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

OpenFOAM komegaSST - full resolution of ROUGH surface wall boundary layer

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 3, 2019, 03:56
Default OpenFOAM komegaSST - full resolution of ROUGH surface wall boundary layer
  #1
Member
 
Join Date: Aug 2018
Posts: 47
Rep Power: 7
foamF is on a distinguished road
I want to simulate the turbulent pipe flow with ROUGH wall surface for a specific ks value, using komegaSST in OpenFOAM with the full resolution on the wall boundary layer (NOT using wall function, e.g. nutkroughwallfunction).

Any expert can give me some advice how to set the boundary conditions on k, omega and nut?

Thanks.
foamF is offline   Reply With Quote

Old   February 4, 2019, 13:32
Default
  #2
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Breda, Netherlands
Posts: 634
Rep Power: 32
tomf will become famous soon enoughtomf will become famous soon enough
Send a message via MSN to tomf Send a message via Skype™ to tomf
Hi,

If you want to resolve the entire (rough) boundary layer you basically need to resolve the exact geometry of your roughness. A lower ks than y+=4 is considered hydraulically smooth if I remember correctly. As a full resolution would require y+~1, you would also need to capture the roughness elements in the mesh. So you would need to have very small cells in the boundary layer. Once you have that, you can specify normal smooth wall boundary layer resolving boundary conditions.

Hope this helps,
Tom
tomf is offline   Reply With Quote

Old   February 5, 2019, 06:29
Default
  #3
Member
 
Join Date: Aug 2018
Posts: 47
Rep Power: 7
foamF is on a distinguished road
Thanks, Tom.

Do you mean that
(1) if the boundary layer of a rough surface needs to be resolved, some small cells (with the thickness = ks) need to be explicitly protruded from the geometry surface and also the meshes, so that the surface roughness can be reflected?

(2) if the ks is very small (which is within the viscous layer; meaning that ks+ < 5), it ts hydraulically smooth. Even if the small cells are protruded from the geometry surface, the case would be exactly the same as smooth surface?
foamF is offline   Reply With Quote

Old   February 5, 2019, 07:00
Default
  #4
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Breda, Netherlands
Posts: 634
Rep Power: 32
tomf will become famous soon enoughtomf will become famous soon enough
Send a message via MSN to tomf Send a message via Skype™ to tomf
Hi,

1) Yes that is what I mean, you would need to resolve this.
2) That is what the general theory would indicate. The roughness may effect the near wall flow field, but in principle you should not see large differences in global parameters (wall shear stress/pressure loss). There may be some effect on transition. However if at some point you get out of the viscous sublayer, things may change rapidly.

I guess it will be case and roughness shape dependent.

Regards,
Tom
tomf is offline   Reply With Quote

Old   February 29, 2020, 17:48
Default
  #5
New Member
 
Pharlin Médard
Join Date: Sep 2018
Posts: 3
Rep Power: 7
locoiam1991 is on a distinguished road
Hello foamF,

1) You do not have to protrude the roughness elements in your CAD to simulate roughness effects (Using RANS) and your cells do not need to be as small as your roughness elements neither. Well, it depends on the turbulence model you are using. The Wilcox k-omega model need a y+(1) < 0.01 if Ks+ <100 and y+(1) < 0.003 if ks+>100. There is an extention to the SST k-omega model proposed by Tobias Knopp et al. that allows you to solve the boundary layer on the same mesh as a smooth surface. There are othe extentions that have been proposed by Boeing and Onera for the Spalart-Allmaras turbulence model. Please bear in mind that those extentions are artifices to the governing equations and have nothing to do with the physical roughness elements other than the Ks value you specify.

2) If your Ks+ value is less than 5, there is no need to resolve for the roughness elements as their effects are negligible. Additionally, if you try to resolve the governing equations for each and every roughness element with Ks+ less than 5, the computational cost will be very high.
locoiam1991 is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
y+ = 1 boundary layer mesh with snappyHexMesh Arzed23 OpenFOAM Running, Solving & CFD 6 November 23, 2022 16:15
[snappyHexMesh] Problem with Sanpper, surface still Rough Zephiro88 OpenFOAM Meshing & Mesh Conversion 7 November 5, 2014 13:05
Radiation interface hinca CFX 15 January 26, 2014 18:11
Question about heat transfer coefficient setting for CFX Anna Tian CFX 1 June 16, 2013 07:28
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05


All times are GMT -4. The time now is 03:32.