Hi I have a problem as shown in the next figure, I allready have the blockMeshDict file for this problem, but I didn't want to use the periodic faces, I want to make a circular array pattern with the domain to generate a cylindrical computational domain. Is there any way to do it?
my blockMeshDict files can be found at this url https://github.com/efirvida/3D-OpenFoam-Wind-Blade
Hello, OpenFoam is not convenient to generate mesh in it. You can use oyher applications as Salome, gridGen ect.
Hi Eduardo,
there are two possibilities:
1) If you really would like to mesh the entire domain you could make several copies of your already existing grid sector and perform a rotation using the command "transformPoints". Afterwards you can repeatedly use the command "mergeMeshes" to add the missing sectors to the growing entire mesh. With the command "stichMesh" cou can combine the neighbouring pathes and thus remove the boundaries of the single sector.
You should make a script since the process will be tedious and won't work at the first time since the openFoam commands usage is not often self-explaining.
2) Maybe it is possible to make use of rotational symmetry using special boundary conditions. You could try e.g. the arbitrary mesh interface to connect the two side faces.
In the description of the arbitrary mesh interface
http://www.openfoam.org/version2.1.0/ami.php
it is suggested to study the tutorial
$FOAM_TUTORIALS/incompressible/simpleFoam/pipeCyclic
for swirled flow in a quater pipe.
Maybe this could be helpful?
Best regards
Bastian
There is no utility to do this job directly (based on my knowledge), but it is possible by using rotateMesh and mergeMeshes utilities.
If you are using a scripting language python to create the blockMesh file, it is more convenient to extend it for the complete geometry. blockMesh is a very good tool and produce excellent meshes do not give up using it.
Best wishes,
Hassan
Hi all Thank for your recomendations.
Ali Tohidi, I arleady tried to make a mirror normal to one face, and works fine for a blade, but not for the third
Hassan I. Kassem, I have also produce this file using pythonscript that I'm developing right now, Im going to try the rotate and merge meshesh to see the result if not, I'll have to redo my script
Bastian Schmandt, I will also try your recommendations, using the combinations of "transformPoints", "mergeMeshes" and "stichMesh"
Madina Tungatarov, I'm using openFOAM directly because im developing a python library to generate a openfoam case for wind tunnel, without using any visual interface for now, I already have builded some openfoam test meshes, I post the url of this test in my question, But thank you very much for your interest, your comment is valid for actual research, I tried the Salome with very good results
Muhammad Faizan-Ur-Rab, thanks for the ICEM recommendation but it is not free, and my purpose is to use only free software
thanl u all again
Finally I did it with this script, thank for your recommendations
========================================================
#!/bin/sh
. $WM_PROJECT_DIR/bin/tools/RunFunctions
orig=$PWD
n=2
declare -A d[$n]
d[0]="(-0.5 0.8660254 0)"
d[1]="(-0.5 -0.8660254 0)"
cd $orig
rm log.*
runApplication blockMesh
for (( i=0; i < $n; i++ ))
do
temp=$(mktemp)-$i
mkdir -p $temp
cp -a $orig/* $temp
cd $temp
runApplication transformPoints -rotate "( (1 0 0) ${d[$i]} )"
runApplication mergeMeshes -overwrite $orig $temp
rm -rf $temp
done
for some versions of openFoam the mergeMesh -overwrite didn’t work so the script will be
========================================================
#!/bin/sh
. $WM_PROJECT_DIR/bin/tools/RunFunctions
orig=$PWD
n=2
declare -A d[$n]
d[0]="(-0.5 0 0.8660254)"
d[1]="(-0.5 0 -0.8660254)"
cd $orig
rm log.*
runApplication blockMesh
runApplication rotateMesh "(1 0 0)" "(-0.5 0.8660254 0)"
for (( i=0; i < $n; i++ ))
do
temp=$HOME/$(mktemp)-$i
mkdir -p $temp
cp -a $orig/* $temp
cd $temp
runApplication transformPoints -rotate "( (1 0 0) ${d[$i]} )"
runApplication mergeMeshes $orig $temp
cp -rf $orig/1/* $orig/constant/
rm -rf $orig/1
rm -rf $temp
done
- Badges
- Science topic
- Similar topics
- Force