|
[Sponsors] |
August 16, 2013, 04:44 |
Relative roughness in openfoam
|
#1 |
Member
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 12 |
How to incorporate relative roughness in openfoam?
I am using pisoFoam to solve a simple turbulent flow through a pipe. I want to validate the result using Moody's chart, where i specify reynolds number and relative roughness to openfoam and check if the frcition factor given by openfoam matches with the value from moody's chart. Do we have to use nutkRoughWallFunction? If yes then what do Ks and Cs mean, and where do i find their values? Also, what is the default relative roughness used by openfoam? |
|
August 16, 2013, 05:06 |
|
#2 |
Senior Member
|
Hi,
I strongly recommend you to study this article: Blocken, B., Stathopoulos, T., Carmeliet, J., 2007. CFD simulation of the atmospheric boundary layer: wall function problems. Atmospheric Environment 41 (2), 238–252. Also check this thread out: http://www.cfd-online.com/Forums/ope...h-surface.html You can see nutkRoughWallFunction source file to see how are they defined. Cs values is something between 0 to 1, but typically it is considered 0.5. Ks (It is called equivalent sand-gran roughness height) differs from case to case, it is often calculated by: Ks = (20 to 30)*y0 in which, y0 is aerodynamic roughness length. a rule of thumb for values of y0 is 0.1 of the real roughness value. for example if height of the roughness is 0.1 m then y0 would be 0.01 m. I hope it helps a bit. Best
__________________
Learn OpenFOAM in Persian SFO (StarCCM+ FLUENT OpenFOAM) Project Team Member Complex Heat & Flow Simulation Research Group If you can't explain it simply, you don't understand it well enough. "Richard Feynman" |
|
August 16, 2013, 06:01 |
|
#3 |
Member
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 12 |
Okay i just realised that my way of validating turbulent flow is wrong.
Can you tell me how to validate a turbulent flow using some analytical results, like we have poiseuille's law for laminar flow. |
|
August 16, 2013, 08:29 |
|
#4 | |
Senior Member
|
Quote:
hope it helps.
__________________
Learn OpenFOAM in Persian SFO (StarCCM+ FLUENT OpenFOAM) Project Team Member Complex Heat & Flow Simulation Research Group If you can't explain it simply, you don't understand it well enough. "Richard Feynman" |
||
August 18, 2013, 23:20 |
|
#5 | |
Member
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 12 |
Quote:
How do i calculate relative roughness from Ks and Cs values? And how do i get the friction factor from openfoam? I read the nutkRoughWallFunction files and understood what Ks and Cs mean but there is no mention of how to obtain relative roughness from them. |
||
August 19, 2013, 12:37 |
|
#6 | |
Senior Member
|
Quote:
OK, first of all, what do you mean by relative roughness? do you mean y0? I haven't worked with nutkRoughWallFunction for a while and forgot some, I think you define Ks values as an input data. Well friction factor can be obtained using wall shear stress, as you know: Cf=Tau/(0.5*rho*U^2) In which Tau is wall shear stress. You can calculate wall shear stress with a utility named as "wallShearStress" in openfoam. later you can calcluate Cf in paraview using its calculator according to rho and U values.
__________________
Learn OpenFOAM in Persian SFO (StarCCM+ FLUENT OpenFOAM) Project Team Member Complex Heat & Flow Simulation Research Group If you can't explain it simply, you don't understand it well enough. "Richard Feynman" |
||
August 19, 2013, 23:09 |
|
#7 | |
Member
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 12 |
Quote:
Also, Cf is skin friction factor. I believe it is not the same as the friction factor f which is on the left hand scale of moody's chart. According to texts - friction factor is calculated experimentally. So the approach i am using is wrong. |
||
August 19, 2013, 23:57 |
|
#8 |
Member
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 12 |
There is one more problem though.
This is the test case i am trying out. Just to learn about turbulence. But even at 10^6 reynolds number i am getting laminar streamlines. Can you look up and tell me what is wrong with the problem. Assume smooth walls. test.zip |
|
August 20, 2013, 04:02 |
|
#9 | |
Senior Member
|
Quote:
I couldn't get why your approach is wrong.
__________________
Learn OpenFOAM in Persian SFO (StarCCM+ FLUENT OpenFOAM) Project Team Member Complex Heat & Flow Simulation Research Group If you can't explain it simply, you don't understand it well enough. "Richard Feynman" |
||
August 20, 2013, 05:14 |
|
#10 | |
Member
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 12 |
Quote:
Now my conclusion is - Obtain Fanning friction coefficient Cf using wallShearStress and then multiply it by 4 to get Darcy friction factor and use Moodys chart with Reynolds number and relative pipe roughness to verify the friction factor. Thanks a lot. I think this solves my problem. Can you also take a look at another problem which i posted right before your current reply? |
||
August 20, 2013, 05:23 |
|
#11 |
Senior Member
|
Well I'm not a turbulence expert, but sure, I will take a look at it
__________________
Learn OpenFOAM in Persian SFO (StarCCM+ FLUENT OpenFOAM) Project Team Member Complex Heat & Flow Simulation Research Group If you can't explain it simply, you don't understand it well enough. "Richard Feynman" |
|
August 20, 2013, 05:35 |
|
#12 |
Member
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 12 |
||
August 23, 2013, 07:21 |
|
#13 | |||
Member
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 12 |
Quote:
The results look similar. The velocity is not blowing. Input bein 1 m/s i am getting a maximum velocity of around 1.98 m/s. The results still look laminar - U.jpg |
||||
August 23, 2013, 13:25 |
|
#14 | |
Senior Member
|
Quote:
__________________
Learn OpenFOAM in Persian SFO (StarCCM+ FLUENT OpenFOAM) Project Team Member Complex Heat & Flow Simulation Research Group If you can't explain it simply, you don't understand it well enough. "Richard Feynman" |
||
August 26, 2013, 02:12 |
|
#16 | |
Senior Member
|
Quote:
You have got to use kOmegaSST model alongside with a finer grid to be able to resolve the boundary layer. Try take a look at these: http://www.computationalfluiddynamic...t-cell-height/ http://www.computationalfluiddynamic...oundary-layer/ http://www.computationalfluiddynamic...oundary-layer/ http://www.computationalfluiddynamic...ds-number-cfd/ http://www.computationalfluiddynamic...-requirements/ http://www.computationalfluiddynamic...nce-modelling/
__________________
Learn OpenFOAM in Persian SFO (StarCCM+ FLUENT OpenFOAM) Project Team Member Complex Heat & Flow Simulation Research Group If you can't explain it simply, you don't understand it well enough. "Richard Feynman" |
||
August 27, 2013, 00:53 |
|
#17 | |
Member
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 12 |
Quote:
Also, for kOmegaSST what boundary conditions should i use? Is it possible for you to simulate the problem and send me the files? I have been trying this problem for 3 weeks now and not able to understand anything. Last edited by inf.vish; August 27, 2013 at 03:27. |
||
August 27, 2013, 05:35 |
|
#18 | |
Senior Member
|
Quote:
you have to make a new initial boundary file named omega in your 0 directory and use omegaWallFunction for your wall boundaries. For example: wall { type omegaWallFunction; value uniform 0; } outlet { type zeroGradient; } inlet { type fixedValue; value uniform 0.0001; } try having a look at this thread: http://www.cfd-online.com/Forums/ope...omega-sst.html I hope it helps a bit , Best
__________________
Learn OpenFOAM in Persian SFO (StarCCM+ FLUENT OpenFOAM) Project Team Member Complex Heat & Flow Simulation Research Group If you can't explain it simply, you don't understand it well enough. "Richard Feynman" |
||
August 27, 2013, 06:58 |
|
#19 | |
Member
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 12 |
Quote:
One more question, do the values of k and omega (or epsilon) affect the final solution? I was trying out various values but found that for k>epsilon i get floating point exception on the courant number and for k<<epsilon (whatever be the value of k and epsilon) I obtain solutions which are very very close to each other. from what i have read y+ should be between 30-300 right? Also I was looking at pitzDaily example from pisoFoam>LES, there you can see vortices but on running the same simulation with say kE you do not get the vortices. I read somewhere on the forum that LES is better at capturing vortices as with kE or kOmega the viscous forces dampen the vortices. |
||
August 27, 2013, 11:59 |
|
#20 | ||||
Senior Member
|
Quote:
Quote:
Quote:
Therefore by using kOmegaSST model, you have got to lower your y+ value to something lower than 1. Quote:
Right now I have found this article which is quite useful: www.engmech.cz/2012/proceedings/pdf/195_Furst_J-FT.pdf It uses openFOAM and a new turbulence model which is best for laminar turbulent transition modeling. And plus take a look at this: http://www.cfd-online.com/Forums/ope...el-low-re.html I am studying about this. You have got to give me some time. Dig them out, maybe you can get what I can't. I hope it helps a bit, Best, Mojtaba
__________________
Learn OpenFOAM in Persian SFO (StarCCM+ FLUENT OpenFOAM) Project Team Member Complex Heat & Flow Simulation Research Group If you can't explain it simply, you don't understand it well enough. "Richard Feynman" |
|||||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Memory protection in OpenFOAM / combinig with FORTRAN | botp | OpenFOAM Programming & Development | 2 | February 15, 2016 12:25 |
ESI-OpenCFD Releases OpenFOAM v2.2.0 | opencfd | OpenFOAM Announcements from ESI-OpenCFD | 13 | March 30, 2013 16:52 |
[Gmsh] gmsh 2.6.0 conversion to OpenFoam 160 | rosswin | OpenFOAM Meshing & Mesh Conversion | 0 | March 5, 2013 07:34 |
[mesh manipulation] createPatch / cyclicGgi / OpenFoam 1.5-dev | OFU | OpenFOAM Meshing & Mesh Conversion | 0 | June 16, 2010 04:36 |
Cross-compiling OpenFOAM 1.6 on Linux for Windows 32 and 64bits with Mingw-w64 | wyldckat | OpenFOAM Announcements from Other Sources | 7 | January 19, 2010 15:39 |