OpenFOAM komegaSST - full resolution of ROUGH surface wall boundary layer

foamF · February 3, 2019, 03:56

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.

tomf · February 4, 2019, 13:32

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

foamF · February 5, 2019, 06:29

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?

tomf · February 5, 2019, 07:00

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

locoiam1991 · February 29, 2020, 17:48

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.

February 3, 2019, 03:56	OpenFOAM komegaSST - full resolution of ROUGH surface wall boundary layer	#1
foamF Member Join Date: Aug 2018 Posts: 47 Rep Power: 8	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.

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

February 4, 2019, 13:32		#2
tomf Senior Member Tom Fahner Join Date: Mar 2009 Location: Breda, Netherlands Posts: 646 Rep Power: 32	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

February 5, 2019, 06:29		#3
foamF Member Join Date: Aug 2018 Posts: 47 Rep Power: 8	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?

February 5, 2019, 07:00		#4
tomf Senior Member Tom Fahner Join Date: Mar 2009 Location: Breda, Netherlands Posts: 646 Rep Power: 32	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

February 29, 2020, 17:48		#5
locoiam1991 New Member Pharlin Médard Join Date: Sep 2018 Posts: 3 Rep Power: 8	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.