View source for HowTo Adding a new boundary condition

First look at [[contrib_groovyBC|groovyBC]].  If this isn't suitable, follow these steps below.

# Choose a boundary condition that is close to the one you want - we'll call it <tt>originalFvPatchField</tt>.
# Copy the directory contents to anywhere (say <tt>run/myCode</tt>).
# Rename all the copied files to a new name (say <tt>customFvPatchField</tt>). <bash>for i in `ls`; do mv $i `echo $i|sed s/originalFvPatchField/customFvPatchField/g`;done</bash>
# Search & replace all text in all the new files old name for new name (<tt>originalFvPatchField</tt> replaced with <tt>customFvPatchField</tt>) <bash> for i in `ls`; do sed -i s/originalFvPatchField/customFvPatchField/g $i;done</bash>
# Modify the code to suit your needs.
# Create the directory structure: <tt>myCode/Make</tt>, and create <tt>files</tt> and <tt>options</tt> in it.
# Put the relevant info into <tt>files</tt>:
## Search for <tt>originalFvPatchField</tt> in <tt>finiteVolume/Make/files</tt>.
## Copy the relevant entry (entries) into your <tt>myCode/Make/files</tt>
## Rename the entries as necessary - rename it with your <tt>customFvPatchField</tt> naming (if there's an <tt>s</tt> on the end, keep it there).
## Tell it what the new library name will be.  Use $(FOAM_USER_LIBBIN) instead of $(FOAM_LIBBIN), and add <tt>lib</tt> to the front of the new name.  It should look something like: <tt>LIB = $(FOAM_USER_LIBBIN)/libcustomPatchField</tt>
# The <tt>options</tt> file should have <tt>EXE_INC</tt> (for any includes such as <tt>-I$(LIB_SRC)/finiteVolume/lnInclude</tt> for finiteVolume) and <tt>LIB_LIBS</tt> (for included libraries, such as <tt>-lfiniteVolume</tt> for finiteVolume). Look at other <tt>LIB_LIBS</tt> for examples.
# <tt>$wmake libso</tt>
# Add whatever new dictionary entries are needed to your initial conditions files, such as <tt>0/U</tt> and <tt>0/P</tt> files.
# Add <tt>libs ( "libcustomFvPatchField.so" "libOpenFOAM.so" )</tt> to <tt>controlDict</tt>
# It should run now.

With reference to [http://www.cfd-online.com/Forums/openfoam/72434-custom-boundary-condition-openfoam.html].
[[User:Marupio|Marupio]] 17:00, 26 February 2010 (UTC)

[[Category:Tutorials]]