CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Wall function for concrete walls, open channel flow

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By vatavuk
  • 1 Post By khedar

Reply
 
LinkBack Thread Tools Display Modes
Old   November 7, 2016, 05:52
Default Wall function for concrete walls, open channel flow
  #1
New Member
 
Tinu
Join Date: Nov 2016
Posts: 11
Rep Power: 2
tinu80 is on a distinguished road
Hi everybody,
I am using OpenFoam to simulate a weir situation in an open channel flow, see attached link. Im am using interFoam / interDyMFoam for this case. Basically I get the simulation to work, and the results overall look OK to me. However, I am struggling a bit to find/use the "best" turbulence modelling, meshing at walls and wall functions.
-The whole geometry is made of concrete of the same roughness
-At the moment I am using the Standard high-Re k-epsilon model (RASModel kEpsilon)
-At wall boundaries, I use fixedValue uniform(0,0,0) for U, kqRWallFunction uniform 1e-20 for k, epsilonWallFunction uniform 1e-07 for epsilon, nutUSpaldingWallFunction uniform 0.001 for nut.

Those boundary conditions and the values itself are defined when using Helyx-OS and defining the geometry as "wall", so basically standard suggestion from Helyx-OS.

My question is:
-Has anyone who is working on similar cases a suggestion which wall functions are best used to model the impact of roughness from concrete walls? Which values would you be using for those wall functions?
-Would you suggest a different turbulence model for this case?
-What would be your strategy when meshing, especially at walls in order to get the wall functions work how they are supposed to?

Any help on this is greatly appreciated! I know that I probably have to dive a bit deeper into wall functions an turbulence modelling, however having some hints for this one would greatly help me.
Tinu

...edit: picture upload isn't working for me at the moment. will try to fix this. Just think of a broad crested weir in a ca. 15 m wide channel.

Last edited by tinu80; November 7, 2016 at 06:00. Reason: picture upload doesn't work
tinu80 is offline   Reply With Quote

Old   November 8, 2016, 09:46
Default
  #2
Senior Member
 
Paulo Vatavuk
Join Date: Mar 2009
Location: Campinas, Brasil
Posts: 149
Rep Power: 10
vatavuk is on a distinguished road
HI Tinu,

To model the effect of roughness you could use the nutkRoughWallFunction for nut. The data for this boundary condition are:

type nutkRoughWallFunction
Ks - The Moody diagram roughness in meters
Cs - The roughness constant. The value is normally 0.5
value - Initial estimate for nut in the iterative calculation

The book “Fluid Mechanics” of F. M. White suggests a value of Ks=0.00004 m for smoothed concrete and Ks=0.002 m for rough concrete.

Best Regards,
Paulo
tinu80 likes this.
vatavuk is offline   Reply With Quote

Old   November 8, 2016, 17:24
Default
  #3
New Member
 
Tinu
Join Date: Nov 2016
Posts: 11
Rep Power: 2
tinu80 is on a distinguished road
Dear Paulo,
Thank you very much for your suggestion! nutkRoughWallFunction is exactly what I am playing around with at the moment, so good to know I am looking in the right place!
Maybe you can help me with my other question about mesh size at walls for nutkRoughWallFunction. Which y+ values should I have for my mesh at walls?

Best regards,
Tinu
tinu80 is offline   Reply With Quote

Old   November 8, 2016, 20:51
Default
  #4
Member
 
khedar
Join Date: Oct 2016
Posts: 72
Rep Power: 2
khedar is on a distinguished road
Hi Tinu,

If you are asking about the mesh size at the boundary for your case then you should keep the first cell size such that your y+ > 30. This is so that it lies in the turbulent region and not in the near wall viscous region.

regards,

khedar
khedar is offline   Reply With Quote

Old   November 9, 2016, 08:36
Default
  #5
New Member
 
Tinu
Join Date: Nov 2016
Posts: 11
Rep Power: 2
tinu80 is on a distinguished road
Hi khedar,
Thanks for your help. I think I get it now.
How important is the maximum allowable value of y+? The suggested values I found in literature are between 100 to 300.
In my case, my y+ is much higher, around 5000.
My plan is to calibrate the model based on known discharges and water levels. So I basically would try to change the Ks value in nutKRoughWallFunction until the simulation matches the experimental data.
So, even if I have underestimated wall shear stress because of too high y+, I could "correct" this by changing Ks value? Does that make sense somehow?
With y+ around 100 my mesh would get way too big to handle.
Best regards,
Tinu

Last edited by tinu80; November 9, 2016 at 08:47. Reason: typo
tinu80 is offline   Reply With Quote

Old   November 9, 2016, 11:30
Talking
  #6
Member
 
khedar
Join Date: Oct 2016
Posts: 72
Rep Power: 2
khedar is on a distinguished road
Hi Tinu,
i am no expert on wall function approach and am still in learning phase And hence i will suggest you the following discussion which you may find useful:

http://www.cfd-online.com/Forums/flu...treatment.html

1. From my basic understanding of Boundary layers, i would say that keeping your y+ too far above 300 will lead to some inaccuracies in solution(how big, can't say). This is because above this y+ one comes out of the boundary layer and into core turbulent flow region and the wall function predicted values may not be that accurate.
2. changing the k values in the wall function approach: can't say if this is the right approach(engineering approach ).

regards,
khedar
tinu80 likes this.
khedar is offline   Reply With Quote

Old   November 9, 2016, 12:16
Default
  #7
New Member
 
Tinu
Join Date: Nov 2016
Posts: 11
Rep Power: 2
tinu80 is on a distinguished road
Quote:
Originally Posted by khedar View Post
Hi Tinu,
i am no expert on wall function approach and am still in learning phase And hence i will suggest you the following discussion which you may find useful:

http://www.cfd-online.com/Forums/flu...treatment.html

1. From my basic understanding of Boundary layers, i would say that keeping your y+ too far above 300 will lead to some inaccuracies in solution(how big, can't say). This is because above this y+ one comes out of the boundary layer and into core turbulent flow region and the wall function predicted values may not be that accurate.
2. changing the k values in the wall function approach: can't say if this is the right approach(engineering approach ).

regards,
khedar
Hi khedar,
Thanks again for your support. You are right, I am looking for some engineering approach :-)
From playing with different Ks values I can say that it has a big impact to mean velocities and consequently to flow depth in the channel flow. It is comparable to changing Strickler or Mannings values in 2d or 1d open channel hydraulics. But it is quite hard to find hints on calibrating 3d open channel cases.
Regards,
Tinu
tinu80 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Swak4Foam funkyDoCalc with OF2.3 massflow NiFl OpenFOAM 11 November 1, 2016 07:43
Issues on the simulation of high-speed compressible flow within turbomachinery dowlee OpenFOAM Running, Solving & CFD 8 October 25, 2016 19:48
Running UDF with Supercomputer roi247 FLUENT 4 October 15, 2015 13:41
Question on the boundary condition for open channel flow, please help! ripperjack OpenFOAM Running, Solving & CFD 0 September 13, 2013 11:44
Compile problem ivanyao OpenFOAM Running, Solving & CFD 1 October 12, 2012 09:31


All times are GMT -4. The time now is 13:37.