Judging onset of turbulence. Reynolds #? TKE?

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

 February 5, 2020, 13:32 Judging onset of turbulence. Reynolds #? TKE? #1 New Member   Chris Bailey Join Date: Dec 2019 Posts: 16 Rep Power: 6 How can you judge whether any turbulence would occur, if you have Reynolds or Rayleigh number available, or TKE (turbulent kinetic energy)? I'm analyzing boxes of dimensions like 50 to 200 mm, full of air, with a heater inside. The heater generates some buoyant advection but typically I think a smooth gentle turnover. I'd like to know if it ever gets into the turbulent regime. In a parametric study of 240 designs I got the following results for the location where air velocity is highest: Reynolds number: median value, 23. Maximum value, 1406. Rayleigh number: median value 1.8e3, max 1.6e6. TKE: median value 1.3e-6 J/kg, max 2e-3 J/kg The highest velocities are below 0.2 m/s. Can I count on flow remaining steady? Is there an easy diagnostic to apply? Could I be barely venturing into turbulence here? There are out there on the web numerous statements about Reynolds number ranges for turbulence, including many that just say 2300 minimum. But I think I've seen numbers as low as 1000 stated for possible turbulence. And, yes, I've read at least some of what the person I'm not has said on the subject. Thank you!

February 5, 2020, 14:04
#2
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,793
Rep Power: 71
Quote:
 Originally Posted by NotOsborneReynolds How can you judge whether any turbulence would occur, if you have Reynolds or Rayleigh number available, or TKE (turbulent kinetic energy)? I'm analyzing boxes of dimensions like 50 to 200 mm, full of air, with a heater inside. The heater generates some buoyant advection but typically I think a smooth gentle turnover. I'd like to know if it ever gets into the turbulent regime. In a parametric study of 240 designs I got the following results for the location where air velocity is highest: Reynolds number: median value, 23. Maximum value, 1406. Rayleigh number: median value 1.8e3, max 1.6e6. TKE: median value 1.3e-6 J/kg, max 2e-3 J/kg The highest velocities are below 0.2 m/s. Can I count on flow remaining steady? Is there an easy diagnostic to apply? Could I be barely venturing into turbulence here? There are out there on the web numerous statements about Reynolds number ranges for turbulence, including many that just say 2300 minimum. But I think I've seen numbers as low as 1000 stated for possible turbulence. And, yes, I've read at least some of what the person I'm not has said on the subject. Thank you!

Unfortunately the answer is that you cannot say much only from the Re number. The numerical value depends on the chosen lenght and velocity but it differently relies on channel/pipe/open flow.
Some references are present in literature for the heat-driven cavity.

I would suggest starting from your 3D geometry, simulating the unsteady flow without any turbulence model assumptions and check if you get a steady state. Of course a quite fine grid is required.

February 5, 2020, 16:24
#3
New Member

Chris Bailey
Join Date: Dec 2019
Posts: 16
Rep Power: 6
Quote:
 Originally Posted by FMDenaro Unfortunately the answer is that you cannot say much only from the Re number. The numerical value depends on the chosen lenght and velocity but it differently relies on channel/pipe/open flow. Some references are present in literature for the heat-driven cavity. I would suggest starting from your 3D geometry, simulating the unsteady flow without any turbulence model assumptions and check if you get a steady state. Of course a quite fine grid is required.
Thanks. Taking your advice I've tried a model with my worst-case parameters except I made the vertical height 7 times my worst-case value, and tried it with no turbulence model. It would not settle down. Model residuals remained high, bounced around a little, and had no long term improvement over hundreds of iterations after maybe the first 300. This, I guess, has strayed into mild turbulence. Then I repeated at 3.5 times my worst-case height, which did kinda sorta settle into a stable state, or at least flow lines not moving around much. This, I guess, is near the onset, and I can find the transition by trial and error.

But, a quite fine grid? Currently I have about 25 cells along the smallest dimension of my volume in the smaller height case. Do you mean finer than that? Is there a better way of choosing grid size than trial and error here?

Thank you! I do appreciate it.

February 5, 2020, 16:37
#4
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,793
Rep Power: 71
Quote:
 Originally Posted by NotOsborneReynolds Thanks. Taking your advice I've tried a model with my worst-case parameters except I made the vertical height 7 times my worst-case value, and tried it with no turbulence model. It would not settle down. Model residuals remained high, bounced around a little, and had no long term improvement over hundreds of iterations after maybe the first 300. This, I guess, has strayed into mild turbulence. Then I repeated at 3.5 times my worst-case height, which did kinda sorta settle into a stable state, or at least flow lines not moving around much. This, I guess, is near the onset, and I can find the transition by trial and error. But, a quite fine grid? Currently I have about 25 cells along the smallest dimension of my volume in the smaller height case. Do you mean finer than that? Is there a better way of choosing grid size than trial and error here? Thank you! I do appreciate it.

First, you need to use at least a second order accurate method in time and space. What method are you using now?

Then, a general rule to guarantee a sufficient resolution of the grid is to ensure a Reynolds cell number = O(1). In a buoyancy-driven case, the Re number is substitute by the Rayleigh number. For smooth laminar flow a grid with O(10^6) nodes should be sufficient to get a good solution at moderate Re/Ra number.

Convergence to a steady state must be controlled by evaluating that the time derivatives are everywhere enough small. I suggest to evaluate the total kinetic energy in time to see if you reach an equilibrium state.

To simplify your check, consider also some simple 2D test-case used in literature https://www.researchgate.net/publica...sport_problems

February 5, 2020, 17:32
#5
New Member

Chris Bailey
Join Date: Dec 2019
Posts: 16
Rep Power: 6
Quote:
 Originally Posted by FMDenaro First, you need to use at least a second order accurate method in time and space. What method are you using now? Then, a general rule to guarantee a sufficient resolution of the grid is to ensure a Reynolds cell number = O(1). In a buoyancy-driven case, the Re number is substitute by the Rayleigh number. For smooth laminar flow a grid with O(10^6) nodes should be sufficient to get a good solution at moderate Re/Ra number. Convergence to a steady state must be controlled by evaluating that the time derivatives are everywhere enough small. I suggest to evaluate the total kinetic energy in time to see if you reach an equilibrium state. To simplify your check, consider also some simple 2D test-case used in literature https://www.researchgate.net/publica...sport_problems
I beg you to forgive my ignorance. You've taken the trouble to give me a most thoughtful answer and yet I do not understand the term "Reynolds cell number" or the notation "O(1)" or "O(10^6)", and web searching and my one text book do not enlighten me. Perhaps this is a reference to the "order function"?

I don't ask you to explain these things. I would only ask if you would just give me more clues, perhaps search terms, so that I can find the explanations myself. But of course if you wish to explain, I would not object!

As to the comment "you need to use at least a second order accurate method in time and space", I understand this to mean how many continuous orders of differentiation there are in the interpolations used, in other words the order of spline. I have not found this out but presume I can. At present I'm solving this as a steady state problem and looking for convergence, rather than solving in the time domain also. Thus it is only interpolating in space.

Thank you for your help, and again I apologize for my early state of knowledge.

February 5, 2020, 17:40
#6
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,793
Rep Power: 71
Quote:
 Originally Posted by NotOsborneReynolds I beg you to forgive my ignorance. You've taken the trouble to give me a most thoughtful answer and yet I do not understand the term "Reynolds cell number" or the notation "O(1)" or "O(10^6)", and web searching and my one text book do not enlighten me. Perhaps this is a reference to the "order function"? I don't ask you to explain these things. I would only ask if you would just give me more clues, perhaps search terms, so that I can find the explanations myself. But of course if you wish to explain, I would not object! As to the comment "you need to use at least a second order accurate method in time and space", I understand this to mean how many continuous orders of differentiation there are in the interpolations used, in other words the order of spline. I have not found this out but presume I can. At present I'm solving this as a steady state problem and looking for convergence, rather than solving in the time domain also. Thus it is only interpolating in space. Thank you for your help, and again I apologize for my early state of knowledge.

It appears quite difficult to help if you have no background in CFD. However,
- "O()" stands for order of magnitude;
- the global order of accuracy of the method is not the degree of the interpolant;
- the cell Re number is the Reynolds number computed using the mesh size.

What CFD textobook are you using?

February 5, 2020, 18:01
#7
New Member

Chris Bailey
Join Date: Dec 2019
Posts: 16
Rep Power: 6
Quote:
 Originally Posted by FMDenaro It appears quite difficult to help if you have no background in CFD. However, - "O()" stands for order of magnitude; - the global order of accuracy of the method is not the degree of the interpolant; - the cell Re number is the Reynolds number computed using the mesh size. What CFD textobook are you using?
Ah. Well, since I have in my worst real case 60 mm height and 5 mm cells, the cell Reynolds numbers would be 120/5 = 24 times smaller than the 23 and 1406 median and maximum I reported at first, because it was 2*height I based those Reynolds numbers on. About 1 and 59, then.

60,000 cells.

If I substitute Rayleigh for Reynolds the numbers become about 60 times bigger, about 60 and 3600.

My textbook is "Computational Fluid Dynamics" by John Anderson Jr., a 1995 text. Perhaps I should update? My background is in physics and I started this cfd effort this past November. Any suggestions?

I'm doing my work in STAR-CCM+ but I think my questions here aren't dependent on software, unless perhaps this software uses different specific names for the same parameters.

February 5, 2020, 18:10
#8
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,793
Rep Power: 71
Quote:
 Originally Posted by NotOsborneReynolds Ah. Well, since I have in my worst real case 60 mm height and 5 mm cells, the cell Reynolds numbers would be 120/5 = 24 times smaller than the 23 and 1406 median and maximum I reported at first, because it was 2*height I based those Reynolds numbers on. About 1 and 59, then. 60,000 cells. If I substitute Rayleigh for Reynolds the numbers become about 60 times bigger, about 60 and 3600. My textbook is "Computational Fluid Dynamics" by John Anderson Jr., a 1995 text. Perhaps I should update? My background is in physics and I started this cfd effort this past November. Any suggestions? I'm doing my work in STAR-CCM+ but I think my questions here aren't dependent on software, unless perhaps this software uses different specific names for the same parameters.

Anderson is a good textbook to start learning CFD at a basic level.
Have also a look to the textbook of Ferziger & Peric.

Be careful that if you want to study the onset of the transition in your specific case you need to simulate the 3D problem.

 February 21, 2020, 04:45 #9 New Member   Sen Wang Join Date: Jul 2018 Location: Singapore / Notre Dame, U.S. Posts: 19 Blog Entries: 1 Rep Power: 7 Hi there, Trying to answer your initial question on identifying the onset of turbulence, we should probably go back to the definition of turbulence. Reynolds number is a dimensionless number through scaling the Navier-Stokes equation, which tells you the ratio of convection vs molecular diffusion of the flow. For large Reynolds number, what it essentially says is that this is a convection-dominated flow. Now in terms of how to identify onset of turbulence, I would suggest that you can look into the follow measures: 1. Turbulent kinetic energy: Measuring the energy of turbulent eddies, which is a direct measurement. 2. Reynolds stress: This can be used in two ways. First one is you can compare the value of Reynolds stress to velocity gradients, which gives you the ratio of turbulent diffusion vs molecular diffusion. Second one is you can calculate reynolds stress multiplied by velocity gradients, which gives you the turbulence kinetic energy production value. As you can imaging, the production term will go up preceding the TKE going up, which can give you an earlier indication. There are quite a lot of content in this topic so I have to omit some supporting content. Let me know if you are interested for more.

 Tags rayleigh, reynolds, turbulence