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

Parabolic inlet velocity profile

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

Like Tree5Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   April 26, 2006, 05:15
Default I did not really want to start
  #1
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 699
Rep Power: 12
msrinath80 is on a distinguished road
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

Thanks a lot for your patience!
skuznet likes this.
msrinath80 is offline   Reply With Quote

Old   April 26, 2006, 13:05
Default The parabolic inlet. I read ab
  #2
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
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).

setParabolicInlet.C
jferrari, pedroxramos and jiaojiao like this.
__________________
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   April 26, 2006, 14:44
Default Hi, I did one of those a while
  #3
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   April 26, 2006, 17:15
Default Bernhard: Many thanks for your
  #4
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 699
Rep Power: 12
msrinath80 is on a distinguished road
Bernhard: Many thanks for your prompt response

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!
msrinath80 is offline   Reply With Quote

Old   April 26, 2006, 18:15
Default Hi p???! (Sorry, can't pronoun
  #5
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
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)
__________________
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   April 26, 2006, 18:46
Default Thanks for the quick response.
  #6
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 699
Rep Power: 12
msrinath80 is on a distinguished road
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);
msrinath80 is offline   Reply With Quote

Old   April 27, 2006, 08:17
Default No. The test (zmax-zmin)==0 ma
  #7
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
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)
__________________
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 7, 2006, 00:38
Default Hi Bernhard, I tried your i
  #8
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 699
Rep Power: 12
msrinath80 is on a distinguished road
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?
msrinath80 is offline   Reply With Quote

Old   May 8, 2006, 04:23
Default The finiteVolume stuff is 1.3-
  #9
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
The finiteVolume stuff is 1.3-specific. Replace the -lfiniteVolume with -lcfdTools
__________________
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 8, 2006, 04:35
Default It works now. Thank you!
  #10
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 699
Rep Power: 12
msrinath80 is on a distinguished road
It works now. Thank you!
msrinath80 is offline   Reply With Quote

Old   July 20, 2006, 10:16
Default hello OpenFoam users, I am
  #11
New Member
 
Sreekanth Kolan
Join Date: Mar 2009
Posts: 13
Rep Power: 8
sreekanth is on a distinguished road
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.
sreekanth is offline   Reply With Quote

Old   July 20, 2006, 18:00
Default The setParabolicInlet source c
  #12
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 699
Rep Power: 12
msrinath80 is on a distinguished road
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
msrinath80 is offline   Reply With Quote

Old   July 21, 2006, 10:13
Default now i have changed my files an
  #13
New Member
 
Sreekanth Kolan
Join Date: Mar 2009
Posts: 13
Rep Power: 8
sreekanth is on a distinguished road
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.
-----------------------------------------------------------------------
sreekanth is offline   Reply With Quote

Old   July 21, 2006, 10:32
Default Are you running your case in p
  #14
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 699
Rep Power: 12
msrinath80 is on a distinguished road
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.
msrinath80 is offline   Reply With Quote

Old   July 21, 2006, 15:17
Default In serial mode, all you need t
  #15
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 699
Rep Power: 12
msrinath80 is on a distinguished road
In serial mode, all you need to give is:

setParabolicInlet /home/user/skolan/OpenFOAM/skolan-1.3/run/tutorials/sonicFoam backwardStep inlet 0.01
msrinath80 is offline   Reply With Quote

Old   July 22, 2006, 03:40
Default I am not running in parallel.
  #16
New Member
 
Sreekanth Kolan
Join Date: Mar 2009
Posts: 13
Rep Power: 8
sreekanth is on a distinguished road
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
sreekanth is offline   Reply With Quote

Old   July 22, 2006, 03:55
Default I need some suggestions so tha
  #17
New Member
 
Sreekanth Kolan
Join Date: Mar 2009
Posts: 13
Rep Power: 8
sreekanth is on a distinguished road
I need some suggestions so that i can have fully developed flow at the outlet
sreekanth is offline   Reply With Quote

Old   July 23, 2006, 03:40
Default I have a problem with paraboli
  #18
New Member
 
Sreekanth Kolan
Join Date: Mar 2009
Posts: 13
Rep Power: 8
sreekanth is on a distinguished road
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
sreekanth is offline   Reply With Quote

Old   July 23, 2006, 14:28
Default If you're still referring to m
  #19
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
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)
__________________
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   December 14, 2006, 08:45
Default Hej, For my project I desid
  #20
mss
Guest
 
Posts: n/a
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
  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
2D air parabolic velocity profile ilker FLUENT 2 November 12, 2008 09:43
UDF Unsteady velocity parabolic profile Rashad FLUENT 2 February 29, 2008 03:36
parabolic velocity profile? bssdyl FLUENT 4 March 22, 2006 12:32
problem in 3d parabolic velocity profile Lokesh FLUENT 8 August 11, 2005 05:36
Parabolic temperature Inlet Profile in a tube majestywzh FLUENT 0 April 9, 2003 06:37


All times are GMT -4. The time now is 21:10.