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

turbulent and laminar vortex shedding with rhoPimpleFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 28, 2016, 02:52
Default turbulent and laminar vortex shedding with rhoPimpleFoam
  #1
New Member
 
Christoph
Join Date: Jul 2016
Posts: 2
Rep Power: 0
c_spkmp is on a distinguished road
Hello everyone,


I am trying to simulate the vortex shedding of air behind a T-shaped bluff body in a pipe using OpenFoam 3.0.1.
The geometry of the pipe and the bluff body is deduced from an industrial application.
I utilize the rhoPimpleFoam-solver and the k-omega-SST turbulence model. For k, omega and nut I am using wallfunctions as suggested in the OpenFoam-tutorialcases of rhoPimpleFoam. Moreover I use the waveTransmissive BC at the outlet for p in order to eliminate the occurrent reflected waves. The case is 2D and the mesh structured and hexahedral.
My problem is, that the case doesn't produce any vortex shedding that makes sense in a physical manner respectively doesn't produce any vortex shedding at all, although the Reynolds number is around 78 000.
In a first test I ran the case with a deactivated turbulence model (turbulenceProperties -> simulationType laminar). In the results vortex shedding was noticeable, but the vortecies were shed symmetrically and not, as expected from the theory of a Karman vortex street, in turns from the two leading edges of the bluff body. Moreover 2 vortex-like structures travel downstream with decreasing velocity but don't seem to dissipate as fast as the other vortecies. They form something like a nozzle which blocks the pipe .
Afterwards I activated the k-omega-SST model in a second case, but then no vortex shedding occurred at all.


I would be very grateful, if anyone could help me and maybe has an idea what might be wrong with the boundaries or the entire case-setup. My main questions are: why is the vortex shedding symmetrical in the laminar case and why does the activated turbulence model seem to suppress the vortex shedding?
Many thanks in advance.


p.s. I attached my case-setup and pictures of the observed phenomena to this post.
Attached Images
File Type: jpg laminar_case_p.jpg (52.4 KB, 14 views)
File Type: jpg laminar_case_U.jpg (54.3 KB, 9 views)
File Type: jpg turbulent_case_p.jpg (36.6 KB, 10 views)
File Type: jpg turbulent_case_U.jpg (43.4 KB, 10 views)
Attached Files
File Type: gz 2D_vortex_shedding.tar.gz (47.2 KB, 5 views)
c_spkmp is offline   Reply With Quote

Old   July 28, 2016, 03:13
Default
  #2
Member
 
Bruno
Join Date: Jun 2016
Location: Siegen, Germany
Posts: 59
Rep Power: 3
MBttR is on a distinguished road
Why do you have zeroGradient for U on your outlet?
MBttR is offline   Reply With Quote

Old   July 28, 2016, 08:23
Default
  #3
Member
 
Bruno Blais
Join Date: Sep 2013
Location: Canada
Posts: 66
Rep Power: 6
blais.bruno is on a distinguished road
Using laminar with such a high reynolds number is a recipee for disaster.
How fine is your mesh? From the pictures it looks relatively coarse, do you have a picture of it?

When you use a RANS turbulence model, sometimes the RANS model will stabilize the flow sufficiently that the transient vortex shedding won't occur. If it is the shedding your are after, I would suggest to use an LES approach, especially for such a 2D geometry, and then average the flow if you want to post-process.

If you want very accurate transient behavior, I really suggest going with LES for this (and with an extremely fine mesh)


Quote:
Originally Posted by c_spkmp View Post
Hello everyone,


I am trying to simulate the vortex shedding of air behind a T-shaped bluff body in a pipe using OpenFoam 3.0.1.
The geometry of the pipe and the bluff body is deduced from an industrial application.
I utilize the rhoPimpleFoam-solver and the k-omega-SST turbulence model. For k, omega and nut I am using wallfunctions as suggested in the OpenFoam-tutorialcases of rhoPimpleFoam. Moreover I use the waveTransmissive BC at the outlet for p in order to eliminate the occurrent reflected waves. The case is 2D and the mesh structured and hexahedral.
My problem is, that the case doesn't produce any vortex shedding that makes sense in a physical manner respectively doesn't produce any vortex shedding at all, although the Reynolds number is around 78 000.
In a first test I ran the case with a deactivated turbulence model (turbulenceProperties -> simulationType laminar). In the results vortex shedding was noticeable, but the vortecies were shed symmetrically and not, as expected from the theory of a Karman vortex street, in turns from the two leading edges of the bluff body. Moreover 2 vortex-like structures travel downstream with decreasing velocity but don't seem to dissipate as fast as the other vortecies. They form something like a nozzle which blocks the pipe .
Afterwards I activated the k-omega-SST model in a second case, but then no vortex shedding occurred at all.


I would be very grateful, if anyone could help me and maybe has an idea what might be wrong with the boundaries or the entire case-setup. My main questions are: why is the vortex shedding symmetrical in the laminar case and why does the activated turbulence model seem to suppress the vortex shedding?
Many thanks in advance.


p.s. I attached my case-setup and pictures of the observed phenomena to this post.
blais.bruno is offline   Reply With Quote

Old   July 28, 2016, 09:51
Default
  #4
New Member
 
Christoph
Join Date: Jul 2016
Posts: 2
Rep Power: 0
c_spkmp is on a distinguished road
Hello you two,

thanks for your replies.

The problem with the turbulent case seems to be a kind of solved, as I ran a case with a reynolds number of about 400 000. There vortex shedding occurred and a wake was formed as expected from the karman vortex street. Therefore I think, that in the case with Re ~78 000 we only observed a part of the development before the shedding starts, which takes much time.

#1 I am using zeroGradient, because I don't think it's necessary to calculate the exact value of the velocity at the outlet in this case. Would you recommend another BC?

#2 Yes, my mesh is rather coarse at the moment, but I will refine it as soon as I know how to do the wall treatment.
I will think about your suggestion to use the LES, but I am not mainly interested in the exact formation of the vortecies but rather in the shedding frequency of the large vortecies. Therefore I hope that RAS is good enough. Or do you have another opinion?

The problem I am working at now, is the wall treatment with the k-omega-SST model. In literature I read that the SST model can be used with wallfunctions or with a detached boundary layer. Can you give me an advice which method might be the best suited for this case?
Attached Images
File Type: jpg mesh.jpg (169.5 KB, 9 views)
c_spkmp is offline   Reply With Quote

Old   July 28, 2016, 11:54
Default
  #5
Member
 
Bruno Blais
Join Date: Sep 2013
Location: Canada
Posts: 66
Rep Power: 6
blais.bruno is on a distinguished road
RANS simulations (or URANS) in that case are rarely good for really transient and oscillating flow. I don't think you can find the right vortex frequency using an URANS model.

At least, I would definitely start with a better mesh than that, at least 50-100k cells to test.

If I were you I would go straight to LES with wall damping functions, especially if your case is 2D.

ZeroGradient U outlet is ok, but generally you will want a longer domain if you don't want your outlet polluting your solution



Quote:
Originally Posted by c_spkmp View Post
Hello you two,

thanks for your replies.

The problem with the turbulent case seems to be a kind of solved, as I ran a case with a reynolds number of about 400 000. There vortex shedding occurred and a wake was formed as expected from the karman vortex street. Therefore I think, that in the case with Re ~78 000 we only observed a part of the development before the shedding starts, which takes much time.

#1 I am using zeroGradient, because I don't think it's necessary to calculate the exact value of the velocity at the outlet in this case. Would you recommend another BC?

#2 Yes, my mesh is rather coarse at the moment, but I will refine it as soon as I know how to do the wall treatment.
I will think about your suggestion to use the LES, but I am not mainly interested in the exact formation of the vortecies but rather in the shedding frequency of the large vortecies. Therefore I hope that RAS is good enough. Or do you have another opinion?

The problem I am working at now, is the wall treatment with the k-omega-SST model. In literature I read that the SST model can be used with wallfunctions or with a detached boundary layer. Can you give me an advice which method might be the best suited for this case?
blais.bruno is offline   Reply With Quote

Old   July 29, 2016, 02:39
Default
  #6
Member
 
Bruno
Join Date: Jun 2016
Location: Siegen, Germany
Posts: 59
Rep Power: 3
MBttR is on a distinguished road
Hi Bruno,

What is the benefit of using zeroGradient for U on the outlet in stead of just specifying the value of velocity as all tutorials do?
MBttR 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
Laminar vs Turbulent Navier-Stokes truman Main CFD Forum 8 July 10, 2017 07:20
CFX Treatment of Laminar and Turbulent Flows Jade M CFX 14 June 15, 2016 09:36
Cylinder vortex shedding (3D) Apocolapse STAR-CCM+ 2 April 3, 2014 20:33
Ratio of eddy viscosity to molecular viscosity : Laminar or turbulent flow? JuPa CFX 7 September 9, 2013 07:45
Vortex shedding behind cylider in cross flow Muthu FLUENT 0 March 6, 2006 11:29


All times are GMT -4. The time now is 09:12.