|
[Sponsors] |
May 13, 2011, 11:39 |
Meshing a pipe
|
#1 |
New Member
Mike
Join Date: May 2011
Posts: 19
Rep Power: 14 |
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! |
|
May 13, 2011, 15:29 |
|
#2 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 555
Rep Power: 27 |
Hello
Take a look here. http://www.salome-platform.org/user-...edf-exercise-4 That should solve your question.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
May 13, 2011, 16:59 |
|
#3 |
New Member
Mike
Join Date: May 2011
Posts: 19
Rep Power: 14 |
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 |
|
May 14, 2011, 01:49 |
|
#4 |
Senior Member
|
Hi,
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 http://www.caelinux.org/wiki/index.p...ELinux_2007.29 |
|
May 14, 2011, 03:31 |
|
#5 |
Member
Bjorn H. Hjertager
Join Date: Mar 2009
Posts: 72
Rep Power: 17 |
||
May 15, 2011, 11:24 |
|
#6 |
Member
Stephen
Join Date: Mar 2009
Posts: 40
Rep Power: 17 |
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 ideasUnvToFoam name.unv checkMesh Run case ( icoFoam etc) foamToVTK ParaView ..... 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 Stephen |
|
May 15, 2011, 12:40 |
one more step
|
#7 |
Senior Member
Wouter van der Meer
Join Date: May 2009
Location: Elahuizen, Netherlands
Posts: 203
Rep Power: 17 |
hello All,
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 Wouter |
|
May 15, 2011, 12:57 |
|
#8 |
Member
Logan Page
Join Date: Sep 2010
Posts: 38
Rep Power: 15 |
Hi
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. |
|
March 1, 2012, 10:47 |
Drawing a Pipe problem
|
#9 |
Senior Member
Goutam Saha
Join Date: Dec 2011
Location: UK
Posts: 131
Rep Power: 14 |
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? |
|
March 2, 2012, 03:12 |
|
#10 | |
Senior Member
Roman Thiele
Join Date: Aug 2009
Location: Eindhoven, NL
Posts: 374
Rep Power: 20 |
Quote:
I still had a mesh with double grading in my repository somewhere. It is attached. I hope it helps.
__________________
~roman |
||
March 4, 2012, 14:03 |
|
#11 | |
Senior Member
Goutam Saha
Join Date: Dec 2011
Location: UK
Posts: 131
Rep Power: 14 |
Quote:
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. |
||
March 5, 2012, 01:49 |
|
#12 | |
Senior Member
Roman Thiele
Join Date: Aug 2009
Location: Eindhoven, NL
Posts: 374
Rep Power: 20 |
Quote:
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 Code:
paraFoam -block
__________________
~roman |
||
March 5, 2012, 11:54 |
|
#13 |
Senior Member
Goutam Saha
Join Date: Dec 2011
Location: UK
Posts: 131
Rep Power: 14 |
Dear Romant,
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. |
|
March 5, 2012, 11:57 |
|
#14 | |
Senior Member
Roman Thiele
Join Date: Aug 2009
Location: Eindhoven, NL
Posts: 374
Rep Power: 20 |
Quote:
__________________
~roman |
||
March 7, 2012, 06:56 |
|
#15 | |
Senior Member
Goutam Saha
Join Date: Dec 2011
Location: UK
Posts: 131
Rep Power: 14 |
Quote:
I understood the blockMesh file clearly. When I use checkMesh command: Create polyMesh for time = 0 Time = 0 Mesh stats points: 136161 faces: 400100 internal faces: 391900 cells: 132000 boundary patches: 3 point zones: 0 face zones: 0 cell zones: 1 Overall number of cells of each type: hexahedra: 132000 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 Checking topology... 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) Checking geometry... 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. End What I will do now? Do I ignore this and continue my work? Last edited by Goutam; March 7, 2012 at 07:15. |
||
March 8, 2012, 03:12 |
|
#16 | |
Senior Member
Roman Thiele
Join Date: Aug 2009
Location: Eindhoven, NL
Posts: 374
Rep Power: 20 |
Quote:
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. Code:
// define the pipe geometry // ----SIZING------------------------------------------------------------------- // all measurement must be given in [mm] lengthZ 180; // ----MESHING------------------------------------------------------------------ radialCells 80; // cells in the radial direction from center piller tangentialCells 7; // angular cell counter per quarter and square of central piller verticalCells 40; // vertical cell count from inlet to outlet meshGrad 1.25e-2; // mesh gradient towards the outer edge and outer edge of the piller
__________________
~roman |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[GAMBIT] meshing in GAMBIT, a flow through a pipe having complex inflow geometry | mazhar1613 | ANSYS Meshing & Geometry | 1 | January 11, 2012 23:18 |
[GAMBIT] Meshing a pipe | vedravi | ANSYS Meshing & Geometry | 1 | March 25, 2010 13:19 |
Meshing divergent nozzle entry of a long pipe | Aly | FLUENT | 1 | September 25, 2005 17:07 |
+ shape circular pipe - meshing possible? | Selina Tracy | Main CFD Forum | 2 | January 16, 2003 13:31 |
Terrible Mistake In Fluid Dynamics History | Abhi | Main CFD Forum | 12 | July 8, 2002 09:11 |