CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Separation bubble inside a tunnel - unexpected assymetric flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 15, 2014, 21:03
Default Separation bubble inside a tunnel - unexpected assymetric flow
  #1
New Member
 
Join Date: May 2013
Posts: 7
Rep Power: 3
Queiroz is on a distinguished road
Good night for all,

I'm posting this message because I already tryied everything that I could but nothing worked. I'm sorry for the errors that I might do in english.

Well, I'm trying to simulate a bubble inside a wind tunnel generated by an adverse to favorable pressure gradient driven flow. I have attached a picture of the wind tunnel so it will help you to visualize the whole process.

I have just two known experimental boundary conditions: 25 m/s the flow velocity at the inlet and turbulence intensity of 0,003 (it's really low). At the outlet I'm setting opening, zero relative pressure and Default Intensity and Autocompute Length Scale. At the suction part, the same as at the outlet and no-slip for the wall.

I used two different turbulence models: k-epsilon and SST Menter. I know the first one is not good to predict well the location of separation and also the amount of separated flow. I used it just for comparison purposes.

For some reason that I don't know, the flow is not symmetric. I was not expecting to see something completely symmetric, but neither to see this flow skewness at the upper wall.

Could you please help me?

Thanks.

Matheus
Attached Images
File Type: jpg Fig. 2.jpg (27.7 KB, 27 views)
File Type: jpg Linhas parede.jpg (27.4 KB, 19 views)
File Type: jpg Tensão cisalhamento - linhas de corrente 2.jpg (49.6 KB, 24 views)
File Type: jpg Tensão cisalhamento - linhas de corrente.jpg (51.2 KB, 22 views)
Queiroz is offline   Reply With Quote

Old   January 15, 2014, 22:24
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,775
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
First of all, have you checked the accuracy of your model? See FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

If you convince yourself the model is accurate then consider that it is common in fluid flow for symmetric geometries to result in asymmetric flows. Laminar vortex shedding behind a cylinder is a classic example.
ghorrocks is offline   Reply With Quote

Old   January 16, 2014, 09:37
Default
  #3
New Member
 
Join Date: May 2013
Posts: 7
Rep Power: 3
Queiroz is on a distinguished road
Thanks for you response Mr. Ghorrocks,

I read what you suggested me, and I'm quite sure, at least based on my knowledge on the physics of the problem and also the steps of simulation, that there is nothing wrong. However, the flow pattern expected to the upper wall of the wind tunnel is quite different from the experimental one I have (it is attached to this message).

As I'm using the SST Menter model, it shouldn't be sensitive to the Y+ value, anyways I've found values like 5.57, and smaller than 2.

The dimensions of the bubble and location of separation and reattachament are closer to the expected ones, the problem is with the symmetry at the upper wall.

Any idea what could be causing it?

Thanks,

Matheus
Attached Images
File Type: jpg Flow pattern at the upper wall.jpg (97.4 KB, 13 views)
Queiroz is offline   Reply With Quote

Old   January 16, 2014, 18:06
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,775
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I see. To accurately model these secondary flows you are going to need a carefully validated model. Check all the parameters discussed in the FAQ I previously linked to. The most important is mesh size - if you have not checked your mesh is adequate then your model will be inaccurate.

Also 2 equation turbulence models often have challenges predicting secondary flows. You might need a Reynolds Stress model, or possibly a LES approach. But before you try any of that consider the optional stuff in SST such as curvature correction.
ghorrocks is offline   Reply With Quote

Old   January 16, 2014, 22:39
Default
  #5
New Member
 
Join Date: May 2013
Posts: 7
Rep Power: 3
Queiroz is on a distinguished road
How can I properly check the mesh size? How to know the best element sizes?

I'm sorry asking these simple questions, but I am a "beginner". I'm reading a lot, but still...

Matheus
Queiroz is offline   Reply With Quote

Old   January 17, 2014, 06:17
Default
  #6
New Member
 
Benedikt
Join Date: Dec 2013
Location: Munich, Germany
Posts: 10
Rep Power: 2
BenMUC is on a distinguished road
This is what he told me a few days ago in my thread, maybe it's helpful for you as well:

Quote:
Originally Posted by ghorrocks View Post
A basic mesh sensitivity analysis is:
1) Do a simulation
2) generate a new mesh which is significantly finer. Halving the element edge length is a good guide.
3) Run the simulation
4) Compare the results of 1) and 3). Look at the parameter of interest to you (flow rate, pressure drop, peak pressure, whatever).
5) Are the two simulations close enough to be within an accuracy tolerance you accept for your application? If yes then your mesh is OK. If no then go to step 2) and generate a new mesh which is even finer again.

This is a crude, simple mesh sensitivity analysis. More sophisticated approaches are described in "Computational Fluid Dynamics" by Roache, and summarised in this paper: http://journaltool.asme.org/Template...umAccuracy.pdf
BenMUC is offline   Reply With Quote

Old   January 18, 2014, 12:45
Default
  #7
New Member
 
Join Date: May 2013
Posts: 7
Rep Power: 3
Queiroz is on a distinguished road
Dear BenMUC,

thanks for you answer. I'm gonna try what you and Mr. Ghorrocks told me. If it does not work (the whole stuff), I will let you know.

At the meantime, I'm running two simulations, just changed the turbulence models from k-omega SST to SSG Reynolds Stress and BSL EARSM.

Thanks,

Matheus
Queiroz is offline   Reply With Quote

Old   November 27, 2014, 13:55
Default
  #8
New Member
 
Join Date: May 2013
Posts: 7
Rep Power: 3
Queiroz is on a distinguished road
Too many simulations ran and too many problems.

Hi guys,

I'm still carrying out simulation for my Ph.D. research. The objetive is to well describe a separated and reattached flow generated by the adverse to favorable pressure gradients, acting in the upper wall of a wind tunnel.

After some good suggestions, I changed the turbulence model employed from SST to RSM and EARSM. As a result, I found that the flow in the upper wall was better described, but not ideally showing what I wanted to see.

The separation line and also the reattachment line were, under and over predicted, respectively, showing a separation bubble length bigger than it should be. I'm comparing simulations with experimental results from the wind tunnel I'm modelling.

I have some questions concerning the validity of what I've done:

Is there some flow problems that can't be described by a specific kind of mesh? I mean, when I was using hybrid meshes, generated in ICEM CFD and using RSM or EARSM model I "easily" got good flow patterns at the upper wall, but the velocity profiles upstream of separation were not good. When I changed the mesh to unstructured hexahedra, also in ICEM CFD, for 2D simulations, I got very good velocity profiles upstream of separation, boundary layer thickness, momentum thickness and displacement thickness. So I transformed this "2D" mesh into a 3D one, just changing the number of nodes in the Z-direction. The resulted flow pattern was quite wrong and not axisymmetric. The y+ value was 0.52.

I've attached some pictures, so you can see what I got. They're the results for hexahedra unstructured mesh. The values for y+, as seen, are equal or too close, what I change was just the number of nodes in the Z-direction, using "bigeometric as bunching law". For the first pictures, the number of nodes were 130 with a total number of mesh nodes of 4.8 M, the second picture 260 nodes in Z-direction with a total number of mesh nodes of approximately 6 M and the third one with 65 nodes in Z-direction with a total number of mesh nodes of 1.5 M.

The experimental result is provided up in this thread.

Note that for the second and third pics, the flow does not separate.

Thanks.
Queiroz is offline   Reply With Quote

Old   November 27, 2014, 18:27
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,775
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If your results are highly sensitive to mesh settings then:
* You might have a mesh which is too coarse. Have you done the mesh refinement study posted above?
* You might be using wall functions which do not converge on mesh refinement - in this case you cannot achieve mesh convergence and you need to consider the applicability of the wall boundary approach you are using
* You might be coming across the well-known deficiencies of RSM turbulence models in modelling separations and reattachments in adverse pressure gradients. There is plenty of literature on this topic.
ghorrocks 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
air flow in a tunnel Tariq Feroze FLUENT 9 January 4, 2014 04:16
Coupled VOF and Multiphase Segregated Flow for a gas bubble problem?? EnronZhang STAR-CCM+ 1 December 19, 2013 09:41
Simulation of air flow inside valve - FSI? Help! farianka Main CFD Forum 0 April 17, 2011 17:30
Modelling a bubble flow ina microchannel Aritra Sur FLUENT 0 April 25, 2008 12:19
Flow visualization vs. Calculated flow patterns Francisco Saldarriaga Main CFD Forum 1 August 3, 1999 00:18


All times are GMT -4. The time now is 03:27.