I did not really want to start
 

I did not really want to start a new thread considering the fact that this subject has been discussed in various forms in the past. However, please bear with me if you can!

I currently have a proper case setup in OpenFoam that solves flow past an obstacle. My C++ is totally rusty and therefore I'm looking for an easy n00bie way to get this parabolic inlet profile done.

For channel flow, I'm looking at an equation of the following form that describes a parabolic velocity profile:

U = 4 * U_max * y (h -y) / (h^2)

Where, 'U_max' and 'h' are constants I provide. 'U_max' is the maximum velocity at the centerline, 'h' refers to the width of the channel.

I would really appreciate if someone could guide me through the relevant steps. I just started using OpenFoam today and I'm impressed with it's ease of use. After a quick walk through the lid-driven cavity tutorial, I was not only able to quickly create my mesh but also run the case for unsteady vortex shedding.

I will put up a tutorial for the same once I get some results I can compare with http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Thanks a lot for your patience!

The parabolic inlet. I read ab
 

The parabolic inlet. I read about cultures in the Pacific where you aren't considered an adult before you havn't programmed your own parabolic-inlet-utility. But this here isn't one of them so it's OK to ask for your help.

I find it difficult to explain things step-by-step (because it's hard to anticipate what the other guy doesn't know) so I'll post you the source of one of my first tries at a OF-Utility and you'll ask about the things you don't understand.

It compiles on 1.3 but the last time I properly tested it was on 1.1 (but I see no reason why it shouldn't work on 1.3). It assumes that your channel is in x-Direction and the inlet a rectangle with borders parallel to y and z. The noncent-options are for cases where you wish to exploit the symmetry of the model (and therefor need only half a parabola).

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif setParabolicInlet.C

Hi, I did one of those a while
 

Hi, I did one of those a while back - it is called parabolicVelocityFvPatchVectorField and should be somewhere on the discussion group. If you'd like the one updated to version 1.3, send me and E-mail and I'll give you the files.

Enjoy,

Hrv

Bernhard: Many thanks for your
 

Bernhard: Many thanks for your prompt response http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

So it's enough if I modify:

scalar vel=maxVel*(1-y*y)*(1-z*z);

to something in the following lines:

scalar vel=4*maxVel*y*(h-y)/(h*h);

My geometry is also a channel (length along x) with an obstacle somewhere inside it. I'm only interested in applying the profile at the inlet, so I won't have to bother about changing anything else?

If that's the case, where do I place this source and how do I get it to compile (wmake?) and subsequently get Openfoam to recognize it?

I know I'm asking for too much here. But I would appreciate if anyone can lend a helping hand. Thanks very much!

Hi p???! (Sorry, can't pronoun
 

Hi p???! (Sorry, can't pronounce your nickname)

Basically both formulations are the same BUT for mine I normalized y from [ymin,ymax] (ymax-ymin)=h to [-1,1] (as you can see in the source)

What this utility does is set the velocity at a patch if on that patch the velocity is fixedValue. Values on a fixed Value patch are not touched by the solver (normally, because he could if he wanted to), just used.

Place the source in a directory. Create a directory Make in it in which you create a file named options with this content

EXE_INC = \
-I$(LIB_SRC)/cfdTools/lnInclude \
-I$(LIB_SRC)/finiteVolume/lnInclude

EXE_LIBS = -lfiniteVolume

and a file files with this content

setParabolicInlet.C
EXE = $(FOAM_USER_APPBIN)/setParabolicInlet

After a wmake the executable is in your path and you can start using it.

BTW: you'll also need a creatFields.H:

Info<< "Vector field U\n" << endl;
volVectorField U
(
IOobject
(
"U",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);

(and look for Hrv's solution. It's always instructive to see the same thing done in different ways)

Thanks for the quick response.
 

Thanks for the quick response. So would I need to impose a parabolic profile in X and Y even if my case will be solved in 2D?

I'm asking because you seem to be doing the following:

maxVel*(1-y*y)*(1-z*z);

No. The test (zmax-zmin)==0 ma
 

No. The test (zmax-zmin)==0 makes sure that you get a 2D-profile for a 2D-case (without having to write a searate utility for 2D and 3D)

Hi Bernhard, I tried your i
 

Hi Bernhard,

I tried your instructions for compiling. This is what I get:

[openfoam@localhost par_inlet]$ wclean && wmake
Making dependency list for source file setParabolicInlet.C

SOURCE_DIR=.
SOURCE=setParabolicInlet.C ; g++ -m64 -DlinuxAMD64 -Wall -W -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -ffast-math -DNoRepository -ftemplate-depth-30 -I/home/openfoam/OpenFOAM/OpenFOAM-1.2/src/cfdTools/lnInclude -I/home/openfoam/OpenFOAM/OpenFOAM-1.2/src/finiteVolume/lnInclude -I/home/openfoam/OpenFOAM/OpenFOAM-1.2/src/cfdTools/general/lnInclude -I/home/openfoam/OpenFOAM/OpenFOAM-1.2/src/OpenFOAM/lnInclude -I/home/openfoam/OpenFOAM/OpenFOAM-1.2/src/OpenFOAM/lnInclude -IlnInclude -I. -fPIC -c $SOURCE -o Make/linuxAMD64Gcc4Opt/setParabolicInlet.o
/home/openfoam/OpenFOAM/OpenFOAM-1.2/wmake/bashScripts/mkObjectDir /home/openfoam/OpenFOAM/openfoam-1.2/applications/bin/linuxAMD64Gcc4Opt/setParab olicInlet
g++ -m64 -DlinuxAMD64 -Wall -W -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -ffast-math -DNoRepository -ftemplate-depth-30 -I/home/openfoam/OpenFOAM/OpenFOAM-1.2/src/cfdTools/lnInclude -I/home/openfoam/OpenFOAM/OpenFOAM-1.2/src/finiteVolume/lnInclude -I/home/openfoam/OpenFOAM/OpenFOAM-1.2/src/cfdTools/general/lnInclude -I/home/openfoam/OpenFOAM/OpenFOAM-1.2/src/OpenFOAM/lnInclude -I/home/openfoam/OpenFOAM/OpenFOAM-1.2/src/OpenFOAM/lnInclude -IlnInclude -I. -fPIC Make/linuxAMD64Gcc4Opt/setParabolicInlet.o -L/home/openfoam/OpenFOAM/OpenFOAM-1.2/lib/linuxAMD64Gcc4Opt \
-lfiniteVolume -lOpenFOAM -lm -o /home/openfoam/OpenFOAM/openfoam-1.2/applications/bin/linuxAMD64Gcc4Opt/setParab olicInlet
/usr/bin/ld: cannot find -lfiniteVolume
collect2: ld returned 1 exit status
make: *** [/home/openfoam/OpenFOAM/openfoam-1.2/applications/bin/linuxAMD64Gcc4Opt/setPara bolicInlet] Error 1


My files file contains:

setParabolicInlet.C
EXE = $(FOAM_USER_APPBIN)/setParabolicInlet


My options file contains:

EXE_INC = \
-I$(LIB_SRC)/cfdTools/lnInclude \
-I$(LIB_SRC)/finiteVolume/lnInclude \
-I$(LIB_SRC)/cfdTools/general/lnInclude \
-I$(LIB_SRC)/OpenFOAM/lnInclude

EXE_LIBS = \
-lfiniteVolume

I'm using OpenFoam 1.2. Any suggestions on what might be wrong?

The finiteVolume stuff is 1.3-
 

The finiteVolume stuff is 1.3-specific. Replace the -lfiniteVolume with -lcfdTools

It works now. Thank you!
 

It works now. Thank you!

hello OpenFoam users, I am
 

hello OpenFoam users,

I am working on backwardFacing step flow. I tried doing as explained above. I created "setParabolic" folder in "/home/user/skolan/OpenFOAM/skolan-1.3/applications" and created setParabolic.C file and Make folder as mentioned above and with same data. When i compile it its running as shown below.

/home/user/skolan/OpenFOAM/skolan-1.3/applications/setParabolic

newton{skolan,204}% wmake
make: `Make/linuxGcc4DPOpt/dependencies' is up to date.

/home/user/skolan/OpenFOAM/OpenFOAM-1.3/wmake/tcshScripts/mkObjectDir /home/user/skolan/OpenFOAM/skolan-1.3/applications/bin/linuxGcc4DPOpt/libsetPara bolic.so
g++ -m32 -Dlinux -DDP -Wall -W -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-30 -I/home/user/skolan/OpenFOAM/OpenFOAM-1.3/src/cfdTools/lnInclude -I/home/user/skolan/OpenFOAM/OpenFOAM-1.3/src/finiteVolume/lnInclude -I/home/user/skolan/OpenFOAM/OpenFOAM-1.3/src/cfdTools/general/lnInclude -I/home/user/skolan/OpenFOAM/OpenFOAM-1.3/src/OpenFOAM/lnInclude -I/home/user/skolan/OpenFOAM/OpenFOAM-1.3/src/OpenFOAM/lnInclude -IlnInclude -I. -fPIC -pthread Make/linuxGcc4DPOpt/libsetParabolic.o -L/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt \
-lfiniteVolume -lOpenFOAM -liberty -o /home/user/skolan/OpenFOAM/skolan-1.3/applications/bin/linuxGcc4DPOpt/libsetPara bolic.so

I tried to use this .so file in my sonicFoam/backwardStep program by giving the library name in Make/options of sonicFoam and then i get the following error.

options file:
EXE_INC = \
-I$(LIB_SRC)/finiteVolume/lnInclude


EXE_LIBS = \
-L$(FOAM_USER_APPBIN)\
-lfiniteVolume\
-lsetParabolic


files file:
sonicFoam.C

EXE = $(FOAM_APPBIN)/sonicFoam

error when i compile sonicFoam is:


/home/user/skolan/OpenFOAM/OpenFOAM-1.3/applications/solvers/compressible/sonicF oam
newton{skolan,132}% wmake
make: `Make/linuxGcc4DPOpt/dependencies' is up to date.

SOURCE_DIR=.
SOURCE=sonicFoam.C ; g++ -m32 -Dlinux -DDP -Wall -W -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-30 -I/home/user/skolan/OpenFOAM/OpenFOAM-1.3/src/finiteVolume/lnInclude -I/home/user/skolan/OpenFOAM/OpenFOAM-1.3/src/OpenFOAM/lnInclude -IlnInclude -I. -fPIC -pthread -c $SOURCE -o Make/linuxGcc4DPOpt/sonicFoam.o
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/wmake/tcshScripts/mkObjectDir /home/user/skolan/OpenFOAM/OpenFOAM-1.3/applications/bin/linuxGcc4DPOpt/sonicFoa m
g++ -m32 -Dlinux -DDP -Wall -W -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-30 -I/home/user/skolan/OpenFOAM/OpenFOAM-1.3/src/finiteVolume/lnInclude -I/home/user/skolan/OpenFOAM/OpenFOAM-1.3/src/OpenFOAM/lnInclude -IlnInclude -I. -fPIC -pthread Make/linuxGcc4DPOpt/sonicFoam.o -L/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt \
-L/home/user/skolan/OpenFOAM/skolan-1.3/applications/bin/linuxGcc4DPOpt -lfiniteVolume -lsetParabolic -lOpenFOAM -liberty -o /home/user/skolan/OpenFOAM/OpenFOAM-1.3/applications/bin/linuxGcc4DPOpt/sonicFoa m
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParabolic.so(.t ext+0x10166): In function `__i686.get_pc_thunk.cx':
: multiple definition of `__i686.get_pc_thunk.cx'
Make/linuxGcc4DPOpt/sonicFoam.o(.gnu.linkonce.t.__i686.get_pc_thunk.cx +0x0):soni cFoam.C: first defined here/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
BS*+0x806e018): In function `__init_array_start':
: multiple definition of `_DYNAMIC'
/usr/lib/crt1.o(.dynamic+0x0):../sysdeps/i386/elf/start.S:65: first de
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
odata+0x0): multiple definition of `_fp_hw'
/usr/lib/crt1.o(.rodata+0x0):../sysdeps/i386/elf/start.S:65: first def
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
nit+0x0): In function `_init':
/usr/src/packages/BUILD/glibc-2.3/cc/csu/crti.S:36: multiple definitio
t'
/usr/lib/crti.o(.init+0x0):/usr/src/packages/BUILD/glibc-2.3/cc/csu/cr
irst defined here
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
ext+0x0): In function `_start':
../sysdeps/i386/elf/start.S:65: multiple definition of `_start'
/usr/lib/crt1.o(.text+0x0):../sysdeps/i386/elf/start.S:65: first defin
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
BS*+0x806e674): In function `_edata':
: multiple definition of `__bss_start'
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
ext+0x1a0): In function `main':
: multiple definition of `main'
Make/linuxGcc4DPOpt/sonicFoam.o(.text+0x6f0):sonicFoam.C: first define
/usr/bin/ld: Warning: size of symbol `main' changed from 43771 in Make
DPOpt/sonicFoam.o to 9467 in /home/user/skolan/OpenFOAM/OpenFOAM-1.3/l
c4DPOpt/libsetParabolic.so
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
ini+0x0): In function `_fini':
/usr/src/packages/BUILD/glibc-2.3/cc/csu/crti.S:52: multiple definitio
i'
/usr/lib/crti.o(.fini+0x0):/usr/src/packages/BUILD/glibc-2.3/cc/csu/cr
t defined here
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
BS*+0x806e674): In function `_edata':
: multiple definition of `_edata'
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
ext+0x1016a): In function `__i686.get_pc_thunk.bx':
: multiple definition of `__i686.get_pc_thunk.bx'
Make/linuxGcc4DPOpt/sonicFoam.o(.gnu.linkonce.t.__i686.get_pc_thunk.bx
cFoam.C: first defined here
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
ot.plt+0x0): multiple definition of `_GLOBAL_OFFSET_TABLE_'
/usr/lib/crt1.o(.got.plt+0x0):../sysdeps/i386/elf/start.S:65: first de
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
BS*+0x806e714): In function `_end':
: multiple definition of `_end'
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
odata+0x4): multiple definition of `_IO_stdin_used'
/usr/lib/crt1.o(.rodata+0x4):../sysdeps/i386/elf/start.S:71: first def
/home/user/skolan/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPOpt/libsetParab
ata+0x0): In function `__data_start':
: multiple definition of `__data_start'
/usr/lib/crt1.o(.data+0x0):../sysdeps/i386/elf/start.S:65: first defin
collect2: ld returned 1 exit status
make: *** [/home/user/skolan/OpenFOAM/OpenFOAM-1.3/applications/bin/li
pt/sonicFoam] Error 1
newton{skolan,133}%

can some one please help me resolve this.

The setParabolicInlet source c
 

The setParabolicInlet source compiles as a utility (an executable file) [1]. I don't remember recompiling icoFoam when I used this utility. So I doubt that you would need to recompile sonicFoam just to get it to work.

In fact, all this utility does is enter into your 0 directory and open the U file and find the patch you specify as an inlet and change the uniform value to a non-uniform list.

Quoting from the executable:
Usage: setParabolicInlet <root> <case> <boundaryname> <maximum> [-z_noncenter] [-parallel] [-y_noncenter]

Just to be on similar terms, I am referring to the utility written by Bernhard Gschaider.

[1] ~/OpenFOAM/openfoam-1.2/applications/bin/linuxAMD64Gcc4Opt/setParabolicInlet

now i have changed my files an
 

now i have changed my files and directory names to setParabolicInlet and tried to execute as follows...i didn't understand the reason. Can some one plz help me resolve this. Are my arguments correct when i have used setParabolicInlet command.


I am working on backwardFacing step flow. I am taking the symmetry of flow as advantage. Hope the code works in that case too. 0.01 is the bulk velocity i want to implement and name of the patch is inlet.


newton{skolan,229}% setParabolicInlet /home/user/skolan/OpenFOAM/skolan-1.3/run/tutorials/sonicFoam backwardStep inlet 0.01 -z_noncenter -parallel -y_noncenter
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.3 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : setParabolicInlet /home/user/skolan/OpenFOAM/skolan-1.3/run/tutorials/sonicFoam backwardStep inlet 0.01 -z_noncenter -parallel -y_noncenter
-----------------------------------------------------------------------------

It seems that there is no lamd running on the host newton.

This indicates that the LAM/MPI runtime environment is not operating.
The LAM/MPI runtime environment is necessary for MPI programs to run
(the MPI program tired to invoke the "MPI_Init" function).

Please run the "lamboot" command the start the LAM/MPI runtime
environment. See the LAM/MPI documentation for how to invoke
"lamboot" across multiple machines.
-----------------------------------------------------------------------

Are you running your case in p
 

Are you running your case in parallel? I think so. Try using the utility in serial mode and see if it works, then you know for sure this is something to do with lam/mpi.

In serial mode, all you need t
 

In serial mode, all you need to give is:

setParabolicInlet /home/user/skolan/OpenFOAM/skolan-1.3/run/tutorials/sonicFoam backwardStep inlet 0.01

I am not running in parallel.
 

I am not running in parallel. I just logged off and logged in and its working now. I have some basic question. What should be my outlet(type & conditions) so that the flow at the outlet is fully developed

my boundary file is......

6
(
inlet
{
type wall;
physicalType fixedTemperatureWall;
nFaces 50;
startFace 64600;
}

outlet
{
type patch;
physicalType pressureOutlet;
nFaces 150;
startFace 64650;
}

bottom
{
type wall;
physicalType fixedTemperatureWall;
nFaces 200;
startFace 64800;
}
top
{
type symmetryPlane;
physicalType symmetryPlane;
nFaces 250;
startFace 65000;
}

obstacle
{
type patch;
physicalType adiabaticWall;
nFaces 150;
startFace 65250;
}

defaultFaces
{
type empty;
nFaces 65000;
startFace 65400;
}
)

I am working on a backwardFacingStep flow taking symmetry on top face and with constant temp(1000 K) of bottom face and inflow fluid with constant temp(300 K). streamlines i have plotted are not matching at the outlet. Can someone please help me out

I need some suggestions so tha
 

I need some suggestions so that i can have fully developed flow at the outlet

I have a problem with paraboli
 

I have a problem with parabolic inlet because my origin is at the edge of step, i mean my origin is not in the center of parabola but at the bottom of parabola. It gave the above half of the parabola whereas i need lower half of the parabola. Can you please suggest me something as soon as possible

If you're still referring to m
 

If you're still referring to my setParabolic.C, commenting out the line

offY -= lenY;

(or the equivalent line with z's) should do the trick. (A bit recompiling might be in order)

Hej, For my project I desid
 

Hej,

For my project I desided to use the icoFoam case, but I need to
specify velocity inlet (it should be parabolic). Could u give me some
hint how I can do it?

Thank u,
Rita

Hej, For my project I desid
 

Hej,

For my project I desided to use the icoFoam case, but I need to
specify velocity inlet (it should be parabolic). Could u give me some
hint how I can do it?

Thank u,
Rita

See Bernhard's responses above
 

See Bernhard's responses above. I used his utility without any problems for 2D cases. Haven't tried for 3D yet; but I guess there should be no problems.

Quoting from Bernhard:

Place the source in a directory. Create a directory called 'Make' in it in which you create a file named 'options' with this content

EXE_INC = \
-I$(LIB_SRC)/cfdTools/lnInclude \
-I$(LIB_SRC)/finiteVolume/lnInclude

EXE_LIBS = -lfiniteVolume

and a file called 'files' with this content

setParabolicInlet.C
EXE = $(FOAM_USER_APPBIN)/setParabolicInlet

After a wmake the executable is in your path and you can start using it.

BTW: you'll also need a creatFields.H:

Info<< "Vector field U\n" << endl;
volVectorField U
(
IOobject
(
"U",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);

Thank u very much, I will try
 

Thank u very much, I will try it.

Rita

Hej, Sorry maybe it is a no
 

Hej,

Sorry maybe it is a not good question about the parabolic inlet...But could u give me some hint where I should put exatly the setParabolicInlet.C Should I put it in the OpenFOAM/OpenFOAM-1.3/applications/solvers/incompressible/icoFoam or where? I am asking because as I understood that the way is very important in OpenFOAM.

Thank u,
Rita

Not very critical to put it in
 

Not very critical to put it in a particular place. However, an organized arrangement always helps. I have mine put in a separate directory:

[username@hostname parabolic_velocity_inlet]$ pwd
/home/username/OpenFOAM/username-1.3/custom_utils/Bernhard_Gschaider/parabolic_v elocity_inlet
[username@hostname parabolic_velocity_inlet]$ ls -la
total 84K
drwxr-xr-x 3 username users 4.0K Nov 15 21:12 .
drwxr-xr-x 3 username users 4.0K Nov 14 16:58 ..
-rw-r--r-- 1 username users 156 Nov 14 16:58 createFields.H
drwxr-xr-x 3 username users 4.0K Nov 15 21:12 Make
-rw-r--r-- 1 username users 7.2K Nov 14 16:58 setParabolicInlet.C
-rw-r--r-- 1 username users 33K Nov 15 21:12 setParabolicInlet.dep
[username@hostname parabolic_velocity_inlet]$

I can't find the solution prop
 

I can't find the solution proposed by Hrvoje. Can someone post it here?

Regards,
Alberto

Attached. http://www.cfd-o
 

Attached.

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif parabolicVelocity_HJ_17Jan2007.tgz

Enjoy,

Hrv

Thanks! Alberto
 

Thanks!

Alberto

Hej pUl|, Thank you very
 

Hej pUl|,

Thank you very much for advice. Now my ParabolicInlet is working
fine.


I created my own folder:
"OpenFOAM/margst-1.3/applications/solvers/Parabolic_velocity_inlet"
and compiled all files there.

The problem with this is that I can "see" my new case only within
OpenFOAM shell and ,for some reason, I can look at the results withy
Paraview.


For example, i create the class:

Case : IcoFoam,
Case root : OpenFOAM/margst-1.3/applications/solvers/Parabolic_velocity_inlet
Case name: test

But as soon as I close OpenFOAM, the case disappears for good from
the case brauser. How can one "save" the case? Plus, how can one use
ParaView for my newly created class?



Best regards,
Rita

Hej I want to create a lin
 

Hej

I want to create a linear profile of Temperature Boundary condition on
the one of the vertical walls. Before I was adding it
as a vector, but if I want to refine my mesh I have to change my vector
manualy.

Could you give me a hint what I should add to the file ParabolicInlet.C to
have both conditions (parabolic Inlet for velocity and linear profile for
temperature).

Thank you in advance,
Rita

Hi Bernhard, stupid questio
 

Hi Bernhard,

stupid question:

I would like to modify my boundary conditions by using your code. Everything works fine, but instead of a list with the data. Simply the maximum value of the velocity is responded in my boundary

So

Inlet
{
type fixedValue;
value uniform (0 0 0);
}
results in

Inlet
{
type fixedValue;
value uniform (1 0 0);
}

if my maximum velocity is 1. Any Idea????

Thanks Bummi

Hi Bummi! You refering to m
 

Hi Bummi!

You refering to my posting from April 26, 2006, are you? That code makes an assumption about the orientation of the patch: that it is parallel to the y-z-plane. Most propably your patch is parallel to xz or xy. Then the result should be the way you described it.
You'll have to modify the code to fit your geometry or rotate the geometry. Or write a more general utility.

regards
Bernhard

Hi Bernhard, I'll try this!
 

Hi Bernhard,

I'll try this! Thank you very much, especially for the fast response!!

regards

Bummi

Hi Bernhard again, the dire
 

Hi Bernhard again,

the direction was not the problem. It was correct, but I added some other parts to your code for modifying the inlet concentration and those caused the problem. By deleting them everything works.

Stupid me.

Regard

Bummi

Hi Hvr, Could you re-post you
 

Hi Hvr,
Could you re-post your "parabolicVelocity_HJ_17Jan2007.tgz", please ?
I could not download it !
Thank you very much!
Phuc-Danh

The archive is good, I've just
 

The archive is good, I've just tried it.
Be careful when you download it to change its name from something like parabolicVelocity_HJ_17Jan2007-3679.unk to parabolicVelocity_HJ_17Jan2007.tgz

Dragos

Hi Hvr, Sorry, I can download
 

Hi Hvr,
Sorry, I can download it now.
Thank you very much!
Phuc-Danh

Hi Dragos, Thanks for your ad
 

Hi Dragos,
Thanks for your additional precision !
Phuc-Danh

Dragos, Once you download th
 

Dragos,
Once you download the files, where do you have to
put them?
In:
~/OpenFOAM/OpenFOAM-1.3/src/finiteVolume/
fields/fvPatchFields/derivedFvPatchFields/

and

/home/radu/OpenFOAM/OpenFOAM-1.3/src/
finiteVolume/lnInclude/
???
What next? Do you have an example of U in one of the 0´s with the correct syntax?
Thanks,
Radu

Hi to everyone, I'm trying
 

Hi to everyone,

I'm trying to implement a parabolic profile in an inlet for reactingFoam, since I want to study an open flame and literature suggest to have such a developed profile before entering the crossflow plane. So, I'm trying two options: to compile the Bernhard's "SetParabolicInlet.C" and that of Dr. Jasak "ParabolicVelocity" under OF-1.4.1.

In the first one i get an error message concerning to fvPatchFieldFields.H. this is the message:

Making dependency list for source file parabolic.C
could not open file fvPatchFieldFields.H for source file parabolic.C
SOURCE=parabolic.C ; g++ -m32 -Dlinux -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-40 -I/home/foam-1.4.1/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude -I/home/foam-1.4.1/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude -IlnInclude -I. -I/home/foam-1.4.1/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude -fPIC -pthread -c $SOURCE -o Make/linuxGccDPOpt/parabolic.o
parabolic.C:36:32: error: fvPatchFieldFields.H: No such file or directory
parabolic.C: In function 'int main(int, char**)':
parabolic.C:74: error: 'fvPatchVectorFieldField' was not declared in this scope
parabolic.C:74: error: 'Upatches' was not declared in this scope
make: *** [Make/linuxGccDPOpt/parabolic.o] Error 1

I looked for this file but didn't find it. I'm not sure if it is not anymore in OF-1.4.1, since I compiled it well under OF-1.3.

With respect to the one of Dr. Jasak, I modified the line he suggests (Alberto Passalacqua's post):

const vectorField& c = patch().Cf();

but I don't know if i have to compile as the one of bernhard's: create a Make, add file and options files.

I also tried to find the message Dr. Jasak refers to concerning a previous long message about compiling and linking new libraries (February 13 2007 answering to Thomas Jung) but i don't find it.

Please, I would thank so much if someone can give me a hint of how to proceed.

Thanks for reading,

best

V