergence during a run - 3 levels 0, 1, 2
Optimisation switches - sub-dictionary OptimisationSwitches
fileModificA time in seconds that should be set higher than the maximum
ationSkew
delay in NFS updates and clock difference for running OpenFOAM
over a NFS.
nProcsSimpleSum Optimises global sum for parallel processing; sets number of processors above which hierarchical sum is performed rather than a
linear sum (default 16)
Table 3.3: Runtime message switches.

3.2.6

Linking new user-defined libraries to existing applications

The situation may arise that a user creates a new library, say new, and wishes the features
within that library to be available across a range of applications. For example, the
user may create a new boundary condition, compiled into new, that would need to be
recognised by a range of solver applications, pre- and post-processing utilities, mesh tools,
etc. Under normal circumstances, the user would need to recompile every application with
the new linked to it.
Instead there is a simple mechanism to link one or more shared object libraries dynamically at run-time in OpenFOAM. Simply add the optional keyword entry libs to
the controlDict file for a case and enter the full names of the libraries within a list (as
quoted string entries). For example, if a user wished to link the libraries new1 and new2
at run-time, they would simply need to add the following to the case controlDict file:
libs
(
"libnew1.so"
"libnew2.so"
);

3.3

Running applications

Each application is designed to be executed from a terminal command line, typically
reading and writing a set of data files associated with a particular case. The data files
for a case are stored in a directory named after the case as described in section 4.1; the
directory name with full path is here given the generic name .
Open∇FOAM-1.6

3.4 Running applications in parallel

U-81

For any application, the form of the command line entry for any can be found by
simply entering the application name at the command line with the -help option, e.g.
typing
blockMesh -help
returns the usage
Usage: blockMesh [-region region name] [-case dir] [-blockTopology]
[-help] [-doc] [-srcDoc]
The arguments in square brackets, [ ], are optional flags. If the application is executed from within a case directory, it will operate on that case. Alternatively, the -case
option allows the case to be specified directly so that the application can be
executed from anywhere in the filing system.
Like any UNIX/Linux executable, applications can be run as as a background process,
i.e. one which does not have to be completed before the user can give the shell additional
commands. If the user wished to run the blockMesh example as a background process
and output the case progress to a log file, they could enter:
blockMesh > log &

3.4

Running applications in parallel

This section describes how to run OpenFOAM in parallel on distributed processors. The
method of parallel computing used by OpenFOAM is known as domain decomposition, in
which the geometry and associated fields are broken into pieces and allocated to separate
processors for solution. The process of parallel computation involves: decomposition of
mesh and fields; running the application in parallel; and, post-processing the decomposed
case as described in the following sections. The parallel running uses the public domain
openMPI implementation of the standard message passing interface (MPI).

3.4.1

Decomposition of mesh and initial field data

The mesh and fields are decomposed using the decomposePar utility. The underlying
aim is to break up the domain with minimal effort but in such a way to guarantee a
fairly economic solution. The geometry and fields are broken up according to a set of
parameters specified in a dictionary named decomposeParDict that must be located in
the system directory of the case of interest. An example decomposeParDict dictionary can
be copied from the interFoam/damBreak tutorial if the user requires one; the dictionary
entries within it are reproduced below:
17
18
19
20
21
22
23
24
25
26
27
28
29
30

numberOfSubdomains 4;
method

simple;

simpleCoeffs
{
n
delta
}
hierarchicalCoeffs
{
n

( 2 2 1 );
0.001;

( 1 1 1 );

Open∇FOAM-1.6

U-82

Applications and libraries
delta
order

31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50

0.001;
xyz;

}
metisCoeffs
{
processorWeights ( 1 1 1 1 );
}
manualCoeffs
{
dataFile
}

"";

distributed

no;

roots

( );

// ************************************************************************* //

The user has a choice of four methods of decomposition, specified by the method keyword
as described below.
simple Simple geometric decomposition in which the domain is split into pieces by direction, e.g. 2 pieces in the x direction, 1 in y etc.
hierarchical

U-83

3.4 Running applications in parallel

Compulsory entries
numberOfSubdomains Total number of subdomains
method
Method of decomposition

simpleCoeffs entries
n
Number of subdomains in x, y, z
delta
Cell skew factor
hierarchicalCoeffs
n
delta
order

entries
Number of subdomains in x, y, z
Cell skew factor
Order of decomposition

N
simple/
hierarchical/
scotch/
metis/
manual/

(nx ny nz )
Typically, 10−3

(nx ny nz )
Typically, 10−3
xyz/xzy/yxz. . .

scotchCoeffs entries
processorWeights
List of weighting factors for allocation (...)
of cells to processors; is the
weighting factor for processor 1, etc.;
weights are normalised so can take any
range of values.
strategy
Decomposition strategy; defaults to
"b"
metisCoeffs entries
processorWeights
As above

(...)

manualCoeffs entries
dataFile
Name of file containing data of alloca- ""
tion of cells to processors
Distributed data entries (optional) — see section 3.4.3
distributed
Is the data distributed across several yes/no
disks?
roots
Root paths to case directories; (...)
is the root path for node 1, etc.
Table 3.4: Keywords in decompositionDict dictionary.

3.4.2

Running a decomposed case

A decomposed OpenFOAM case is run in parallel using the openMPI implementation of
MPI.
openMPI can be run on a local multiprocessor machine very simply but when running on machines across a network, a file must be created that contains the host names
of the machines. The file can be given any name and located at any path. In the following description we shall refer to such a file by the generic name, including full path,
.
The file contains the names of the machines listed one machine per line.
Open∇FOAM-1.6

U-84

Applications and libraries

The names must correspond to a fully resolved hostname in the /etc/hosts file of the
machine on which the openMPI is run. The list must contain the name of the machine
running the openMPI. Where a machine node contains more than one processor, the node
name may be followed by the entry cpu=n where n is the number of processors openMPI
should run on that node.
For example, let us imagine a user wishes to run openMPI from machine aaa on the
following machines: aaa; bbb, which has 2 processors; and ccc. The would
contain:
aaa
bbb cpu=2
ccc
An application is run in parallel using mpirun.
mpirun --hostfile -np
-parallel > log &
where: is the number of processors; is the executable, e.g.icoFoam;
and, the output is redirected to a file named log. For example, if icoFoam is run on 4
nodes, specified in a file named machines, on the cavity tutorial in the $FOAM RUN/tutorials/incompressible/icoFoam directory, then the following command should be executed:
mpirun --hostfile machines -np 4 icoFoam -parallel > log &

3.4.3

Distributing data across several disks

Data files may need to be distributed if, for example, if only local disks are used in
order to improve performance. In this case, the user may find that the root path to the
case directory may differ between machines. The paths must then be specified in the
decomposeParDict dictionary using distributed and roots keywords. The distributed
entry should read
distributed

yes;

and the roots entry is a list of root paths, , , . . . , for each node
roots

(
""
""
...
);
where is the number of roots.
Each of the processorN directories should be placed in the case directory at each of
the root paths specified in the decomposeParDict dictionary. The system directory and
files within the constant directory must also be present in each case directory. Note: the
files in the constant directory are needed, but the polyMesh directory is not.
Open∇FOAM-1.6

U-85

3.5 Standard solvers

3.4.4

Post-processing parallel processed cases

When post-processing cases that have been run in parallel the user has two options:
• reconstruction of the mesh and field data to recreate the complete domain and fields,
which can be post-processed as normal;
• post-processing each segment of decomposed domain individually.
3.4.4.1

Reconstructing mesh and data

After a case has been run in parallel, it can be reconstructed for post-processing. The case
is reconstructed by merging the sets of time directories from each processorN directory into
a single set of time directories. The reconstructPar utility performs such a reconstruction
by executing the command:
reconstructPar
When the data is distributed across several disks, it must be first copied to the local case
directory for reconstruction.
3.4.4.2

Post-processing decomposed cases

The user may post-process decomposed cases using the paraFoam post-processor, described in section 6.1. The whole simulation can be post-processed by reconstructing the
case or alternatively it is possible to post-process a segment of the decomposed domain
individually by simply treating the individual processor directory as a case in its own
right.

3.5

Standard solvers

The solvers with the OpenFOAM distribution are in the $FOAM SOLVERS directory,
reached quickly by typing app at the command line. This directory is further subdivided
into several directories by category of continuum mechanics, e.g. incompressible flow,
combustion and solid body stress analysis. Each solver is given a name that is reasonably
descriptive, e.g.icoFoam solves incompressible, laminar flow. The current list of solvers
distributed with OpenFOAM is given in Table 3.5.
‘Basic’ CFD codes
laplacianFoam
potentialFoam
scalarTransportFoam

Solves a simple Laplace equation, e.g. for thermal diffusion
in a solid
Simple potential flow solver which can be used to generate
starting fields for full Navier-Stokes codes
Solves a transport equation for a passive scalar

Incompressible flow
boundaryFoam
Steady-state solver for 1D turbulent flow, typically to generate
boundary layer conditions at an inlet, for use in a simulation
channelFoam
Incompressible LES solver for flow in a channel
icoFoam
Transient solver for incompressible, laminar flow of Newtonian
fluids
Continued on next page
Open∇FOAM-1.6

U-86

Applications and libraries

Continued from previous page

nonNewtonianIcoFoam
pimpleDyMFoam

pimpleFoam
pisoFoam
shallowWaterFoam
simpleFoam
Compressible flow
rhoCentralFoam
rhoPimpleFoam
rhoPisoFoam
rhoPorousSimpleFoam

rhopSonicFoam
rhoSimpleFoam
rhoSonicFoam
sonicDyMFoam
sonicFoam
sonicLiquidFoam

Multiphase flow
bubbleFoam
cavitatingFoam
compressibleInterDyMFoam

compressibleInterFoam

interDyMFoam

Transient solver for incompressible, laminar flow of nonNewtonian fluids
Transient solver for incompressible, flow of Newtonian fluids on a moving mesh using the PIMPLE (merged PISOSIMPLE) algorithm
Large time-step transient solver for incompressible, flow using
the PIMPLE (merged PISO-SIMPLE) algorithm
Transient solver for incompressible flow
Transient solver for inviscid shallow-water equations with rotation
Steady-state solver for incompressible, turbulent flow

Density-based compressible flow solver based on centralupwind schemes of Kurganov and Tadmor
Transient solver for laminar or turbulent flow of compressible
fluids for HVAC and similar applications
Transient PISO solver for compressible, laminar or turbulent
flow
Steady-state solver for turbulent flow of compressible fluids
with RANS turbulence modelling, and implicit or explicit
porosity treatment
Pressure-density-based compressible flow solver
Steady-state SIMPLE solver for laminar or turbulent RANS
flow of compressible fluids
Density-based compressible flow solver
Transient solver for trans-sonic/supersonic, laminar or turbulent flow of a compressible gas with mesh motion
Transient solver for trans-sonic/supersonic, laminar or turbulent flow of a compressible gas
Transient solver for trans-sonic/supersonic, laminar flow of a
compressible liquid

Solver for a system of 2 incompressible fluid phases with one
phase dispersed, e.g. gas bubbles in a liquid
Transient cavitation code based on the barotropic equation of
state
Solver for 2 compressible, isothermal immiscible fluids using a
VOF (volume of fluid) phase-fraction based interface capturing approach, with optional mesh motion and mesh topology
changes including adaptive re-meshing
Solver for 2 compressible, isothermal immiscible fluids using
a VOF (volume of fluid) phase-fraction based interface capturing approach
Solver for 2 incompressible, isothermal immiscible fluids using
a VOF (volume of fluid) phase-fraction based interface capturing approach, with optional mesh motion and mesh topology
changes including adaptive re-meshing
Continued on next page

Open∇FOAM-1.6

U-87

3.5 Standard solvers
Continued from previous page

interFoam

Solver for 2 incompressible, isothermal immiscible fluids using a VOF (volume of fluid) phase-fraction based interface
capturing approach
interPhaseChangeFoam Solver for 2 incompressible, isothermal immiscible fluids with
phase-change (e.g. cavitation). Uses a VOF (volume of fluid)
phase-fraction based interface capturing approach
multiphaseInterFoam
Solver for n incompressible fluids which captures the interfaces
and includes surface-tension and contact-angle effects for each
phase
settlingFoam
Solver for 2 incompressible fluids for simulating the settling
of the dispersed phase
twoLiquidMixingFoam
Solver for mixing 2 incompressible fluids
twoPhaseEulerFoam
Solver for a system of 2 incompressible fluid phases with one
phase dispersed, e.g. gas bubbles in a liquid
Direct numerical simulation (DNS)
dnsFoam
Direct numerical simulation solver for boxes of isotropic turbulence
Combustion
coldEngineFoam
dieselEngineFoam
dieselFoam
engineFoam
PDRFoam
reactingFoam
rhoReactingFoam
XiFoam

Solver for cold-flow in internal combustion engines
Solver for diesel engine spray and combustion
Solver for diesel spray and combustion
Solver for internal combustion engines
Solver for compressible premixed/partially-premixed combustion with turbulence modelling
Solver for combustion with chemical reactions
Solver for combustion with chemical reactions using density
based thermodynamics package
Solver for compressible premixed/partially-premixed combustion with turbulence modelling

Heat transfer and buoyancy-driven flows
buoyantBoussinesqPiTransient solver for buoyant, turbulent flow of incompressible
soFoam
fluids

U-88

Applications and libraries

Continued from previous page

coalChemistryFoam
porousExplicitSourceReactingParcelFoam
reactingParcelFoam
uncoupledKinematicParcelFoam

Transient solver for compressible, turbulent flow with coal and
limestone parcel injections, and combustion
Transient PISO solver for compressible, laminar or turbulent
flow with reacting Lagrangian parcels for porous media, including explicit sources
Transient PISO solver for compressible, laminar or turbulent
flow with reacting Lagrangian parcels
Transient solver for the passive transport of a single kinematic
particle could

Molecular dynamics methods
mdEquilibrationFoam
Equilibrates and/or preconditions molecular dynamics systems
mdFoam
Molecular dynamics solver for fluid dynamics
Direct simulation Monte Carlo methods
dsmcFoam
Direct simulation Monte Carlo (DSMC) solver for 3D, transient, multi- species flows
Electromagnetics
electrostaticFoam
mhdFoam

Solver for electrostatics
Solver for magnetohydrodynamics (MHD): incompressible,
laminar flow of a conducting fluid under the influence of a
magnetic field

Stress analysis of solids
solidDisplacementTransient segregated finite-volume solver of linear-elastic,
Foam
small-strain deformation of a solid body, with optional thermal diffusion and thermal stresses
solidEquilibriumDisSteady-state segregated finite-volume solver of linear-elastic,
placementFoam
small-strain deformation of a solid body, with optional thermal diffusion and thermal stresses
Finance
financialFoam

Solves the Black-Scholes equation to price commodities
Table 3.5: Standard library solvers.

U-89

3.6 Standard utilities
Continued from previous page

Pre-processing
applyBoundaryLayer

Apply a simplified boundary-layer model to the velocity and
turbulence fields based on the 1/7th power-law
applyWallFunctionUpdates OpenFOAM RAS cases to use the new wall function
BoundaryConditions
framework Attempts to determine whether case is compressible or incompressible, or can be supplied with -compressible
command line argument
boxTurb
Makes a box of turbulence which conforms to a given energy
spectrum and is divergence free
changeDictionary
Utility to change dictionary entries, e.g. can be used to change
the patch type in the field and polyMesh/boundary files
dsmcInitialise
Initialise a case for dsmcFoam by reading the initialisation
dictionary system/dsmcInitialise
engineSwirl
Generates a swirling flow for engine calulations
foamUpgradeFvSolution Simple tool to upgrade the syntax of system/fvSolution::solvers
mapFields
Maps volume fields from one mesh to another, reading and
interpolating all fields present in the time directory of both
cases. Parallel and non-parallel cases are handled without the
need to reconstruct them first
mdInitialise
Initialises fields for a molecular dynamics (MD) simulation
setFields
Selects a cell set through a dictionary
Mesh generation
blockMesh
extrude2DMesh

extrudeMesh
snappyHexMesh
Mesh conversion
ansysToFoam
cfx4ToFoam
fluent3DMeshToFoam
fluentMeshToFoam
foamMeshToFluent
foamToStarMesh
gambitToFoam
gmshToFoam
ideasUnvToFoam
kivaToFoam
mshToFoam
netgenNeutralToFoam
plot3dToFoam

A multi-block mesh generator
Takes 2D mesh (all faces 2 points only, no front and back
faces) and creates a 3D mesh by extruding with specified
thickness
Extrude mesh from existing patch (by default outwards facing
normals; optional flips faces) or from patch read from file
Automatic split hex mesher. Refines and snaps to surface

Converts an ANSYS input mesh file, exported from I-DEAS,
to OpenFOAM format
Converts a CFX 4 mesh to OpenFOAM format
Converts a Fluent mesh to OpenFOAM format
Converts a Fluent mesh to OpenFOAM format including multiple region and region boundary handling
Writes out the OpenFOAM mesh in Fluent mesh format
Reads an OpenFOAM mesh and writes a PROSTAR (v4)
bnd/cel/vrt format
Converts a GAMBIT mesh to OpenFOAM format
Reads .msh file as written by Gmsh
I-Deas unv format mesh conversion
Converts a KIVA grid to OpenFOAM format
Converts .msh file generated by the Adventure system
Converts neutral file format as written by Netgen v4.4
Plot3d mesh (ascii/formatted format) converter
Continued on next page

Open∇FOAM-1.6

U-90

Applications and libraries

Continued from previous page

polyDualMesh
sammToFoam
star4ToFoam
starToFoam
tetgenToFoam
writeMeshObj

Calculate the dual of a polyMesh. Adheres to all the feature
and patch edges
Converts a STAR-CD SAMM mesh to OpenFOAM format
Converts a STAR-CD (v4) PROSTAR mesh into OpenFOAM
format
Converts a STAR-CD PROSTAR mesh into OpenFOAM format
Converts .ele and .node and .face files, written by tetgen
For mesh debugging: writes mesh as three separate OBJ files
which can be viewed with e.g. javaview

Mesh manipulation
attachMesh
Attach topologically detached mesh using prescribed mesh
modifiers
autoPatch
Divides external faces into patches based on (user supplied)
feature angle
cellSet
Selects a cell set through a dictionary
checkMesh
Checks validity of a mesh
createBaffles
Makes internal faces into boundary faces. Does not duplicate
points, unlike mergeOrSplitBaffles
createPatch
Utility to create patches out of selected boundary faces. Faces
come either from existing patches or from a faceSet
deformedGeom
Deforms a polyMesh using a displacement field U and a scaling
factor supplied as an argument
faceSet
Selects a face set through a dictionary
flattenMesh
Flattens the front and back planes of a 2D cartesian mesh
insideCells
Picks up cells with cell centre ’inside’ of surface. Requires
surface to be closed and singly connected
mergeMeshes
Merge two meshes
mergeOrSplitBaffles
Detects faces that share points (baffles). Either merge them
or duplicate the points
mirrorMesh
Mirrors a mesh around a given plane
moveDynamicMesh
Mesh motion and topological mesh changes utility
moveEngineMesh
Solver for moving meshes for engine calculations.
moveMesh
Solver for moving meshes
objToVTK
Read obj line (not surface!) file and convert into vtk
pointSet
Selects a point set through a dictionary
refineMesh
Utility to refine cells in multiple directions
renumberMesh
Renumbers the cell list in order to reduce the bandwidth,
reading and renumbering all fields from all the time directories
rotateMesh
Rotates the mesh and fields from the direcion n1 to the direction n2
setSet
Manipulate a cell/face/point set interactively
setsToZones
Add pointZones/faceZones/cellZones to the mesh from similar
named pointSets/faceSets/cellSets
splitMesh
Splits mesh by making internal faces external. Uses attachDetach
splitMeshRegions
Splits mesh into multiple regions
stitchMesh
’Stitches’ a mesh
Continued on next page
Open∇FOAM-1.6

U-91

3.6 Standard utilities
Continued from previous page

subsetMesh
transformPoints
zipUpMesh

Other mesh tools
autoRefineMesh
collapseEdges
combinePatchFaces

modifyMesh
refineHexMesh
refinementLevel
refineWallLayer
removeFaces
selectCells
splitCells

Selects a section of mesh based on a cellSet
Transforms the mesh points in the polyMesh directory according to the translate, rotate and scale options
Reads in a mesh with hanging vertices and zips up the cells
to guarantee that all polyhedral cells of valid shape are closed

Utility to refine cells near to a surface
Collapse short edges and combines edges that are in line
Checks for multiple patch faces on same cell and combines
them. These result from e.g. refined neighbouring cells getting removed, leaving 4 exposed faces with same owner
Manipulates mesh elements
Refines a hex mesh by 2x2x2 cell splitting
Tries to figure out what the refinement level is on refined
cartesian meshes. Run before snapping
Utility to refine cells next to patches
Utility to remove faces (combines cells on both sides)
Select cells in relation to surface
Utility to split cells with flat faces

Post-processing graphics
ensightFoamReader
EnSight library module to read OpenFOAM data directly
without translation
fieldview9Reader
Reader module for Fieldview 9 to read OpenFOAM mesh and
data
PV3FoamReader
ParaView 3 reader module
PVFoamReader
ParaView reader module
Post-processing data
foamDataToFluent
foamToEnsight
foamToEnsightParts
foamToFieldview9
foamToGMV
foamToVTK
smapToFoam

converters
Translates OpenFOAM data to Fluent format
Translates OpenFOAM data to EnSight format
Translates OpenFOAM data to Ensight format. An Ensight
part is created for each cellZone and patch
Write out the OpenFOAM mesh in Version 3.0 Fieldview-UNS
format (binary)
Translates foam output to GMV readable files
Legacy VTK file format writer
Translates a STAR-CD SMAP data file into OpenFOAM field
format

Post-processing velocity fields
Co
Configurable graph drawing program
enstrophy
Calculates and writes the enstrophy of the velocity field U
flowType
Calculates and writes the flowType of velocity field U
Lambda2
Calculates and writes the second largest eigenvalue of the sum
of the square of the symmetrical and anti-symmetrical parts
of the velocity gradient tensor
Continued on next page
Open∇FOAM-1.6

U-92

Applications and libraries

Continued from previous page

Mach
Pe
Q
streamFunction
uprime
vorticity

Calculates and optionally writes the local Mach number from
the velocity field U at each time
Calculates
and
writes
the
Pe
number
as
a
surfaceScalarField obtained from field phi
Calculates and writes the second invariant of the velocity gradient tensor
Calculates and writes the stream function of velocity field U
at each time
p
Calculates and writes the scalar field of uprime ( 2k/3)
Calculates and writes the vorticity of velocity field U

Post-processing stress fields
stressComponents
Calculates and writes the scalar fields of the six components
of the stress tensor sigma for each time
Post-processing scalar fields
pPrime2
Calculates and writes the scalar field of pPrime2 ([p − p]2 ) at
each time
Post-processing at walls
wallGradU
Calculates and writes the gradient of U at the wall
wallHeatFlux
Calculates and writes the heat flux for all patches as the
boundary field of a volScalarField and also prints the integrated flux for all wall patches
wallShearStress
Calculates and writes the wall shear stress, for the specified
times
yPlusLES
Calculates and reports yPlus for all wall patches, for the specified times
yPlusRAS
Calculates and reports yPlus for all wall patches, for the specified times
Post-processing turbulence
createTurbulenceFields Creates a full set of turbulence fields
R
Calculates and writes the Reynolds stress R for the current
time step
Post-processing patch data
patchAverage
Calculates the average of the specified field over the specified
patch
patchIntegrate
Calculates the integral of the specified field over the specified
patch
Post-processing Lagrangian simulation
particleTracks
Generates a VTK file of particle tracks for cases that were
computed using a tracked-parcel-type cloud
Sampling post-processing
probeLocations
Probe locations
Continued on next page
Open∇FOAM-1.6

U-93

3.6 Standard utilities
Continued from previous page

sample

Sample field data with a choice of interpolation schemes, sampling options and write formats

Miscellaneous post-processing
dsmcFieldsCalc
Calculate intensive fields (U and T) from averaged extensive
fields from a DSMC calculation
engineCompRatio
Calculate the geometric compression ratio. Note that if you
have valves and/or extra volumes it will not work, since it
calculates the volume at BDC and TCD
execFlowFunctionObjects Execute the set of functionObjects specified in the selected
dictionary (which defaults to system/controlDict) for the selected set of times
pdfPlot
Generates an .obj file to plot a probability distribution function
postChannel
Post-processes data from channel flow calculations
ptot
For each time: calculate the total pressure
wdot
Calculates and writes wdot for each time
writeCellCentres
Write the three components of the cell centres as
volScalarFields so they can be used in postprocessing in
thresholding
Parallel processing
decomposePar
reconstructPar
reconstructParMesh
redistributeMeshPar

Automatically decomposes a mesh and fields of a case for
parallel execution of OpenFOAM
Reconstructs a mesh and fields of a case that is decomposed
for parallel execution of OpenFOAM
Reconstructs a mesh using geometric information only
Redistributes existing decomposed mesh and fields according
to the current settings in the decomposeParDict file

Thermophysical-related utilities
adiabaticFlameT
Calculates the adiabatic flame temperature for a given fuel
over a range of unburnt temperatures and equivalence ratios
chemkinToFoam
Converts CHEMKIN 3 thermodynamics and reaction data files
into OpenFOAM format
equilibriumCO
Calculates the equilibrium level of carbon monoxide
equilibriumFlameT
Calculates the equilibrium flame temperature for a given fuel
and pressure for a range of unburnt gas temperatures and
equivalence ratios; the effects of dissociation on O2 , H2 O and
CO2 are included
mixtureAdiabaticFlameT Calculates the adiabatic flame temperature for a given mixture at a given temperature
Error estimation
estimateScalarError
icoErrorEstimate

Estimates the error in the solution for a scalar transport equation in the standard form
Estimates error for the incompressible laminar CFD application icoFoam
Continued on next page
Open∇FOAM-1.6

U-94

Applications and libraries

Continued from previous page

icoMomentError
momentScalarError

Estimates error for the incompressible laminar CFD application icoFoam
Estimates the error in the solution for a scalar transport equation in the standard form

Miscellaneous utilities
expandDictionary
Read the dictionary provided as an argument, expand the
macros etc. and write the resulting dictionary to standard
output
foamDebugSwitches
Write out all library debug switches
foamFormatConvert
Converts all IOobjects associated with a case into the format
specified in the controlDict
foamInfoExec
Interrogates a case and prints information to screen
patchSummary
Writes fields and boundary condition info for each patch at
each requested time instance
Table 3.6: Standard library utilities.

3.7

Standard libraries

The libraries with the OpenFOAM distribution are in the $FOAM LIB/$WM OPTIONS
directory, reached quickly by typing lib at the command line. Again, the names are
prefixed by lib and reasonably descriptive, e.g.incompressibleTransportModels contains
the library of incompressible transport models. For ease of presentation, the libraries are
separated into two types:
General libraries those that provide general classes and associated functions listed in
Table 3.7;
Model libraries those that specify models used in computational continuum mechanics,
listed in Table 3.8, Table 3.9 and Table 3.10.

Library of basic OpenFOAM tools — OpenFOAM
algorithms
Algorithms
containers
Container classes
db
Database classes
dimensionedTypes
dimensioned class and derivatives
dimensionSet
dimensionSet class
fields
Field classes
global
Global settings
graph
graph class
interpolations
Interpolation schemes
matrices
Matrix classes
memory
Memory management tools
meshes
Mesh classes
primitives
Primitive classes
Continued on next page
Open∇FOAM-1.6

3.7 Standard libraries

U-95

Continued from previous page

Finite volume method library — finiteVolume
cfdTools
CFD tools
fields
Volume, surface and patch field classes; includes boundary
conditions
finiteVolume
Finite volume discretisation
fvMatrices
Matrices for finite volume solution
fvMesh
Meshes for finite volume discretisation
interpolation
Field interpolation and mapping
surfaceMesh
Mesh surface data for finite volume discretisation
Mesh volume (cell) data for finite volume discretisation
Post-processing libraries
fieldFunctionObjects
Field function objects including field averaging, min/max, etc.
foamCalcFunctions
Functions for the foamCalc utility
forces
Tools for post-processing force/lift/drag data with function
objects
postCalc
For using functionality of a function object as a postprocessing activity
sampling
Tools for sampling field data at prescribed locations in a domain
systemCall
General function object for making system calls while running
a case
utilityFunctionObjects
Utility function objects
Solution and mesh manipulation libraries
autoMesh
Library of functionality for the snappyHexMesh utility
dynamicMesh
For solving systems with moving meshes
dynamicFvMesh
Library for a finite volume mesh that can move and undergo
topological changes
edgeMesh
For handling edge-based mesh descriptions
errorEstimation
Error estimation tools
fvMotionSolver
Finite volume mesh motion solvers
ODE
Solvers for ordinary differential equations
meshTools
Tools for handling a OpenFOAM mesh
surfMesh
Library for handling surface meshes of different formats
triSurface
For handling standard triangulated surface-based mesh descriptions
topoChangerFvMesh
Topological changes functionality (largely redundant)
Lagrangian particle
coalCombustion
dieselSpray
dsmc
lagrangian
lagrangianIntermediate

tracking libraries
Coal dust combustion modelling
Diesel spray and injection modelling
Direct simulation Monte Carlo method modelling
Basic Lagrangian, or particle-tracking, solution scheme
Particle-tracking kinematics, thermodynamics, multispecies
reactions, particle forces, etc.
potential
Intermolecular potentials for molecular dynamics
molecule
Molecule classes for molecular dynamics
molecularMeasurements For making measurements in molecular dynamics
Continued on next page
Open∇FOAM-1.6

U-96

Applications and libraries

Continued from previous page

solidParticle

Solid particle implementation

Miscellaneous libraries
conversion
Tools for mesh and data conversions
decompositionMethods Tools for domain decomposition
engine
Tools for engine calculations
MGridGenGAMGAgglomeration
Library for cell agglomeration using the MGridGen algorithm
OSspecific
Operating system specific functions
randomProcesses
Tools for analysing and generating random processes
Table 3.7: Shared object libraries for general use.

Basic thermophysical models — basicThermophysicalModels
hPsiThermo
General thermophysical model calculation based on enthalpy h and compressibility ψ
ePsiThermo
General thermophysical model calculation based on internal energy e and compressibility ψ
hRhoThermo
General thermophysical model calculation based on enthalpy h
pureMixture

General thermophysical model calculation for passive gas
mixtures

Reaction models — reactionThermophysicalModels
hPsiMixtureThermo
Calculates enthalpy for combustion mixture based on ψ
hRhoMixtureThermo
Calculates enthalpy for combustion mixture based on ρ
hhuMixtureThermo
Calculates enthalpy for unburnt gas and combustion mixture
homogeneousMixture

Combustion mixture based on normalised fuel mass fraction b
inhomogeneousMixture
Combustion mixture based on b and total fuel mass fraction
ft
veryInhomogeneousMixture Combustion mixture based on b, ft and unburnt fuel mass
fraction fu
dieselMixture
Combustion mixture based on ft and fu
basicMultiComponentBasic mixture based on multiple components
Mixture
multiComponentMixture
Derived mixture based on multiple components
reactingMixture
Combustion mixture using thermodynamics and reaction
schemes
egrMixture
Exhaust gas recirculation mixture

Radiation models — radiation
P1
P1 model
fvDOM
Finite volume discrete ordinate method
Continued on next page
Open∇FOAM-1.6

U-97

3.7 Standard libraries
Continued from previous page

Laminar flame speed models — laminarFlameSpeedModels
constLaminarFlameSpeed Constant laminar flame speed
GuldersLaminarFlameSpeed Gülder’s laminar flame speed model
GuldersEGRLaminarGülder’s laminar flame speed model with exhaust gas reFlameSpeed
circulation modelling
Barotropic compressibility models — barotropicCompressibilityModels
linear
Linear compressibility model
Chung
Chung compressibility model
Wallis
Wallis compressibility model
Thermophysical properties of gaseous species — specie
icoPolynomial
Incompressible polynomial equation of state, e.g. for liquids
perfectGas
Perfect gas equation of state
eConstThermo
Constant specific heat cp model with evaluation of internal
energy e and entropy s
hConstThermo
Constant specific heat cp model with evaluation of enthalpy
h and entropy s
hPolynomialThermo
cp evaluated by a function with coefficients from polynomials, from which h, s are evaluated
janafThermo
cp evaluated by a function with coefficients from JANAF
thermodynamic tables, from which h, s are evaluated
specieThermo
Thermophysical properties of species, derived from cp , h
and/or s
constTransport
Constant transport properties
polynomialTransport
Polynomial based temperature-dependent transport properties
sutherlandTransport
Sutherland’s formula for temperature-dependent transport
properties
Functions/tables of thermophysical properties — thermophysicalFunctions
NSRDSfunctions
National Standard Reference Data System (NSRDS) American Institute of Chemical Engineers (AICHE) data
compilation tables
APIfunctions
American Petroleum Institute (API) function for vapour
mass diffusivity
Probability density functions — pdf
RosinRammler
Rosin-Rammler distribution
normal
Normal distribution
uniform
Uniform distribution
exponential
Exponential distribution
general
General distribution
Chemistry model — chemistryModel
chemistryModel
Chemical reaction model
chemistrySolver
Chemical reaction solver
Continued on next page
Open∇FOAM-1.6

U-98

Applications and libraries

Continued from previous page

Other libraries
liquids
liquidMixture
solids
solidMixture

Thermophysical
Thermophysical
Thermophysical
Thermophysical

properties
properties
properties
properties

of
of
of
of

liquids
liquid mixtures
solids
solid mixtures

Table 3.8: Libraries of thermophysical models.

RAS turbulence models for incompressible fluids — incompressibleRASModels
laminar
Dummy turbulence model for laminar flow
kEpsilon
Standard high-Re k − ε model
kOmega
Standard high-Re k − ω model
kOmegaSST
k − ω-SST model
RNGkEpsilon
RNG k − ε model
NonlinearKEShih
Non-linear Shih k − ε model
LienCubicKE
Lien cubic k − ε model
qZeta
q − ζ model
LaunderSharmaKE
Launder-Sharma low-Re k − ε model
LamBremhorstKE
Lam-Bremhorst low-Re k − ε model
LienCubicKELowRe
Lien cubic low-Re k − ε model
LienLeschzinerLowRe
Lien-Leschziner low-Re k − ε model
LRR
Launder-Reece-Rodi RSTM
LaunderGibsonRSTM
Launder-Gibson RSTM with wall-reflection terms
realizableKE
Realizable k − ε model
SpalartAllmaras
Spalart-Allmaras 1-eqn mixing-length model
RAS turbulence models for compressible fluids — compressibleRASModels
laminar
Dummy turbulence model for laminar flow
kEpsilon
Standard k − ε model
kOmegaSST
k − ω − SST model
RNGkEpsilon
RNG k − ε model
LaunderSharmaKE
Launder-Sharma low-Re k − ε model
LRR
Launder-Reece-Rodi RSTM
LaunderGibsonRSTM
Launder-Gibson RSTM
realizableKE
Realizable k − ε model
SpalartAllmaras
Spalart-Allmaras 1-eqn mixing-length model
Large-eddy simulation
laplaceFilter
simpleFilter
anisotropicFilter

(LES) filters — LESfilters
Laplace filters
Simple filter
Anisotropic filter

Large-eddy simulation
PrandtlDelta
cubeRootVolDelta
smoothDelta

deltas — LESdeltas
Prandtl delta
Cube root of cell volume delta
Smoothing of delta
Continued on next page

Open∇FOAM-1.6

U-99

3.7 Standard libraries
Continued from previous page

Incompressible LES turbulence models — incompressibleLESModels
Smagorinsky
Smagorinsky model
Smagorinsky2
Smagorinsky model with 3-D filter
dynSmagorinsky
Dynamic Smagorinsky
scaleSimilarity
Scale similarity model
mixedSmagorinsky
Mixed Smagorinsky/scale similarity model
dynMixedSmagorinsky
Dynamic mixed Smagorinsky/scale similarity model
kOmegaSST
k − ω-SST scale adaptive simulation (SAS) model
oneEqEddy
k-equation eddy-viscosity model
dynOneEqEddy
Dynamic k-equation eddy-viscosity model
locDynOneEqEddy
Localised dynamic k-equation eddy-viscosity model
spectEddyVisc
Spectral eddy viscosity model
LRDDiffStress
LRR differential stress model
DeardorffDiffStress
Deardorff differential stress model
SpalartAllmaras
Spalart-Allmaras model
SpalartAllmarasDDES
Spalart-Allmaras delayed detached eddy simulation
(DDES) model
SpalartAllmarasIDDES
Spalart-Allmaras improved DDES (IDDES) model
Compressible LES turbulence models — compressibleLESModels
Smagorinsky
Smagorinsky model
oneEqEddy
k-equation eddy-viscosity model
dynOneEqEddy
Dynamic k-equation eddy-viscosity model
lowReOneEqEddy
Low-Re k-equation eddy-viscosity model
DeardorffDiffStress
Deardorff differential stress model
SpalartAllmaras
Spalart-Allmaras 1-eqn mixing-length model
Table 3.9: Libraries of RAS and LES turbulence models.

Transport models for incompressible fluids — incompressibleTransportModels
Newtonian
Linear viscous fluid model
CrossPowerLaw
Cross Power law nonlinear viscous model
BirdCarreau
Bird-Carreau nonlinear viscous model
HerschelBulkley
Herschel-Bulkley nonlinear viscous model
powerLaw
Power-law nonlinear viscous model
interfaceProperties
Models for the interface, e.g. contact angle, in multiphase
simulations
Table 3.10: Shared object libraries of transport models.

Open∇FOAM-1.6

U-100

Open∇FOAM-1.6

Applications and libraries

Chapter 4
OpenFOAM cases
This chapter deals with the file structure and organisation of OpenFOAM cases. Normally, a user would assign a name to a case, e.g. the tutorial case of flow in a cavity is simply named cavity. This name becomes the name of a directory in which all
the case files and subdirectories are stored. The case directories themselves can be
located anywhere but we recommend they are within a run subdirectory of the user’s
project directory, i.e.$HOME/OpenFOAM/${USER}-1.6 as described at the beginning of
chapter 2. One advantage of this is that the $FOAM RUN environment variable is set
to $HOME/OpenFOAM/${USER}-1.6/run by default; the user can quickly move to that
directory by executing a preset alias, run, at the command line.
The tutorial cases that accompany the OpenFOAM distribution provide useful examples of the case directory structures. The tutorials are located in the $FOAM TUTORIALS
directory, reached quickly by executing the tut alias at the command line. Users can view
tutorial examples at their leisure while reading this chapter.

4.1

File structure of OpenFOAM cases

The basic directory structure for a OpenFOAM case, that contains the minimum set of
files required to run an application, is shown in Figure 4.1 and described as follows:

system
controlDict
fvSchemes
fvSolution

see section 4.3
see section 4.4
see section 4.5

constant
. . . Properties
polyMesh
points
cells
faces
boundary
time directories

see chapter 7
see section 5.1.2

see section 4.2.8

Figure 4.1: Case directory structure

U-102

OpenFOAM cases

A constant directory that contains a full description of the case mesh in a subdirectory polyMesh and files specifying physical properties for the application concerned,
e.g.transportProperties.
A system directory for setting parameters associated with the solution procedure itself.
It contains at least the following 3 files: controlDict where run control parameters are
set including start/end time, time step and parameters for data output; fvSchemes
where discretisation schemes used in the solution may be selected at run-time; and,
fvSolution where the equation solvers, tolerances and other algorithm controls are
set for the run.
The ‘time’ directories containing individual files of data for particular fields. The
data can be: either, initial values and boundary conditions that the user must
specify to define the problem; or, results written to file by OpenFOAM. Note that
the OpenFOAM fields must always be initialised, even when the solution does not
strictly require it, as in steady-state problems. The name of each time directory is
based on the simulated time at which the data is written and is described fully in
section 4.3. It is sufficient to say now that since we usually start our simulations
at time t = 0, the initial conditions are usually stored in a directory named 0 or
0.000000e+00, depending on the name format specified. For example, in the cavity
tutorial, the velocity field U and pressure field p are initialised from files 0/U and
0/p respectively.

4.2

Basic input/output file format

OpenFOAM needs to read a range of data structures such as strings, scalars, vectors,
tensors, lists and fields. The input/output (I/O) format of files is designed to be extremely
flexible to enable the user to modify the I/O in OpenFOAM applications as easily as
possible. The I/O follows a simple set of rules that make the files extremely easy to
understand, in contrast to many software packages whose file format may not only be
difficult to understand intuitively but also not be published anywhere. The description
of the OpenFOAM file format is described in the following sections.

4.2.1

General syntax rules

The format follows the following some general principles of C++ source code.
• Files have free form, with no particular meaning assigned to any column and no
need to indicate continuation across lines.
• Lines have no particular meaning except to a // comment delimiter which makes
OpenFOAM ignore any text that follows it until the end of line.
• A comment over multiple lines is done by enclosing the text between /* and */
delimiters.

4.2.2

Dictionaries

OpenFOAM uses dictionaries as the most common means of specifying data. A dictionary
is an entity that contains as set data entries that can be retrieved by the I/O by means
of keywords. The keyword entries follow the general format
Open∇FOAM-1.6

4.2 Basic input/output file format

U-103

... ;

Most entries are single data entries of the form:

;

Most OpenFOAM data files are themselves dictionaries containing a set of keyword entries. Dictionaries provide the means for organising entries

U-104
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46

OpenFOAM cases

}
U
{

}
PISO
{

}

relTol

solver
preconditioner
tolerance
relTol

PBiCG;
DILU;
1e-05;
0;

nCorrectors
2;
nNonOrthogonalCorrectors 0;
pRefCell
0;
pRefValue
0;

}
// ************************************************************************* //

4.2.4

Lists

OpenFOAM applications contain lists, e.g. a list of vertex coordinates for a mesh description. Lists are commonly found in I/O and have a format of t

U-105

4.2 Basic input/output file format

4.2.5

Scalars, vectors and tensors

A scalar is a single number represented as such in a data file. A vector is a VectorSpace
of rank 1 and dimension 3, and since the number of elements is always fixed to 3, the
simple List format is used. Therefore a vector (1.0, 1.1, 1.2) is written:
(1.0 1.1 1.2)
In OpenFOAM, a tensor is a VectorSpace of rank 2 and dimension 3 and therefore the
data entries are always fixed to 9 real numbers. Therefore the identity tensor, described
in section 1.3.7 of the Programmer’s Guide, can be written:
(
1 0 0
0 1 0
0 0 1
)
This example demonstrates the way in which OpenFOAM ignores the line return is so
that the entry can be written over multiple lines. It is treated no differently to listing the
numbers on a single line:
( 1 0 0 0 1 0 0 0 1 )

4.2.6

Dimensional units

In continuum mechanics, properties are represented in some chosen units, e.g. mass in
kilograms (kg), volume in cubic metres (m3 ), pressure in Pascals (kg m−1 s−2 ). Algebraic
operations must be performed on these properties using consistent units of measurement;
in particular, addition, subtraction and equality are only physically meaningful for properties of the same dimensional units. As a safeguard against implementing a meaningless
operation, OpenFOAM attaches dimensions to field data and physical properties and
performs dimension checking on any tensor operation.
The I/O format for a dimensionSet is 7 scalars delimited by square brackets, e.g.
[0 2 -1 0 0 0 0]
No.
1
2
3
4
5
6
7

Property
Mass
Length
Time
Temperature
Quantity
Current
Luminous intensity

SI unit
USCS unit
kilogram (kg)
pound-mass (lbm)
metre (m)
foot (ft)
————
second (s)
————
Kelvin (K)
degree Rankine (◦ R)
kilogram-mole (kgmol) pound-mole (lbmol)
————
ampere (A)
————
————
candela (cd)
————

Table 4.2: Base units for SI and USCS
where each of the values corresponds to the power of each of the base units of measurement listed in Table 4.2. The table gives the base units for the Système International
(SI) and the United States Customary System (USCS) but OpenFOAM can be used
Open∇FOAM-1.6

U-106

OpenFOAM cases

with any system of units. All that is required is that the input data is correct for the
chosen set of units. It is particularly important to recognise that OpenFOAM requires
some dimensioned physical constants, e.g. the Universal Gas Constant R, for certain calculations, e.g. thermophysical modelling. These dimensioned constants are specified in
a DimensionedConstant sub-dictionary of main controlDict file of the OpenFOAM installation ($WM PROJECT DIR/etc/controlDict). By default these constants are set in SI
units. Those wishing to use the USCS or any other system of units should modify these
constants to their chosen set of units accordingly.

4.2.7

Dimensioned types

Physical properties are typically specified with their associated dimensions. These entries
have the format that the following example of a dimensionedScalar demonstrates:
nu

[0 2 -1 0 0 0 0]

The first nu is the keyword; the second nu is the word name stored in class word, usually
chosen to be the same as the keyword; the next entry is the dimensionSet and the final
entry is the scalar value.

4.2.8

Fields

Much of the I/O data in OpenFOAM are tensor fields, e.g. velocity, pressure data, that
are read from and written into the time directories. OpenFOAM writes field data using
keyword entries as described in Table 4.3.
Keyword
dimensions
internalField
boundaryField

Description
Example
Dimensions of field
[1 1 -2 0 0 0 0]
Value of internal field uniform (1 0 0)
Boundary field
see file listing in section 4.2.8

Table 4.3: Main keywords used in field dictionaries.
The data begins with an entry for its dimensions. Following that, is the internalField,
described in one of the following ways.
Uniform field a single value is assigned to all elements within the field, taking the form:
internalField uniform ;
Nonuniform field each field element is assigned a unique value from a list, taking the
following form where the token identifier form of list is recommended:
internalField nonuniform ;
The boundaryField is a dictionary containing a set of entries whose names correspond
to each of the names of the boundary patches listed in the boundary file in the polyMesh
directory. Each patch entry is itself a dictionary containing a list of keyword entries.
The compulsory entry, type, describes the patch field condition specified for the field.
The remaining entries correspond to the type of patch field condition selected and can
Open∇FOAM-1.6

4.2 Basic input/output file format

U-107

typically include field data specifying initial conditions on patch faces. A selection of
patch field conditions available in OpenFOAM are listed in Table 5.3 and Table 5.4 with
a description and the data that h

U-108

OpenFOAM cases

type fixedValue;
value $pressure;
}

}

This is a fairly trivial example that simply demonstrates how this functionality works.
However, the functionality can be used in many, more powerful ways particularly as a
means of generalising case data to suit the user’s needs. For example, if a user has a set
of cases that require the same RAS turbulence model settings, a single file can be created
with those settings which is simply included in the RASProperties file of each case. Macro
substitutions can extend well beyond a singe value so that, for example, sets of boundary
conditions can be predefined and called by a single macro. The extent to which such
functionality can be used is almost endless.

4.3

Time and data input/output control

The OpenFOAM solvers begin all runs by setting up a database. The database controls
I/O and, since output of data is usually requested at intervals of time during the run, time
is an inextricable part of the database. The controlDict dictionary sets input parameters
essential for the creation of the database. The keyword entries in controlDict are listed in
Table 4.4. Only the time control and writeInterval entries are truly compulsory, with
the database taking default values indicated by † in Table 4.4 for any of the optional
entries that are omitted.

Time control
startFrom
- firstTime
- startTime
- latestTime

Controls the start time of the simulation.
Earliest time step from the set of time directories.
Time specified by the startTime keyword entry.
Most recent time step from the set of time directories.

startTime

Start time for the simulation with startFrom startTime;

stopAt
- endTime
- writeNow

endTime

Controls the end time of the simulation.
Time specified by the endTime keyword entry.
Stops simulation on completion of current time step and writes
data.
Stops simulation on completion of current time step and does not
write out data.
Stops simulation on completion of next scheduled write time, specified by writeControl.
End time for the simulation when stopAt endTime; is specified.

deltaT

Time step of the simulation.

Data writing
writeControl
- timeStep†
- runTime

Controls the timing of write output to file.
Writes data every writeInterval time steps.
Writes data every writeInterval seconds of simulated time.

- noWriteNow
- nextWrite

Continued on next page
Open∇FOAM-1.6

U-109

4.3 Time and data input/output control
Continued from previous page

- adjustableRunTime Writes data every writeInterval seconds of simulated time,
adjusting the time steps to coincide with the writeInterval if
necessary — used in cases with automatic time step adjustment.
- cpuTime
Writes data every writeInterval seconds of CPU time.
- clockTime
Writes data out every writeInterval seconds of real time.
writeInterval

Scalar used in conjunction with writeControl described above.

purgeWrite

Integer representing a limit on the number of time directories that
are stored by overwriting time directories on a cyclic basis. Example of t0 = 5s, ∆t = 1s and purgeWrite 2;: data written into 2
directories, 6 and 7, before returning to write the data at 8 s in 6,
data at 9 s into 7, etc.
To disable the time directory limit, specify purgeWrite 0;†
For steady-state solutions, results from previous iterations can be
continuously overwritten by specifying purgeWrite 1;

writeFormat
- ascii†
- binary

Specifies the format of the data files.
ASCII format, written to writePrecision significant figures.
Binary format.

writePrecision Integer used in conjunction with writeFormat described above, 6†
by default
writeCompression Specifies the compression of the data files.
- uncompressed No compression.†
- compressed gzip compression.
timeFormat
- fixed
- scientific
- general†

Choice of format of the naming of the time directories.
±m.dddddd where the number of ds is set by timePrecision.
±m.dddddde±xx where the number of ds is set by timePrecision.
Specifies scientific format if the exponent is less than -4 or
greater than or equal to that specified by timePrecision.

timePrecision

Integer used in conjunction with timeFormat described above, 6†
by default

graphFormat
- raw†
- gnuplot
- xmgr
- jplot

Format for graph data written by an application.
Raw ASCII format in columns.
Data in gnuplot format.
Data in Grace/xmgr format.
Data in jPlot format.

Data reading
runTimeModifiable yes†/no switch for whether dictionaries, e.g.controlDict, are reread by OpenFOAM at the beginning of each time step.
Continued on next page

Open∇FOAM-1.6

U-110

OpenFOAM cases

Continued from previous page

Run-time loadable functionality
libs
List of additional libraries (on $LD LIBRARY PATH) to be loaded
at run-time, e.g.( "libUser1.so" "libUser2.so" )
functions
List of functions, e.g. probes to be loaded at run-time; see examples
in $FOAM TUTORIALS
† denotes default entry if associated keyword is omitted.
Table 4.4: Keyword entries in the controlDict dictionary.
Example entries from a controlDict dictionary are given below:
17
18
19
20
21
22
23
24

application

icoFoam;

startFrom

startTime;

startTime

U-111

4.4 Numerical schemes

The set of terms, for which numerical schemes must be specified, are subdivided within
the fvSchemes dictionary into the categories listed in Table 4.5. Each keyword in Table 4.5
is the name of a sub-dictionary which contains terms of a particular type, e.g.gradSchemes
contains all the gradient derivative terms such as grad(p) (which represents ∇p). Further
examples can be seen in the extract from an fvSchemes dictionary below:
Keyword
interpolationSchemes
snGradSchemes
gradSchemes
divSchemes
laplacianSchemes
timeScheme
fluxRequired

Category of mathematical terms
Point-to-point interpolations of values
Component of gradient normal to a cell face
Gradient ∇
Divergence ∇ •
Laplacian ∇2
First and second time derivatives ∂/∂t, ∂ 2 /∂ 2 t
Fields which require the generation of a flux

Table 4.5: Main keywords used in fvSchemes.

17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60

ddtSchemes
{
default
}

Euler;

gradSchemes
{
default
grad(p)
}

Gauss linear;
Gauss linear;

divSchemes
{
default
div(phi,U)
}

none;
Gauss linear;

laplacianSchemes
{
default
none;
laplacian(nu,U) Gauss linear corrected;
laplacian((1|A(U)),p) Gauss linear corrected;
}
interpolationSchemes
{
default
linear;
interpolate(HbyA) linear;
}
snGradSchemes
{
default
}

corrected;

fluxRequired
{
default
p
}

no;
;

// ************************************************************************* //

The example shows that the fvSchemes dictionary contains the following:
• 6 . . . Schemes subdictionaries containing keyword entries for each term specified
within including: a default entry; other entries whose names correspond to a word
identifier for the particular term specified, e.g.grad(p) for ∇p
Open∇FOAM-1.6

U-112

OpenFOAM cases

• a fluxRequired sub-dictionary containing fields for which the flux is generated in the
application, e.g.p in the example.
If a default scheme is specified in a particular . . . Schemes sub-dictionary, it is assigned
to all of the terms to which the sub-dictionary refers, e.g. specifying a default in gradSchemes sets the scheme for all gradient terms in the application, e.g. ∇p, ∇U. When
a default is specified, it is not necessary to specify each specific term itself in that subdictionary, i.e. the entries for grad(p), grad(U) in this example. However, if any of these
terms are included, the specified scheme overrides the default scheme for that term.
Alternatively the user may insist on no default scheme by the none entry. In this
instance the user is obliged to specify all terms in that sub-dictionary individually. Setting
default to none may appear superfluous since default can be overridden. However,
specifying none forces the user to specify all terms individually which can be useful to
remind the user which terms are actually present in the application.
The following sections describe the choice of schemes for each of the categories of
terms in Table 4.5.

4.4.1

Interpolation schemes

The interpolationSchemes sub-dictionary contains terms that are interpolations of values typically from cell centres to face centres. A selection of interpolation schemes in
OpenFOAM are listed in Table 4.6, being divided into 4 categories: 1 category of general schemes; and, 3 categories of schemes used primarily in conjunction with Gaussian
discretisation of convection (divergence) terms in fluid flow, described in section 4.4.5.
It is highly unlikely that the user would adopt any of the convection-specific schemes
for general field interpolations in the interpolationSchemes sub-dictionary, but, as valid
interpolation schemes, they are described here rather than in section 4.4.5. Note that
additional schemes such as UMIST are available in OpenFOAM but only those schemes
that are generally recommended are listed in Table 4.6.
A general scheme is simply specified by quoting the keyword and entry, e.g. a linear
scheme is specified as default by:
default linear;
The convection-specific schemes calculate the interpolation based on the flux of the
flow velocity. The specification of these schemes requires the name of the flux field
on which the interpolation is based; in most OpenFOAM applications this is phi, the
name commonly adopted for the surfaceScalarField velocity flux φ. The 3 categories of
convection-specific schemes are referred to in this text as: general convection; normalised
variable (NV); and, total variation diminishing (TVD). With the exception of the blended
scheme, the general convection and TVD schemes are specified by the scheme and flux,
e.g. an upwind scheme based on a flux phi is specified as default by:
default upwind phi;
Some TVD/NVD schemes require a coefficient ψ, 0 ≤ ψ ≤ 1 where ψ = 1 corresponds
to TVD conformance, usually giving best convergence and ψ = 0 corresponds to best
accuracy. Running with ψ = 1 is generally recommended. A limitedLinear scheme
based on a flux phi with ψ = 1.0 is specified as default by:
default limitedLinear 1.0 phi;
Open∇FOAM-1.6

U-113

4.4 Numerical schemes

4.4.1.1

Schemes for strictly bounded scalar fields

There are enhanced versions of some of the limited schemes for scalars that need to be
strictly bounded. To bound between user-specified limits, the scheme name should be
preprended by the word limited and followed by the lower and upper limits respectively.
For example, to bound the vanLeer scheme strictly between -2 and 3, the user would
specify:
default limitedVanLeer -2.0 3.0;
There are specialised versions of these schemes for scalar fields that are commonly bounded
between 0 and 1. These are selected by adding 01 to the name of the scheme. For example,
to bound the vanLeer scheme strictly between 0 and 1, the user would specify:
default vanLeer01;
Strictly bounded versions are available for the following schemes: limitedLinear, vanLeer,
Gamma, limitedCubic, MUSCL and SuperBee.
4.4.1.2

Schemes for vector fields

There are improved versions of some of the limited schemes for vector fields in which
the limited is formulated to take into account the direction of the field. These schemes
are selected by adding V to the name of the general scheme, e.g.limitedLinearV for
limitedLinear. ‘V’ versions are available for the following schemes: limitedLinearV,
vanLeerV, GammaV, limitedCubicV and SFCDV.
Centred schemes
linear
Linear interpolation (central differencing)
cubicCorrection Cubic scheme
midPoint
Linear interpolation with symmetric weighting
Upwinded convection schemes
upwind
Upwind differencing
linearUpwind
Linear upwind differencing
skewLinear
Linear with skewness correction
QUICK
Quadratic upwind differencing
TVD schemes
limitedLinear
vanLeer
MUSCL
limitedCubic

limited linear differencing
van Leer limiter
MUSCL limiter
Cubic limiter

NVD schemes
SFCD
Gamma ψ

Self-filtered central differencing
Gamma differencing

Table 4.6: Interpolation schemes.

Open∇FOAM-1.6

U-114

4.4.2

OpenFOAM cases

Surface normal gradient schemes

The snGradSchemes sub-dictionary contains surface normal gradient terms. A surface
normal gradient is evaluated at a cell face; it is the component, normal to the face, of the
gradient of values at the centres of the 2 cells that the face connects. A surface normal
gradient may be specified in its own right and is also required to evaluate a Laplacian
term using Gaussian integration.
The available schemes are listed in Table 4.7 and are specified by simply quoting the
keyword and entry, with the exception of limited which requires a coefficient ψ, 0 ≤ ψ ≤
1 where

0
corresponds to uncorrected,



0.333 non-orthogonal correction ≤ 0.5 × orthogonal part,
ψ=
(4.1)

0.5
non-orthogonal
correction
≤
orthogonal
part,



1
corresponds to corrected.
A limited scheme with ψ = 0.5 is therefore specified as default by:
default limited 0.5;

Scheme
corrected
uncorrected
limited ψ
bounded
fourth

Description
Explicit non-orthogonal correction
No non-orthogonal correction
Limited non-orthogonal correction
Bounded correction for positive scalars
Fourth order

Table 4.7: Surface normal gradient schemes.

4.4.3

Gradient schemes

The gradSchemes sub-dictionary contains gradient terms. The discretisation scheme for
each term can be selected from those listed in Table 4.8.
Discretisation scheme
Gauss
leastSquares
fourth
limited

Description
Second order, Gaussian integration
Second order, least squares
Fourth order, least squares
Limited version of one of the above schemes

Table 4.8: Discretisation schemes available in gradSchemes.

The discretisation scheme is sufficient to specify the scheme completely in the cases
of leastSquares and fourth, e.g.
grad(p) leastSquares;
Open∇FOAM-1.6

4.4 Numerical schemes

U-115

The Gauss keyword specifies the standard finite volume discretisation of Gaussian
integration which requires the interpolation of values from cell centres to face centres.
Therefore, the Gauss entry must be followed by the choice of interpolation scheme from
Table 4.6. It would be extremely unusual to select anything other than general interpolation schemes and in most cas(u)-0.342058(s).59 -14.4449 Td [(l)0.218o9gsassa

U-116

OpenFOAM cases

Gauss
The interpolation scheme is selected from the full range of schemes in Table 4.6, both
general and convection-specific. The choice critically determines numerical behaviour as
described in Table 4.10. The syntax here for specifying convection-specific interpolation
schemes does not include the flux as it is already known for the particular term, i.e. for
div(phi,U), we know the flux is phi so specifying it in the interpolation scheme would
only invite an inconsistency. Specification of upwind interpolation in our example would
therefore be:
div(phi,U) Gauss upwind;
Scheme
linear
skewLinear
cubicCorrected
upwind
linearUpwind
QUICK
TVD schemes
SFCD
NVD schemes

Numerical behaviour
Second order, unbounded
Second order, (more) unbounded, skewness correction
Fourth order, unbounded
First order, bounded
First/second order, bounded
First/second order, bounded
First/second order, bounded
Second order, bounded
First/second order, bounded

Table 4.10: Behaviour of interpolation schemes used in divSchemes.

4.4.6

Time schemes

The first time derivative (∂/∂t) terms are specified in the ddtSchemes sub-dictionary. The
discretisation scheme for each term can be selected from those listed in Table 4.11.
There is an off-centering coefficient ψ with the CrankNicholson scheme that blends
it with the Euler scheme. A coefficient of ψ = 1 corresponds to pure CrankNicholson
and and ψ = 0 corresponds to pure Euler. The blending coefficient can help to improve
stability in cases where pure CrankNicholson are unstable.
Scheme
Euler
CrankNicholson ψ
backward
steadyState

Description
First order, bounded, implicit
Second order, bounded, implicit
Second order, implicit
Does not solve for time derivatives

Table 4.11: Discretisation schemes available in ddtSchemes.
When specifying a time scheme it must be noted that an application designed for
transient problems will not necessarily run as steady-state and visa versa. For example
the solution will not converge if steadyState is specified when running icoFoam, the
transient, laminar incompressible flow code; rather, simpleFoam should be used for steadystate, incompressible flow.
Any second time derivative (∂ 2 /∂t2 ) terms are specified in the d2dt2Schemes subdictionary. Only the Euler scheme is available for d2dt2Schemes.
Open∇FOAM-1.6

4.5 Solution and algorithm control

4.4.7

U-117

Flux calculation

The fluxRequired sub-dictionary lists the fields for which the flux is generated in the
application. For example, in many fluid dynamics applications the flux is generated after
solving a pressure equation, in which case the fluxRequired sub-dictionary would simply
be entered as follows, p being the word identifier for pressure:
fluxRequired
{
p;
}

4.5

Solution and algorithm control

The equation solvers, tolerances and algorithms are controlled from the fvSolution dictionary in the system directory. Below is an example set of entries from the fvSolution
dictionary required for the icoFoam solver.
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46

solvers
{
p
{

}
U
{

}

solver
preconditioner
tolerance
relTol

PCG;
DIC;
1e-06;
0;

solver
preconditioner
tolerance
relTol

PBiCG;
DILU;
1e-05;
0;

PISO
{
nCorrectors
2;
nNonOrthogonalCorrectors 0;
pRefCell
0;
pRefValue
0;
}
// ************************************************************************* //

fvSolution contains a set of subdictionaries that are specific to the solver being run. However, there is a small set of standard subdictionaries that cover most of those used by
the standard solvers. These subdictionaries include solvers, relaxationFactors, PISO and
SIMPLE which are described in the remainder of this section.

4.5.1

Linear solver control

The first sub-dictionary in our example, and one that appears in all solver applications,
is solvers. It specifies each linear-solver that is used for each discretised equation; it
is emphasised that the term linear-solver refers to the method of number-crunching to
solve the set of linear equations, as opposed to application solver which describes the set
of equations and algorithms to solve a particular problem. The term ‘linear-solver’ is
abbreviated to ‘solver’ in much of the following discussion; we hope the context of the
term avoids any ambiguity.
Open∇FOAM-1.6

U-118

OpenFOAM cases

The syntax for each entry within solvers uses a keyword that is the word relating to the
variable being solved in the particular equation. For example, icoFoam solves equations
for velocity U and pressure p, hence the entries for U and p. The keyword is followed
by a dictionary containing the type of solver and the parameters that the solver uses.
The solver is selected through the solver keyword from the choice in OpenFOAM, listed
in Table 4.12. The parameters, including tolerance, relTol, preconditioner, etc. are
described in following sections.
Solver
Keyword
Preconditioned (bi-)conjugate gradient
PCG/PBiCG†
Solver using a smoother
smoothSolver
Generalised geometric-algebraic multi-grid GAMG
†PCG for symmetric matrices, PBiCG for asymmetric
Table 4.12: Linear solvers.
The solvers distinguish between symmetric matrices and asymmetric matrices. The
symmetry of the matrix depends on the structure of the equation being solved and, while
the user may be able to determine this, it is not essential since OpenFOAM will produce
an error message to advise the user if an inappropriate solver has been selected, e.g.
--> FOAM FATAL IO ERROR : Unknown asymmetric matrix solver PCG
Valid asymmetric matrix solvers are :
3
(
PBiCG
smoothSolver
GAMG
)
4.5.1.1

Solution tolerances

The sparse matrix solvers are iterative, i.e. they are based on reducing the equation
residual over a succession of solutions. The residual is ostensibly a measure of the error
in the solution so that the smaller it is, the more accurate the solution. More precisely,
the residual is evaluated by substituting the current solution into the equation and taking
the magnitude of the difference between the left and right hand sides; it is also normalised
in to make it independent of the scale of problem being analysed.
Before solving an equation for a particular field, the initial residual is evaluated based
on the current values of the field. After each solver iteration the residual is re-evaluated.
The solver stops if either of the following conditions are reached:
• the residual falls below the solver tolerance, tolerance;
• the ratio of current to initial residuals falls below the solver relative tolerance,
relTol;
The solver tolerance should represents the level at which the residual is small enough
that the solution can be deemed sufficiently accurate. The solver relative tolerance limits
the relative improvement from initial to final solution. It is quite common to set the
solver relative tolerance to 0 to force the solution to converge to the solver tolerance. The
tolerances, tolerance and relTol must be specified in the dictionaries for all solvers.
Open∇FOAM-1.6

U-119

4.5 Solution and algorithm control

4.5.1.2

Preconditioned conjugate gradient solvers

There are a range of options for preconditioning of matrices in the conjugate gradient
solvers, represented by the preconditioner keyword in the solver dictionary. The preconditioners are listed in Table 4.13.
Preconditioner
Keyword
Diagonal incomplete-Cholesky (symmetric)
DIC
Faster diagonal incomplete-Cholesky (DIC with caching) FDIC
Diagonal incomplete-LU (asymmetric)
DILU
Diagonal
diagonal
Geometric-algebraic multi-grid
GAMG
No preconditioning
none
Table 4.13: Preconditioner options.

4.5.1.3

Smooth solvers

The solvers that use a smoother require the smoother to be specified. The smoother options are listed in Table 4.14. Generally GaussSeidel is the most reliable option, but for
bad matrices DIC can offer better convergence. In some cases, additional post-smoothing
using GaussSeidel is further beneficial, i.e. the method denoted as DICGaussSeidel
Smoother
Gauss-Seidel
Diagonal incomplete-Cholesky (symmetric)
Diagonal incomplete-Cholesky with Gauss-Seidel (symmetric)

Keyword
GaussSeidel
DIC
DICGaussSeidel

Table 4.14: Smoother options.
The user must also pecify the number of sweeps, by the nSweeps keyword, before the
residual is recalculated, following the tolerance parameters.
4.5.1.4

Geometric-algebraic multi-grid solvers

The generalised method of geometric-algebraic multi-grid (GAMG) uses the principle of:
generating a quick solution on a mesh with a small number of cells; mapping this solution
onto a finer mesh; using it as an initial guess to obtain an accurate solution on the fine
mesh. GAMG is faster than standard methods when the increase in speed by solving first
on coarser meshes outweighs the additional costs of mesh refinement and mapping of field
data. In practice, GAMG starts with the mesh specified by the user and coarsens/refines
the mesh in stages. The user is only required to specify an approximate mesh size at the
most coarse level in terms of the number of cells nCoarsestCells.
The agglomeration of cells is performed by the algorithm specified by the agglomerator
keyword. Presently we recommend the faceAreaPair method. It is worth noting there is
an MGridGen option that requires an additional entry specifying the shared object library
for MGridGen:
geometricGamgAgglomerationLibs ("libMGridGenGamgAgglomeration.so");
Open∇FOAM-1.6

U-120

OpenFOAM cases

In the experience of OpenCFD, the MGridGen method offers no obvious benefit over the
faceAreaPair method. For all methods, agglomeration can be optionally cached by the
cacheAgglomeration switch.
Smoothing is specified by the smoother as described in section 4.5.1.3. The number
of sweeps used by the smoother at different levels of mesh density are specified by the
nPreSweeps, nPostSweeps and nFinestSweeps keywords. The nPreSweeps entry is used
as the algorithm is coarsening the mesh, nPostSweeps is used as the algorithm is refining,
and nFinestSweeps is used when the solution is at its finest level.
The mergeLevels keyword controls the speed at which coarsening or refinement levels
is performed. It is often best to do so only at one level at a time, i.e. set mergeLevels
1. In some cases, particularly for simple meshes, the solution can be safely speeded up
by coarsening/refining two levels at a time, i.e. setting mergeLevels 2.

4.5.2

Solution under-relaxation

A second sub-dictionary of fvSolution that is often used in OpenFOAM is relaxationFactors
which controls under-relaxation, a technique used for improving stability of a computation, particularly in solving steady-state problems. Under-relaxation works by limiting
the amount which a variable changes from one iteration to the next, either by modifying
the solution matrix and source prior to solving for a field or by modifying the field directly. An under-relaxation factor α, 0 < α ≤ 1 specifies the amount of under-relaxation,
ranging from none at all for α = 1 and increasing in strength as α → 0. The limiting case
where α = 0 represents a solution which does not change at all with successive iterations.
An optimum choice of α is one that is small enough to ensure stable computation but
large enough to move the iterative process forward quickly; values of α as high as 0.9
can ensure stability in some cases and anything much below, say, 0.2 are prohibitively
restrictive in slowing the iterative process.
The user can specify the relaxation factor for a particular field by specifying first the
word associated with the field, then the factor. The user can view the relaxation factors
used in a tutorial example of simpleFoam for incompressible, laminar, steady-state flows.
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50

solvers
{
p
{

}
U
{

}
k
{

}

solver
preconditioner
tolerance
relTol

PCG;
DIC;
1e-06;
0.01;

solver
preconditioner
tolerance
relTol

PBiCG;
DILU;
1e-05;
0.1;

solver
preconditioner
tolerance
relTol

PBiCG;
DILU;
1e-05;
0.1;

epsilon
{
solver
preconditioner
tolerance
relTol
}

Open∇FOAM-1.6

PBiCG;
DILU;
1e-05;
0.1;

4.5 Solution and algorithm control
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85

R
{

solver
preconditioner
tolerance
relTol

PBiCG;
DILU;
1e-05;
0.1;

nuTilda
{
solver
preconditioner
tolerance
relTol
}

PBiCG;
DILU;
1e-05;
0.1;

}

U-121

SIMPLE
{
nNonOrthogonalCorrectors 0;
}
relaxationFactors
{
p
U
k
epsilon
R
nuTilda
}

0.3;
0.7;
0.7;
0.7;
0.7;
0.7;

// ************************************************************************* //

4.5.3

PISO and SIMPLE algorithms

Most fluid dynamics solver applications in OpenFOAM use the pressure-implicit splitoperator (PISO) or semi-implicit method for pressure-linked equations (SIMPLE) algorithms. These algorithms are iterative procedures for solving equations for velocity and
pressure, PISO being used for transient problems and SIMPLE for steady-state.
Both algorithms are based on evaluating some initial solutions and then correcting
them. SIMPLE only makes 1 correction whereas PISO requires more than 1, but typically
not more than 4. The user must therefore specify the number of correctors in the PISO
dictionary by the nCorrectors keyword as shown in the example on page U-117.
An additional correction to account for mesh non-orthogonality is available in both
SIMPLE and PISO in the standard OpenFOAM solver applications. A mesh is orthogonal
if, for each face within it, the face normal is parallel to the vector between the centres of
the cells that the face connects, e.g. a mesh of hexahedral cells whose faces are aligned
with a Cartesian coordinate system. The number of non-orthogonal correctors is specified
by the nNonOrthogonalCorrectors keyword as shown in the examples above and on
page U-117. The number of non-orthogonal correctors should correspond to the mesh for
the case being solved, i.e. 0 for an orthogonal mesh and increasing with the degree of
non-orthogonality up to, say, 20 for the most non-orthogonal meshes.
4.5.3.1

Pressure referencing

In a closed incompressible system, pressure is relative: it is the pressure range that matters
not the absolute values. In these cases, the solver sets a reference level of pRefValue in
cell pRefCell where p is the name of the pressure solution variable. Where the pressure
is pd, the names are pdRefValue and pdRefCell respectively. These entries are generally
stored in the PISO/SIMPLE sub-dictionary and are used by those solvers that require
them when the case demands it. If ommitted, the solver will not run, but give a message
to alert the user to the problem.
Open∇FOAM-1.6

U-122

4.5.4

OpenFOAM cases

Other parameters

The fvSolutions dictionaries in the majority of standard OpenFOAM solver applications
contain no other entries than those described so far in this section. However, in general
the fvSolution dictionary may contain any parameters to control the solvers, algorithms,
or in fact anything. For a given solver, the user can look at the source code to find the
parameters required. Ultimately, if any parameter or sub-dictionary is missing when an
solver is run, it will terminate, printing a detailed error message. The user can then add
missing parameters accordingly.

Open∇FOAM-1.6

Chapter 5
Mesh generation and conversion
This chapter describes all topics relating to the creation of meshes in OpenFOAM:
section 5.1 gives an overview of the ways a mesh may be described in OpenFOAM;
section 5.3 covers the blockMesh utility for generating simple meshes of blocks of hexahedral cells; section 5.4 covers the snappyHexMesh utility for generating complex meshes
of hexahedral and split-hexahedral cells automatically from triangulated surface geometries; section 5.5 describes the options available for conversion of a mesh that has been
generated by a third-party product into a format that OpenFOAM can read.

5.1

Mesh description

This section provides a specification of the way the OpenFOAM C++ classes handle a
mesh. The mesh is an integral part of the numerical solution and must satisfy certain
criteria to ensure a valid, and hence accurate, solution. During any run, OpenFOAM
checks that the mesh satisfies a fairly stringent set of validity constraints and will cease
running if the constraints are not satisfied. The consequence is that a user may experience
some frustration in ‘correcting’ a large mesh generated by third-party mesh generators
before OpenFOAM will run using it. This is unfortunate but we make no apology for
OpenFOAM simply adopting good practice to ensure the mesh is valid; otherwise, the
solution is flawed before the run has even begun.
By default OpenFOAM defines a mesh of arbitrary polyhedral cells in 3-D, bounded
by arbitrary polygonal faces, i.e. the cells can have an unlimited number of faces where,
for each face, there is no limit on the number of edges nor any restriction on its alignment.
A mesh with this general structure is known in OpenFOAM as a polyMesh. It is described
in further detail in section 2.3 of the Programmer’s Guide, but it is sufficient to mention
here that this type of mesh offers great freedom in mesh generation and manipulation
in particular when the geometry of the domain is complex or changes over time. The
price of absolute mesh generality is, however, that it can be difficult to convert meshes
generated using conventional tools. The OpenFOAM library therefore provides cellShape
tools to manage conventional mesh formats based on sets of pre-defined cell shapes.

5.1.1

Mesh specification and validity constraints

Before describing the OpenFOAM mesh format, polyMesh, and the cellShape tools, we
will first set out the validity constraints used in OpenFOAM. The conditions that a mesh
must satisfy are:

U-124
5.1.1.1

Mesh generation and conversion

Points

A point is a location in 3-D space, defined by a vector in units of metres (m). The points
are compiled into a list and each point is referred to by a label, which represents its
position in the list, starting from zero. The point list cannot contain two different points
at an exactly identical position nor any point that is not part at least one face.
5.1.1.2

Faces

A face is an ordered list of points, where a point is referred to by its label. The ordering
of point labels in a face is such that each two neighbouring points are connected by an
edge, i.e. you follow points as you travel around the circumference of the face. Faces are
compiled into a list and each face is referred to by its label, representing its position in
the list. The direction of the face normal vector is defined by the right-hand rule, i.e.
looking towards a face, if the numbering of the points follows an anti-clockwise path, the
normal vector points towards you, as shown in Figure 5.1.
3

Sf
4
0
Figure 5.1: Face area vector from point numbering on the face
There are two types of face:
Internal faces Those faces that connect two cells (and it can never be more than two).
For each internal face, the ordering of the point labels is such that the face normal
points into the cell with the larger label, i.e. for cells 2 and 5, the normal points
into 5;
Boundary faces Those belonging to one cell since they coincide with the boundary
of the domain. A boundary face is therefore addressed by one cell(only) and a
boundary patch. The ordering of the point labels is such that the face normal
points outside of the computational domain.
Faces are generally expected to be convex; at the very least the face centre needs to
be inside the face. Faces are allowed to be warped, i.e. not all points of the face need to
be coplanar.
5.1.1.3

Cells

A cell is a list of faces in arbitrary order. Cells must have the properties listed below.
Contiguous The cells must completely cover the computational domain and are must
not overlap one another.
Open∇FOAM-1.6

U-125

5.1 Mesh description

Convex Every cell must be convex and its cell centre inside the cell.
Closed Every cell must be closed, both geometrically and topologically where:
• geometrical closedness requires that when all face area vectors are oriented to
point outwards of the cell, their sum should equal the zero vector to machine
accuracy;
• topological closedness requires that all the edges in a cell are used by exactly
two faces of the cell in question.
Orthogonality For all internal faces of the mesh, we define the centre-to-centre vector
as that connecting the centres of the 2 cells that it adjoins oriented from the the
centre of the cell with smaller label to the centre of the cell with larger label. The
orthogonality constraint requires that for each internal face, the angle between the
face area vector, oriented as described above, and the centre-to-centre vector must
always be less than 90◦ .
5.1.1.4

Boundary

A boundary is a list of patches, each of which is associated with a boundary condition.
A patch is a list of face labels which clearly must contain only boundary faces and no
internal faces. The boundary is required to be closed, i.e. the sum all boundary face area
vectors equates to zero to machine tolerance.

5.1.2

The polyMesh description

The constant directory contains a full description of the case polyMesh in a subdirectory
polyMesh. The polyMesh description is based around faces and, as already discussed,
internal cells connect 2 cells and boundary faces address a cell and a boundary patch.
Each face is therefore assigned an ‘owner’ cell and ‘neighbour’ cell so that the connectivity
across a given face can simply be described by the owner and neighbour cell labels. In
the case of boundaries, the connected cell is the owner and the neighbour is assigned the
label ‘-1’. With this in mind, the I/O specification consists of the following files:
points a list of vectors describing the cell vertices, where the first vector in the list represents vertex 0, the second vector represents vertex 1, etc.;
faces a list of faces, each face being a list of indices to vertices in the points list, where
again, the first entry in the list represents face 0, etc.;
owner a list of owner cell labels, the index of entry relating directly to the index of the
face, so that the first entry in the list is the owner label for face 0, the second entry
is the owner label for face 1, etc;
neighbour a list of neighbour cell labels;
boundary a list of patches, containing a dictionary entry for each patch, declared using
the patch name, e.g.
movingWall
{
type patch;
nFaces 20;
startFace 760;
Open∇FOAM-1.6

U-126

Mesh generation and conversion

}
The startFace is the index into the face list of the first face in the patch, and
nFaces is the number of faces in the patch.
Note that if the user wishes to know how many cells are in their domain, there is a
note in the FoamFile header of the owner file that contains an entry for nCells.

5.1.3

The cellShape tools

We shall describe the alternative cellShape tools that may be used particularly when
converting some standard (simpler) mesh formats for the use with OpenFOAM library.
The vast majority of mesh generators and post-processing systems support only a
fraction of the possible polyhedral cell shapes in existence. They define a mesh in terms
of a limited set of 3D cell geometries, referred to as cell shapes. The OpenFOAM library
contains definitions of these standard shapes, to enable a conversion of such a mesh into
the polyMesh format described in the previous section.
The cellShape models supported by OpenFOAM are shown in Table 5.1. The shape is
defined by the ordering of point labels in accordance with the numbering scheme contained
in the shape model. The ordering schemes for points, faces and edges are shown in
Table 5.1. The numbering of the points must not be such that the shape becomes twisted
or degenerate into other geometries, i.e. the same point label cannot be used more that
once is a single shape. Moreover it is unnecessary to use duplicate points in OpenFOAM
since the available shapes in OpenFOAM cover the full set of degenerate hexahedra.
The cell description consists of two parts: the name of a cell model and the ordered
list of labels. Thus, using the following list of points
8
(
(0
(1
(1
(0
(0
(1
(1
(0

0
0
1
1
0
0
1
1

0)
0)
0)
0)
0.5)
0.5)
0.5)
0.5)

)

A hexahedral cell would be written as:
(hex 8(0 1 2 3 4 5 6 7))
Here the hexahedral cell shape is declared using the keyword hex. Other shapes are
described by the keywords listed in Table 5.1.

5.1.4

1- and 2-dimensional and axi-symmetric problems

OpenFOAM is designed as a code for 3-dimensional space and defines all meshes as
such. However, 1- and 2- dimensional and axi-symmetric problems can be simulated
in OpenFOAM by generating a mesh in 3 dimensions and applying special boundary
conditions on any patch in the plane(s) normal to the direction(s) of interest. More
specifically, 1- and 2- dimensional problems use the empty patch type and axi-symmetric
problems use the wedge type. The use of both are described in section 5.2.2 and the
generation of wedge geometries for axi-symmetric problems is discussed in section 5.3.3.
Open∇FOAM-1.6

U-127

5.2 Boundaries

Cell type

Keyword

Vertex numbering Face numbering Edge numbering
7

Hexahedron

hex

0
10

8
1

3
2

5
3

2
0

wedge

Wedge

3
3

3
1

8
4

Prism

prism

7
0

Pyramid

pyr

4
0

3
5

2
2

Tetrahedron tet

0
3

1 0

tetWedge

0
3

Tet-wedge

6
1

Table 5.1: Vertex, face and edge numbering for cellShapes.

Open∇FOAM-1.6

U-128

5.2

Mesh generation and conversion

Boundaries

In this section we discuss the way in which boundaries are treated in OpenFOAM. The
subject of boundaries is a little involved because their role in modelling is not simply that
of a geometric entity but an integral part of the solution and numerics through boundary
conditions or inter-boundary ‘connections’. A discussion of boundaries sits uncomfortably
between a discussion on meshes, fields, discretisation, computational processing etc. Its
placement in this Chapter on meshes is a choice of convenience.
We first need to consider that, for the purpose of applying boundary conditions, a
boundary is generally broken up into a set of patches. One patch may include one or
more enclosed areas of the boundary surface which do not necessarily need to be physically
connected.
There are three attributes associated with a patch that are described below in their
natural hierarchy and Figure 5.2 shows the names of different patch types introduced
at each level of the hierarchy. The hierarchy described below is very similar, but not
identical, to the class hierarchy used in the OpenFOAM library.
Base type The type of patch described purely in terms of geometry or a data ‘communication link’.
Primitive type The base numerical patch condition assigned to a field variable on the
patch.
Derived type A complex patch condition, derived from the primitive type, assigned to
a field variable on the patch.

Base type

patch
wall

symmetry
empty
wedge
cyclic
processor

Primitive type

fixedValue
fixedGradient
zeroGradient
mixed
directionMixed
calculated

Derived type

e.g.inletOutlet
Figure 5.2: Patch attributes

5.2.1

Specification of patch types in OpenFOAM

The patch types are specified in the mesh and field files of a OpenFOAM case. More
precisely:
• the base type is specified under the type keyword for each patch in the boundary
file, located in the constant/polyMesh directory;
Open∇FOAM-1.6

U-129

5.2 Boundaries

• the numerical patch type, be it a primitive or derived type, is specified under the
type keyword for each patch in a field file.
An example boundary file is shown below for a sonicFoam case, followed by a pressure
field file, p, for the same case:
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50

6
(

)

inlet
{
type
nFaces
startFace
}
outlet
{
type
nFaces
startFace
}
bottom
{
type
nFaces
startFace
}
top
{
type
nFaces
startFace
}
obstacle
{
type
nFaces
startFace
}
defaultFaces
{
type
nFaces
startFace
}

patch;
50;
10325;
patch;
40;
10375;
symmetryPlane;
25;
10415;

symmetryPlane;
125;
10440;
patch;
110;
10565;
empty;
10500;
10675;

// ************************************************************************* //
dimensions

[1 -1 -2 0 0 0 0];

internalField

uniform 1;

boundaryField
{
inlet
{
type
value
}

fixedValue;
uniform 1;

outlet
{
type
field
phi
rho
psi
gamma
fieldInf
lInf
value
}

waveTransmissive;
p;
phi;
rho;
psi;
1.4;
1;
3;
uniform 1;

bottom
{
type
}

symmetryPlane;

top
{

type

symmetryPlane;

}

Open∇FOAM-1.6

U-130
51
52
53
54
55
56
57
58
59
60
61
62
63

}

Mesh generation and conversion

obstacle
{
type
}

zeroGradient;

defaultFaces
{
type
}

empty;

// ************************************************************************* //

The type in the boundary file is patch for all patches except those that patches that have
some geometrical constraint applied to them, i.e. the symmetryPlane and empty patches.
The p file includes primitive types applied to the inlet and bottom faces, and a more
complex derived type applied to the outlet. Comparison of the two files shows that the
base and numerical types are consistent where the base type is not a simple patch, i.e.
for the symmetryPlane and empty patches.

5.2.2

Base types

The base and geometric types are described below; the keywords used for specifying these
types in OpenFOAM are summarised in Table 5.2.
wedge patch 2

Axis of symmetry

5◦

wedge patch 1

wedge aligned along
coordinate plane
Figure 5.3: Axi-symmetric geometry using the wedge patch type.

Selection Key
patch
symmetryPlane
empty
wedge
cyclic
wall
processor

Description
generic patch
plane of symmetry
front and back planes of a 2D geometry
wedge front and back for an axi-symmetric geometry
cyclic plane
wall — used for wall functions in turbulent flows
inter-processor boundary
Table 5.2: Basic patch types.

Open∇FOAM-1.6

U-131

5.2 Boundaries

patch The basic patch type for a patch condition that contains no geometric or topological
information about the mesh (with the exception of wall), e.g. an inlet or an outlet.
wall There are instances where a patch that coincides with a wall needs to be identifiable
as such, particularly where specialist modelling is applied at wall boundaries. A
good example is wall turbulence modelling where a wall must be specified with a
wall patch type, so that the distance from the wall of the cell centres next to the
wall are stored as part of the patch.
symmetryPlane For a symmetry plane.
empty While OpenFOAM always generates geometries in 3 dimensions, it can be instructed to solve in 2 (or 1) dimensions by specifying a special empty condition on
each patch whose plane is normal to the 3rd (and 2nd) dimension for which no
solution is required.
wedge For 2 dimensional axi-symmetric cases, e.g. a cylinder, the geometry is specified as
a wedge of 5◦ angle and 1 cell thick running along the plane of symmetry, straddling
one of the coordinate planes, as shown in Figure 5.3. The axi-symmetric wedge
planes must be specified as separate patches of wedge type. The details of generating
wedge-shaped geometries using blockMesh are described in section 5.3.3.
cyclic Enables two patches to be treated as if they are physically connected; used for
repeated geometries, e.g. heat exchanger tube bundles. A single cyclic patch splits
the faces in its faceList into two, and links the two sets of faces as shown in Figure 5.4.
Each face-face pair must be of the same area but the faces do not need to be of the
same orientation.
processor If a code is being run in parallel, on a number of processors, then the mesh
must be divided up so that each processor computes on roughly the same number
of cells. The boundaries between the different parts of the mesh are called processor
boundaries.
Repeated geometry
cyclic
faceList
1
2
3
4
5
6

1
2
3

4
5
6
computational links
Figure 5.4: Repeated geometry using the cyclic patch type.

Open∇FOAM-1.6

U-132

5.2.3

Mesh generation and conversion

Primitive types

The primitive types are listed in Table 5.3.
Type
fixedValue
fixedGradient
zeroGradient
calculated
mixed

Description of condition for patch field φ
Value of φ is specified
Normal gradient of φ is specified
Normal gradient of φ is zero
Boundary field φ derived from other fields
Mixed fixedValue/ fixedGradient condition depending on the value in valueFraction

Data to specify
value
gradient
—
—
refValue,
refGradient,
valueFraction,
value
directionMixed A mixed condition normal to the patch with a refValue,
fixedGradient condition tangential to the patch
refGradient,
valueFraction,
value
Table 5.3: Primitive patch field types.

5.2.4

Derived types

There are numerous derived types of boundary conditions in OpenFOAM, too many to
list here. Instead a small selection is listed in Table 5.4. If the user wishes to obtain
a list of all available model, they should consult the OpenFOAM source code. Derived
boundary condition source code can be found at the following locations:
• in $FOAM SRC/finiteVolume/fields/fvPatchFields/derived
• within certain model libraries, that can be located by typing the following command
in a terminal window
find $FOAM SRC -name "*derivedFvPatch*"
• within certain solvers, that can be located by typing the following command in a
terminal window
find $FOAM SOLVERS -name "*fvPatch*"

5.3

Mesh generation with the blockMesh utility

This section describes the mesh generation utility, blockMesh, supplied with OpenFOAM.
The blockMesh utility creates parametric meshes with grading and curved edges.
The mesh is generated from a dictionary file named blockMeshDict located in the
constant/polyMesh directory of a case. blockMesh reads this dictionary, generates the
mesh and writes out the mesh data to points and faces, cells and boundary files in the
same directory.
The principle behind blockMesh is to decompose the domain geometry into a set of 1
or more three dimensional, hexahedral blocks. Edges of the blocks can be straight lines,
Open∇FOAM-1.6

surfaceNormalFixedValue
totalPressure
turbulentInlet

Data to specify
value
value
value,
inletDirection
Specifies a vector boundary condition, normal to the patch, by its magnitude; +ve value
for vectors pointing out of the domain
Total pressure p0 = p + 12 ρ|U|2 is fixed; when U changes, p is adjusted accordingly p0
Calculates a fluctuating variable based on a scale of a mean value
referenceField,
fluctuationScale

Types derived from fixedGradient/zeroGradient
fluxCorrectedVelocity
Calculates normal component of U at inlet from flux
wallBuoyantPressure
Sets fixedGradient pressure based on the atmospheric pressure gradient

value
—

Types derived from mixed
inletOutlet
Switches U and p between fixedValue and zeroGradient depending on direction of U inletValue, value
outletInlet
Switches U and p between fixedValue and zeroGradient depending on direction of U outletValue,
value
pressureInletOutletVelocity Combination of pressureInletVelocity and inletOutlet
value
pressureDirectedCombination of pressureDirectedInletVelocity and inletOutlet
value,
InletOutletVelocity
inletDirection
pressureTransmissive
Transmits supersonic pressure waves to surrounding pressure p∞
pInf
supersonicFreeStream
Transmits oblique shocks to surroundings at p∞ , T∞ , U∞
pInf, TInf, UInf

zeroGradient if φ is a scalar; if φ is a vector, normal component is fixedValue zero,
tangential components are zeroGradient
partialSlip
Mixed zeroGradient/ slip condition depending on the valueFraction; = 1 for slip
Note: p is pressure, U is velocity
Table 5.4: Derived patch field types.

—
valueFraction
U-133

Open∇FOAM-1.6

Other types
slip

5.3 Mesh generation with the blockMesh utility

Types derived from fixedValue
movingWallVelocity
Replaces the normal of the patch value so the flux across the patch is zero
pressureInletVelocity
When p is known at inlet, U is evaluated from the flux, normal to the patch
pressureDirectedInletVelocity When p is known at inlet, U is calculated from the flux in the inletDirection

U-134

Mesh generation and conversion

arcs or splines. The mesh is ostensibly specified as a number of cells in each direction of
the block, sufficient information for blockMesh to generate the mesh data.
Each block of the geometry is defined by 8 vertices, one at each corner of a hexahedron.
The vertices are written in a list so that each vertex can be accessed using its label,
remembering that OpenFOAM always uses the C++ convention that the first element of
the list has label ‘0’. An example block is shown in Figure 5.5 with each vertex numbered
according to the list. The edge connecting vertices 1 and 5 is curved to remind the reader
that curved edges can be specified in blockMesh.
It is possible to generate blocks with less than 8 vertices by collapsing one or more
pairs of vertices on top of each other, as described in section 5.3.3.
Each block has a local coordinate system (x1 , x2 , x3 ) that must be right-handed. A
right-handed set of axes is defined such that to an observer looking down the Oz axis,
with O nearest them, the arc from a point on the Ox axis to a point on the Oy axis is in
a clockwise sense.
The local coordinate system is defined by the order in which the vertices are presented
in the block definition according to:
• the axis origin is the first entry in the block definition, vertex 0 in our example;
• the x1 direction is described by moving from vertex 0 to vertex 1;

U-135

5.3 Mesh generation with the blockMesh utility

Keyword
Description
convertToMeters Scaling factor for the vertex
coordinates
vertices
List of vertex coordinates
edges
Used to describe arc or
spline edges
block
Ordered list of vertex labels
and mesh size
patches

List of patches

mergePatchPairs List of patches to be merged

Example/selection
0.001 scales to mm
(0 0 0)
arc 1 4 (0.939 0.342 -0.5)
hex (0 1 2 3 4 5 6 7)
(10 10 1)
simpleGrading (1.0 1.0 1.0)
symmetryPlane base
( (0 1 2 3) )
see section 5.3.2

Table 5.5: Keywords used in blockMeshDict.

convertToMeters

0.001;

means that all coordinates are multiplied by 0.001, i.e. the values quoted in the blockMeshDict file are in mm.
5.3.1.1

The vertices

The vertices of the blocks of the mesh are given next as a standard list named vertices,
e.g. for our example block in Figure 5.5, the vertices are:
vertices
(
( 0
0
( 1
0
( 1.1 1
( 0
1
(-0.1 -0.1
( 1.3 0
( 1.4 1.1
( 0
1
);
5.3.1.2

0 )
0.1)
0.1)
0.1)
1 )
1.2)
1.3)
1.1)

//
//
//
//
//
//
//
//

vertex
vertex
vertex
vertex
vertex
vertex
vertex
vertex

number
number
number
number
number
number
number
number

0
1
2
3
4
5
6
7

The edges

Each edge joining 2 vertex points is assumed to be straight by default. However any edge
may be specified to be curved by entries in a list named edges. The list is optional; if
the geometry contains no curved edges, it may be omitted.
Each entry for a curved edge begins with a keyword specifying the type of curve from
those listed in Table 5.6.
The keyword is then followed by the labels of the 2 vertices that the edge connects.
Following that, interpolation points must be specified through which the edge passes.
For a arc, a single interpolation point is required, which the circular arc will intersect.
For simpleSpline, polyLine and polySpline, a list of interpolation points is required.
The line edge is directly equivalent to the option executed by default, and requires no
Open∇FOAM-1.6

U-136

Mesh generation and conversion

Keyword selection
arc
simpleSpline
polyLine
polySpline
line

Description
Additional entries
Circular arc
Single interpolation point
Spline curve List of interpolation points
Set of lines
List of interpolation points
Set of splines List of interpolation points
Straight line —

Table 5.6: Edge types available in the blockMeshDict dictionary.

interpolation points. Note that there is no need to use the line edge but it is included
for completeness. For our example block in Figure 5.5 we specify an arc edge connecting
vertices 1 and 5 as follows through the interpolation point (1.1, 0.0, 0.5):
edges
(
arc 1 5 (1.1 0.0 0.5)
);
5.3.1.3

The blocks

The block definitions are contained in a list named blocks. Each block definition is a
compound entry consisting of a list of vertex labels whose order is described in section 5.3,
a vector giving the number of cells required in each direction, the type and list of cell
expansion ratio in each direction.
Then the blocks are defined as follows:
blocks
(
hex (0 1 2 3 4 5 6 7)
(10 10 10)
simpleGrading (1 2 3)
);

// vertex numbers
// numbers of cells in each direction
// cell expansion ratios

The definition of each block is as follows:
Vertex numbering The first entry is the is the shape identifier of the block, as defined
in the .OpenFOAM-1.6/cellModels file. The shape is always hex since the blocks are
always hexahedra. There follows a list of vertex numbers, ordered in the manner
described on page U-134.
Number of cells The second entry gives the number of cells in each of the x1 x2 and
x3 directions for that block.
Cell expansion ratios The third entry gives the cell expansion ratios for each direction
in the block. The expansion ratio enables the mesh to be graded, or refined, in
specified directions. The ratio is that of the width of the end cell δe along one edge
of a block to the width of the start cell δs along that edge, as shown in Figure 5.6.
Each of the following keywords specify one of two types of grading specification
available in blockMesh.
simpleGrading The simple description specifies uniform expansions in the local x1 ,
x2 and x3 directions respectively with only 3 expansion ratios, e.g.
Open∇FOAM-1.6

U-137

5.3 Mesh generation with the blockMesh utility

simpleGrading (1 2 3)
edgeGrading The full cell expansion description gives a ratio for each edge of the
block, numbered according to the scheme shown in Figure 5.5 with the arrows
representing the direction ‘from first cell. . . to last cell’ e.g. something like
edgeGrading (1 1 1 1 2 2 2 2 3 3 3 3)
This means the ratio of cell widths along edges 0-3 is 1, along edges 4-7 is 2
and along 8-11 is 3 and is directly equivalent to the simpleGrading example
given above.

δs

Expansion ratio =

δe
δs

δe

Expansion direction
Figure 5.6: Mesh grading along a block edge

5.3.1.4

The patches

The patches of the mesh are given in a list named patches. Each patch in the list is a
compound entry containing:
• the patch type, either a generic patch on which some boundary conditions are
applied or a particular geometric condition, as listed in Table 5.2 and described in
section 5.2.2;
• a list of block faces that make up the patch and whose name is the choice of the
the user, although we recommend something that conveniently identifies the patch,
e.g. quoteTextinlet; the name is used as an identifier for for for setting boundary
conditions in the field data files.
blockMesh collects faces from any boundary patch that is omitted from the patches
list and assigns them to a default patch named defaultFaces of type empty. This means
that for a 2 dimensional geometry, the user has the option to omit block faces lying in
the 2D plane, knowing that they will be collected into an empty patch as required.
Returning to the example block in Figure 5.5, if it has an inlet on the left face, an
output on the right face and the four other faces are walls then the patches could be
defined as follows:
patches
(
patch
inlet
(
(0 4 7 3)
)
patch
outlet
(
(1 2 6 5)

// keyword
// patch type for patch 0
// patch name
// block face in this patch
// end of 0th patch definition
// patch type for patch 1
// arbitrary patch name

Open∇FOAM-1.6

U-138

Mesh generation and conversion

)
wall
walls
(
(0
(0
(3
(4
)

1
3
7
5

5
2
6
6

4)
1)
2)
7)

);
Each block face is defined by a list of 4 vertex numbers. The order in which the vertices
are given must be such that, looking from inside the block and starting with any vertex,
the face must be traversed in a clockwise direction to define the other vertices.

5.3.2

Multiple blocks

A mesh can be created using more than 1 block. In such circumstances, the mesh is
created as has been described in the preceeding text; the only additional issue is the
connection between blocks, in which there are two distinct possibilities:
face matching the set of faces that comprise a patch from one block are exactly collocated with a set of faces patch that comprise a patch from another block;
face merging a group of faces from a patch from one block are connected to another
group of faces from a patch from another block, to create a new set of internal faces
connecting the two blocks.
To connect two blocks with face matching, the two patches that form the connection
should simply be ignored from the patches list. blockMesh then identifies that the faces
do not form an external boundary and combines each collocated pair into a single internal
faces that connects cells from the two blocks.
The alternative, face merging, requires that the block patches to be merged are first
defined in the patches list. Each pair of patches whose faces are to be merged must then
be included in an optional list named mergePatchPairs. The format of mergePatchPairs
is:
mergePatchPairs
(
( ) // merge patch pair 0
( ) // merge patch pair 1
...
)
The pairs of patches are interpreted such that the first patch becomes the master and
the second becomes the slave. The rules for merging are as follows:
• the faces of the master patch remain as originally defined, with all vertices in their
original location;
• the faces of the slave patch are projected onto the master patch where there is some
separation between slave and master patch;
Open∇FOAM-1.6

5.3 Mesh generation with the blockMesh utility

U-139

• the location of any vertex of a slave face might be adjusted by blockMesh to eliminate
any face edge that is shorter than a minimum tolerance;
• if patches overlap as shown in Figure 5.7, each face that does not merge remains as
an external face of the original patch, on which boundary conditions must then be
applied;
• if all the faces of a patch are merged, then the patch itself will contain no faces and
is removed.

patch 1

patch 2

region of internal connecting faces
region of external boundary faces
Figure 5.7: Merging overlapping patches
The consequence is that the original geometry of the slave patch will not necessarily be
completely preserved during merging. Therefore in a case, say, where a cylindrical block
is being connected to a larger block, it would be wise to the assign the master patch to the
cylinder, so that its cylindrical shape is correctly preserved. There are some additional
recommendations to ensure successful merge procedures:
• in 2 dimensional geometries, the size of the cells in the third dimension, i.e. out of
the 2D plane, should be similar to the width/height of cells in the 2D plane;
• it is inadvisable to merge a patch twice, i.e. include it twice in mergePatchPairs;
• where a patch to be merged shares a common edge with another patch to be merged,
both should be declared as a master patch.

5.3.3

Creating blocks with fewer than 8 vertices

It is possible to collapse one or more pair(s) of vertices onto each other in order to create
a block with fewer than 8 vertices. The most common example of collapsing vertices is
when creating a 6-sided wedge shaped block for 2-dimensional axi-symmetric cases that
use the wedge patch type described in section 5.2.2. The process is best illustrated by
using a simplified version of our example block shown in Figure 5.8. Let us say we wished
to create a wedge shaped block by collapsing vertex 7 onto 4 and 6 onto 5. This is simply
done by exchanging the vertex number 7 by 4 and 6 by 5 respectively so that the block
numbering would become:
Open∇FOAM-1.6

U-140

Mesh generation and conversion

hex (0 1 2 3 4 5 5 4)

Figure 5.8: Creating a wedge shaped block with 6 vertices
The same applies to the patches with the main consideration that the block face
containing the collapsed vertices, previously (4 5 6 7) now becomes (4 5 5 4). This
is a block face of zero area which creates a patch with no faces in the polyMesh, as the
user can see in a boundary file for such a case. The patch should be specified as empty
in the blockMeshDict and the boundary condition for any fields should consequently be
empty also.

5.3.4

Running blockMesh

As described in section 3.3, the following can be executed at the command line to run
blockMesh for a case in the directory:
blockMesh -case
The blockMeshDict file must exist in subdirectory constant/polyMesh.

5.4

Mesh generation with the snappyHexMesh utility

This section describes the mesh generation utility, snappyHexMesh, supplied with OpenFOAM. The snappyHexMesh utility generates 3-dimensional meshes containing hexahedra
(hex) and split-hexahedra (split-hex) automatically from triangulated surface geometries
in Stereolithography (STL) format. The mesh approximately conforms to the surface
by iteratively refining a starting mesh and morphing the resulting split-hex mesh to the
surface. An optional phase will shrink back the resulting mesh and insert cell layers. The
specification of mesh refinement level is very flexible and the surface handling is robust
with a pre-specified final mesh quality. It runs in parallel with a load balancing step every
iteration.
Open∇FOAM-1.6

U-141

5.4 Mesh generation with the snappyHexMesh utility

STL surface

Figure 5.9: Schematic 2D meshing problem for snappyHexMesh

5.4.1

The mesh generation process of snappyHexMesh

The process of generating a mesh using snappyHexMesh will be described using the
schematic in Figure 5.9. The objective is to mesh a rectangular shaped region (shaded
grey in the figure) surrounding an object described by and STL surface, e.g. typical for
an external aerodynamics simulation. Note that the schematic is 2-dimensional to make
it easier to understand, even though the snappyHexMesh is a 3D meshing tool.
In order to run snappyHexMesh, the user requires the following:
• surface data files in STL format, either binary or ASCII, located in a triSurface
sub-directory of the case directory;
• a background hex mesh which defines the extent of the computational domain
and a base level mesh density; typically generated using blockMesh, discussed in
section 5.4.2.
• a snappyHexMeshDict dictionary, with appropriate entries, located in the system
sub-directory of the case.
The snappyHexMeshDict dictionary includes: switches at the top level that control the
various stages of the meshing process; and, individual sub-directories for each process.
The entries are listed in Table 5.7.
All the geometry used by snappyHexMesh is specified in a geometry sub-dictionary
in the snappyHexMeshDict dictionary. The geometry can be specified through an STL
surface or bounding geometry entities in OpenFOAM. An example is given below:
geometry
{
sphere.stl // STL filename
{
type triSurfaceMesh;
regions
{
secondSolid
// Named region in the STL file
{
name mySecondPatch; // User-defined patch name
}
// otherwise given sphere.stl_secondSolid
}
}
box1x1x1
{
type
min

// User defined region name
searchableBox;
(1.5 1 -0.5);

// region defined by bounding box

Open∇FOAM-1.6

U-142

Mesh generation and conversion

Keyword
castellatedMesh
snap
doLayers
mergeTolerance

Description
Example
Create the castellated mesh?
true
Do the surface snapping stage?
true
Add surface layers?
true
Merge tolerance as fraction of bounding box 1e-06
of initial mesh
debug
Controls writing of intermediate meshes and
screen printing
— Write final mesh only
0
— Write intermediate meshes
1
— Write volScalarField with cellLevel for 2
post-processing
— Write current intersections as .obj files
4
geometry
Sub-dictionary of all surface geometry used
castellatedMeshControls Sub-dictionary of controls for castellated mesh
snapControls
Sub-dictionary of controls for surface snapping
addLayersControls
Sub-dictionary of controls for layer addition
meshQualityControls
Sub-dictionary of controls for mesh quality
Table 5.7: Keywords at the top level of snappyHexMeshDict.

max

(3.5 2 0.5);

}
sphere2 // User defined region name
{
type
searchableSphere;
// region defined by bounding sphere
centre (1.5 1.5 1.5);
radius 1.03;
}
};

5.4.2

Creating the background hex mesh

Before snappyHexMesh is executed the user must create a background mesh of hexahedral
cells that fills the entire region within by the external boundary as shown in Figure 5.10.
This can be done simply using blockMesh. The following criteria must be observed when

5.4 Mesh generation with the snappyHexMesh utility

U-143

• the mesh must consist purely of hexes;
• the cell aspect ratio should be approximately 1, at least near surfaces at which
the subsequent snapping procedure is applied, otherwise the convergence of the
snapping procedure is slow, possibly to the point of failure;
• there must be at least one intersection of a cell edge with the STL surface, i.e. a
mesh of one cell will not work.

5.4.3

Cell splitting at feature edges and surfaces

Cell splitting is performed according to the specification supplied by the user in the
castellatedMeshControls sub-dictionary in the snappyHexMeshDict. The entries for castellatedMeshControls are presented in Table 5.8.
Keyword
locationInMesh

Description
Example
Location vector inside the region to be meshed (5 0 0)
N.B. vector must not coincide with a cell face either before
or during refinement
maxLocalCells
Max number of cells per processor during re- 1e+06
finement
maxGlobalCells
Overall cell limit during refinement (i.e. before 2e+06
removal)
minRefinementCells
If ≥ number of cells to be refined, surface re- 0
finement stops
nCellsBetweenLevels Number of buffer layers of cells between dif- 1
ferent levels of refinement
resolveFeatureAngle Applies maximum level of refinement to cells 30
that can see intersections whose angle exceeds
this
features
List of features for refinement
refinementSurfaces
Dictionary of surfaces for refinement
refinementRegions
Dictionary of regions for refinement
Table 5.8: Keywords in the castellatedMeshControls sub-dictionary of snappyHexMeshDict.
The splitting process begins with cells being selected according to specified edge features first within the domain as illustrated in Figure 5.11. The features list in the
castellatedMeshControls sub-dictionary permits dictionary entries containing a name of an
edgeMesh file and the level of refinement, e.g.:
features
(
{
file "someLine.eMesh"; // file containing edge mesh
level 2;
// level of refinement
}
);

Following feature refinement, cells are selected for splitting in the locality of specified
surfaces as illustrated in Figure 5.12. The refinementSurfaces dictionary in castellatedMeshControls requires dictionary entries for each STL surface and a default level
specification of the minimum and maximum refinement in the form ( ).
Open∇FOAM-1.6

U-144

Mesh generation and conversion

Figure 5.11: Cell splitting by feature edge in snappyHexMesh meshing process

Figure 5.12: Cell splitting by surface in snappyHexMesh meshing process
The minimum level is applied generally across the surface; the maximum level is applied to cells that can see intersections that form an angle in excess of that specified by
resolveFeatureAngle.
The refinement can optionally be overridden on one or more specific region of an STL
surface. The region entries are collected in a regions sub-dictionary. The keyword for
each region entry is the name of the region itself and the refinement level is contained
within a further sub-dictionary. An example is given below:
refinementSurfaces
{
sphere.stl
{
level (2 2); // default (min max) refinement for whole surface
regions
{
secondSolid
{
level (3 3); // optional refinement for secondSolid region
}
}
}
}

5.4.4

Cell removal

Once the feature and surface splitting is complete a process of cell removal begins. Cell
removal requires one or more regions enclosed entirely by a bounding surface within the
Open∇FOAM-1.6

U-145

5.4 Mesh generation with the snappyHexMesh utility

domain. The region in which cells are retained are simply identified by a location vector
within that region, specified by the locationInMesh keyword in castellatedMeshControls.
Cells are retained if, approximately speaking, 50% or more of their volume lies within the
region. The remaining cells are removed accordingly as illustrated in Figure 5.13.

Figure 5.13: Cell removal in snappyHexMesh meshing process

5.4.5

Cell splitting in specified regions

Those cells that lie within one or more specified volume regions can be further split as illustrated in Figure 5.14 by a rectangular region shown by dark shading. The refinement-

Figure 5.14: Cell splitting by region in snappyHexMesh meshing process
Regions sub-dictionary in castellatedMeshControls contains entries for refinement of the
volume regions specified in the geometry sub-dictionary. A refinement mode is applied to
each region which can be:
• inside refines inside the volume region;
• outside refines outside the volume region
• distance refines according to distance to the surface; and can accommodate different levels at multiple distances with the levels keyword.
Open∇FOAM-1.6

U-146

Mesh generation and conversion

For the refinementRegions, the refinement level is specified by the levels list of entries
with the format( ). In the case of inside and outside refinement,
the is not required so is ignored (but it must be specified). Examples are
shown below:
refinementRegions
{
box1x1x1
{
mode inside;
levels ((1.0 4));
}

// refinement level 4 (1.0 entry ignored)

sphere.stl
{
// refinement level 5 within 1.0 m
mode distance;
// refinement level 3 within 2.0 m
levels ((1.0 5) (2.0 3)); // levels must be ordered nearest first
}
}

5.4.6

Snapping to surfaces

The next stage of the meshing process involves moving cell vertex points onto surface
geometry to remove the jagged castellated surface from the mesh. The process is:
1. displace the vertices in the castellated boundary onto the STL surface;
2. solve for relaxation of the internal mesh with the latest displaced boundary vertices;
3. find the vertices that cause mesh quality parameters to be violated;
4. reduce the displacement of those vertices from their initial value (at 1) and repeat
from 2 until mesh quality is satisfied.
The method uses the settings in the snapControls sub-dictionary in snappyHexMeshDict,
listed in Table 5.9. An example is illustrated in the schematic in Figure 5.15 (albeit with
Keyword
Description
nSmoothPatch Number of patch smoothing iterations before
finding correspondence to surface
tolerance
Ratio of distance for points to be attracted
by surface feature point or edge, to local
maximum edge length
nSolveIter
Number of mesh displacement relaxation iterations
nRelaxIter
Maximum number of snapping relaxation iterations

Example
3
4.0

30
5

Table 5.9: Keywords in the snapControls dictionary of snappyHexMeshDict.
mesh motion that looks slightly unrealistic).

5.4.7

Mesh layers

The mesh output from the snapping stage may be suitable for the purpose, although it
can produce some irregular cells along boundary surfaces. There is an optional stage of
the meshing process which introduces additional layers of hexahedral cells aligned to the
boundary surface as illustrated by the dark shaded cells in Figure 5.16.
Open∇FOAM-1.6

5.4 Mesh generation with the snappyHexMesh utility

Figure 5.15: Surface snapping in snappyHexMesh meshing process

U-147

U-148

Mesh generation and conversion

Keyword
layers
relativeSizes

Description
Dictionary of layers
Are layer thicknesses relative to undistorted cell
size outside layer or absolute?
expansionRatio
Expansion factor for layer mesh
finalLayerRatio
Thickness of layer furthest from the wall, either relative or absolute according to the
relativeSizes entry
minThickness
Minimum thickness of cell layer, either relative
or absolute (as above)
nGrow
Number of layers of connected faces that are not
grown if points get not extruded; helps convergence of layer addition close to features
featureAngle
Angle above which surface is not extruded
nRelaxIter
Maximum number of snapping relaxation iterations
nSmoothSurfaceNormals Number of smoothing iterations of surface normals
nSmoothNormals
Number of smoothing iterations of interior mesh
movement direction
nSmoothThickness
Smooth layer thickness over surface patches
maxFaceThicknessRatio Stop layer growth on highly warped cells
maxThicknessToReduce layer growth where ratio thickness to meMedialRatio
dial distance is large
minMedianAxisAngle
Angle used to pick up medial axis points
nBufferCellsNoExtrude Create buffer region for new layer terminations
nLayerIter
Overall max number of layer addition iterations
nRelaxedIter
Max number of iterations after which the
controls in the relaxed sub dictionary of
meshQuality are used

Example
true/false
1.0
0.3

0.25
1

60
5
1
3
10
0.5
0.3
130
0
50
20

Table 5.10: Keywords in the addLayersControls sub-dictionary of snappyHexMeshDict.

{
nSurfaceLayers 1;
}
maxY
{
nSurfaceLayers 1;
}
}

5.4.8

Mesh quality controls

The mesh quality is controlled by the entries in the meshQualityControls sub-dictionary
in snappyHexMeshDict; entries are listed in Table 5.11.

5.5

Mesh conversion

The user can generate meshes using other packages and convert them into the format
that OpenFOAM uses. There are numerous mesh conversion utilities listed in Table 3.6.
Open∇FOAM-1.6

U-149

5.5 Mesh conversion

Keyword
maxNonOrtho

Description
Maximum non-orthogonality allowed; 180 disables
maxBoundarySkewness Max boundary face skewness allowed; <0 disables
maxInternalSkewness Max internal face skewness allowed; <0 disables
maxConcave
Max concaveness allowed; 180 disables
minFlatness
Ratio of minimum projected area to actual area;
-1 disables
minVol
Minimum pyramid volume; large negative number, e.g.-1e30 disables
minArea
Minimum face area; <0 disables
minTwist
Minimum face twist; <-1 disables
minDeterminant
Minimum normalised cell determinant; 1 = hex;
≤ 0 illegal cell
minFaceWeight
0→0.5
minVolRatio
0→1.0
minTriangleTwist
>0 for Fluent compatability
nSmoothScale
Number of error distribution iterations
errorReduction
Amount to scale back displacement at error
points
relaxed
Sub-dictionary that can include modified values
for the above keyword entries to be used when
nRelaxedIter is exceeded in the layer addition
process

Example
65
20
4
80
0.5
1e-13
-1
0.05
0.001
0.05
0.01
-1
4
0.75
relaxed
{
...
}

Table 5.11: Keywords in the meshQualityControls sub-dictionary of snappyHexMeshDict.

Some of the more popular mesh converters are listed below and their use is presented in
this section.
fluentMeshToFoam reads a Fluent.msh mesh file, working for both 2-D and 3-D cases;
starToFoam reads STAR-CD/PROSTAR mesh files.
gambitToFoam reads a GAMBIT.neu neutral file;
ideasToFoam reads an I-DEAS mesh written in ANSYS.ans format;
cfx4ToFoam reads a CFX mesh written in .geo format;

5.5.1

fluentMeshToFoam

Fluent writes mesh data to a single file with a .msh extension. The file must be written
in ASCII format, which is not the default option in Fluent. It is possible to convert
single-stream Fluent meshes, including the 2 dimensional geometries. In OpenFOAM, 2
dimensional geometries are currently treated by defining a mesh in 3 dimensions, where
the front and back plane are defined as the empty boundary patch type. When reading
a 2 dimensional Fluent mesh, the converter automatically extrudes the mesh in the third
direction and adds the empty patch, naming it frontAndBackPlanes.
The following features should also be observed.
Open∇FOAM-1.6

U-150

Mesh generation and conversion

• The OpenFOAM converter will attempt to capture the Fluent boundary condition

U-151

5.5 Mesh conversion

5.5.2.1

General advice on conversion

We strongly recommend that the user run the STAR-CD mesh checking tools before
attempting a starToFoam conversion and, after conversion, the checkMesh utility should
be run on the newly converted mesh. Alternatively, starToFoam may itself issue warnings
containing PROSTAR commands that will enable the user to take a closer look at cells with
problems. Problematic cells and matches should be checked and fixed before attempting
to use the mesh with OpenFOAM. Remember that an invalid mesh will not run with
OpenFOAM, but it may run in another environment that does not impose the validity
criteria.
Some problems of tolerance matching can be overcome by the use of a matching
tolerance in the converter. However, there is a limit to its effectiveness and an apparent
need to increase the matching tolerance from its default level indicates that the original
mesh suffers from inaccuracies.
5.5.2.2

Eliminating extraneous data

When mesh generation in is completed, remove any extraneous vertices and compress the
cells boundary and vertex numbering, assuming that fluid cells have been created and all
other cells are discarded. This is done with the following PROSTAR commands:
CSET NEWS FLUID
CSET INVE
The CSET should be empty. If this is not the case, examine the cells in CSET and adjust
the model. If the cells are genuinely not desired, they can be removed using the PROSTAR
command:
CDEL CSET
Similarly, vertices will need to be discarded as well:
CSET NEWS FLUID
VSET NEWS CSET
VSET INVE
Before discarding these unwanted vertices, the unwanted boundary faces have to be collected before purging:
CSET
VSET
BSET
BSET

NEWS FLUID
NEWS CSET
NEWS VSET ALL
INVE

If the BSET is not empty, the unwanted boundary faces can be deleted using:
BDEL BSET
At this time, the model should contain only the fluid cells and the supporting vertices,
as well as the defined boundary faces. All boundary faces should be fully supported by the
vertices of the cells, if this is not the case, carry on cleaning the geometry until everything
is clean.
Open∇FOAM-1.6

U-152
5.5.2.3

Mesh generation and conversion

Removing default boundary conditions

By default, STAR-CD assigns wall boundaries to any boundary faces not explicitly associated with a boundary region. The remaining boundary faces are collected into a default
boundary region, with the assigned boundary type 0. OpenFOAM deliberately does not
have a concept of a default boundary condition for undefined boundary faces since it
invites human error, e.g. there is no means of checking that we meant to give all the
unassociated faces the default condition.
Therefore all boundaries for each OpenFOAM mesh must be specified for a mesh to
be successfully converted. The default boundary needs to be transformed into a real
one using the procedure described below:
1. Plot the geometry with Wire Surface option.
2. Define an extra boundary region with the same parameters as the default region
0 and add all visible faces into the new region, say 10, by selecting a zone option
in the boundary tool and drawing a polygon around the entire screen draw of the
model. This can be done by issuing the following commands in PROSTAR:
RDEF 10 WALL
BZON 10 ALL
3. We shall remove all previously defined boundary types from the set. Go through
the boundary regions:
BSET NEWS REGI 1
BSET NEWS REGI 2
... 3, 4, ...
Collect the vertices associated with the boundary set and then the boundary faces
associated with the vertices (there will be twice as many of them as in the original
set).
BSET
VSET
BSET
BSET
REPL

NEWS
NEWS
NEWS
DELE

REGI 1
BSET
VSET ALL
REGI 1

This should give the faces of boundary Region 10 which have been defined on top
of boundary Region 1. Delete them with BDEL BSET. Repeat these for all regions.
5.5.2.4

Renumbering the model

Renumber and check the model using the commands:
CSET NEW FLUID
CCOM CSET
VSET
VSET
VSET
VCOM

NEWS CSET
INVE (Should be empty!)
INVE
VSET

Open∇FOAM-1.6

5.5 Mesh conversion

BSET
BSET
BSET
BCOM

U-153

NEWS VSET ALL
INVE (Should be empty also!)
INVE
BSET

CHECK ALL
GEOM
Internal PROSTAR checking is performed by the last two commands, which may reveal
some other unforeseeable error(s). Also, take note of the scaling factor because PROSTAR
only applies the factor for STAR-CD and not the geometry. If the factor is not 1, use the
scalePoints utility in OpenFOAM.
5.5.2.5

Writing out the mesh data

Once the mesh is completed, place all the integral matches of the model into the couple
type 1. All other types will be used to indicate arbitrary matches.
CPSET NEWS TYPE INTEGRAL
CPMOD CPSET 1
The components of the computational grid must then be written to their own files. This
is done using PROSTAR for boundaries by issuing the command
BWRITE
by default, this writes to a .23 file (versions prior to 3.0) or a .bnd file (versions 3.0 and
higher). For cells, the command
CWRITE
outputs the cells to a .14 or .cel file and for vertices, the command
VWRITE
outputs to file a .15 or .vrt file. The current default setting writes the files in ASCII
format. If couples are present, an additional couple file with the extension .cpl needs to
be written out by typing:
CPWRITE

After outputting to the three files, exit PROSTAR or close the files. Look through
the panels and take note of all STAR-CD sub-models, material and fluid properties used
– the material properties and mathematical model will need to be set up by creating and
editinge0l74s4.876490113(o)0.2450Rf
fileber(r is ne files, exit
90.8720490113(r)-551(n)-0.99(l)-300.901(m)-0.8509(n)ia426(i)5237

U-154
5.5.2.6

Mesh generation and conversion

Problems with the .vrt file

The .vrt file is written in columns of data of specified width, rather than free format. A
typical line of data might be as follows, giving a vertex number followed by the coordinates:
19422

-0.105988957

-0.413711881E-02 0.000000000E+00

If the ordinates are written in scientific notation and are negative, there may be no space
between values, e.g.:
19423

-0.953953117E-01-0.338810333E-02 0.000000000E+00

The starToFoam converter reads the data using spaces to delimit the ordinate values and
will therefore object when reading the previous example. Therefore, OpenFOAM includes
a simple script, foamCorrectVrt to insert a space between values where necessary, i.e. it
would convert the previous example to:
19423

-0.953953117E-01 -0.338810333E-02 0.000000000E+00

The foamCorrectVrt script should therefore be executed if necessary before running the
starToFoam converter, by typing:
foamCorrectVrt .vrt
5.5.2.7

Converting the mesh to OpenFOAM format

The translator utility starToFoam can now be run to create the boundaries, cells and
points files necessary for a OpenFOAM run:
starToFoam
where is the name of the the prefix of the mesh files, including the
full or relative path. After the utility has finished running, OpenFOAM boundary types
should be specified by editing the boundary file by hand.

5.5.3

gambitToFoam

GAMBIT writes mesh data to a single file with a .neu extension. The procedure of converting a GAMBIT.neu file is first to create a new OpenFOAM case, then at a command
prompt, the user should execute:
gambitToFoam
where is the name of the .neu file, including the full or relative path.
The GAMBIT file format does not provide information about type of the boundary
patch, e.g. wall, symmetry plane, cyclic. Therefore all the patches have been created as
type patch. Please reset after mesh conversion as necessary.
Open∇FOAM-1.6

5.6 Mapping fields between different geometries

5.5.4

U-155

ideasToFoam

OpenFOAM can convert a mesh generated by I-DEAS but written out in ANSYS format
as a .ans file. The procedure of converting the .ans file is first to create a new OpenFOAM
case, then at a command prompt, the user should execute:
ideasToFoam
where is the name of the .ans file, including the full or relative path.

5.5.5

cfx4ToFoam

CFX writes mesh data to a single file with a .geo extension. The mesh format in CFX is
block-structured, i.e. the mesh is specified as a set of blocks with glueing information and
the vertex locations. OpenFOAM will convert the mesh and capture the CFX boundary
condition as best as possible. The 3 dimensional ‘patch’ definition in CFX, containing
information about the porous, solid regions etc. is ignored with all regions being converted
into a single OpenFOAM mesh. CFX supports the concept of a ‘default’ patch, where
each external face without a defined boundary condition is treated as a wall. These faces
are collected by the converter and put into a defaultFaces patch in the OpenFOAM
mesh and given the type wall; of course, the patch type can be subsequently changed.
Like, OpenFOAM 2 dimensional geometries in CFX are created as 3 dimensional
meshes of 1 cell thickness [**]. If a user wishes to run a 2 dimensional case on a mesh
created by CFX, the boundary condition on the front and back planes should be set to
empty; the user should ensure that the boundary conditions on all other faces in the
plane of the calculation are set correctly. Currently there is no facility for creating an
axi-symmetric geometry from a 2 dimensional CFX mesh.
The procedure of converting a CFX.geo file is first to create a new OpenFOAM case,
then at a command prompt, the user should execute:
cfx4ToFoam
where is the name of the .geo file, including the full or relative path.

5.6

Mapping fields between different geometries

The mapFields utility maps one or more fields relating to a given geometry onto the

U-156

5.6.1

Mesh generation and conversion

Mapping consistent fields

A mapping of consistent fields is simply performed by executing mapFields on the (target)
case using the -consistent command line option as follows:
mapFields -consistent

5.6.2

Mapping inconsistent fields

When the fields are not consistent, as shown in Figure 5.17, mapFields requires a mapFieldsDict dictionary in the system directory of the target case. The following rules apply
to the mapping:
• the field data is mapped from source to target wherever possible, i.e. in our example
all the field data within the target geometry is mapped from the source, except those
in the shaded region which remain unaltered;
• the patch field data is left unaltered unless specified otherwise in the mapFieldsDict
dictionary.
The mapFieldsDict dictionary contain two lists that specify mapping of patch data. The
first list is patchMap that specifies mapping of data between pairs of source and target
patches that are geometrically coincident, as shown in Figure 5.17. The list contains
each pair of names of source and target patch. The second list is cuttingPatches that
contains names of target patches whose values are to be mapped from the source internal
field through which the target patch cuts. In the situation where the target patch only
cuts through part of the source internal field, e.g. bottom left target patch in our example,
those values within the internal field are mapped and those outside remain unchanged.
An example mapFieldsDict dictionary is shown below:
17
18
19
20
21
22
23

patchMap

( lid movingWall );

cuttingPatches

( fixedWalls );

// ************************************************************************* //

mapFields

5.6.3

Mapping parallel cases

If either or both of the source and target cases are decomposed for running in parallel,
additional options must be supplied when executing mapFields:
-parallelSource if the source case is decomposed for parallel running;
-parallelTarget if the target case is decomposed for parallel running.

Open∇FOAM-1.6

U-157

5.6 Mapping fields between different geometries

Coincident patches:
can be mapped using patchMap
Internal target patches:
can be mapped using cuttingPatches
Source field geometry
Target field geometry
Figure 5.17: Mapping inconsistent fields

Open∇FOAM-1.6

U-158

Open∇FOAM-1.6

Mesh generation and conversion

Chapter 6
Post-processing
This chapter describes options for post-processing with OpenFOAM. OpenFOAM is supplied with a post-processing utility paraFoam that uses ParaView, an open source visualisation application described in section 6.1.
Other methods of post-processing using third party products are offered, including
EnSight, Fieldview and the post-processing supplied with Fluent.

6.1

paraFoam

The main post-processing tool provided with OpenFOAM is the a reader module to run
with ParaView, an open-source, visualization application. The module is compiled into
2 libraries, PV3FoamReader and vtkPV3Foam using version 3.6.1 of ParaView supplied
with the OpenFOAM release (PVFoamReader and vtkFoam in ParaView version 2.x). It
is recommended that this version of ParaView is used, although it is possible that the
latest binary release of the software will run adequately. Further details about ParaView
can be found at http://www.paraview.org and further documentation is available at
http://www.kitware.com/products/paraviewguide.html.
ParaView uses the Visualisation Toolkit (VTK) as its data processing and rendering
engine and can therefore read any data in VTK format. OpenFOAM includes the foamToVTK utility to convert data from its native format to VTK format, which means that
any VTK-based graphics tools can be used to post-process OpenFOAM cases. This provides an alternative means for using ParaView with OpenFOAM. For users who wish
to experiment with advanced, parallel visualisation, there is also the free VisIt software,
available at http://www.llnl.gov/visit.
In summary, we recommend the reader module for ParaView as the primary postprocessing tool for OpenFOAM. Alternatively OpenFOAM data can be converted into
VTK format to be read by ParaView or any other VTK -based graphics tools.

6.1.1

Overview of paraFoam

paraFoam is strictly a script that launches ParaView using the reader module supplied
with OpenFOAM. It is executed like any of the OpenFOAM utilities either by the single
command from within the case directory or with the -case option with the case path as
an argument, e.g.:
paraFoam -case
ParaView is launched and opens the window shown in Figure 6.1. The case is controlled
from the left panel, which contains the following:

U-160

Post-processing

Figure 6.1: The paraFoam window
Pipeline Browser lists the modules opened in ParaView, where the selected modules are
highlighted in blue and the graphics for the given module can be enabled/disabled
by clicking the eye button alongside;
Properties panel contains the input selections for the case, such as times, regions and
fields;
Display panel controls the visual representation of the selected module, e.g. colours;
Information panel gives case statistics such as mesh geometry and size.
ParaView operates a tree-based structure in which data can be filtered from the toplevel case module to create sets of sub-modules. For example, a contour plot of, say,
pressure could be a sub-module of the case module which contains all the pressure data.
The strength of ParaView is that the user can create a number of sub-modules and display
whichever ones they feel to create the desired image or animation. For example, they
may add some solid geometry, mesh and velocity vectors, to a contour plot of pressure,
switching any of the items on and off as necessary.
The general operation of the system is based on the user making a selection and then
clicking the green Apply button in the Properties panel. The additional buttons are: the
Reset

U-161

6.1 paraFoam

The user can select internalMesh
region and/or individual patches

The user can select the fields
read into the case module

Figure 6.2: The Properties panel for the case module
in the current reader module, data in all time directories are loaded into ParaView (in
the reader module for ParaView 2.x, a set of check boxes controlled the time that were
displayed). In the current reader module, the buttons in the Current Time Controls
and VCR Controls toolbars select the time data to be displayed, as shown is section 6.1.4.
As with any operation in paraFoam, the user must click Apply after making any changes
to any selections. The Apply button is highlighted in green to alert the user if changes have
been made but not accepted. This method of operation has the advantage of allowing the
user to make a number of selections before accepting them, which is particularly useful
in large cases where data processing is best kept to a minimum.
There are occasions when the case data changes on file and ParaView needs to load the
changes, e.g. when field data is written into new time directories. To load the changes,
the user should check the Update GUI button at the top of the Properties panel and then
apply the changes.

6.1.3

The Display panel

The Display panel contains the settings for visualising the data for a given case module.
The following points are particularly important:
• the data range may not be automatically updated to the max/min limits of a field,
so the user should take care to select Rescale to Data Range at appropriate intervals,
in particular after loading the initial case module;
• clicking the Edit Color Map button, brings up a window in which there are two
panels:
Open∇FOAM-1.6

U-162

Post-processing

View case data

Colour geometry/entity by. . .
Set colour map range/appearance

Outline, surface, wireframe or points
Data interpolation method

Change image opacity
e.g. to make transluscent

Geometry manipulation tools

Figure 6.3: The Display panel
1. The Color Scale panel in which the colours within the scale can be chosen. The
standard blue to red colour scale for CFD can be selected by clicking Choose
Preset and selecting Blue to Red Rainbox HSV.
2. The Color Legend panel has a toggle switch for a colour bar legend and contains
settings for the layout of the legend, e.g. font.
• the underlying mesh can be represented by selecting Wireframe in the Representation menu of the Style panel;
• the geometry, e.g. a mesh (if Wireframe is selected), can be visualised as a single
colour by selecting Solid Color from the Color By menu and specifying the colour
in the Set Solid Color window;
Open∇FOAM-1.6

U-163

6.1 paraFoam

• the image can be made translucent by editing the value in the Opacity text box (1
= solid, 0 = invisible) in the Style panel.

6.1.4

The button toolbars

ParaView duplicates functionality from pull-down menus at the top of the main window
and the major panels, within the toolbars below the main pull-down menus. The displayed
toolbars can be selected from Toolbars in the main View menu. The default layout with
all toolbars is shown in Figure 6.4 with each toolbar labelled. The function of many of
the buttons is clear from their icon and, with tooltips enabled in the Help menu, the user
is given a concise description of the function of any button.
Main controls

Undo/Redo Controls
Selection Controls
VCR Controls

Current Time Controls

Common Filters
Camera Controls
Active Variable Controls | Representation
Centre Axes Controls

Figure 6.4: Toolbars in ParaView

6.1.5

Manipulating the view

This section describes operations for setting and manipulating the view of objects in
paraFoam.
6.1.5.1

View settings

The View Settings are selected from the Edit menu, which opens a Render View Options
window with a table of 3 items: General, Lights and Annotation. The General panel includes
the following items which are often worth setting at startup:
• the background colour, where white is often a preferred choice for printed material;
• Use parallel projection which is the usual choice for CFD, especially for 2D cases;
The Lights panel contains detailed lighting controls within the Light Kit panel. A
separate Headlight panel controls the direct lighting of the image. Checking the Headlight
button with white light colour of strength 1 seems to help produce images with strong
bright colours, e.g. with an isosurface.
The Annotation panel includes options for including annotations in the image. The
Orientation Axes feature controls an axes icon in the image window, e.g. to set the colour
of the axes labels x, y and z.
6.1.5.2

General settings

The general Settings are selected from the Edit menu, which opens a general Options
window with General and Render View menu items.
The General panel controls some default behaviour of ParaView. In particular, there
is an Auto Accept button that enables ParaView to accept changes automatically without
Open∇FOAM-1.6

U-164

Post-processing

clicking the green Apply button in the Properties window. For larger cases, this option is
generally not recommended: the user does not generally want the image to be re-rendered
between each of a number of changes he/she selects, but be able to apply a number of
changes to be re-rendered in their entirety once.
The Render View panel contains 3 sub-items: General, Camera and Server. The General
panel includes the level of detail (LOD) which controls the rendering of the image while it
is being manipulated, e.g. translated, resized, rotated; lowering the levels set by the sliders,
allows cases with large numbers of cells to be re-rendered quickly during manipulation.
The Camera panel includes control settings for 3D and 2D movements. This presents
the user with a map of rotation, translate and zoom controls using the mouse in combination with Shift- and Control-keys. The map can be edited to suit by the user.

6.1.6

Contour plots

A contour plot is created by selecting Contour from the Filter menu at the top menu
bar. The filter acts on a given module so that, if the module is the 3D case module itself,
the contours will be a set of 2D surfaces that represent a constant value, i.e. isosurfaces.
The Properties panel for contours contains an Isosurfaces list that the user can edit, most
conveniently by the New Range window. The chosen scalar field is selected from a pull
down menu.
6.1.6.1

Introducing a cutting plane

Very often a user will wish to create a contour plot across a plane rather than producing
isosurfaces. To do so, the user must first use the Slice filter to create the cutting plane,
on which the contours can be plotted. The Slice filter allows the user to specify a cutting
Plane, Box or Sphere in the Slice Type menu by a center and normal/radius respectively.
The user can manipulate the cutting plane like any other using the mouse.
The user can then run the Contour filter on the cut plane to generate contour lines.

6.1.7

Vector plots

Vector plots are created using the Glyph filter. The filter reads the field selected in
Vectors and offers a range of Glyph Types for which the Arrow provides a clear vector
plot images. Each glyph has a selection of graphical controls in a panel which the user
can manipulate to best effect.
The remainder of the Properties panel contains mainly the Scale Mode menu for the
glyphs. The most common options are Scale Mode are: Vector, where the glyph length
is proportional to the vector magnitude; and, Off where each glyph is the same length.
The Set Scale Factor parameter controls the base length of the glyphs.
6.1.7.1

Plotting at cell centres

Vectors are by default plotted on cell vertices but, very often, we wish to plot data at cell
centres. This is done by first applying the Cell Centers filter to the case module, and
then applying the Glyph filter to the resulting cell centre data.

6.1.8

Streamlines

Streamlines are created by first creating tracer lines using the Stream Tracer filter. The
tracer Seed panel specifies a distribution of tracer points over a Line Source or Point
Open∇FOAM-1.6

6.1 paraFoam

U-165

Cloud. The user can view the tracer source, e.g. the line, but it is displayed in white, so
they may need to change the background colour in order to see it.
The distance the tracer travels and the length of steps the tracer takes are specified in
the text boxes in the main Stream Tracer panel. The process of achieving desired tracer
lines is largely one of trial and error in which the tracer lines obviously appear smoother
as the step length is reduced but with the penalty of a longer calculation time.
Once the tracer lines have been created, the Tubes filter can be applied to the Tracer
module to produce high quality images. The tubes follow each tracer line and are not
strictly cylindrical but have a fixed number of sides and given radius. When the number
of sides is set above, say, 10, the tubes do however appear cylindrical, but again this adds
a computational cost.

6.1.9

Image output

The simplest way to output an image to file from ParaView is to select Save Screenshot
from the File menu. On selection, a window appears in which the user can select the
resolution for the image to save. There is a button that, when clicked, locks the aspect
ratio, so if the user changes the resolution in one direction, the resolution is adjusted in
the other direction automatically. After selecting the pixel resolution, the image can be
saved. To achieve high quality output, the user might try setting the pixel resolution to
1000 or more in the x-direction so that when the image is scaled to a typical size of a
figure in an A4 or US letter document, perhaps in a PDF document, the resolution is
sharp.

6.1.10

Animation output

To create an animation, the user should first select Save Animation from the File menu.
A dialogue window appears in which the user can specify a number of things including
the image resolution. The user should specify the resolution as required. The other
noteworthy setting is number of frames per timestep. While this would intuitively be
set to 1, it can be set to a larger number in order to introduce more frames into the
animation artificially. This technique can be particularly useful to produce a slower
animation because some movie players have limited speed control, particularly over mpeg
movies.
On clicking the Save Animation button, another window appears in which the user specifies a file name root and file format for a set of images. On clicking OK, the set of files will
be saved according to the naming convention “ .”,
e.g. the third image of a series with the file root “animation”, saved in jpg format would
be named “animation 0002.jpg” ( starts at 0000).
Once the set of images are saved the user can convert them into a movie using their
software of choice. The convert utility in the ImageMagick package can do this from the
command line, e.g. by
convert animation*jpg movie.mpg
When creating an mpg movie it can be worth increasing the default quality setting, e.g.
with -quality 90%, to reduce the graininess that can occur with the default setting.
Open∇FOAM-1.6

U-166

6.2

Post-processing

Post-processing with Fluent

It is possible to use Fluent as a post-processor for the cases run in OpenFOAM. Two converters are supplied for the purpose: foamMeshToFluent which converts the OpenFOAM
mesh into Fluent format and writes it out as a .msh file; and, foamDataToFluent converts the OpenFOAM results data into a .dat file readable by Fluent. foamMeshToFluent
is executed in the usual manner. The resulting mesh is written out in a fluentInterface
subdirectory of the case directory, i.e./fluentInterface/.msh
foamDataToFluent converts the OpenFOAM data results into the Fluent format. The
conversion is controlled by two files. First, the controlDict dictionary specifies startTime,
giving the set of results to be converted. If you want to convert the latest result,
startFrom can be set to latestTime. The second file which specifies the translation
is the foamDataToFluentDict dictionary, located in the constant directory. An example
foamDataToFluentDict dictionary is given below:
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33

/*--------------------------------*- C++ -*----------------------------------*\
| =========
|
|
| \\
/ F ield
| OpenFOAM: The Open Source CFD Toolbox
|
| \\
/
O peration
| Version: 1.6
|
|
\\ /
A nd
| Web:
www.OpenFOAM.org
|
|
\\/
M anipulation |
|
\*---------------------------------------------------------------------------*/
FoamFile
{
version
2.0;
format
ascii;
class
dictionary;
location
"system";
object
foamDataToFluentDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
p

epsilon

gamma

150;

// ************************************************************************* //

The dictionary contains entries of the form

The is a label used by the Fluent post-processor that only recognises a fixed set of fields. The basic set of numbers are quoted in
Table 6.1. The dictionary must contain all the entries the user requires to post-process,
e.g. in our example we have entries for pressure p and velocity U. The list of default entries
described in Table 6.1. The user can run foamDataToFluent like any utility.
To view the results using Fluent, go to the fluentInterface subdirectory of the case
directory and start a 3 dimensional version of Fluent with
fluent 3d
The mesh and data files can be loaded in and the results visualised. The mesh is read
by selecting Read Case from the File menu. Support items should be selected to read
Open∇FOAM-1.6

U-167

6.3 Post-processing with Fieldview

Fluent name
PRESSURE
MOMENTUM
TEMPERATURE
ENTHALPY
TKE
TED
SPECIES
G
XF RF DATA VOF
TOTAL PRESSURE
TOTAL TEMPERATURE

Unit number Common OpenFOAM name
1
p
2
U
3
T
4
h
5
k
6
epsilon
7
—
8
—
150
gamma
192
—
193
—

Table 6.1: Fluent unit numbers for post-processing.

certain data types, e.g. to read turbulence data for k and epsilon, the user would select
k-epsilon from the Define->Models->Viscous menu. The data can then be read by
selecting Read Data from the File menu.
A note of caution: users MUST NOT try to use an original Fluent mesh file that has
been converted to OpenFOAM format in conjunction with the OpenFOAM solution that
has been converted to Fluent format since the alignment of zone numbering cannot be
guaranteed.

6.3

Post-processing with Fieldview

OpenFOAM offers the capability for post-processing OpenFOAM cases with Fieldview.
The method involves running a post-processing utility foamToFieldview to convert case
data from OpenFOAM to Fieldview.uns file format. For a given case, foamToFieldview is
executed like any normal application. foamToFieldview creates a directory named Fieldview
in the case directory, deleting any existing Fieldview directory in the process. By default
the converter reads the data in all time directories and writes into a set of files of the
form nn.uns, where nn is an incremental counter starting from 1 for the first time
directory, 2 for the second and so on. The user may specify the conversion of a single time
directory with the option -time , where is a time in general, scientific
or fixed format.
Fieldview provides certain functions that require information about boundary conditions, e.g. drawing streamlines that uses information about wall boundaries. The converter tries, wherever possible, to include this information in the converted files by default.
The user can disable the inclusion of this information by using the -noWall option in the
execution command.
The data files for Fieldview have the .uns extension as mentioned already. If the original
OpenFOAM case includes a dot ‘.’, Fieldview may have problems interpreting a set of data
files as a single case with multiple time steps.

6.4

Post-processing with EnSight

OpenFOAM offers the capability for post-processing OpenFOAM cases with EnSight,
with a choice of 2 options:
Open∇FOAM-1.6

U-168

Post-processing

• converting the OpenFOAM data to EnSight format with the foamToEnsight utility;
• reading the OpenFOAM data directly into EnSight using the ensight74FoamExec
module.

6.4.1

Converting data to EnSight format

The foamToEnsight utility converts data from OpenFOAM to EnSight file format. For a
given case, foamToEnsight is executed like any normal application. foamToEnsight creates
a directory named Ensight in the case directory, deleting any existing Ensight directory in
the process. The converter reads the data in all time directories and writes into a case
file and a set of data files. The case file is named EnSight Case and contains details of
the data file names. Each data file has a name of the form EnSight nn.ext, where nn is an
incremental counter starting from 1 for the first time directory, 2 for the second and so
on and ext is a file extension of the name of the field that the data refers to, as described
in the case file, e.g.T for temperature, mesh for the mesh. Once converted, the data can
be read into EnSight by the normal means:
1. from the EnSight GUI, the user should select Data (Reader) from the File menu;

2. 311426(g)-318.2(t)-0.147034(.147034(h)-0.310405(e300324(3901157(m)-317.765(t)-0.147034(h)-0.3

U-169

6.5 Sampling data

Environment variable
$CEI HOME
$CEI ARCH

$ENSIGHT7 READER
$ENSIGHT7 INPUT

Description and options
Path where EnSight is installed, eg /usr/local/ensight, added
to the system path by default
Machine architecture, from a choice of names corresponding to the machine directory names in
$CEI HOME/ensight74/machines; default settings include
linux 2.4 and sgi 6.5 n32
Path that EnSight searches for the user defined libuserd-foam
reader library, set by default to $FOAM LIBBIN
Set by default to dummy

Table 6.2: Environment variable settings for EnSight.

3. The user should find their case directory from the File Selection window, highlight
one of top 2 entries in the Directories box ending in /. or /.. and click (Set)
Geometry.
4. The path field should now contain an entry for the case. The (Set) Geometry text
box should contain a ‘/’.
5. The user may now click Okay and EnSight will begin reading the data.
6. When the data is read, a new Data Part Loader window will appear, asking which
part(s) are to be read. The user should select Load all.
7. When the mesh is displayed in the EnSight window the user should close the Data
Part Loader window, since some features of EnSight will not work with this window
open.

U-170
34
35
36
37
38
39

Post-processing

surfaces

();

fields

( sigmaxx );

// ************************************************************************* //

Keyword
Options
interpolation- cell
Scheme
cellPoint
cellPointFace
setFormat
raw
gnuplot
xmgr
jplot

Description
Cell-centre value assumed constant over cell
Linear weighted interpolation using cell values
Mixed linear weighted / cell-face interpolation

U-171

6.5 Sampling data

The setFormat entry for line sampling includes a raw data format and formats for
gnuplot, Grace/xmgr and jPlot graph drawing packages. The data are written into a sets
directory within the case directory. The directory is split into a set of time directories and
the data files are contained therein. Each data file is given a name containing the field
name, the sample set name, and an extension relating to the output format, including
.xy for raw data, .agr for Grace/xmgr and .dat for jPlot. The gnuplot format has the data
in raw form with an additional commands file, with .gplt extension, for generating the
graph. Note that any existing sets directory is deleted when sample is run.
The surfaceFormat entry for surface sampling includes a raw data format and formats
for gnuplot, Grace/xmgr and jPlot graph drawing packages. The data are written into a
surfaces directory within the case directory. The directory is split into time directories
and files are written much as with line sampling.
The fields list contains the fields that the user wishes to sample. The sample utility
can parse the following restricted set of functions to enable the user to manipulate vector
and tensor fields, e.g. for U:
U.component(n) writes the nth component of the vector/tensor, n = 0, 1 . . .;
mag(U) writes the magnitude of the vector/tensor.
The sets list contains sub-dictionaries of locations where the data is to be sampled.
The sub-dictionary is named according to the name of the set and contains a set of entries,
also listed in Table 6.4, that describes the locations where the data is to be sampled. For
example, a uniform sampling provides a uniform distribution of nPoints sample locations
along a line specified by a start and end point. All sample sets are also given: a type;
and, means of specifying the length ordinate on a graph by the axis keyword.

Entries
type
axis

•
•
•
•

points

•
•
•
•

nPoints

•
•
•
•
•
•

end

•
•
•
•
•
•

start

Sample locations
Uniformly distributed points on a line
Intersection of specified line and cell faces
Midpoint between line-face intersections
Combination of midPoint and face
Specified points, tracked along a curve
Specified points

axis

Sampling type
uniform
face
midPoint
midPointAndFace
curve
cloud

name

Required entries

•

•
•

Description
Sampling type
Output of sample location

Options
see list above
x
x ordinate
y
y ordinate
z
z ordinate
xyz
xyz coordinates
distance distance from point 0
start
Start point of sample line
e.g.(0.0 0.0 0.0)
end
End point of sample line
e.g.(0.0 2.0 0.0)
nPoints Number of sampling points e.g.200
points
List of sampling points
Table 6.4: Entries within sets sub-dictionaries.
Open∇FOAM-1.6

U-172

Post-processing

Keyword
basePoint
normalVector
interpolate
triangulate

Description
Point on plane
Normal vector to plane
Interpolate data?
Triangulate surface? (optional)

Options
e.g.(0 0 0)
e.g.(1 0 0)
true/false
true/false

Table 6.5: Entries for a plane in surfaces sub-dictionaries.
Keyword
patchName
interpolate
triangulate

Description
Name of patch
Interpolate data?
Triangulate surface? (optional)

Options
e.g.movingWall
true/false
true/false

Table 6.6: Entries for a patch in surfaces sub-dictionaries.

The surfaces list contains sub-dictionaries of locations where the data is to be sampled. The sub-dictionary is named according to the name of the surface and contains
a set of entries beginning with the type: either a plane, defined by point and normal
direction, with additional sub-dictionary entries a specified in Table 6.5; or, a patch, coinciding with an existing boundary patch, with additional sub-dictionary entries a specified
in Table 6.6.

6.6

Monitoring and managing jobs

This section is concerned primarily with successful running of OpenFOAM jobs and extends on the basic execution of solvers described in section 3.3. When a solver is executed,
it reports the status of equation solution to standard output, i.e. the screen, if the level
debug switch is set to 1 or 2 (default) in DebugSwitches in the $WM PROJECT DIR/etc/controlDict file. An example from the beginning of the solution of the cavity tutorial is
shown below where it can be seen that, for each equation that is solved, a report line is
written with the solver name, the variable that is solved, its initial and final residuals and
number of iterations.
Starting time loop
Time = 0.005
Max Courant Number = 0
BICCG: Solving for Ux, Initial residual = 1, Final residual = 2.96338e-06, No Iterations 8
ICCG: Solving for p, Initial residual = 1, Final residual = 4.9336e-07, No Iterations 35
time step continuity errors : sum local = 3.29376e-09, global = -6.41065e-20, cumulative = -6.41065e-20
ICCG: Solving for p, Initial residual = 0.47484, Final residual = 5.41068e-07, No Iterations 34
time step continuity errors : sum local = 6.60947e-09, global = -6.22619e-19, cumulative = -6.86725e-19
ExecutionTime = 0.14 s

Time = 0.01
Max Courant Number = 0.585722
BICCG: Solving for Ux, Initial residual = 0.148584, Final residual = 7.15711e-06, No Iterations 6
BICCG: Solving for Uy, Initial residual = 0.256618, Final residual = 8.94127e-06, No Iterations 6
ICCG: Solving for p, Initial residual = 0.37146, Final residual = 6.67464e-07, No Iterations 33
time step continuity errors : sum local = 6.34431e-09, global = 1.20603e-19, cumulative = -5.66122e-19
ICCG: Solving for p, Initial residual = 0.271556, Final residual = 3.69316e-07, No Iterations 33
time step continuity errors : sum local = 3.96176e-09, global = 6.9814e-20, cumulative = -4.96308e-19
ExecutionTime = 0.16 s

Open∇FOAM-1.6

6.6 Monitoring and managing jobs

U-173

Time = 0.015
Max Courant Number = 0.758267
BICCG: Solving for Ux, Initial residual = 0.0448679, Final residual = 2.42301e-06, No Iterations 6
BICCG: Solving for Uy, Initial residual = 0.0782042, Final residual = 1.47009e-06, No Iterations 7
ICCG: Solving for p, Initial residual = 0.107474, Final residual = 4.8362e-07, No Iterations 32
time step continuity errors : sum local = 3.99028e-09, global = -5.69762e-19, cumulative = -1.06607e-18
ICCG: Solving for p, Initial residual = 0.0806771, Final residual = 9.47171e-07, No Iterations 31
time step continuity errors : sum local = 7.92176e-09, global = 1.07533e-19, cumulative = -9.58537e-19
ExecutionTime = 0.19 s

6.6.1

The foamJob script for running jobs

The user may be happy to monitor the residuals, iterations, Courant number etc. as
report data passes across the screen. Alternatively, the user can redirect the report to a
log file which will improve the speed of the computation. The foamJob script provides
useful options for this purpose with the following executing the specified as a
background process and redirecting the output to a file named log:
foamJob
For further options the user should execute foamJob -h. The user may monitor the log
file whenever they wish, using the UNIXtail command, typically with the -f ‘follow’ option
which appends the new data as the log file grows:
tail -f log

6.6.2

The foamLog script for monitoring jobs

There are limitations to monitoring a job by reading the log file, in particular it is difficult
to extract trends over a long period of time. The foamLog script is therefore provided to
extract data of residuals, iterations, Courant number etc. from a log file and present it in
a set of files that can be plotted graphically. The script is executed by:
foamLog
The files are stored in a subdirectory of the case directory named logs. Each file has
the name where is the name of the variable specified in the log
file and is the iteration number within the time step. Those variables that
are solved for, the initial residual takes the variable name and final residual takes
FinalRes. By default, the files are presented in two-column format of time and the
extracted values.
For example, in the cavity tutorial we may wish to observe the initial residual of the
Ux equation to see whether the solution is converging to a steady-state. In that case, we
would plot the data from the logs/Ux 0 file as shown in Figure 6.5. It can be seen here
that the residual falls monotonically until it reaches the convergence tolerance of 10−5 .
foamLog generates files for everything it feasibly can from the log file. In the cavity
tutorial example, this includes:
• the Courant number, Courant 0;
• Ux equation initial and final residuals, Ux 0 and UxFinalRes 0, and iterations,
UxIters 0 (and equivalent Uy data);
Open∇FOAM-1.6

U-174

Post-processing

1e+00

Ux 0

1e-01
1e-02
1e-03
1e-04
1e-05
0.00

0.02

0.04 0.06

0.08 0.10
Time [s]

0.12 0.14

0.16

0.18

Figure 6.5: Initial residual of Ux in the cavity tutorial
• cumulative, global and local continuity errors after each of the 2 p equations,
contCumulative 0, contGlobal 0, contLocal 0 and contCumulative 1, contGlobal 1,
contLocal 1;
• residuals and iterations from the the 2 p equations p 0, pFinalRes 0, pIters 0 and
p 1, pFinalRes 1, pIters 1;
• and execution time, executionTime.

Open∇FOAM-1.6

Chapter 7
Models and physical properties
OpenFOAM includes a large range of solvers each designed for a specific class of problem.
The equations and algorithms differ from one solver to another so that the selection of
a solver involves the user making some initial choices on the modelling for their particular case. The choice of solver typically involves scanning through their descriptions in
Table 3.5 to find the one suitable for the case. It ultimately determines many of the parameters and physical properties required to define the case but leaves the user with some
modelling options that can be specified at runtime through the entries in dictionary files
in the constant directory of a case. This chapter deals with many of the more common
models and associated properties that may be specified at runtime.

7.1

Thermophysical models

Thermophysical models are concerned with the energy, heat and physical properties.
The thermophysicalProperties dictionary is read by any solver that uses the thermophysical model library. A thermophysical model is constructed in OpenFOAM as a pressuretemperature p − T system from which other properties are computed. There is one compulsory dictionary entry called thermoType which specifies the complete thermophysical
model that is used in the simulation. The thermophysical modelling starts with a layer
that defines the basic equation of state and then adds more layers of modelling that derive properties from the previous layer(s). The naming of the thermoType reflects these
multiple layers of modelling as listed in Table 7.1.
Equation of State — equationOfState
icoPolynomial
Incompressible polynomial equation of state, e.g. for liquids
perfectGas
Perfect gas equation of state
Basic thermophysical properties — thermo
eConstThermo
Constant specific heat cp model with evaluation of internal
energy e and entropy s
hConstThermo
Constant specific heat cp model with evaluation of enthalpy
h and entropy s
hPolynomialThermo
cp evaluated by a function with coefficients from polynomials, from which h, s are evaluated
janafThermo
cp evaluated by a function with coefficients from JANAF
thermodynamic tables, from which h, s are evaluated
Derived thermophysical properties — specieThermo
Continued on next page

U-176

Models and physical properties

Continued from previous page

specieThermo

Thermophysical properties of species, derived from cp , h
and/or s

Transport properties — transport
constTransport
Constant transport properties
polynomialTransport
Polynomial based temperature-dependent transport properties
sutherlandTransport
Sutherland’s formula for temperature-dependent transport
properties
Mixture properties — mixture
pureMixture
General thermophysical model calculation for passive gas
mixtures
homogeneousMixture
Combustion mixture based on normalised fuel mass fraction b
inhomogeneousMixture
Combustion mixture based on b and total fuel mass fraction
ft
veryInhomogeneousMixture Combustion mixture based on b, ft and unburnt fuel mass
fraction fu
dieselMixture
Combustion mixture based on ft and fu
basicMultiComponentBasic mixture based on multiple components
Mixture
multiComponentMixture
Derived mixture based on multiple components
reactingMixture
Combustion mixture using thermodynamics and reaction
schemes
egrMixture
Exhaust gas recirculation mixture
Thermophysical model — thermoModel
hPsiThermo
General thermophysical model calculation based on enthalpy h and compressibility ψ
ePsiThermo
General thermophysical model calculation based on internal energy e and compressibility ψ
hRhoThermo
General thermophysical model calculation based on enthalpy h
hPsiMixtureThermo
Calculates enthalpy for combustion mixture based on ψ
hRhoMixtureThermo
Calculates enthalpy for combustion mixture based on ρ
hhuMixtureThermo
Calculates enthalpy for unburnt gas and combustion mixture
Table 7.1: Layers of thermophysical modelling.

The thermoType entry typically takes the form:
thermoModel>>>>
so that the following is an example entry for thermoType:
hThermo>>>>

Open∇FOAM-1.6

U-177

7.1 Thermophysical models

7.1.1

Thermophysical property data

The basic thermophysical properties are specified for each species from input data. The
data is specified using a compound entry with the following format for a specie accessed
through the keyword mixture:
mixture
The specie coefficients contains the entries listed in Table 7.2 in the
order that they are specified in input.
Description
Entry
String name
e.g.mixture
Number of moles of this specie nmoles
Molecular weight
W (kg/kmol)
Table 7.2: Specie coefficients.
The thermodynamic coefficients are ostensibly concerned with evaluating the specific heat cp from which other properties are derived. The current thermo
models are described as follows:
hConstThermo assumes a constant cp and a heat of fusion Hf which is simply specified
by a two values cp Hf following the .
eConstThermo assumes a constant cv and a heat of fusion Hf which is simply specified
by a two values cv Hf following the .
janafThermo calculates cp as a function of temperature T from a set of coefficients taken
from JANAF tables of thermodynamics. The ordered list of coefficients is given in
Table 7.3. The function is valid between a lower and upper limit in temperature Tl
and Th respectively. Two sets of coefficients are specified, the first set for temperatures above a common temperature Tc (and below Th , the second for temperatures
below Tc (and above Tl ). The function relating cp to temperature is:
cp = R((((a4 T + a3 )T + a2 )T + a1 )T + a0 )

(7.1)

In addition, there are constants of integration, a5 and a6 , both at high and low
temperature, used to evaluating h and s respectively.
hPolynomialThermo calculates Cp as a function of temperature by a polynomial of any order. The following case provides an example of its use: $FOAM TUTORIALS/lagrangian/porousExplicitSourceReactingParcelFoam/filter
The transport coefficients are used to to evaluate dynamic viscosity µ, thermal conductivity κ and laminar thermal conductivity (for enthalpy equation)
α. The current transport models are described as follows:
constTransport assumes a constant µ and Prandtl number P r = cp µ/κ which is simply
specified by a two values µ P r following the .
sutherlandTransport calculates µ as a function of temperature T from a Sutherland coefficient As and Sutherland temperature Ts , specified by values following the ;
µ is calculated according to:
√
As T
(7.2)
µ=
1 + Ts /T
Open∇FOAM-1.6

U-178

Models and physical properties

Description
Lower temperature limit
Upper temperature limit
Common temperature
High temperature coefficients
High temperature enthalpy offset
High temperature entropy offset
Low temperature coefficients
Low temperature enthalpy offset
Low temperature entropy offset

Entry
Tl (K)
Th (K)
Tc (K)
a 0 . . . a4
a5
a6
a 0 . . . a4
a5
a6

Table 7.3: JANAF thermodynamics coefficients.

polynomialTransport calculates µ and κ as a function of temperature T from a polynomial
of any order.
The following is an example entry for a specie named fuel modelled using sutherlandTransport and janafThermo

U-179

7.2 Turbulence models

is selected, the choice of LES modelling is specified in a LESProperties dictionary and the
LES turbulence model is selected by the LESModel entry.
The entries required in the RASProperties are listed in Table 7.4 and those for LESProperties dictionaries are listed in Table 7.5.
RASModel
Name of RAS turbulence model
turbulence
Switch to turn turbulence modelling on/off
Coeffs Optional dictionary of coefficients for the respective RASModel
Table 7.4: Keyword entries in the RASProperties dictionary.

LESmodel
delta
Coeffs
Coeffs

Name of LES model
Name of delta δ model
Dictionary of coefficients for the respective LESmodel
Dictionary of coefficients for each delta model

Table 7.5: Keyword entries in the LESProperties dictionary.
The incompressible and compressible RAS turbulence models, isochoric and anisochoric LES models and delta models are all named and described in Table 3.9. Examples
of their use can be found in the $FOAM TUTORIALS.

7.2.1

Model coefficients

The coefficients for the RAS turbulence models are given default values in their respective
source code. If the user wishes to override these default values, then they can do so by
adding a sub-dictionary entry to the RASproperties file, whose keyword name is that of
the model with Coeffs appended, e.g. kEpsilonCoeffs for the kEpsilon model. If the
printCoeffs switch is on in the RASproperties file, an example of the relevant ...Coeffs
dictionary is printed to standard output when the model is created at the beginning of
a run. The user can simply copy this into the RASproperties file and edit the entries as
required.

7.2.2

Wall functions

From version 1.6 onwards, a range of wall function models is available in OpenFOAM
that are applied as boundary conditions on individual patches. This enables different wall
function models to be applied to different wall regions. The choice of wall function model
is specified through: νt in the 0/nut file for incompressible RAS; µt in the 0/mut file for
compressible RAS; νsgs in the 0/nuSgs file for incompressible LES; µsgs in the 0/muSgs
file for incompressible LES. For example, a 0/nut file:
17
18
19
20
21
22
23
24
25
26
27
28
29

dimensions

[0 2 -1 0 0 0 0];

internalField

uniform 0;

boundaryField
{
movingWall
{
type
value
}
fixedWalls

nutWallFunction;
uniform 0;

Open∇FOAM-1.6

U-180
{

30
31
32
33
34
35
36
37
38
39
40
41

Models and physical properties

}

type
value

}
frontAndBack
{
type
}

nutWallFunction;
uniform 0;
empty;

// ************************************************************************* //

There are a number of wall function models available in the release, e.g. nutWallFunction,
nutRoughWallFunction, nutSpalartAllmarasStandardRoughWallFunction, nutSpalartAllmarasStandardWallFunction and nutSpalartAllmarasWallFunction. The user
can consult the relevant directories for a full list of wall function models:
find $FOAM SRC/turbulenceModels -name wallFunctions
Within each wall function boundary condition the user can over-ride default settings for
E and κ through optional E and kappa keyword entries.
Having selected the particular wall functions on various patches in the nut/mut file,
the user should select epsilonWallFunction on corresponding patches in the epsilon field
and kqRwallFunction on corresponding patches in the turbulent fields k, q and R.

Open∇FOAM-1.6

U-181

Index

Index
Symbols Numbers A B C D E F G H I J K L M N O P Q R S T U V W X Z

Symbols
*
tensor member function, P-25
+
tensor member function, P-25
tensor member function, P-25
/
tensor member function, P-25
/*...*/
C++ syntax, U-78
//
C++ syntax, U-78
OpenFOAM file syntax, U-102
# include
C++ syntax, U-72, U-78
&
tensor member function, P-25
&&
tensor member function, P-25
^
tensor member function, P-25
Coeffs keyword, U-179
Coeffs keyword, U-179
Coeffs keyword, U-179
cellSet utility, U-90
faceSet utility, U-90
pointSet utility, U-90
0.000000e+00 directory, U-102
1-dimensional mesh, U-126
1D mesh, U-126
2-dimensional mesh, U-126
2D mesh, U-126

Numbers
0 directory, U-102

A
access functions, P-23
addLayersControls keyword, U-142
adiabaticFlameT utility, U-93
adjustableRunTime
keyword entry, U-60, U-109

adjustTimeStep keyword, U-60
agglomerator keyword, U-119
algorithms tools, U-94
alphaContactAngle
boundary condition, U-58
analytical solution, P-45
anisotropicFilter model, U-98
Annotation window panel, U-26, U-163
ansysToFoam utility, U-89
APIfunctions model, U-97
applications, U-69
Apply button, U-160, U-164
applyBoundaryLayer utility, U-89
applyWallFunctionBoundaryConditions
utility,
U-89
arbitrarily unstructured, P-31
arc
keyword entry, U-136
arc keyword, U-135
ascii
keyword entry, U-109
attachMesh utility, U-90
Auto Accept button, U-163
autoMesh
library, U-95
autoPatch utility, U-90
autoRefineMesh utility, U-91
axes
right-handed, U-134
right-handed rectangular Cartesian, P-15,
U-20
axi-symmetric cases, U-131, U-139
axi-symmetric mesh, U-126

B
background
process, U-26, U-81
backward
keyword entry, U-116
Backward differencing, P-39
barotropicCompressibilityModels
library, U-97
Open∇FOAM-1.6

U-182
basicMultiComponentMixture model,
U-96,
U-176
basicThermophysicalModels
library, U-96
binary
keyword entry, U-109
BirdCarreau model, U-99
blended differencing, P-38
block
expansion ratio, U-136
block keyword, U-135
blockMesh solver, P-47
blockMesh utility, U-38, U-89, U-132
blockMesh executable
vertex numbering, U-136
blockMeshDict
dictionary, U-20, U-22, U-37, U-49, U-132,
U-140
blocks keyword, U-22, U-32, U-136
boundaries, U-128
boundary, U-128
boundary
dictionary, U-125, U-132
boundary condition
alphaContactAngle, U-58
calculated, U-132
cyclic, U-131
directionMixed, U-132
empty, P-63, P-69, U-20, U-126, U-131
fixedGradient, U-132
fixedValue, U-132
fluxCorrectedVelocity, U-133
inlet, P-69
inletOutlet, U-133
mixed, U-132
movingWallVelocity, U-133
outlet, P-69
outletInlet, U-133
partialSlip, U-133
patch, U-131
pressureDirectedInletVelocity, U-133
pressureInletVelocity, U-133
pressureOutlet, P-63
pressureTransmissive, U-133
processor, U-131
setup, U-22
slip, U-133
supersonicFreeStream, U-133
surfaceNormalFixedValue, U-133
symmetryPlane, P-63, U-131
totalPressure, U-133
turbulentInlet, U-133
wall, U-41
wall, P-63, P-69, U-58, U-131
Open∇FOAM-1.6

Index
wallBuoyantPressure, U-133
wedge, U-126, U-131, U-139
zeroGradient, U-132
boundary conditions, P-43
Dirichlet, P-43
inlet, P-44
Neumann, P-43
no-slip impermeable wall, P-44
outlet, P-44
physical, P-44
symmetry plane, P-44
boundaryField keyword, U-22, U-106
boundaryFoam solver, U-85
bounded
keyword entry, U-114, U-115
boxToCell keyword, U-59
boxTurb utility, U-89
breaking of a dam, U-56
bubbleFoam solver, U-86
buoyantBoussinesqPisoFoam solver, U-87
buoyantBoussinesqSimpleFoam solver, U-87
buoyantPisoFoam solver, U-87
buoyantSimpleFoam solver, U-87
buoyantSimpleRadiationFoam solver, U-87
button
Apply, U-160, U-164
Auto Accept, U-163
Choose Preset, U-162
Delete, U-160
Edit Color Map, U-161
Enable Line Series, U-36
Orientation Axes, U-26, U-163
Rescale to Data Range, U-28
Reset, U-160
Set Solid Color, U-162
Update GUI, U-28, U-161
Use Parallel Projection, U-25
Use parallel projection, U-163

C
C++ syntax
/*...*/, U-78
//, U-78
# include, U-72, U-78
cacheAgglomeration keyword, U-120
calculated
boundary condition, U-132
cAlpha keyword, U-62
cases, U-101
castellatedMesh keyword, U-142
castellatedMeshControls
dictionary, U-143, U-145
castellatedMeshControls keyword, U-142
cavitatingFoam solver, U-86

Index
cavity flow, U-19
CEI ARCH
environment variable, U-169
CEI HOME
environment variable, U-169
cell
expansion ratio, U-136
cell class, P-31
cell
keyword entry, U-170
cellPoint
keyword entry, U-170
cellPointFace
keyword entry, U-170
cells
dictionary, U-132
central differencing, P-38
cfdTools tools, U-95
cfx4ToFoam utility, U-89, U-149
changeDictionary utility, U-89
channelFoam solver, U-85
Chart Options window, U-36
checkMesh utility, U-90, U-151
chemistryModel
library, U-97
chemistryModel model, U-97
chemistrySolver model, U-97
chemkinToFoam utility, U-93
Choose Preset button, U-162
chtMultiRegionFoam solver, U-87
Chung
library, U-97
class
cell, P-31
dimensionSet, P-25, P-32, P-33
face, P-31
finiteVolumeCalculus, P-33
finiteVolumeMethod, P-33
fvMesh, P-31
fvSchemes, P-36
fvc, P-36
fvm, P-36
pointField, P-31
polyBoundaryMesh, P-31
polyMesh, P-31, U-123, U-125
polyPatchList, P-31
polyPatch, P-31
scalarField, P-29
scalar, P-23
slice, P-31
symmTensorField, P-29
symmTensorThirdField, P-29
tensorField, P-29
tensorThirdField, P-29

U-183
tensor, P-23
vectorField, P-29
vector, P-23, U-105
word, P-25, P-31
class keyword, U-103
clockTime
keyword entry, U-109
cloud keyword, U-171
cmptAv
tensor member function, P-25
Co utility, U-91
coalChemistryFoam solver, U-88
coalCombustion
library, U-95
cofactors
tensor member function, P-25
coldEngineFoam solver, U-87
collapseEdges utility, U-91
Color By menu, U-162
Color Legend window, U-30
Color Legend window panel, U-162
Color Scale window panel, U-162
combinePatchFaces utility, U-91
comments, U-78
compressed
keyword entry, U-109
compressibleInterDyMFoam solver, U-86
compressibleInterFoam solver, U-86
compressibleLESModels
library, U-99
compressibleRASModels
library, U-98
constant directory, U-102, U-175
constLaminarFlameSpeed model, U-97
constTransport model, U-97, U-176
containers tools, U-94
continuum
mechanics, P-15
control
of time, U-108
controlDict
dictionary, P-65, U-23, U-32, U-42, U-51,
U-60, U-102, U-155
controlDict file, P-49
convection, see divergence, P-38
convergence, U-40
conversion
library, U-96
convertToMeters keyword, U-134, U-135
coordinate
system, P-15
coordinate system, U-20
corrected
keyword entry, U-114, U-115
Open∇FOAM-1.6

U-184

Index

Courant number, P-42, U-24
cpuTime
keyword entry, U-109
Crank Nicholson
temporal discretisation, P-42
CrankNicholson
keyword entry, U-116
createBaffles utility, U-90
createPatch utility, U-90
createTurbulenceFields utility, U-92
cross product, see tensor, vector cross product
CrossPowerLaw
keyword entry, U-59
CrossPowerLaw model, U-99
cubeRootVolDelta model, U-98
cubicCorrected
keyword entry, U-116
cubicCorrection
keyword entry, U-113
curl, P-37
curl
fvc member function, P-37
Current Time Controls menu, U-28, U-161
curve keyword, U-171
cyclic
boundary condition, U-131
cyclic
keyword entry, U-130
cylinder
flow around a, P-45

D
d2dt2
fvc member function, P-37
fvm member function, P-37
dam
breaking of a, U-56
db tools, U-94
ddt
fvc member function, P-37
fvm member function, P-37
DeardorffDiffStress model, U-99
debug keyword, U-142
decomposePar utility, U-81, U-82, U-93
decomposeParDict
dictionary, U-81
decomposition
of field, U-81
of mesh, U-81
decompositionMethods
library, U-96
decompression of a tank, P-62
defaultFieldValues keyword, U-59
deformedGeom utility, U-90
Open∇FOAM-1.6

Delete button, U-160
delta keyword, U-83, U-179
deltaT keyword, U-108
dependencies, U-72
dependency lists, U-72
det
tensor member function, P-25
determinant, see tensor, determinant
dev
tensor member function, P-25
diag
tensor member function, P-25
diagonal
keyword entry, U-119
DIC
keyword entry, U-119
DICGaussSeidel
keyword entry, U-119
dictionary
LESProperties, U-179
PISO, U-25
blockMeshDict, U-20, U-22, U-37, U-49,
U-132, U-140
boundary, U-125, U-132
castellatedMeshControls, U-143, U-145
cells, U-132
controlDict, P-65, U-23, U-32, U-42, U-51,
U-60, U-102, U-155
decomposeParDict, U-81
faces, U-125, U-132
fvSchemes, U-61, U-102, U-110, U-111
fvSolution, U-102, U-117
mechanicalProperties, U-51
neighbour, U-125
owner, U-125
points, U-125, U-132
thermalProperties, U-51
thermophysicalProperties, U-175
transportProperties, U-23, U-39, U-42
turbulenceProperties, U-42, U-60, U-178
dieselEngineFoam solver, U-87
dieselFoam solver, U-87
dieselMixture model, U-96, U-176
dieselSpray
library, U-95
differencing
Backward, P-39
blended, P-38
central, P-38
Euler implicit, P-39
Gamma, P-38
MINMOD, P-38
SUPERBEE, P-38
upwind, P-38

U-185

Index
van Leer, P-38
DILU
keyword entry, U-119
dimension
checking in OpenFOAM, P-25, U-105
dimensional units, U-105
dimensioned template class, P-25
dimensionedTypes tools, U-94
dimensions keyword, U-22, U-106
dimensionSet class, P-25, P-32, P-33
dimensionSet tools, U-94
direct numerical simulation, U-61
directionMixed
boundary condition, U-132
directory
0.000000e+00, U-102
0, U-102
Make, U-73
constant, U-102, U-175
fluentInterface, U-166
polyMesh, U-102, U-125
processorN , U-82
run, U-101
system, P-49, U-102
tutorials, P-45, U-19
discretisation
equation, P-33
Display
window
panel,
U-25,
U-28,
U-160, U-161
distance
keyword entry, U-145, U-171
distributed keyword, U-83, U-84
div
fvc member function, P-37
fvm member function, P-37
divergence, P-37, P-39
divSchemes keyword, U-111
dnsFoam solver, U-87
doLayers keyword, U-142
double inner product, see tensor,double inner
product
dsmc
library, U-95
dsmcFieldsCalc utility, U-93
dsmcFoam solver, U-88
dsmcInitialise utility, U-89
dx
keyword entry, U-170
dynamicFvMesh
library, U-95
dynamicMesh
library, U-95
dynMixedSmagorinsky model, U-99
dynOneEqEddy model, U-99

dynSmagorinsky model, U-99

E
eConstThermo model, U-97, U-175
edgeGrading keyword, U-137
edgeMesh
library, U-95
edges keyword, U-135
Edit menu, U-163
Edit Color Map button, U-161
egrMixture model, U-96, U-176
electrostaticFoam solver, U-88
empty
boundary condition, P-63, P-69, U-20,
U-126, U-131
empty
keyword entry, U-130
Enable Line Series button, U-36
endTime keyword, U-24, U-108
engine
library, U-96
engineCompRatio utility, U-93
engineFoam solver, U-87
engineSwirl utility, U-89
ensight74FoamExec utility, U-168
ENSIGHT7 INPUT
environment variable, U-169
ENSIGHT7 READER
environment variable, U-169
ensightFoamReader utility, U-91
enstrophy utility, U-91
environment variable
CEI ARCH, U-169
CEI HOME, U-169
ENSIGHT7 INPUT, U-169
ENSIGHT7 READER, U-169
FOAM RUN, U-101
WM ARCH, U-76
WM COMPILER BIN, U-76
WM COMPILER DIR, U-76
WM COMPILER LIB, U-76
WM COMPILER, U-76
WM COMPILE OPTION, U-76
WM DIR, U-76
WM JAVAC OPTION, U-76
WM LINK LANGUAGE, U-76
WM MPLIB, U-76
WM OPTIONS, U-76
WM PROJECT DIR, U-76
WM PROJECT INST DIR, U-76
WM PROJECT LANGUAGE, U-76
WM PROJECT USER DIR, U-76
WM PROJECT VERSION, U-76
WM PROJECT, U-76
Open∇FOAM-1.6

U-186

Index

WM SHELL, U-76
wmake, U-75
ePsiThermo model, U-96, U-176
equilibriumCO utility, U-93
equilibriumFlameT utility, U-93
errorEstimation
library, U-95
errorReduction keyword, U-149
estimateScalarError utility, U-93
Euler
keyword entry, U-116
Euler implicit
differencing, P-39
temporal discretisation, P-42
examples
decompression of a tank, P-62
flow around a cylinder, P-45
flow over backward step, P-53
Hartmann problem, P-67
supersonic flow over forward step, P-58
execFlowFunctionObjects utility, U-93
expandDictionary utility, U-94
expansionRatio keyword, U-148
explicit
temporal discretisation, P-42
exponential model, U-97
extrude2DMesh utility, U-89
extrudeMesh utility, U-89

F
face class, P-31
face keyword, U-171
faceAreaPair
keyword entry, U-119
faces
dictionary, U-125, U-132
FDIC
keyword entry, U-119
featureAngle keyword, U-148
features keyword, U-143
field
U, U-24
p, U-24
decomposition, U-81
FieldField template class, P-32
fieldFunctionObjects
library, U-95
fields, P-29
mapping, U-155
fields tools, U-94, U-95
fields keyword, U-170
Field template class, P-29
fieldValues keyword, U-59
fieldview9Reader utility, U-91
Open∇FOAM-1.6

file
Make/files, U-74
controlDict, P-49
files, U-73
g, U-59
options, U-73
snappyHexMeshDict, U-141
transportProperties, U-59
file format, U-102
files file, U-73
finalLayerRatio keyword, U-148
financialFoam solver, U-88
finite volume
discretisation, P-27
mesh, P-31
finiteVolume
library, U-95
finiteVolume tools, U-95
finiteVolumeCalculus class, P-33
finiteVolumeMethod class, P-33
firstTime keyword, U-108
fixed
keyword entry, U-109
fixedGradient
boundary condition, U-132
fixedValue
boundary condition, U-132
flattenMesh utility, U-90
flow
free surface, U-56
laminar, U-19
steady, turbulent, P-53
supersonic, P-58
turbulent, U-19
flow around a cylinder, P-45
flow over backward step, P-53
flowType utility, U-91
fluent3DMeshToFoam utility, U-89
fluentInterface directory, U-166
fluentMeshToFoam utility, U-89, U-149
fluxCorrectedVelocity
boundary condition, U-133
fluxRequired keyword, U-111
OpenFOAM
cases, U-101
FOAM RUN
environment variable, U-101
foamCalc utility, U-34
foamCalcFunctions
library, U-95
foamCorrectVrt script/alias, U-154
foamDataToFluent utility, U-91, U-166
foamDebugSwitches utility, U-94
FoamFile keyword, U-103

U-187

Index
foamFile
keyword entry, U-170
foamFormatConvert utility, U-94
foamInfoExec utility, U-94
foamJob script/alias, U-173
foamLog script/alias, U-173
foamMeshToFluent utility, U-89, U-166
foamToEnsight utility, U-91
foamToEnsightParts utility, U-91
foamToFieldview9 utility, U-91
foamToGMV utility, U-91
foamToStarMesh utility, U-89
foamToVTK utility, U-91
foamUpgradeFvSolution utility, U-89
forces
library, U-95
foreground
process, U-26
format keyword, U-103
fourth
keyword entry, U-114, U-115
functions keyword, U-110
fvc class, P-36
fvc member function
curl, P-37
d2dt2, P-37
ddt, P-37
div, P-37
gGrad, P-37
grad, P-37
laplacian, P-37
lsGrad, P-37
snGrad, P-37
snGradCorrection, P-37
sqrGradGrad, P-37
fvDOM
library, U-96
fvm class, P-36
fvm member function
d2dt2, P-37
ddt, P-37
div, P-37
laplacian, P-37
Su, P-37
SuSp, P-37
fvMatrices tools, U-95
fvMatrix template class, P-33
fvMesh class, P-31
fvMesh tools, U-95
fvMotionSolver
library, U-95
fvSchemes
dictionary, U-61, U-102, U-110, U-111
fvSchemes class, P-36

fvSchemes
menu entry, U-52
fvSolution
dictionary, U-102, U-117

G
g file, U-59
gambitToFoam utility, U-89, U-149
GAMG
keyword entry, U-53, U-118, U-119
Gamma
keyword entry, U-113
Gamma differencing, P-38
Gauss
keyword entry, U-114
Gauss’s theorem, P-36
GaussSeidel
keyword entry, U-119
General window panel, U-163
general model, U-97
general
keyword entry, U-109
geometric-algebraic multi-grid, U-119
GeometricBoundaryField template class, P-32
geometricField template class, P-32
geometry keyword, U-142
gGrad
fvc member function, P-37
global tools, U-94
gmshToFoam utility, U-89
gnuplot
keyword entry, U-109, U-170
grad
fvc member function, P-37
(Grad Grad) squared, P-37
gradient, P-37, P-40
Gauss scheme, P-40
Gauss’s theorem, U-52
least square fit, U-52
least squares method, P-40, U-52
surface normal, P-40
gradSchemes keyword, U-111
graph tools, U-94
graphFormat keyword, U-109
GuldersEGRLaminarFlameSpeed model, U-97
GuldersLaminarFlameSpeed model, U-97

hConstThermo model, U-97, U-175
Help menu, U-163
HerschelBulkley model, U-99
hhuMixtu6(e)-0.2349880 0 cm BT /R276 10.9091 Tf 1 0 0 1 299.907 107

U-188

Index

homogeneousMixture model, U-96, U-176
hPolynomialThermo model, U-97, U-175
hPsiMixtureThermo model, U-96, U-176
hPsiThermo model, U-96, U-176
hRhoMixtureThermo model, U-96, U-176
hRhoThermo model, U-96, U-176

I
I
tensor member function, P-25
icoErrorEstimate utility, U-93
icoFoam solver, U-19, U-23, U-24, U-26, U-85
icoMomentError utility, U-94
icoPolynomial model, U-97, U-175
ideasToFoam utility, U-149
ideasUnvToFoam utility, U-89
identities, see tensor, identities
identity, see tensor, identity
incompressibleLESModels
library, U-99
incompressibleRASModels
library, U-98
incompressibleTransportModels
library, P-55, U-99
incompressibleTurbulenceModels
library, P-55
index
notation, P-16, P-17
Information window panel, U-160
inhomogeneousMixture model, U-96, U-176
inlet
boundary condition, P-69
inletOutlet
boundary condition, U-133
inner product, see tensor, inner product
inside
keyword entry, U-145
insideCells utility, U-90
interDyMFoam solver, U-86
interfaceProperties model, U-99
interFoam solver, U-87
internalField keyword, U-22, U-106
interPhaseChangeFoam solver, U-87
interpolation tools, U-95
interpolationScheme keyword, U-170
interpolations tools, U-94
interpolationSchemes keyword, U-111
inv
tensor member function, P-25

J
janafThermo model, U-97, U-175
jplot
keyword entry, U-109, U-170
Open∇FOAM-1.6

K
kEpsilon model, U-98
keyword
FoamFile, U-103
LESmodel, U-179
RASModel, U-179
addLayersControls, U-142
adjustTimeStep, U-60
agglomerator, U-119
arc, U-135
blocks, U-22, U-32, U-136
block, U-135
boundaryField, U-22, U-106
boxToCell, U-59
cAlpha, U-62
cacheAgglomeration, U-120
castellatedMeshControls, U-142
castellatedMesh, U-142
class, U-103
cloud, U-171
convertToMeters, U-134, U-135
curve, U-171
debug, U-142
defaultFieldValues, U-59
deltaT, U-108
delta, U-83, U-179
dimensions, U-22, U-106
distributed, U-83, U-84
divSchemes, U-111
doLayers, U-142
edgeGrading, U-137
edges, U-135
endTime, U-24, U-108
errorReduction, U-149
expansionRatio, U-148
face, U-171
featureAngle, U-148
features, U-143
fieldValues, U-59
fields, U-170
finalLayerRatio, U-148
firstTime, U-108
fluxRequired, U-111
format, U-103
functions, U-110
geometry, U-142
gradSchemes, U-111
graphFormat, U-109
internalField, U-22, U-106
interpolationSchemes, U-111
interpolationScheme, U-170
laplacianSchemes, U-111
latestTime, U-39
layers, U-148

Index
leastSquares, U-52
levels, U-146
libs, U-80, U-110
locationInMesh, U-143, U-145
location, U-103
manualCoeffs, U-83
maxBoundarySkewness, U-149
maxConcave, U-149
maxCo, U-60
maxDeltaT, U-60
maxFaceThicknessRatio, U-148
maxGlobalCells, U-143
maxInternalSkewness, U-149
maxLocalCells, U-143
maxNonOrtho, U-149
maxThicknessToMedialRatio, U-148
mergeLevels, U-120
mergePatchPairs, U-135
mergeTolerance, U-142
meshQualityControls, U-142
method, U-83
metisCoeffs, U-83
midPointAndFace, U-171
midPoint, U-171
minArea, U-149
minDeterminant, U-149
minFaceWeight, U-149
minFlatness, U-149
minMedianAxisAngle, U-148
minRefinementCells, U-143
minThickness, U-148
minTriangleTwist, U-149
minTwist, U-149
minVolRatio,

U-189

U-190
uniform, U-171
valueFraction, U-132
value, U-23, U-132
version, U-103
vertices, U-22, U-135
writeCompression, U-109
writeControl, U-24, U-60, U-108
writeFormat, U-55, U-109
writeInterval, U-24, U-33, U-109
writePrecision, U-109
Coeffs, U-179
Coeffs, U-179
Coeffs, U-179
keyword entry
CrankNicholson, U-116
CrossPowerLaw, U-59
DICGaussSeidel, U-119
DIC, U-119
DILU, U-119
Euler, U-116
FDIC, U-119
GAMG, U-53, U-118, U-119
Gamma, U-113
GaussSeidel, U-119
Gauss, U-114
LESmodel, U-42, U-178
MGridGen, U-119
MUSCL, U-113
Newtonian, U-59
PBiCG, U-118
PCG, U-118
QUICK, U-113, U-116
RASmodel, U-42, U-178
SFCD, U-113, U-116
UMIST, U-112
adjustableRunTime, U-60, U-109
arc, U-136
ascii, U-109
backward, U-116
binary, U-109
bounded, U-114, U-115
cellPointFace, U-170
cellPoint, U-170
cell, U-170
clockTime, U-109
compressed, U-109
corrected, U-114, U-115
cpuTime, U-109
cubicCorrected, U-116
cubicCorrection, U-113
cyclic, U-130
diagonal, U-119
distance, U-145, U-171
dx, U-170
Open∇FOAM-1.6

Index
empty, U-130
faceAreaPair, U-119
fixed, U-109
foamFile, U-170
fourth, U-114, U-115
general, U-109
gnuplot, U-109, U-170
hierarchical, U-82, U-83
inside, U-145
jplot, U-109, U-170
laminar, U-42, U-178
latestTime, U-108
leastSquares, U-114
limitedCubic, U-113
limitedLinear, U-113
limited, U-114, U-115
linearUpwind, U-113, U-116
linear, U-113, U-116
line, U-136
manual, U-82, U-83
metis, U-82, U-83
midPoint, U-113
nextWrite, U-108
noWriteNow, U-108
none, U-112, U-119
null, U-170
outside, U-145
patch, U-130, U-172
polyLine, U-136
polySpline, U-136
processor, U-130
raw, U-109, U-170
runTime, U-33, U-108
scientific, U-109
scotch, U-82, U-83
simpleSpline, U-136
simple, U-82, U-83
skewLinear, U-113, U-116
smoothSolver, U-118
startTime, U-23, U-108
steadyState, U-116
stl, U-170
symmetryPlane, U-130
timeStep, U-24, U-33, U-108
uncompressed, U-109
uncorrected, U-114, U-115
upwind, U-113, U-116
vanLeer, U-113
vtk, U-170
wall, U-130
wedge, U-130
writeControl, U-108
writeNow, U-108
xmgr, U-109, U-170

U-191

Index
xyz, U-171
x, U-171
y, U-171
z, U-171
kivaToFoam utility, U-89
kOmega model, U-98
kOmegaSST model, U-98, U-99
Kronecker delta, P-20

L
lagrangian
library, U-95
lagrangianIntermediate
library, U-95
Lambda2 utility, U-91
LamBremhorstKE model, U-98
laminar model, U-98
laminar
keyword entry, U-42, U-178
laminarFlameSpeedModels
library, U-97
laplaceFilter model, U-98
Laplacian, P-38
laplacian, P-37
laplacian
fvc member function, P-37
fvm member function, P-37
laplacianFoam solver, U-85
laplacianSchemes keyword, U-111
latestTime
keyword entry, U-108
latestTime keyword, U-39
LaunderGibsonRSTM model, U-98
LaunderSharmaKE model, U-98
layers keyword, U-148
leastSquares
keyword entry, U-114
leastSquares keyword, U-52
LESdeltas
library, U-98
LESfilters
library, U-98
LESmodel
keyword entry, U-42, U-178
LESmodel keyword, U-179
LESProperties
dictionary, U-179
levels keyword, U-146
libraries, U-69
library
Chung, U-97
LESdeltas, U-98
LESfilters, U-98
MGridGenGAMGAgglomeration, U-96

ODE, U-95
OSspecific, U-96
OpenFOAM, U-94
P1, U-96
PV3FoamReader, U-159
PVFoamReader, U-159
Wallis, U-97
autoMesh, U-95
barotropicCompressibilityModels, U-97
basicThermophysicalModels, U-96
chemistryModel, U-97
coalCombustion, U-95
compressibleLESModels, U-99
compressibleRASModels, U-98
conversion, U-96
decompositionMethods, U-96
dieselSpray, U-95
dsmc, U-95
dynamicFvMesh, U-95
dynamicMesh, U-95
edgeMesh, U-95
engine, U-96
errorEstimation, U-95
fieldFunctionObjects, U-95
finiteVolume, U-95
foamCalcFunctions, U-95
forces, U-95
fvDOM, U-96
fvMotionSolver, U-95
incompressibleLESModels, U-99
incompressibleRASModels, U-98
incompressibleTransportModels, P-55, U-99
incompressibleTurbulenceModels, P-55
lagrangianIntermediate, U-95
lagrangian, U-95
laminarFlameSpeedModels, U-97
linear, U-97
liquidMixture, U-98
liquids, U-98
meshTools, U-95
molecularMeasurements, U-95
molecule, U-95
pdf, U-97
postCalc, U-95
potential, U-95
primitive, P-23
radiation, U-96
randomProcesses, U-96
reactionThermophysicalModels, U-96
sampling, U-95
solidMixture, U-98
solidParticle, U-96
solids, U-98
specie, U-97
Open∇FOAM-1.6

U-192

Index

surfMesh, U-95
systemCall, U-95
thermophysicalFunctions, U-97
thermophysical, U-175
topoChangerFvMesh, U-95
triSurface, U-95
utilityFunctionObjects, U-95
vtkFoam, U-159
vtkPV3Foam, U-159
libs keyword, U-80, U-110
lid-driven cavity flow, U-19
LienCubicKE model, U-98
LienCubicKELowRe model, U-98
LienLeschzinerLowRe model, U-98
Lights window panel, U-163
limited
keyword entry, U-114, U-115
limitedCubic
keyword entry, U-113
limitedLinear
keyword entry, U-113
line
keyword entry, U-136
Line Style menu, U-36
linear
library, U-97
linear
keyword entry, U-113, U-116
linearUpwind
keyword entry, U-113, U-116
liquid
electrically-conducting, P-67
liquidMixture
library, U-98
liquids
library, U-98
lists, P-29
List template class, P-29
location keyword, U-103
locationInMesh keyword, U-143, U-145
locDynOneEqEddy model, U-99
lowReOneEqEddy model, U-99
LRDDiffStress model, U-99
LRR model, U-98
lsGrad
fvc member function, P-37

M
Mach utility, U-92
mag
tensor member function, P-25
magnetohydrodynamics, P-67
magSqr
tensor member function, P-25
Open∇FOAM-1.6

Make directory, U-73
make script/alias, U-71
Make/files file, U-74
manual
keyword entry, U-82, U-83
manualCoeffs keyword, U-83
mapFields utility, U-32, U-39, U-43, U-55, U-89,
U-155
mapping
fields, U-155
Marker Style menu, U-36
matrices tools, U-94
max
tensor member function, P-25
maxBoundarySkewness keyword, U-149
maxCo keyword, U-60
maxConcave keyword, U-149
maxDeltaT keyword, U-60
maxFaceThicknessRatio keyword, U-148
maxGlobalCells keyword, U-143
maxInternalSkewness keyword, U-149
maxLocalCells keyword, U-143
maxNonOrtho keyword, U-149
maxThicknessToMedialRatio keyword, U-148
mdEquilibrationFoam solver, U-88
mdFoam solver, U-88
mdInitialise utility, U-89
mechanicalProperties
dictionary, U-51
memory tools, U-94
menu
Color By, U-162
Current Time Controls, U-28, U-161
Edit, U-163
Help, U-163
Line Style, U-36
Marker Style, U-36
Plot Type, U-35
VCR Controls, U-28, U-161
View, U-163
menu entry
Plot Over Line, U-35
Save Animation, U-165
Save Screenshot, U-165
Settings, U-163
Show Color Legend, U-28
Solid Color, U-162
Toolbars, U-163
View Settings..., U-25
View Settings, U-26, U-163
Wireframe, U-162
fvSchemes, U-52
mergeLevels keyword, U-120
mergeMeshes utility, U-90

Index
mergeOrSplitBaffles utility, U-90
mergePatchPairs keyword, U-135
mergeTolerance keyword, U-142
mesh
1-dimensional, U-126
1D, U-126
2-dimensional, U-126
2D, U-126
axi-symmetric, U-126
basic, P-31
block structured, U-132
decomposition, U-81
description, U-123
finite volume, P-31
generation, U-132, U-140
grading, U-132, U-136
grading, example of, P-53
non-orthogonal, P-45
refinement, P-62
resolution, U-30
specification, U-123
split-hex, U-140
Stereolithography (STL), U-140
surface, U-140
validity constraints, U-123
meshes tools, U-94
meshQualityControls keyword, U-142
meshTools
library, U-95
message passing interface
openMPI, U-83
method keyword, U-83
metis
keyword entry, U-82, U-83
metisCoeffs keyword, U-83
MGridGen
keyword entry, U-119
MGridGenGAMGAgglomeration
library, U-96
mhdFoam solver, P-69, U-88
midPoint
keyword entry, U-113
midPoint keyword, U-171
midPointAndFace keyword, U-171
min
tensor member function, P-25
minArea keyword, U-149
minDeterminant keyword, U-149
minFaceWeight keyword, U-149
minFlatness keyword, U-149
minMedianAxisAngle keyword, U-148
MINMOD differencing, P-38
minRefinementCells keyword, U-143
minThickness keyword, U-148

U-193
minTriangleTwist keyword, U-149
minTwist keyword, U-149
minVol keyword, U-149
minVolRatio keyword, U-149
mirrorMesh utility, U-90
mixed
boundary condition, U-132
mixedSmagorinsky model, U-99
mixtureAdiabaticFlameT utility, U-93
mode keyword, U-145
model
APIfunctions, U-97
BirdCarreau, U-99
CrossPowerLaw, U-99
DeardorffDiffStress, U-99
GuldersEGRLaminarFlameSpeed, U-97
GuldersLaminarFlameSpeed, U-97
HerschelBulkley, U-99
LRDDiffStress, U-99
LRR, U-98
LamBremhorstKE, U-98
LaunderGibsonRSTM, U-98
LaunderSharmaKE, U-98
LienCubicKELowRe, U-98
LienCubicKE, U-98
LienLeschzinerLowRe, U-98
NSRDSfunctions, U-97
Newtonian, U-99
NonlinearKEShih, U-98
PrandtlDelta, U-98
RNGkEpsilon, U-98
RosinRammler, U-97
Smagorinsky2, U-99
Smagorinsky, U-99
SpalartAllmarasDDES, U-99
SpalartAllmarasIDDES, U-99
SpalartAllmaras, U-98, U-99
anisotropicFilter, U-98
basicMultiComponentMixture, U-96, U-176
chemistryModel, U-97
chemistrySolver, U-97
constLaminarFlameSpeed, U-97
constTransport, U-97, U-176
cubeRootVolDelta, U-98
dieselMixture, U-96, U-176
dynMixedSmagorinsky, U-99
dynOneEqEddy, U-99
dynSmagorinsky, U-99
eConstThermo, U-97, U-175
ePsiThermo, U-96, U-176
egrMixture, U-96, U-176
exponential, U-97
general, U-97
hConstThermo, U-97, U-175
Open∇FOAM-1.6

U-194

Index

hPolynomialThermo, U-97, U-175
hPsiMixtureThermo, U-96, U-176
hPsiThermo, U-96, U-176
hRhoMixtureThermo, U-96, U-176
hRhoThermo, U-96, U-176
hhuMixtureThermo, U-96 0 0 10 0 0 cm BT /R251 10.9091 Tf 1 0 0 1 211.806 759.658 Tm [(,)-0.248413]TJ

U-195

Index
applications, U-69
file format, U-102
libraries, U-69
OpenFOAM
library, U-94
OpenFOAM file syntax
//, U-102
openMPI
message passing interface, U-83
MPI, U-83
operator
scalar, P-28
vector, P-27
Options window, U-163
options file, U-73
order keyword, U-83
Orientation Axes button, U-26, U-163
OSspecific
library, U-96
outer product, see tensor, outer product
outlet
boundary condition, P-69
outletInlet
boundary condition, U-133
outside
keyword entry, U-145
owner
dictionary, U-125

P
p field, U-24
P1
library, U-96
paraFoam, U-25, U-159
parallel
running, U-81
partialSlip
boundary condition, U-133
particleTracks utility, U-92
patch
boundary condition, U-131
patch
keyword entry, U-130, U-172
patchAverage utility, U-92
patches keyword, U-135, U-137
patchIntegrate utility, U-92
patchMap keyword, U-156
patchSummary utility, U-94
PBiCG
keyword entry, U-118
PCG
keyword entry, U-118
pdf
library, U-97

pdfPlot utility, U-93
pdRefCell keyword, U-121
pdRefValue keyword, U-121
PDRFoam solver, U-87
Pe utility, U-92
perfectGas model, U-97, U-175
permutation symbol, P-19
pimpleDyMFoam solver, U-86
pimpleFoam solver, U-86
Pipeline Browser window, U-25, U-160
PISO
dictionary, U-25
pisoFoam solver, U-19, U-86
Plot Over Line
menu entry, U-35
Plot Type menu, U-35
plot3dToFoam utility, U-89
pointField class, P-31
pointField template class, P-33
points
dictionary, U-125, U-132
polyBoundaryMesh class, P-31
polyDualMesh utility, U-90
polyLine
keyword entry, U-136
polyMesh directory, U-102, U-125
polyMesh class, P-31, U-123, U-125
polynomialTransport model, U-97, U-176
polyPatch class, P-31
polyPatchList class, P-31
polySpline
keyword entry, U-136
porousExplicitSourceReactingParcelFoam solver,
U-88
post-processing, U-159
post-processing
paraFoam, U-159
postCalc
library, U-95
postChannel utility, U-93
potential
library, U-95
potentialFoam solver, P-46, U-85
pow
tensor member function, P-25
powerLaw model, U-99
pPrime2 utility, U-92
PrandtlDelta model, U-98
preconditioner keyword, U-118, U-119
pRefCell keyword, U-25, U-121
pRefValue keyword, U-25, U-121
pressure keyword, U-50
pressure waves
in liquids, P-62
Open∇FOAM-1.6

U-196

Index

pressureDirectedInletVelocity
boundary condition, U-133
pressureInletVelocity
boundary condition, U-133
pressureOutlet
boundary condition, P-63
pressureTransmissive
boundary condition, U-133
primitive
library, P-23
primitives tools, U-94
printCoeffs keyword, U-42
processorWeights keyword, U-82
probeLocations utility, U-92
process
background, U-26, U-81
foreground, U-26
processor
boundary condition, U-131
processor
keyword entry, U-130
processorN directory, U-82
processorWeights keyword, U-83
Properties window panel, U-28, U-160
ptot utility, U-93
pureMixture model, U-96, U-176
purgeWrite keyword, U-109
PV3FoamReader
library, U-159
PV3FoamReader utility, U-91
PVFoamReader
library, U-159
PVFoamReader utility, U-91

Q
Q utility, U-92
QUICK
keyword entry, U-113, U-116
qZeta model, U-98

R
R utility, U-92
radiation
library, U-96
randomProcesses
library, U-96
RASModel keyword, U-179
RASmodel
keyword entry, U-42, U-178
raw
keyword entry, U-109, U-170
reactingFoam solver, U-87
reactingMixture model, U-96, U-176
reactingParcelFoam solver, U-88
Open∇FOAM-1.6

reactionThermophysicalModels
library, U-96
realizableKE model, U-98
reconstructPar utility, U-85, U-93
reconstructParMesh utility, U-93
redistributeMeshPar utility, U-93
refGradient keyword, U-132
refineHexMesh utility, U-91
refinementRegions keyword, U-145
refinementLevel utility, U-91
refinementRegions keyword, U-143, U-146
refinementSurfaces keyword, U-143
refineMesh utility, U-90
refineWallLayer utility, U-91
Region Status window panel, U-25
regions keyword, U-59
relative tolerance, U-118
relativeSizes keyword, U-148
relaxed keyword, U-149
relTol keyword, U-53, U-118
removeFaces utility, U-91
Render View window, U-164
Render View window panel, U-163
Render View Options window, U-163
renumberMesh utility, U-90
Rescale to Data Range button, U-28
Reset button, U-160
resolveFeatureAngle keyword, U-143, U-144
restart, U-39
Reynolds number, U-19, U-23
rhoCentralFoam solver, U-86
rhoPisoFoam solver, U-86
rhoPimpleFoam solver, U-86
rhoPorousSimpleFoam solver, U-86
rhopSonicFoam solver, U-86
rhoReactingFoam solver, U-87
rhoSimpleFoam solver, U-86
rhoSonicFoam solver, U-86
rmdepall script/alias, U-76
RNGkEpsilon model, U-98
roots keyword, U-83, U-84
RosinRammler model, U-97
rotateMesh utility, U-90
run
parallel, U-81
run directory, U-101
runTime
keyword entry, U-33, U-108
runTimeModifiable keyword, U-109

S
sammToFoam utility, U-90
sample utility, U-93, U-169
sampling

Index
library, U-95
Save Animation
menu entry, U-165
Save Screenshot
menu entry, U-165
scalar, P-16
operator, P-28
scalar class, P-23
scalarField class, P-29
scalarTransportFoam solver, U-85
scale
tensor member function, P-25
scalePoints utility, U-153
scaleSimilarity model, U-99
scientific
keyword entry, U-109
scotch
keyword entry, U-82, U-83
scotchCoeffs keyword, U-83
script/alias
foamCorrectVrt, U-154
foamJob, U-173
foamLog, U-173
make, U-71
rmdepall, U-76
wclean, U-75
wmake, U-71
second time derivative, P-37
Seed window, U-164
selectCells utility, U-91
Set Solid Color button, U-162
setFields utility, U-58, U-59, U-89
setFormat keyword, U-170
sets keyword, U-170
setSet utility, U-90
setsToZones utility, U-90
Settings
menu entry, U-163
settlingFoam solver, U-87
SFCD
keyword entry, U-113, U-116
shallowWaterFoam solver, U-86
shape, U-136
Show Color Legend
menu entry, U-28
SI units, U-105
simple
keyword entry, U-82, U-83
simpleFilter model, U-98
simpleFoam solver, P-54, U-86
simpleGrading keyword, U-136
simpleSpline
keyword entry, U-136
simulationType keyword, U-42, U-60, U-178

U-197
skew
tensor member function, P-25
skewLinear
keyword entry, U-113, U-116
slice class, P-31
slip
boundary condition, U-133
Smagorinsky model, U-99
Smagorinsky2 model, U-99
smapToFoam utility, U-91
smoothDelta model, U-98
smoother keyword, U-120
smoothSolver
keyword entry, U-118
snap keyword, U-142
snapControls keyword, U-142
snappyHexMesh utility
background mesh, U-142
cell removal, U-144
cell splitting, U-143
mesh layers, U-146
meshing process, U-141
snapping to surfaces, U-146
snappyHexMesh utility, U-89, U-140
snappyHexMeshDict file, U-141
snGrad
fvc member function, P-37
snGradCorrection
fvc member function, P-37
snGradSchemes keyword, U-111
Solid Color
menu entry, U-162
solidDisplacementFoam solver, U-88
solidDisplacementFoam solver, U-51
solidEquilibriumDisplacementFoam solver, U-88
solidMixture
library, U-98
solidParticle
library, U-96
solids
library, U-98
solver
PDRFoam, U-87
XiFoam, U-87
blockMesh, P-47
boundaryFoam, U-85
bubbleFoam

U-198
chtMultiRegionFoam,

Index

U-199

Index
double inner product, P-19
geometric transformation, P-20
Hodge dual, P-22
hydrostatic, P-21
identities, P-21
identity, P-20
inner product, P-18
inverse, P-22
magnitude, P-20
magnitude squared, P-20
mathematics, P-15
notation, P-17
nth power, P-20
outer product, P-19
rank, P-16
rank 3, P-16
scalar division, P-18
scalar multiplication, P-17
scale function, P-20
second rank, P-16
T
skew, P-21
T()
square of, P-20
tensor member function, P-25
subtraction, P-17
template class
symmetric, P-21
GeometricBoundaryField, P-32
symmetric rank 2, P-16
fvMatrix, P-33
symmetric rank 3, P-16
dimensioned, P-25
trace, P-21
FieldField, P-32
transformation, P-20
Field, P-29
transpose, P-16, P-21
geometricField, P-32
triple inner product, P-19
List, P-29
vector cross product, P-19
pointField, P-33
tensor class, P-23
surfaceField, P-33
tensor member function
volField, P-33
*, P-25
temporal discretisation, P-42
+, P-25
Crank Nicholson, P-42
-, P-25
Euler implicit, P-42
/, P-25
explicit, P-42
&, P-25
in OpenFOAM, P-43
&&, P-25
tensor, P-15
^, P-25
addition, P-17
cmptAv, P-25
algebraic operations, P-17
cofactors, P-25
algebraic operations in OpenFOAM, P-23
det, P-25
antisymmetric, see tensor, skew
dev, P-25
calculus, P-27
diag, P-25
classes in OpenFOAM, P-23
I, P-25
cofactors, P-22
inv, P-25
component average, P-20
mag, P-25
component maximum, P-20
magSqr, P-25
component minimum, P-20
max, P-25
determinant, P-22
min, P-25
deviatoric, P-21
pow, P-25
diagonal, P-21
scale, P-25
dimension, P-16
skew, P-25
surfaceNormalFixedValue
boundary condition, U-133
surfaces keyword, U-170
surfMesh
library, U-95
SuSp
fvm member function, P-37
sutherlandTransport model, U-97, U-176
symm
tensor member function, P-25
symmetryPlane
boundary condition, P-63, U-131
symmetryPlane
keyword entry, U-130
symmTensorField class, P-29
symmTensorThirdField class, P-29
system directory, P-49, U-102
systemCall
library, U-95

Open∇FOAM-1.6

U-200
sqr, P-25
symm, P-25
T(), P-25
tr, P-25
transform, P-25
tensorField class, P-29
tensorThirdField class, P-29
tetgenToFoam utility, U-90
text box
Opacity, U-163
thermalProperties
dictionary, U-51
thermophysical
library, U-175
thermophysicalFunctions
library, U-97
thermophysicalProperties
dictionary, U-175
thermoType keyword, U-175
time
control, U-108
time derivative, P-37
first, P-39

Index

U-201

uniform keyword, U-171
units
base, U-105
of measurement, P-25, U-105
S.I. base, P-25
SI, U-105
Système International, U-105
United States Customary System, U-105
USCS, U-105
Update GUI button, U-28, U-161
uprime utility, U-92
upwind
keyword entry, U-113, U-116
upwind differencing, P-38, U-61
USCS units, U-105
Us30.247294]TJ .0492351]TJT Q 0 0 0 1 K 0 0 0 1 k q 10 0 0 10 0 0 cm BT /R251 10.9091 Tf 1 0 0 1 70.86 596.515 Tm [(u)0.32898(

U-202
pdfPlot, U-93
plot3dToFoam, U-89
polyDualMesh, U-90
postChannel, U-93
probeLocations, U-92
ptot, U-93
reconstructParMesh, U-93
reconstructPar, U-85, U-93
redistributeMeshPar, U-93
refineHexMesh, U-91
refineMesh, U-90
refineWallLayer, U-91
refinementLevel, U-91
removeFaces, U-91
renumberMesh, U-90
rotateMesh, U-90
sammToFoam, U-90
sample, U-93, U-169
scalePoints, U-153
selectCells, U-91
setFields, U-58, U-59, U-89
setSet, U-90
setsToZones, U-90
smapToFoam, U-91
snappyHexMesh, U-89, U-140
splitCells, U-91
splitMeshRegions, U-90
splitMesh, U-90
star4ToFoam, U-90
starToFoam, U-90, U-149
stitchMesh, U-90
streamFunction, U-92
stressComponents, U-92
subsetMesh, U-91
tetgenToFoam, U-90
transformPoints, U-91
uprime, U-92
vorticity, U-92
wallGradU, U-92
wallHeatFlux, U-92
wallShearStress, U-92
wdot, U-93
writeCellCentres, U-93
writeMeshObj, U-90
yPlusLES, U-92
yPlusRAS, U-92
zipUpMesh, U-91
cellSet, U-90
faceSet, U-90
pointSet, U-90
utilityFunctionObjects
library, U-95
Open∇FOAM-1.6

Index

V
value keyword, U-23, U-132
valueFraction keyword, U-132
van Leer differencing, P-38
vanLeer
keyword entry, U-113
VCR Controls menu, U-28, U-161
vector, P-16
operator, P-27
unit, P-20
vector class, P-23, U-105
vector product, see tensor, vector cross product
vectorField class, P-29
version keyword, U-103
vertices keyword, U-22, U-135
veryInhomogeneousMixture model, U-96, U-176
View menu, U-163
View Settings
menu entry, U-26, U-163
View Settings...
menu entry, U-25
viscosity
kinematic, U-23, U-42
volField template class, P-33
vorticity utility, U-92
vtk
keyword entry, U-170
vtkFoam
library, U-159
vtkPV3Foam
library, U-159

W
wall
boundary condition, P-63, P-69, U-58,
U-131
wall
keyword entry, U-130
wallBuoyantPressure
boundary condition, U-133
wallGradU utility, U-92
wallHeatFlux utility, U-92
Wallis
library, U-97
wallShearStress utility, U-92
wclean script/alias, U-75
wdot utility, U-93
wedge
boundary condition, U-126, U-131, U-139
wedge
keyword entry, U-130
window
Chart Options, U-36
Color Legend, U-30

U-203

Index
Options, U-163
Pipeline Browser, U-25, U-160
Render View Options, U-163
Render View, U-164
Seed, U-164
window panel
Annotation, U-26, U-163
Color Legend, U-162
Color Scale, U-162
Display, U-25, U-28, U-160, U-161
General, U-163
Information, U-160
Lights, U-163
Properties, U-28, U-160
Region Status, U-25
Render View, U-163
Style, U-25, U-162
Wireframe
menu entry, U-162
WM ARCH
environment variable, U-76
WM COMPILE OPTION
environment variable, U-76
WM COMPILER
environment variable, U-76
WM COMPILER BIN
environment variable, U-76
WM COMPILER DIR
environment variable, U-76
WM COMPILER LIB
environment variable, U-76
WM DIR
environment variable, U-76
WM JAVAC OPTION
environment variable, U-76
WM LINK LANGUAGE
environment variable, U-76
WM MPLIB
environment variable, U-76
WM OPTIONS
environment variable, U-76
WM PROJECT
environment variable, U-76
WM PROJECT DIR
environment variable, U-76
WM PROJECT INST DIR

environment variable, U-76
WM PROJECT LANGUAGE
environment variable, U-76
WM PROJECT USER DIR
environment variable, U-76
WM PROJECT VERSION
environment variable, U-76
WM SHELL
environment variable, U-76
wmake
platforms, U-73
wmake script/alias, U-71
word class, P-25, P-31
writeCellCentres utility, U-93
writeCompression keyword, U-109
writeControl
keyword entry, U-108
writeControl keyword, U-24, U-60, U-108
writeFormat keyword, U-55, U-109
writeInterval keyword, U-24, U-33, U-109
writeMeshObj utility, U-90
writeNow
keyword entry, U-108
writePrecision keyword, U-109

X
x
keyword entry, U-171
XiFoam solver, U-87
xmgr
keyword entry, U-109, U-170
xyz
keyword entry, U-171

Y
y
keyword entry, U-171
yPlusLES utility, U-92
yPlusRAS utility, U-92

Z
z
keyword entry, U-171
zeroGradient
boundary condition, U-132
zipUpMesh utility, U-91

Open∇FOAM-1.6

Source Exif Data:

File Type                       : PDF
File Type Extension             : pdf
MIME Type                       : application/pdf
PDF Version                     : 1.4
Linearized                      : No
Warning                         : Invalid xref table

EXIF Metadata provided by EXIF.tools

User Guide

Navigation menu

Versions of this User Manual:

Views

Navigation