|
[Sponsors] |
how to accurately simulate flow around cylinder |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
March 4, 2014, 07:58 |
|
#21 |
Senior Member
|
It seems that you've got diverging solution (at 1.4 s it just blows up). Can you post the output of the solver?
Also I've got several question about your BCs: 1. You set fixed velocity at the outlet and yet you'd like to plot outlet velocity over time. Though you can plot velocity at the inlet boundary. 2. You've got symmetry BC at sides patch, though if you like to simulate flow past ONE cylinder, it should be wall. 3. For some reason you've decided to set symmetry plane also on walls patch (surface of the cylinder), though it again should be wall with non-slip BC. This is just quick look at the case files. What you've described with your initial conditions and boundary conditions is very different from what you've written in attached PDF file. Also I'm not quite sure it is good idea to simulate this flow using symmetry BCs as the flow itself is not symmetric (for example http://youtu.be/57-URbKeWME). Last edited by alexeym; March 4, 2014 at 08:28. Reason: addition |
|
March 4, 2014, 08:42 |
|
#22 |
Senior Member
ok
Join Date: Oct 2013
Posts: 346
Rep Power: 13 |
Dear Alexey,
I tried to attached all output, but unfortunately the size of the folder doesn’t accepted so I will post for one time step for p file dimensions [0 2 -2 0 0 0 0]; internalField nonuniform List<scalar> 2000 (zY\BAB\DCT1\C0\AC-\91*!1\C0\DCB`m\85 1\C0-\D1kI\A11\C0\B4Ɲ\D9 1\C0 \90\FA\C2R1\C0\B1W\A1J\B8\001\C0O\BFǙm\FD0\C0e/\8B \FD0\C0\86.\C4\CE\D8\FC0\C0¯Qr1\C0\89\DB[\F0\EB61\C0?\E0^\A851\C0?\B8n\BE"1\C0QV\E2\E6d1 \C0%\8A{\CEz1\C0\9D\94\99w 1\C0\A7Rt\A3\A8 1\C0v\A5gop1\C0\BD(R1\C0\DB\F3Z\D1\8F1\C0\BA# XGML1\C0\FC\A2\90\9EdJ1\C0\A2\BF\8EO31\C0ܭҞ(1\C0 V\95Z* 1\C0\CFb'\E41\C0\B8~p\D51\C0\E3\A0"\9D\C71\C0 \A47ܗ\C71\C0\F1\A2o\AA1\C0\E15ȶ`1\C0\D0A\AAQ^ 1\C0t\AB\FE \E7B1\C0\BD]r171\C0\EC :-1\C0\E3\9Bs\BA\A2%1\C0]\8Dv#\971\C0N\ADI T1\C0u^\F0oH1\C0\D4.\BB\8F\94\C31\C0\B1\87\F7.\9 8s1\C0\BD\9B\FDJp1\C0-*{\C1Q1\C0n4\E6\C2\CBD1\C0\A3r\94\C8I91\C01\9Cz 01\C0Gϰ\B1m)1\C0\96\D2+4$1\C0\9DJK\9Ef1\C0\86\E C\C9\DA\D91\C0\9E\E8O!w\841\C0a\A0k\801\C0T\8EH \97]1\C0\AC\F8\*Q1\C0\A4\EF\C6D1\C0u:B1:1\C02\F5\B 1\A0D21\C0/\B0 @#,1\C0,\FC\E2o\B2&1\C0\A4\FC\99[\AB\EC1\C0\F1/t\E9\921\C0\B7\8E\E34\8E1\C0%J\89Kh1\C0*\EF\A8[\D4[1\C0\E7r\BB}UM1\C0Ó\9B\E7\8CB1\C0=\D9\F8[\E591\C0\A4\ACI31\C0\B5\E2~\E7-1\C0\F465 That is not whole but only part of p file because the post doesn't accepted more that 20000 characters. There is something error given in the output files. Same in other output files. There are all output which I didn't post them give such that unclear samples. In addition to the attached uniform folder which is given in each timestep. |
|
March 4, 2014, 08:46 |
|
#23 |
Senior Member
ok
Join Date: Oct 2013
Posts: 346
Rep Power: 13 |
Do you have another way to post large size of files to show you whole output?
Anyway, all output file give the same error (unclear samples). There is something wrong. I hope you can help me. Kind regards |
|
March 4, 2014, 08:59 |
|
#24 |
Senior Member
|
Actually I don't need whole log file, just lines before the crash, in other word - the output for the last time step.
Also I'd like to know your thoughts about: Also I've got several question about your BCs: 1. You set fixed velocity at the outlet and yet you'd like to plot outlet velocity over time. Though you can plot velocity at the inlet boundary. 2. You've got symmetry BC at sides patch, though if you like to simulate flow past ONE cylinder, it should be wall. 3. For some reason you've decided to set symmetry plane also on walls patch (surface of the cylinder), though it again should be wall with non-slip BC. This is just quick look at the case files. What you've described with your initial conditions and boundary conditions is very different from what you've written in attached PDF file. If you've got wrong boundary conditions not solver will get you right results. Also I'm not quite sure it is good idea to simulate this flow using symmetry BCs as the flow itself is not symmetric (for example http://youtu.be/57-URbKeWME). |
|
March 4, 2014, 09:43 |
|
#25 |
Senior Member
ok
Join Date: Oct 2013
Posts: 346
Rep Power: 13 |
Dear Alexey,
many thanks for your help. Do you mean now I have to change sides and walls boundary conditions to wall instead of symmetryPlane? |
|
March 4, 2014, 09:53 |
|
#26 |
Senior Member
|
Well, it depends
If you'd like to simulate the problem you've described in attached PDF (I guess development of von Karman vortex street), then I'd suggest you to create a mesh with a whole cylinder (not just a half of it). Set non-slip boundary conditions of the walls (cylinder and walls of a channel), constant inlet velocity, zero-gradient outlet velocity, constant value of outlet pressure (let's say 0), zero gradient of inlet pressure (and empty BCs for top and bottom planes as you'd like to do 2D simulation). If you'd like to simulate something else, describe it more precisely. Currently your boundary conditions describe rather bizarre system. |
|
March 4, 2014, 10:24 |
|
#27 |
Senior Member
ok
Join Date: Oct 2013
Posts: 346
Rep Power: 13 |
Dear Alexey,
that what I'm looking for exactly. I will try to do all what you post and then I will let you know about the result. I have one more question please, what is the best way or software to create a mesh with whole cylinder? |
|
March 4, 2014, 10:34 |
|
#28 |
Senior Member
|
The best software is the one you know how to use
As the mesh if rather simple you can use blockMesh. If you'd like to have a "template" where you just need to correct sizes, you can start with the one I've made some time ago. Though the case files are rather messy, so you just can take a blockMeshDict from there. If I needed to make the mesh now I'd use Gmsh (http://gmsh.info). |
|
March 4, 2014, 10:46 |
|
#29 |
Senior Member
ok
Join Date: Oct 2013
Posts: 346
Rep Power: 13 |
Thank you very much Alexey. I will try all possibilities now.:-)
|
|
March 4, 2014, 11:11 |
|
#30 |
Senior Member
|
Here's a file for Gmsh (I've created rather simple meshing, surely it can be enhanced).
After you open this file in Gmsh it will create channel-with-cylinder.msh file, which then can be converted to OpenFOAM format with gmshToFoam utility. You can find the names of the boundaries in the file. Maybe after conversion you'll need to correct type of the boundary for walls, top, and bottom patches, cause converter will set type to patch. You can do it with changeDictionary utility and following changeDictionaryDict: Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object changeDictionaryDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dictionaryReplacement { boundary { walls { type wall; } top { type empty; } bottom { type empty; } } } // ************************************************************************* // |
|
March 4, 2014, 11:48 |
|
#31 |
Senior Member
ok
Join Date: Oct 2013
Posts: 346
Rep Power: 13 |
Dear Alexy,
sorry, I'm still confused about changing the names of the boundaries. Could you try please to mach the boundaries that you suggests and the boundary that I have. I never used Gmesh to create mesh or any of the software, all meshes that I have before were easy to create without using any program. So, what are these variable mean CX = 4.5*D; CY = 0.0; S = 1.0/Sqrt(2); N1 = 100; N2 = 400; Many thanks for your help. |
|
March 4, 2014, 12:31 |
|
#32 |
Senior Member
|
I've attached case files to the message. You need to correct velocity in 0/U to correspond to your case. Allprepare script assumes that you have gmsh in your PATH.
Also to plot drag force you have to wait until the flow develops otherwise you'll get something meaningless. I'd suggest you to run simulation for at least 2*L/U (where L is channel length and U is inlet velocity). Concerning your questions: I've tried to reproduce the channel from your PDF. So 1. D is a diameter of the cylinder. 2. CX, CY - coordinates of the center of the cylinder. 3. S is sin(pi/4), I need it for calculation of the coordinates of the points on the surface of the cylinder. 4. N1 and N2 is the densities of the different parts of the mesh. Actually if you open GEO file in Gmsh, you'll be able to see how I've split the mesh. |
|
March 4, 2014, 13:03 |
|
#33 | |
Senior Member
ok
Join Date: Oct 2013
Posts: 346
Rep Power: 13 |
Dear Alexy,
when executed gmshToFoam 2D-cylinder.geo in the command window it gives this error Quote:
and what do you mean by run simulation for at least 2*L/U? Many thanks in advanced. |
||
March 4, 2014, 13:05 |
|
#34 |
Senior Member
|
First you have to convert GEO file to MSH file using Gmsh. Then you can use gmshToFoam. See Allprepare script for the command sequence.
|
|
March 4, 2014, 13:18 |
|
#35 | |
Senior Member
ok
Join Date: Oct 2013
Posts: 346
Rep Power: 13 |
Dear Alexey,
Now, the converting to foam is going fine. Then, execution of pimpleFoam gives Quote:
|
||
March 4, 2014, 13:25 |
|
#36 |
Senior Member
|
I guess it is funny feature of openfoam-extend-3.0, as with OpenFOAM 2.2.2 there's not defaultFaces patch after conversion of the MSH file.
You can add Code:
defaultFaces { type empty; } |
|
March 4, 2014, 13:33 |
|
#37 | |
Senior Member
ok
Join Date: Oct 2013
Posts: 346
Rep Power: 13 |
Again, this error
Quote:
|
||
March 4, 2014, 13:52 |
|
#38 |
Senior Member
|
Well,
you can add Code:
defaultFaces { type empty; } |
|
March 4, 2014, 14:01 |
|
#39 | |
Senior Member
ok
Join Date: Oct 2013
Posts: 346
Rep Power: 13 |
paraFoam command gives the follwing fatal error
Quote:
|
||
March 4, 2014, 16:31 |
|
#40 |
Senior Member
ok
Join Date: Oct 2013
Posts: 346
Rep Power: 13 |
It works perfect in OpenFOAM. I just go to p, U and changeDictionary files and commit
defaultFaces { type empty; } and the visualization is shown in paraview. But I'm still being confused about lift and drag coefficients for Reynolds number 100? Any idea? What shall I change for Re = 100? |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[Other] OpenFoam Flow over a Circular Cylinder | WolfgangS. | OpenFOAM Meshing & Mesh Conversion | 12 | March 3, 2014 11:53 |
benchmark: flow over a circular cylinder | goodegg | Main CFD Forum | 12 | January 22, 2013 12:47 |
Particle deposition on circular cylinder in turbulent flow | Julian K. | CFX | 1 | October 3, 2011 18:51 |
flow around a cylinder | pXYZ | Main CFD Forum | 14 | July 25, 2011 11:05 |
Flow induced vibration of a mobile cylinder | Hooman | Main CFD Forum | 0 | December 31, 2010 09:48 |