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

Hooking new BC is not successful

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 5, 2008, 09:29
Default Hello to FOAMing user, I am w
  #1
New Member
 
David Sponiar
Join Date: Mar 2009
Location: Prague, Czech rep.
Posts: 27
Rep Power: 9
sponiar is on a distinguished road
Hello to FOAMing user,
I am working very hard on to implement new BC. My situation is quite strange:
While I am compiling new BC I follow this 3 basic steps:
____________

• compile new BC, which create new library
• compile foamUser, which called new BC's library
• compile little bit modified simpleFoam, which called updated foamUser's library
____________

Every steps are finished successfuly, it means: new dynamic library are update and modified simpleFoam is compiled without any errors.

When I run application simpleFoam with case, where is new BC defined on outlet, FOAM FATAL ERROR says to me:
"Unknown patchField type modifiedOutlet for patch type patch"

The strange thing is to me, when I follow same compiling steps on another PC (notebook with OpenSuSE 10.3.) with same source codes, I can successfuly hook new BC.

I was looking for any mistake for two days. I did not find anything weird. So I packed whole OpenFOAM directory on notebook and copy and unpacked on worskation with SuSE Linux Enterprise Desktop 10.0.
foamInstalationTest is after that OK. Every is OK, but after 3 compiling steps, new BC is unknown.

Give me please any hint, where could be any mistake. Thans a lot.
David

I attach list of Make/files and Make/options from new BC, foamuser and modified simpleFoam:

__________________________

• new BC Make/files
modifiedOutlet.C
LIB = $(FOAM_LIBBIN)/libNewBC

• new BC Make/options
EXE_INC = \
-I$(LIB_SRC)/finiteVolume/lnInclude

LIB_LIBS = \
-lfiniteVolume

__________________________


• foamUser Make/files
libfoamUser.C
LIB = $(FOAM_USER_LIBBIN)/libfoamUser

• foamUser Make/options
LIB_LIBS = \
-lNewBC

__________________________


• simpleFaom Make/files
simpleFoamModified.C

EXE = $(FOAM_USER_APPBIN)/simpleFoamModified

• simpleFaom Make/options
EXE_INC = \
-I$(LIB_SRC)/finiteVolume/lnInclude \
-I$(LIB_SRC)/turbulenceModels \
-I$(LIB_SRC)/transportModels \
-I$(FOAM_USER_LIBBIN)

EXE_LIBS = \
-lincompressibleTurbulenceModels \
-lincompressibleTransportModels \
-lfiniteVolume \
-lmeshTools

LIB_LIBS = \
-lfoamUser
sponiar is offline   Reply With Quote

Old   March 5, 2008, 14:55
Default David, to answer your quest
  #2
kar
Senior Member
 
Kārlis Repsons
Join Date: Mar 2009
Location: Latvia
Posts: 111
Rep Power: 9
kar is on a distinguished road
David,

to answer your question it is necessary that you post in relevant BCs in /0/{U,p,...} and beginning of BC class definition (if you didn't wrote it from scratch, that is - if you modified some OF's class)!

Kārlis
kar is offline   Reply With Quote

Old   March 6, 2008, 18:21
Default David, some ideas for you:
  #3
kar
Senior Member
 
Kārlis Repsons
Join Date: Mar 2009
Location: Latvia
Posts: 111
Rep Power: 9
kar is on a distinguished road
David,
some ideas for you:

* what happens if you compile your BCs in solver? (I agree it's better to make a libraries, but maybe you can try that - just add *.C files to Make/files)

* be sure to access solver variables in a right way (take a look at buoyantFoam's BCs, parabolic U inlet etc)

* Its not likely to be the case for problem you stated, but it's not a very good idea to use in code things you don't know about.

Kārlis
kar is offline   Reply With Quote

Old   March 6, 2008, 20:00
Default Hello Kārlis, It's kind of y
  #4
New Member
 
David Sponiar
Join Date: Mar 2009
Location: Prague, Czech rep.
Posts: 27
Rep Power: 9
sponiar is on a distinguished road
Hello Kārlis,
It's kind of you, that you are responding to my problem with implementing new BC. I'll promise to share my progres in "fighting with my implementation new BC and self-conquest".


>> what happens if you compile your BCs in solver?


When I compile modified simpleFoam with calling dynamic library (noticed above), every goes right way = compiling is successful and new application simpleFoamModified is created. But hookin new BC type in boundary file /0/q is not successful.



>> be sure to access solver variables in a right way (take a look at buoyantFoam's BCs, parabolic U inlet etc)


Actualy, I copy source code of totalPressure BC, just rename everything in code to modifiedOutletFvPatchScalarField and added new operator with evaluating mathematical operations with normal gradients. (Of course with regards to corect programing standard in C++ and OpenFOAM philosophy).
Strange thing is to me, that same code in same OpenFOAM, but on another PC was compilied and implemented succesfull.

I'll check my steps and share my more or less satisfactory progres.

David
sponiar is offline   Reply With Quote

Old   March 7, 2008, 07:31
Default The easiest way of exposing ex
  #5
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 13
eugene is on a distinguished road
The easiest way of exposing existing solvers and utilities to new boundary conditions is to add an entry like this to your controlDict:

libs ("<path>/<library>");

Much easier than recompiling and copying stuff around.
eugene is offline   Reply With Quote

Old   March 7, 2008, 09:05
Default Hello foaming users, I find t
  #6
New Member
 
David Sponiar
Join Date: Mar 2009
Location: Prague, Czech rep.
Posts: 27
Rep Power: 9
sponiar is on a distinguished road
Hello foaming users,
I find the right way: After lot of testing combination, I added this line:
libs ("libfinite.so");
to /system/controlDict and simpleFoam goes smoothly without any FOAM FATAL ERROR.

That's the way!
David
sponiar 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
Successful Installation My report quartzian OpenFOAM Installation 2 April 30, 2009 03:59
Successful PhD grtabor OpenFOAM Running, Solving & CFD 2 February 24, 2009 05:08
Problem FoamXHostBrowser not found after successful compilation david_flo1 OpenFOAM 0 January 21, 2008 23:04
UDF Hooking Bhaskar Roy FLUENT 1 April 20, 2006 01:50
Hooking Problem bowling FLUENT 0 April 30, 2004 04:38


All times are GMT -4. The time now is 18:23.