Meshing a pipe
Hello. I am trying to simulate the flow in a heat exchanger like the one that you can see here: https://docs.google.com/viewer?a=v&p...thkey=CNSL76UH
The problem is that i don't know how to create the corresponding mesh. I was trying to do that with the blockMesh tool but it's too complicated and I always get errors :(
If anybody has dealt with a problem like that, I would appreciate some advice!
Take a look here.
That should solve your question.
Well, salome is a program with gui, and tools that help you generate mesh automatically, while OenFoam uses geometry blocks. Is there a way I can import the geometry and
its corresponding mesh in openFoam, having created them in another program? Otherwise, i dont't understand how this tutorial would help me :S
ideasUnvToFoam will do the job for you.
have a look at http://www.caelinux.org/wiki/downloa...7/PipeMesh.htm video meshing with salome 3.2.6 and foamX is not in OF anymore ;-), it is a good start
syntax for ideasUnvToFoam little different today to what video shows
Discretizer migth be an option for you, see http://www.discretizer.org/
Just done the same thing, a nice fella called Martin helped
My work flow was:.... draw a solid pipe in CAD
export as STEP
import to salome and set up faces and mesh etc ( caelinux has a tutorial called pipe)
export to UNV
then in the openFOAM terminal
cd to your case directory
Run case ( icoFoam etc)
my problem was with the courant number ( time) and a tweak to the FVsolutions card )
Least that worked for me
I use CAElinux 64 bit ubuntu based
Hope this was of some help
one more step
I use salome for the complete drawing and meshing. In my experience you need a step before running the case namely edit the boundary conditions
I mostly need to change patch to wall, for the wall patches.
Hope this adds something
I'm partial to gmsh. Very powerful little mesher.
see attached example for a pipe.
> gmsh -3 Pipe.geo
> gmshToFoam Pipe.msh
only down side is you have to manually edit the constant/polyMesh/boundary file with the patch types you assign for you boundary conditions.
Drawing a Pipe problem
I am new user of openFOAM.
I want to draw a pipe of length of 1 meter with diameter 1 meter using blockMesh. How I will do it? Could you please share a blockMeshDict file?
I still had a mesh with double grading in my repository somewhere. It is attached. I hope it helps.
I saw this geometry. Its great. But I didn't understand how you wrote the blockMesh file. Could you please explain me, how you wrote this?
First of all, you wrote 8 points, it means length of x and y is 0.02 m respectively, and length of z is 0.18 m. Am I right?
Then next 8 points, what you did?
I am considering a simple pipe of 10 m with radius 1 m for inlet and outlet. Your one is ok for me but I want to understand the basic of the blockMesh file that you created.
Thanks for your help.
If you take a look at the blocks part you can see that I desribe which parts I create in which ordere, where the point numbers correspond to the numbers in the vertices section.
At first a normal block is created in the center, and then block that sit around this one. The outer block have edged which are defined as arcs instead of straight lines, so that they create a round x-y plane.
if you run
Thanks for your details description.
I have another ques: How to calculate the points for arc boundary?
arc 8 9 (diagouter diagouter 0)
how you calculate that point?
You define diagOuter 21.213, diagOuterNeg -21.213. How?
I understood others settings.
Thanks again for your time.
I understood the blockMesh file clearly. When I use checkMesh command:
Create polyMesh for time = 0
Time = 0
internal faces: 391900
boundary patches: 3
point zones: 0
face zones: 0
cell zones: 1
Overall number of cells of each type:
tet wedges: 0
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).
Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
Walls 1600 1640 ok (non-closed singly connected)
inlet 3300 3321 ok (non-closed singly connected)
outlet 3300 3321 ok (non-closed singly connected)
Overall domain bounding box (-0.02595 -0.02595 0) (0.02595 0.02595 1.2)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (-1.86565e-16 8.61985e-18 -7.27923e-17) OK.
***High aspect ratio cells found, Max aspect ratio: 4095.21, number of cells 33280
<<Writing 33280 cells with high aspect ratio to set highAspectRatioCells
Minumum face area = 2.9739e-08. Maximum face area = 0.000122163. Face area magnitudes OK.
Min volume = 8.92169e-10. Max volume = 1.52642e-07. Total volume = 0.00252834. Cell volumes OK.
Mesh non-orthogonality Max: 34.8018 average: 4.32731
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 2.33588 OK.
Coupled point location match (average 0) OK.
Failed 1 mesh checks.
What I will do now? Do I ignore this and continue my work?
You can get rid of these high aspect ratios by checking where they occur. Use paraFoam for this and enable to see sets, which will then give you the option to view this set of high aspect ratio cells. After identifying the cells, change the number of cells in the directions. For this check the file pipeDefinition.
|All times are GMT -4. The time now is 08:11.|