|
[Sponsors] |
August 5, 2011, 22:33 |
laminar to turbulent transitonal pipe flow
|
#41 |
New Member
hasan
Join Date: Aug 2011
Location: Diyarbakır / Turkey
Posts: 3
Rep Power: 15 |
I am studying transitional pipe flow in numerical. This is my doctorate thesis. My aim is to simulate pressure fluctuation on the entire pipe flow or I want to simulate the existance of transition through the pipe flow.
*How can I carried out this one by using LES model in FLUENT. My package program is ANSYS 12. * how can I impose the perturbations into the pipe flow for transition. is there any tutorial about this or any notes I will be pleased with your helpings |
|
March 29, 2012, 07:53 |
|
#42 |
New Member
senpatras
Join Date: Mar 2012
Posts: 16
Rep Power: 14 |
To all, and specially Cedric,
I was trying to emulate the exact case that Cedric had discussed. For starters, I would like to know, as to how long approximately, one has to wait, for the flow to depict Turbulence? I have already completed around 70 time cycles, but I see no turbulence yet I am using inlet/outlet boundary condition, for inlet and outlet respectively, and 'wall' for my walls. I initialize my flow field using the perturbU code by Eugene. Any help, is most welcome. |
|
March 29, 2012, 08:11 |
|
#43 | |
Senior Member
Florian Krause
Join Date: Mar 2009
Location: Munich
Posts: 103
Rep Power: 17 |
Quote:
What is your y+ at the wall and what schemes are you using? Are you setting your case up as a short periodic pipe with dimensions as approx. length = 5 diameter? Best, Florian |
||
March 29, 2012, 08:35 |
|
#44 | ||
New Member
senpatras
Join Date: Mar 2012
Posts: 16
Rep Power: 14 |
Quote:
My y+ at the wall is 70, Here is a copy of my fvschemes file, Quote:
In my case Length of pipe= 5.7 * D Will this help? |
|||
March 29, 2012, 09:09 |
|
#45 |
Senior Member
Florian Krause
Join Date: Mar 2009
Location: Munich
Posts: 103
Rep Power: 17 |
Well, if y+=70 at the wall is not a typo, then for a LES it is far too large.
You have to resolve the flow near the wall, so you should have at least 3 cells within the viscous sublayer (y+ approx. 5) and the smallest y+ should be approx. 0.3-0.5. Using that, I generally obtain acceptable results. Hope that helps! Florian |
|
March 29, 2012, 09:25 |
|
#46 | |
New Member
senpatras
Join Date: Mar 2012
Posts: 16
Rep Power: 14 |
Quote:
Last edited by sen.1986; March 29, 2012 at 10:20. |
||
March 30, 2012, 08:53 |
|
#47 |
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Nantes, France
Posts: 195
Rep Power: 17 |
Senpatras,
As already mention by Florian, for a LES simulation, y+ should be less than 1 and 3 cells within the viscous layer is really the minimum. If your mesh is too coarse, you will dissipate the perturbation created by perturbU. If I remember correcly, in perturbU, you can change few parameters such as the amplitude of the noise added. This might be the easiest way. let us know if it's working or not. I my case, I was interesting in swirling flow that's why I've used an other method which is to add a bodyforce in the orthoradial direction to let the flow become unsteady (rotating flow is more unstable than pure axial flow). After few time cycle, you can remove this bodyforce and let the flow converge to an non-rotating flow. Then you can start the averaging of your fields. Of course you will need to modified the solver with this method. I hope this will help you, Cedric |
|
March 30, 2012, 09:41 |
|
#48 | |
New Member
senpatras
Join Date: Mar 2012
Posts: 16
Rep Power: 14 |
Quote:
|
||
April 2, 2012, 09:00 |
|
#49 | ||
New Member
senpatras
Join Date: Mar 2012
Posts: 16
Rep Power: 14 |
@Cedric and Florian
Now, I need some help with refining the mesh, I can't make proper headway because of this. Firstly, I would like to ask you, is there a proper tutorial for topoSet and refineMesh application of OpenFoam, I am really confused with the two as of now. I am presently trying to mesh near the wall, as suggested by you guys, i.e to have 4 cells within y+ = 5. For doing that, I am presently using the following refinemeshdict and toposetdict files, but I do not see refinement after I run toposet and refineMesh at the terminal, though they do not report any error. My geometry is a circular pipe with x [0 0.12], y[-0.01 0.01] and z[-0.01 0.01]. Quote:
Quote:
|
|||
April 4, 2012, 04:37 |
|
#50 |
Senior Member
Florian Krause
Join Date: Mar 2009
Location: Munich
Posts: 103
Rep Power: 17 |
I have never used these utilities, so I cannot help you with that. I created my pipe grids in a different grid generator calculating the thickness of the viscous sublayer as
y_{visc. sublayer} = y^+(=5)*d_{pipe} / Re_{tau} Did you search the forum for the utilities? There is also a sub-forum Meshing & Mesh Conversion, I guess your question is better placed there. Regards, Florian |
|
April 5, 2012, 03:06 |
|
#51 |
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Nantes, France
Posts: 195
Rep Power: 17 |
I don't know how you've generate your mesh but, there is somewhere in the forum a blockMesh file to do simple pipe configuration (butterfly mesh).
In this case it is really easy to modify the distribution close to the wall and not too much time consuming. I've never used these utilities either. Regards, Cédric |
|
April 12, 2012, 09:13 |
|
#52 |
New Member
senpatras
Join Date: Mar 2012
Posts: 16
Rep Power: 14 |
So after a bit of a struggle, I need more help. This is what I did in the meanwhile, I couldn't grasp how one could remesh specifically near the wall using blockmesh (meshing uniformly and stayisfying the condition of having 3 elements inside y+=5 seemed to expensive. So I decided to mesh with icemcfd. The mesh looks, as is shown in the attachment.
pic1.jpg pic2.jpg pic3.jpg After I did this, I exported the mesh and then using Fluent3dtoFoam converted it. When I tried running perturbU initially, an annoying face ordering problem was reported, with 1.98%. This has something to do with the periodic/cyclic boundary conditions. After rechecking my association of edges and curves again, the only way to work around it was to increase the matchTolerance to 2, from the preset value of 1d-4. After that perturbU ran just fine, and then when I run my case, the Courant Number goes fine for about 70 iterations, and then suddenly the residuals shoot up, and my simulation blows off. My calculated deltaT for a Courant no. of 0.5 is 7.5d-5, hence I am using a time step of 1d-5. Any ideas, how one could go about it next? |
|
April 13, 2012, 06:43 |
|
#53 |
New Member
senpatras
Join Date: Mar 2012
Posts: 16
Rep Power: 14 |
Also, this is where the simulation blows up. I am using a time step of 1d-5. From the 76th time step to 77th time step, something suddenly goes wrong with Uy, which causes the residuals to Uy to go very high, eventually causing the simulation to diverge. I am attaching the two plots of Uy at time 0.00076 and 0.00077.
0.00076.jpg 0.00077.jpg Kindly give it a look, and let me know if you have any idea. |
|
April 13, 2012, 07:15 |
|
#54 |
Member
Timo K.
Join Date: Feb 2010
Location: University of Stuttgart
Posts: 66
Rep Power: 16 |
Hi,
which solver do you use? What is your Courant number? which sgs-model? What is your inlet BC? Which case do you run? Best |
|
April 13, 2012, 08:59 |
|
#55 |
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Nantes, France
Posts: 195
Rep Power: 17 |
Hi Senpatras,
Are you sure there is no influence fixing the matchTolerance to 2, from the preset value of 1e-4 (4 orders magnitudes are quite a lot ....) ? In an other word, is your periodic BC really cyclic ? To avoid this problem, you could create a simple blockMeshDict file. Maybe you can have a look at the turbomachinery SIG: http://openfoamwiki.net/index.php/Si...nical_diffuser This test case includes parametrizations of an axisymetric geometry using O-grid, you will find the blockMeshDict.m4 file to create both geometry and mesh. It straithforward to get a periodic pipe mesh in the native blockMesh format. I hope this will help you, Cedric |
|
June 29, 2013, 06:40 |
Source term in the momentum equation
|
#56 | |
New Member
|
Quote:
Could you explain how to implement the referenced momentum source term? You implement a constant force or something like a pressure gradient? Thanks, Antonio |
||
December 20, 2013, 06:38 |
|
#57 |
New Member
Join Date: Feb 2013
Posts: 10
Rep Power: 13 |
Hi guys,
I am trying to simulate a turbulent pipe flow, Re=5300 (based on bulk velocity and diameter of cylinder pipe). My problem is in the initialization of turbulent field. I saw the existence of perturbU utility for this purpose, but when I download the .tgz file am not able to open it as its changes to .unk (unknown) type. Any suggestions? Thanks! |
|
March 4, 2014, 04:32 |
|
#58 | |
Senior Member
Huang Xianbei
Join Date: Sep 2013
Location: Yangzhou,China
Posts: 302
Rep Power: 14 |
Quote:
I'm looking for your Phd thesis for a long time in order to study the channel flow using openfoam with LES and DNS. But I can't find it for my net can't connect to some website. So can you be so kind to send me a copy of your thesis? My email is znhuang@163.com Best regards |
||
January 24, 2018, 14:05 |
postChannel
|
#59 |
Senior Member
Guilherme
Join Date: Apr 2017
Posts: 245
Rep Power: 10 |
Did you find out anything about this?
|
|
September 16, 2019, 10:58 |
|
#60 |
New Member
George Sof
Join Date: Jun 2019
Posts: 13
Rep Power: 7 |
Hello, still interested about postprocessing turbulent pipe flows. I need to average spatially U.z over a homogeneous direction z of a pipe. Result of the averaging should be a surface field U.z(x,y). Is it possible? Is there any progress regarding pipe postprocessing that you can share? Thank you very much! |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
MapFields turbulent pipe flow | anita | OpenFOAM Pre-Processing | 5 | July 4, 2008 00:29 |
pipe turbulent flow | Hao | FLUENT | 4 | April 29, 2008 23:30 |
turbulent pipe flow | John | FLUENT | 2 | August 2, 2005 14:00 |
fully developed turbulent flow in a pipe | Dipak | Phoenics | 3 | July 20, 2000 06:53 |
Measurements on turbulent pipe flow | Bo B. B. Jensen | Main CFD Forum | 4 | June 30, 1999 06:34 |