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

RANS to LES turbulent velocity profile

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

Like Tree1Likes
  • 1 Post By nskelly

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 17, 2019, 09:51
Default RANS to LES turbulent velocity profile
  #1
Member
 
Nat K
Join Date: Oct 2017
Posts: 68
Rep Power: 8
nskelly is on a distinguished road
Hi all,

I am running a RANS (k-omega SST) simulation as a precursor for LES simulation over a backward facing step. When running the RANS simulation I obtain a block profile (using a mapped patch BC).

However, when I change to LES, the block profile becomes parabolic at the step (which is not what I need for my experiment).

I am running using pisoFoam solver with Smagorinsky SGS model. I believe the mesh is fine enough for LES so I am not sure what the problem is. Re = 2000 ( 0.63 m/s) based on outlet height.


Any help/advice would be appreciated.
nskelly is offline   Reply With Quote

Old   January 18, 2019, 12:40
Default
  #2
Senior Member
 
Michael Alletto
Join Date: Jun 2018
Location: Bremen
Posts: 615
Rep Power: 15
mAlletto will become famous soon enough
If your profile becomes parabolic that means that you have a laminar flow.

If the Re number in the experiment is the same as in your LES simulation, this is a hint that your numerical dissipation is too high (did you ensure you simulated 2nd Order).

But this is only a guess since your problem description is not very detailed.
mAlletto is offline   Reply With Quote

Old   January 18, 2019, 12:42
Default
  #3
Senior Member
 
Michael Alletto
Join Date: Jun 2018
Location: Bremen
Posts: 615
Rep Power: 15
mAlletto will become famous soon enough
A just a comment: Re = 2000 is very close to the Reynolds number very the transition from laminar to turbulent flow happens.


By the way how do you define the Re number? based on the channel half width or the width?
mAlletto is offline   Reply With Quote

Old   January 18, 2019, 13:13
Default
  #4
Member
 
Nat K
Join Date: Oct 2017
Posts: 68
Rep Power: 8
nskelly is on a distinguished road
Thanks for responding.

I have attached my fvSchemes, they are all second order (I believe).

You are right that Re =2000 is in the transitional regime. However, simulating Re = 5000, parabolic profile is still evident.

My Reynolds number is based on the inlet height (h) --> Re = 2h*U/v.
nskelly is offline   Reply With Quote

Old   January 18, 2019, 13:15
Default
  #5
Member
 
Nat K
Join Date: Oct 2017
Posts: 68
Rep Power: 8
nskelly is on a distinguished road
Forgot to attache fvSchemes
Attached Files
File Type: txt fvSchemes.txt (1.4 KB, 13 views)
nskelly is offline   Reply With Quote

Old   January 18, 2019, 13:18
Default
  #6
Senior Member
 
Michael Alletto
Join Date: Jun 2018
Location: Bremen
Posts: 615
Rep Power: 15
mAlletto will become famous soon enough
I do not see any attachments. By the way, very do you get your parabolic profile?

Can you attach some slides of paraview to get a better picture what's happening?
mAlletto is offline   Reply With Quote

Old   January 18, 2019, 13:28
Default
  #7
Member
 
Nat K
Join Date: Oct 2017
Posts: 68
Rep Power: 8
nskelly is on a distinguished road
Velocity profiles for RANS and LES are attached.
Attached Images
File Type: jpg RANSVP.jpg (74.1 KB, 42 views)
File Type: jpg LESVP.jpg (76.6 KB, 44 views)
nskelly is offline   Reply With Quote

Old   January 18, 2019, 13:57
Default
  #8
Senior Member
 
Michael Alletto
Join Date: Jun 2018
Location: Bremen
Posts: 615
Rep Power: 15
mAlletto will become famous soon enough
I guess you show the profile right befor the step. Isn't it?

What kind of boundary conditions did you apply?

So the profile gets laminar. What is the resolution in terms of y+ close to the wall?

Do you know this boundary condition: https://www.openfoam.com/documentati...ty-dfsem.html?
mAlletto is offline   Reply With Quote

Old   January 18, 2019, 14:16
Default
  #9
Member
 
Nat K
Join Date: Oct 2017
Posts: 68
Rep Power: 8
nskelly is on a distinguished road
Sorry this is right at the step - attached are just before the step.

So I have been using mapped patch boundary condition which I hope maps a plane downstream of the step. But I have also been running a simulation with a turbulentInlet BC prescribing some turbulent fluctuations

y+ < 0.5 from what I calculated. Could it possibly be my BC for turbulent viscosity (nut)? I am using zeroGradient on all faces (inlet, outlet, walls).

I have not heard of the DFSEM BC but looks like it might help.
Attached Images
File Type: jpg LESVP2.jpg (82.8 KB, 17 views)
File Type: jpg RANSVP2.jpg (80.7 KB, 18 views)
Imran358 likes this.
nskelly is offline   Reply With Quote

Old   January 18, 2019, 15:25
Default
  #10
Senior Member
 
Michael Alletto
Join Date: Jun 2018
Location: Bremen
Posts: 615
Rep Power: 15
mAlletto will become famous soon enough
Can you also post the 0/U file. In order to unterstand from whitch patch you map the inflow velocity
mAlletto is offline   Reply With Quote

Old   January 18, 2019, 15:56
Default
  #11
Member
 
Nat K
Join Date: Oct 2017
Posts: 68
Rep Power: 8
nskelly is on a distinguished road
I have attached my U file and blockMeshDict
Attached Files
File Type: txt U.txt (1.5 KB, 17 views)
File Type: txt blockMeshDict.txt (4.7 KB, 9 views)
nskelly is offline   Reply With Quote

Old   January 19, 2019, 07:14
Default
  #12
Senior Member
 
Michael Alletto
Join Date: Jun 2018
Location: Bremen
Posts: 615
Rep Power: 15
mAlletto will become famous soon enough
Having a quick look at the blockMeshDict i saw that you used only 10 cells in spanwise direction. This are too few for a wall bounded LES. check for the resolution requirement for wall bounded LES of Piomelli. As fare as I remember in spanwise direction you need
a resolution of Delta z+ of 30 to 50 to resolve the streamwise vortices responsible for the mixing between the viscous sublayer and the inertial layer.


Furthermore the offset is also too low. For such a low Re number you need at least 5 channel heights of offset in order that the two point correlation drop to zero. You need to ensure that the flow field on the position of the plane you map from and your inlet plane are uncorrelated.





Best


Michael
mAlletto is offline   Reply With Quote

Old   January 24, 2019, 06:26
Default
  #13
Member
 
Nat K
Join Date: Oct 2017
Posts: 68
Rep Power: 8
nskelly is on a distinguished road
Sorry for the late reply.

Thank you for all the advice.

I will increase the both the number of cells and the refinement in the z direction to resolve the three dimensional vortices.

I was always unsure of the offset of the mapping plane, I will increase to your suggestions.

I will keep you updated.

Thanks again.
nskelly 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
3D UDF Paraboilc Velocity Profile (Can't Maintain) Sing FLUENT 12 August 7, 2017 07:25
Comparison of LES based turbulent quantity with RANS based turbulence mali28 FLUENT 1 May 11, 2017 17:57
Velocity profile reading in Fluent mkpm FLUENT 0 July 28, 2016 03:12
How to apply an outlet velocity profile to another inlet? siw FLUENT 4 April 10, 2013 12:19
LES: mean velocity and turbulent kinetic energy MET FLUENT 8 December 8, 2006 06:08


All times are GMT -4. The time now is 02:59.