tutorial

tutorial
How To extrude 2D mesh into 3D in Calculix – pipe mesh example
Tutorial – CalculiX meshing for OpenFOAM: pipe mesh
Previous steps:
The 2D mesh was created in Blender with the use of the fbd export script. The generation of
the 2D mesh itself is the subject of an other Tutorial document.
Starting up and opening the 2D mesh:
Start up CalculiX:
cgx ­b cylinder3.fbd
The next step is to swep the 2D mesh in 3D among a strait line. Let's call the other end of the
pipe “top”. All the entities (points, lines, surfaces imported) are stored in the “all” selection at
the beginning. We will use a translation vector of [0,0,18] – z direction:
swep all top tra 0 0 18
1
Tutorial – CalculiX meshing for OpenFOAM: pipe mesh
Check what is the default division for the lines. We would like to use hexahedron cells, all the
2
Tutorial – CalculiX meshing for OpenFOAM: pipe mesh
lines will be divided due to its division definition. The division definition can be visulaized for
example for all the lines in the model:
plot ld all
Note that the new lines – the ones parallel to the z axis - have 4 as division! Change the
division of these lines!
Switch the “+x” view:
3
Tutorial – CalculiX meshing for OpenFOAM: pipe mesh
Now change the division:
qdiv
Selection mode “all”:
a
Define the opposite corners of the selection rectangle:
r
r
4
Tutorial – CalculiX meshing for OpenFOAM: pipe mesh
Hit “r”!
Hit “r”!
Type in the new division definition (for two digit definitions type a <SPACE> before the
numbers!):
99
Quit the division definition command:
q
Now define the cell type which the mesher should use as hexahedrons
elty all he8
Start meshing:
mesh all
The reply is the following:
please wait for 'ready' 5
Tutorial – CalculiX meshing for OpenFOAM: pipe mesh
numFaces:456192 numElems:76032 size:32845824 ready Visualize the newly created elements:
plot e all
Toggle on “Element Edges”:
6
Tutorial – CalculiX meshing for OpenFOAM: pipe mesh
Switch visualization for element face visualization for smaller memory usage:
plot f all
Now create selections for inlet, outlet and wall. To do the selection the first letter of the
element name should be typed in – p for points, l for lines, s for surfaces, etc.. For the
boundary conditions element faces should be selected (f). Let's begin with the inlet boundary
(“in”):
qadd in
a
r
r
f
q
7
Tutorial – CalculiX meshing for OpenFOAM: pipe mesh
Check what was selected (with green color):
plot f all
plus f in g
8
Tutorial – CalculiX meshing for OpenFOAM: pipe mesh
Remove non necessary faces from selection:
qrem in
a
r
r
f
q
Create the outlet (“out”) and wall (“wall”) selections on the similar way. Visulizing the result “in” with green, “out” with red and “wall” with blue:
plot f all
plus f in g
plus f out r
plus f wall b
9
Tutorial – CalculiX meshing for OpenFOAM: pipe mesh
Check what selections are existing with what content:
prnt se
The reply is the following:
1 all stat:o n:80100 e:76032 f:7872 p:1602 l:3937 s:3104 b:768 L:0 S:0 se:0 2 top stat:c n:801 e:0 f:768 p:801 l:1568 s:768 b:0 L:0 S:0 se:0 3 in stat:c n:0 e:0 f:768 p:0 l:0 s:0 b:0 L:0 S:0 se:0 4 ­NJBY stat:c n:0 e:0 f:0 p:0 l:0 s:0 b:0 L:0 S:0 se:0 5 out stat:c n:0 e:0 f:768 p:0 l:0 s:0 b:0 L:0 S:0 se:0 6 wall stat:c n:0 e:0 f:6336 p:0 l:0 s:0 b:0 L:0 S:0 se:0 Export mesh in OpenFOAM format with the existing face selections (“in” - patch type, “out” patch type and “wall” - wall type):
send all foam patch in patch out wall wall
Reply:
please wait for 'ready' use boundary: type:patch set:in use boundary: type:patch set:out use boundary: type:wall set:wall 10
Tutorial – CalculiX meshing for OpenFOAM: pipe mesh
wrote foam mesh ready The mesh is ready to be used in OpenFOAM now! You can quit CalculiX:
quit
11