# Parabolic inlet velocity profile

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

 April 26, 2006, 05:15 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: 703 Rep Power: 13 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.

 April 26, 2006, 13:05 The parabolic inlet. I read ab #2 Assistant Moderator   Bernhard Gschaider Join Date: Mar 2009 Posts: 3,931 Rep Power: 41 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

 April 26, 2006, 14:44 Hi, I did one of those a while #3 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,783 Rep Power: 22 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

 April 26, 2006, 17:15 Bernhard: Many thanks for your #4 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 13 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!

 April 26, 2006, 18:15 Hi p???! (Sorry, can't pronoun #5 Assistant Moderator   Bernhard Gschaider Join Date: Mar 2009 Posts: 3,931 Rep Power: 41 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

 April 26, 2006, 18:46 Thanks for the quick response. #6 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 13 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);

 April 27, 2006, 08:17 No. The test (zmax-zmin)==0 ma #7 Assistant Moderator   Bernhard Gschaider Join Date: Mar 2009 Posts: 3,931 Rep Power: 41 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

 May 7, 2006, 00:38 Hi Bernhard, I tried your i #8 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 13 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?

 May 8, 2006, 04:23 The finiteVolume stuff is 1.3- #9 Assistant Moderator   Bernhard Gschaider Join Date: Mar 2009 Posts: 3,931 Rep Power: 41 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

 May 8, 2006, 04:35 It works now. Thank you! #10 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 13 It works now. Thank you!

 July 20, 2006, 10:16 hello OpenFoam users, I am #11 New Member   Sreekanth Kolan Join Date: Mar 2009 Posts: 13 Rep Power: 9 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.

 July 20, 2006, 18:00 The setParabolicInlet source c #12 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 13 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 [-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

 July 21, 2006, 10:13 now i have changed my files an #13 New Member   Sreekanth Kolan Join Date: Mar 2009 Posts: 13 Rep Power: 9 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. -----------------------------------------------------------------------

 July 21, 2006, 10:32 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: 703 Rep Power: 13 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.

 July 21, 2006, 15:17 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: 703 Rep Power: 13 In serial mode, all you need to give is: setParabolicInlet /home/user/skolan/OpenFOAM/skolan-1.3/run/tutorials/sonicFoam backwardStep inlet 0.01

 July 22, 2006, 03:40 I am not running in parallel. #16 New Member   Sreekanth Kolan Join Date: Mar 2009 Posts: 13 Rep Power: 9 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

 July 22, 2006, 03:55 I need some suggestions so tha #17 New Member   Sreekanth Kolan Join Date: Mar 2009 Posts: 13 Rep Power: 9 I need some suggestions so that i can have fully developed flow at the outlet

 July 23, 2006, 03:40 I have a problem with paraboli #18 New Member   Sreekanth Kolan Join Date: Mar 2009 Posts: 13 Rep Power: 9 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

 July 23, 2006, 14:28 If you're still referring to m #19 Assistant Moderator   Bernhard Gschaider Join Date: Mar 2009 Posts: 3,931 Rep Power: 41 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

 December 14, 2006, 08:45 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post ilker FLUENT 2 November 12, 2008 09:43 Rashad FLUENT 2 February 29, 2008 03:36 bssdyl FLUENT 4 March 22, 2006 12:32 Lokesh FLUENT 8 August 11, 2005 05:36 majestywzh FLUENT 0 April 9, 2003 06:37

All times are GMT -4. The time now is 16:58.