CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Specifying nonuniform initial condition

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree3Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 28, 2006, 05:19
Default C() is described in Table 2.1
  #21
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,840
Rep Power: 38
gschaider will become famous soon enoughgschaider will become famous soon enough
C() is described in Table 2.1 of the Programmer's guide. component() accesses components of a tensor/vector.
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   March 28, 2006, 05:56
Default so then why is it component(0
  #22
Member
 
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 7
anja is on a distinguished road
so then why is it component(0 ?! )
anja is offline   Reply With Quote

Old   March 28, 2006, 06:15
Default Because C++ (==Foam) starts to
  #23
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,840
Rep Power: 38
gschaider will become famous soon enoughgschaider will become famous soon enough
Because C++ (==Foam) starts to count with 0 (as opposed to Fortran which starts with 1). Therefor the first component (== x-coordinate) is accessed with the index 0.
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   March 28, 2006, 06:37
Default OK, let's do chapter and verse
  #24
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,742
Rep Power: 20
hjasak will become famous soon enough
OK, let's do chapter and verse on this:

1) OpenFOAM field class is called GeometricField and it can contain scalars, vectors, tensors etc. These things are defined as surfaceScalarField, volVectorField, pointScalarField, volTensorField etc.

2) For some of those fiels it makes sense to ask for a component. So, if I've got a volVectorField, I could ask for the x() component (this is a sensible and meaningful operation), whereas for the volTensorField I may asn for the xy() component. How do I do that?

Well, since volVectorField is a GeometricField<vector,>, I cannot add the x() member function to it - it would not make sense for scalar or tensor fields, right? Thus, I need a general way to as for a component of a field.

3) The first step is in the definition of scalars, vectors and tensors. Here, I define two things:
- an enumeration for the component. For a vector, this will say X, Y, Z and for a tensor XX, XY, XZ, YX, YY, YZ, etc. Note that enumeration is basically an int wrapped up for use and that the count starts from zero. Thus, in a vector X is 0, Y is 1 etc. and the tensor you can work it out yourself.
- a member function returning a component. Thus, you know what the following bit of the code does:


vector a(1, 2, 3);
a.component(vector::Y);


Now, we can pull through the component function through the fields and GeometricFields. Examples:


vectorField a(10);
// fill it up
scalarField ax = a.component(vector::X);


or


tensorField t(33);
scalarField tyz = t.component(tensor::YZ);


Alll clear, I hope.

Thus:

- mesh.C() returns a volVectorField of cell centres.
- mesh.C()[cellI] gets the cellI element from the internal field (you have jumped into the internal field directly because the GeometricField is derived from the internal field.
- mesh.C()[cellI].component(0) is equivalent to mesh.C()[cellI].component(vector::X), which should be clear.

Note that you can also do:

volScalarField cx = mesh.C().component(vector::X);

or

scalarField cxIn = mesh.C().internalField().component(vector::X);


Better?

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   March 28, 2006, 06:50
Default Thanks a lot
  #25
Member
 
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 7
anja is on a distinguished road
Thanks a lot
anja is offline   Reply With Quote

Old   May 22, 2006, 12:24
Default Hello, I would like to read
  #26
Member
 
anne dejoan
Join Date: Mar 2009
Location: madrid, spain
Posts: 66
Rep Power: 7
anne is on a distinguished road
Hello,

I would like to read the velocity
field U obtained as an output in time directory.

My mesh is made of several blocks.
when using one block I had no problem to read
the file through the loop:

do k=1,nz
do j=1,ny
do i=1,nx
...
where nx ,ny and nx were the total number of cell.

However, now using several blocks in the
0x, 0y and 0z directions I can not
read correctely the file.
(Looking at the file with ParaFoam all
is OK, so that the file is OK).

Could you let me know the writing format of the
output file when uing several blocks?
Is this a writing block by block?

Thanks,

Anne
anne is offline   Reply With Quote

Old   May 27, 2007, 04:08
Default Can someone verify if I'm doin
  #27
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 697
Rep Power: 10
msrinath80 is on a distinguished road
Can someone verify if I'm doing this right using funkySetFields. I wish to create a sphere of radius 0.5 in the center of the 3D geometry. The syntax I'm using is:

funkySetFields . cavity -field gamma -expression '(grad(dist())^vector(0,0,0))*mag(pos()-vector(0.5,0.5,0.5))/0.5' -time 0

If this is incorrect, I would appreciate if someone can help. Thanks!
msrinath80 is offline   Reply With Quote

Old   May 29, 2007, 07:15
Default Hi! I would suggest funk
  #28
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,840
Rep Power: 38
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi!

I would suggest

funkySetFields . cavity -field gamma -condition "mag(pos()-vector(0.5,0.5,0.5))<0.5" -expression "1." -time 0 -keepPatches

assuming that (0.5,0.5,0.5) is the center of your geometry and gamma originally was set to "uniform 0"
Whatever the other stuff in your example does it is going to become zero because of the product with vector(0,0,0).

Bernhard
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   May 29, 2007, 07:51
Default Only one word for you Bernhard
  #29
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,742
Rep Power: 20
hjasak will become famous soon enough
Only one word for you Bernhard: BEAUTIFUL!

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 29, 2007, 13:53
Default Thanks Bernhard. That was very
  #30
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 697
Rep Power: 10
msrinath80 is on a distinguished road
Thanks Bernhard. That was very useful
msrinath80 is offline   Reply With Quote

Old   June 15, 2007, 13:20
Default Hi Bernhard, funkySetFields
  #31
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 697
Rep Power: 10
msrinath80 is on a distinguished road
Hi Bernhard,

funkySetFields[1] compiles and runs as intended on OF 1.3. However, OF 1.4 does not like it. Can you post the API modifications required for it to work on OF 1.4.

Thanks!

[1] http://openfoamwiki.net/images/7/79/...s.r7241.tar.gz
msrinath80 is offline   Reply With Quote

Old   June 17, 2007, 04:00
Default Hi, One might be able to try
  #32
Super Moderator
 
Takuya OSHIMA
Join Date: Mar 2009
Location: Niigata City, Japan
Posts: 515
Blog Entries: 1
Rep Power: 10
7islands is on a distinguished road
Hi,
One might be able to try this patch (with some modifications for my own purpose) until Bernhard makes a new release (I believe it won't be so long anyway) for OF 1.4. This contains
* harsh fix for building problem and SIGFPE crash by constant scalar division on OF 1.4
* deltaT(): returns the value of deltaT in controlDict
* rdist(x, y, z): equivalent of mag(pos() - vec(x,y,z)) where x, y, z are scalars

Takuya

funkySetFields.r7241-20070528.diff
7islands is offline   Reply With Quote

Old   June 17, 2007, 05:14
Default Thanks Takuya. It compiled nic
  #33
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 697
Rep Power: 10
msrinath80 is on a distinguished road
Thanks Takuya. It compiled nicely!

Here are the quick instructions for those new to patching:

1. First patch the file using patch -p0 < funkySetFields.r7241-20070528.diff

2. Copy all files from the GeneratedFiles subdirectory to the current directory (i.e. directory which contains funkySetFields.C).

3. Execute wmake in the same directory.
msrinath80 is offline   Reply With Quote

Old   June 20, 2007, 09:23
Default Hi! Thanks to Takuya for hi
  #34
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,840
Rep Power: 38
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi!

Thanks to Takuya for his fixes. I've incorporated these into my sources (which are now updated to 1.4, plus they sould be less restrictive in their choice of a bison-version). I've also added a time()-function (don't need it, but the deltaT was there, so it seemed logical)


Description and download link:

http://openfoamwiki.net/index.php/Co...funkySetFields

http://openfoamwiki.net/images/7/79/...s.r7241.tar.gz

Bernhard
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   June 20, 2007, 12:12
Default Ignor the link for the downloa
  #35
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,840
Rep Power: 38
gschaider will become famous soon enoughgschaider will become famous soon enough
Ignor the link for the download in the last posting. It should have been
http://openfoamwiki.net/images/f/fe/...s.r7568.tar.gz
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   July 27, 2007, 12:31
Default Can somebody tell me how to ex
  #36
New Member
 
Mark Dowling
Join Date: Mar 2009
Posts: 6
Rep Power: 7
markdowlinguk is on a distinguished road
Can somebody tell me how to extract and compile the funkySetFields .gz file and which directory in which to place the files ?

Apologies for the stupid question - but I'm completely new to linux.

Thanks
Mark
markdowlinguk is offline   Reply With Quote

Old   July 29, 2007, 14:55
Default Hello, I am using funkySetFiel
  #37
Member
 
Quinn Tian
Join Date: Mar 2009
Posts: 62
Rep Power: 7
qtian is on a distinguished road
Hello, I am using funkySetFields to set my non uniform inflow boundary

Here is the command I used for epsilon,

funkySetFields . nufbump -time 0 -field epsilon -keepPatches -valuePatches 'inlet' -expression '0.4983*pow(pos().y,-1.209)'

Here is the error message I got,

#0 Foam::error::printStack(Foam:stream&)
#1 Foam::sigFpe::sigFpeHandler(int)
#2 Uninterpreted: [0xffffe420]
#3 pow
#4 Foam::pow(Foam::Field<double>&, Foam::UList<double> const&, double const&)
#5 Foam::tmp<foam::geometricfield<double,> > Foam::pow<foam::fvpatchfield,>(Foam::GeometricFiel d<double,> const&, Foam::dimensioned<double> const&)
#6 Foam::tmp<foam::geometricfield<double,> > Foam::pow<foam::fvpatchfield,>(Foam::GeometricFiel d<double,> const&, double const&)
#7 .L25229 at ValueExpressionParser.C:0
#8 ValueExpressionDriver::parse(std::string const&)
#9 doAnExpression(Foam::fvMesh const&, Foam::word const&, Foam::string const&, Foam::string const&, Foam::Time const&, bool, bool, Foam::dimensionSet const&, bool, Foam::List<foam::word> const&)
#10 main
#11 __libc_start_main
#12 Foam::regIOobject::readIfModified()
Floating point exception (core dumped)

I also found out if I change -1.209 to 1, error message disappear. I guess this might be the format problem for pow(,),but I really don't know how to make it work. Sorry about the silly question. Can anyone give me some help? Thanks for your help.

Best
QT
qtian is offline   Reply With Quote

Old   July 29, 2007, 18:09
Default Apologies for the delay. Here
  #38
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 697
Rep Power: 10
msrinath80 is on a distinguished road
Apologies for the delay. Here you go Mark:

[madhavan@head01 ~]$ cd OpenFOAM/madhavan-1.4/

[madhavan@head01 madhavan-1.4]$ ls
applications custom_utils lib run

[madhavan@head01 madhavan-1.4]$ cd custom_utils/

[madhavan@head01 custom_utils]$ cd Bernhard_Gschaider/

[madhavan@head01 Bernhard_Gschaider]$ ls
parabolic_velocity_inlet

[madhavan@head01 Bernhard_Gschaider]$ mkdir funkySetFields

[madhavan@head01 Bernhard_Gschaider]$ cd funkySetFields/

[madhavan@head01 funkySetFields]$ wget http://openfoamwiki.net/images/f/fe/...s.r7568.tar.gz
--15:59:40-- http://openfoamwiki.net/images/f/fe/...s.r7568.tar.gz
=> `FunkySetFields.r7568.tar.gz'
Resolving openfoamwiki.net... 193.171.80.115
Connecting to openfoamwiki.net|193.171.80.115|:80... connected.
HTTP request sent, awaiting response... 200 OK
Length: 48,785 (48K) [application/x-tar]

100%[================================================== ===>] 48,785 102.10K/s

15:59:41 (101.89 KB/s) - `FunkySetFields.r7568.tar.gz' saved [48785/48785]

[madhavan@head01 funkySetFields]$ ls
FunkySetFields.r7568.tar.gz

[madhavan@head01 funkySetFields]$ tar xzf FunkySetFields.r7568.tar.gz

[madhavan@head01 funkySetFields]$ cd funkySetFields.r7568/

[madhavan@head01 funkySetFields.r7568]$ ls
GeneratedFiles ValueExpressionDriverLogicalTemplates.H funkySetFieldsDict
Make ValueExpressionLexer.ll getGenerated.sh
ValueExpressionDriver.C ValueExpressionParser.yy insertGenerated.sh
ValueExpressionDriver.H funkySetFields.C

[madhavan@head01 funkySetFields.r7568]$ cp -r GeneratedFiles/* .

[madhavan@head01 funkySetFields.r7568]$ wmake
Making dependency list for source file ValueExpressionParser.C
Making dependency list for source file ValueExpressionLexer.C
Making dependency list for source file funkySetFields.C
SOURCE=ValueExpressionParser.C ; g++ -m64 -Dlinux64 -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -DNoRepository -ftemplate-depth-40 -IMake/linux64Gcc4DPOpt -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/finiteVolume/lnInclude -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/meshTools/lnInclude -IlnInclude -I. -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/OpenFOAM/lnInclude -fPIC -c $SOURCE -o Make/linux64Gcc4DPOpt/ValueExpressionParser.o
ValueExpressionParser.tab.cc: In member function 'unsigned char ve::ValueExpressionParser::yytranslate_(int)':
ValueExpressionParser.tab.cc:1814: warning: use of old-style cast
SOURCE=ValueExpressionLexer.C ; g++ -m64 -Dlinux64 -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -DNoRepository -ftemplate-depth-40 -IMake/linux64Gcc4DPOpt -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/finiteVolume/lnInclude -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/meshTools/lnInclude -IlnInclude -I. -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/OpenFOAM/lnInclude -fPIC -c $SOURCE -o Make/linux64Gcc4DPOpt/ValueExpressionLexer.o
ValueExpressionLexer.C:245: warning: use of old-style cast
ValueExpressionLexer.C:296: warning: use of old-style cast
ValueExpressionLexer.C:296: warning: use of old-style cast
lex.ve.c: In function 'int velex(ve::ValueExpressionParser::semantic_type*, ve::location*, ValueExpressionDriver&)':
lex.ve.c:3894: warning: use of old-style cast
lex.ve.c:3894: warning: use of old-style cast
lex.ve.c:3910: warning: use of old-style cast
lex.ve.c:4229: warning: use of old-style cast
lex.ve.c: In function 'int yy_get_next_buffer()':
lex.ve.c:4397: warning: use of old-style cast
lex.ve.c:4424: warning: use of old-style cast
lex.ve.c:4437: warning: use of old-style cast
lex.ve.c:4438: warning: use of old-style cast
lex.ve.c:4459: warning: use of old-style cast
lex.ve.c: In function 'yy_state_type yy_get_previous_state()':
lex.ve.c:4507: warning: use of old-style cast
lex.ve.c:4507: warning: use of old-style cast
lex.ve.c: In function 'int yyinput()':
lex.ve.c:4664: warning: use of old-style cast
lex.ve.c: In function 'yy_buffer_state* ve_create_buffer(FILE*, int)':
lex.ve.c:4741: warning: use of old-style cast
lex.ve.c:4750: warning: use of old-style cast
lex.ve.c: In function 'void ve_delete_buffer(yy_buffer_state*)':
lex.ve.c:4773: warning: use of old-style cast
lex.ve.c:4776: warning: use of old-style cast
lex.ve.c:4778: warning: use of old-style cast
lex.ve.c: In function 'yy_buffer_state* ve_scan_buffer(char*, yy_size_t)':
lex.ve.c:4857: warning: use of old-style cast
lex.ve.c: In function 'yy_buffer_state* ve_scan_bytes(const char*, int)':
lex.ve.c:4911: warning: use of old-style cast
lex.ve.c: In function 'void yy_push_state(int)':
lex.ve.c:4950: warning: use of old-style cast
lex.ve.c:4954: warning: use of old-style cast
lex.ve.c:4954: warning: use of old-style cast
lex.ve.c: In function 'void* yy_flex_alloc(yy_size_t)':
lex.ve.c:5061: warning: use of old-style cast
lex.ve.c: In function 'void* yy_flex_realloc(void*, yy_size_t)':
lex.ve.c:5079: warning: use of old-style cast
lex.ve.c:5079: warning: use of old-style cast
lex.ve.c: At global scope:
lex.ve.c:4936: warning: 'void yy_push_state(int)' defined but not used
lex.ve.c:4969: warning: 'void yy_pop_state()' defined but not used
lex.ve.c:4980: warning: 'int yy_top_state()' defined but not used
SOURCE=ValueExpressionDriver.C ; g++ -m64 -Dlinux64 -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -DNoRepository -ftemplate-depth-40 -IMake/linux64Gcc4DPOpt -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/finiteVolume/lnInclude -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/meshTools/lnInclude -IlnInclude -I. -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/OpenFOAM/lnInclude -fPIC -c $SOURCE -o Make/linux64Gcc4DPOpt/ValueExpressionDriver.o
SOURCE=funkySetFields.C ; g++ -m64 -Dlinux64 -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -DNoRepository -ftemplate-depth-40 -IMake/linux64Gcc4DPOpt -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/finiteVolume/lnInclude -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/meshTools/lnInclude -IlnInclude -I. -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/OpenFOAM/lnInclude -fPIC -c $SOURCE -o Make/linux64Gcc4DPOpt/funkySetFields.o
g++ -m64 -Dlinux64 -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -DNoRepository -ftemplate-depth-40 -IMake/linux64Gcc4DPOpt -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/finiteVolume/lnInclude -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/meshTools/lnInclude -IlnInclude -I. -I/homes/madhavan/OpenFOAM/OpenFOAM-1.4/src/OpenFOAM/lnInclude -fPIC Make/linux64Gcc4DPOpt/ValueExpressionParser.o Make/linux64Gcc4DPOpt/ValueExpressionLexer.o Make/linux64Gcc4DPOpt/ValueExpressionDriver.o Make/linux64Gcc4DPOpt/funkySetFields.o -L/homes/madhavan/OpenFOAM/OpenFOAM-1.4/lib/linux64Gcc4DPOpt \
-lfiniteVolume -lmeshTools -lOpenFOAM -liberty -ldl -lm -o /homes/madhavan/OpenFOAM/madhavan-1.4/applications/bin/linux64Gcc4DPOpt/funkySet Fields
[madhavan@head01 funkySetFields.r7568]$

PS: The first half of the instructions are not mandatory. I keep all custom utilities organized in folders. You can do the same or else put them somewhere you find convenient. On a side-note, you can survive longer in the OpenFOAM world without knowing C++, but you certainly will not if you are not familiar with the terminal/command line. My advice is to try and get familiar with it as soon as you can.
msrinath80 is offline   Reply With Quote

Old   July 29, 2007, 20:23
Default Srinath or anyone, Is it po
  #39
Member
 
Quinn Tian
Join Date: Mar 2009
Posts: 62
Rep Power: 7
qtian is on a distinguished road
Srinath or anyone,

Is it possible for you to answer my above question also? I am really stuck. Thanks.

Quinn
qtian is offline   Reply With Quote

Old   July 31, 2007, 10:25
Default Srinath, Huge thanks for th
  #40
New Member
 
Mark Dowling
Join Date: Mar 2009
Posts: 6
Rep Power: 7
markdowlinguk is on a distinguished road
Srinath,

Huge thanks for the very clear instructions...
It turns out I was doing something similar, but my lack of linux experience (which I'm having to rapidly overcome) made me wonder if I'd done something wrong...

Either way - when following your instructions about the program fails to compile with the following error (NB I used the insertGenerated.sh command because I have an earlier version of bison)

[PTS@tcad funkySetFields.r7568]$ . insertGenerated.sh
Preparing run to avoid usage of bison
[PTS@tcad funkySetFields.r7568]$ wmake
Making dependency list for source file ValueExpressionParser.C
Making dependency list for source file ValueExpressionLexer.C
Making dependency list for source file funkySetFields.C
Making dependency list for source file ValueExpressionDriver.C
SOURCE=ValueExpressionParser.C ; g++ -m32 -Dlinux -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-40 -IMake/linuxGcc4DPOpt -I/home/PTS/OpenFOAM/OpenFOAM-1.4/src/finiteVolume/lnInclude -I/home/PTS/OpenFOAM/OpenFOAM-1.4/src/meshTools/lnInclude -IlnInclude -I. -I/home/PTS/OpenFOAM/OpenFOAM-1.4/src/OpenFOAM/lnInclude -fPIC -pthread -c $SOURCE -o Make/linuxGcc4DPOpt/ValueExpressionParser.o
ValueExpressionParser.tab.cc: In member function 'unsigned char ve::ValueExpressionParser::yytranslate_(int)':
ValueExpressionParser.tab.cc:1814: warning: use of old-style cast
/tmp/ccvmLazQ.s: Assembler messages:
/tmp/ccvmLazQ.s:13: Internal error, aborting at ../../gas/config/tc-i386.c line 3501 in output_imm
Please report this bug.
make: *** [Make/linuxGcc4DPOpt/ValueExpressionParser.o] Error 1


Any ideas??

Many thanks again - in the couple of times I have used it I am struck by how rapid and helpful the responses are from the OpenFoam forum - so huge thanks to everybody for that!

Mark
markdowlinguk is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Specifying nonuniform boundary condition maka OpenFOAM Running, Solving & CFD 59 October 22, 2014 14:52
Nonuniform initial condition using cellSetDict rinao OpenFOAM Running, Solving & CFD 6 January 9, 2013 00:42
Initial Condition Tang Kuei FLUENT 0 May 17, 2006 19:54
Nonuniform gradient boundary condition ankgupta8um OpenFOAM Running, Solving & CFD 1 March 14, 2006 01:34
Nonuniform initial conditions nico OpenFOAM Pre-Processing 2 January 4, 2006 06:37


All times are GMT -4. The time now is 22:37.