
[Sponsors] 
what is the Raynolds number for the transition from laminar to turtulent 

LinkBack  Thread Tools  Display Modes 
February 21, 2012, 03:14 
what is the Raynolds number for the transition from laminar to turtulent

#1 
New Member
Sivan NatanKnaz
Join Date: Jul 2011
Posts: 7
Rep Power: 6 
For HVAC systems.
Can I assume that 30000 is still a laminar flow? thanks Sivan 

February 21, 2012, 08:36 

#3 
New Member
Sivan NatanKnaz
Join Date: Jul 2011
Posts: 7
Rep Power: 6 
this is not a pipe but a large room with air flow


February 21, 2012, 11:55 

#4 
New Member
Chris
Join Date: Jan 2012
Location: St. Louis
Posts: 14
Rep Power: 5 
You need a fundamental length scale to define the Reynold's Number... I'm going to guess that you're modeling an HVAC duct discharge into a room and the Reynold's number you're asking about is based on the hydraulic diameter of the air duct.
If that's the case, you're probably dealing with a free shear flow of a highspeed jet entering a control volume. Last time I was in school, this was defined as a constant momentun flux flow that can be characterized by Similarity Analysis, and the behavior may not be readily described by the Reynolds number alone. http://www.cfdonline.com/Wiki/Intro...nt_shear_flows To answer your question; I doubt you can assume the flow is laminar. 

February 21, 2012, 14:52 

#5 
New Member
Sivan NatanKnaz
Join Date: Jul 2011
Posts: 7
Rep Power: 6 
the simulation is of a clean room that air enters the room through filters from the ceiling. the velocity is very low and close to 0.1 m/s. the air is sucked from holes in the floating floor. the size of the room are 60x20x4 meters (4 is the height of the room).
the question was raised because I use FLOVENT for simulation and I can choose Laminar solver or turbulent (Ke) one. SO , in order to calculate the Raynolds number near the walls I just took a velocity close to 0.1 m/s and the hieght of the room. the resulted Raynolds was 80000 which, a turulance expert told me, is in the transition region. what I actualy did is , I solved first as laminar, and then as turtulent and compared the speed. I saw that there were small differences in the relevant locations in the room , so I decided to keep it laminar, but I am not sure I did right. Sivan 

February 21, 2012, 17:44 

#6 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9 
In general, I would say a RANS solver is inappropriate for this type of flow.


February 21, 2012, 18:00 

#7 
Senior Member
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 8 
Heat transfer is a higly turbulencedependant phenomenon. even if your speeds are similar in your locations of choiche (i'd guess away from the walls) the temperature might not be.
also the lenghtt for defining the Reynolds Number is in part arbitrary. are you shure that the height of the room can be taken as a refence value? 

February 21, 2012, 19:10 

#8 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9 
OK, I'm going to rock the boat and say the term "turbulence" is misleading. Instead, lets use the term eddies.
In general, a RANS solver is inappropriate for flow dominated by large eddies. It also sounds like the flow being model is not that dependent on small eddies, at least outside the area of the exhaust and intake. In general, a laminar NS solver does not mean one does not have "turbulence", i.e. eddies. It only means one is interested in modeling the eddies, i.e. the eddies are not averaged out. After all, a laminar NS solver is a DNS solver. Of course wall functions fuzzy up this definition. But, using a laminar NS solver does not necessarily mean one is using a laminar wall function or any wall function at all. IMO, the traditional usage of the term laminar and turbulent is only appropriate slightly off the wall. All flow is linear, i.e. laminar, right against the wall. Regardless of whether it is turbulent or laminar slightly off the wall. Personally, I do not believe the flow mentioned here will have a turbulent region slightly off the wall where the eddies will need to be averaged. Since, I believe, at this flow rate, the boundary layer on the room walls will be thick. So, IMO, flow slightly off the wall should be categorized by laminar or turbulent. Flow further off the surface should be categorized by the size of the eddies. Therefore, this room will have a laminar wall boundary layer with large eddies throughout the room and smaller eddies by the exhaust and intake. 

February 22, 2012, 04:06 

#9  
Senior Member

Quote:
If you just solving NS with laminar air coming uniformly from the intake, then your model does not play role: at this Reynolds number the thikness of boundary layer along the wall is of order of centimiters, no matter if it is laminar or turbulent, so you will not get any difference as dimensions of your room are order of meters (this problem similar to that for the flow in the wind tunnel, where flow is laminar at much more bigger reynolds numbers). If you considering mass/heat transfer effects due to temperature gradients, or turbulent or nonuniform air entering the intake, then the situation might be different Which boundary conditions are you using at inlet and outlet? 

February 22, 2012, 04:48 

#10 
New Member
Sivan NatanKnaz
Join Date: Jul 2011
Posts: 7
Rep Power: 6 
there are also heat flux defined at the side walls of the room , so this is a couple analysis with mass and heat transfer.
until now I dont understant what is the right way of solving this problem. I have an HVAC software, and I can only play with the solver type. Can I have a good prediction with an NS laminar solver or the Ke solver? what should I take? what is the process of solving such a problem? thanks Sivan 

February 22, 2012, 05:10 

#11 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,651
Rep Power: 23 
for heat flux you need to manage several phoenomena ... Re number is indicating only one, perhaps you need to see if buoyancy effects can be important. I think the the problem you want to solve possess all characteristic scales going (locally) from laminar to transition to turbulence... and this is the normal situation you encounter in real flows ...
I suggest to use URANS or LES formulations 

February 22, 2012, 05:18 

#12 
New Member
Sivan NatanKnaz
Join Date: Jul 2011
Posts: 7
Rep Power: 6 
what is the difference between URANS and RANS?


February 22, 2012, 05:40 

#13 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,651
Rep Power: 23 
the difference is in the statistical average you use... in RANS you get statistically steady flows, in URANS you have statistically unsteady flows. Of courses the turbulence model is different... I suggest the reading of
Wilcox  Turbulence Modeling for CFD 

February 22, 2012, 13:57 

#14  
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9 
Quote:
BTW, if possible, could you show one of the eddy viscosity plots. I would be curious to see it. I also am assuming that you are modeling buoyancy. What's your Re based on the diameter of the inlet? How many inlets do you have and what is the ratio of the sum of all the inlet areas to the room floor area (i.e. (sum of inlets)/(60x20)) Also, very important, how are you determining the velocity profile of the air entering the room? You mentioned filters, so I assume the flow is turbulent but how do you determine the velocity profile, eddy viscosity, and k coming in is beyond me. I gather the outlet is a bunch of small holes in the floor panels. I also am assuming that the only reason you are calculating Re is to choose between laminar and turbulent solver. Also, is your calculated flow steady or unsteady? I'm assuming it is unsteady for the laminar solver. I'm not sure what the RANS solver will do. Did you try refining your grid for the laminar case? BTW, are you using wall functions? I don't think they are appropriate here, but considering you mentioned HVAC system and ke model, there is a chance you are. You are also modeling a clean room. The room is going to have machines in it. I assume this will significantly change the air flow. The machines may even have air specifically directed/transported to them. I assume you are not modeling the machines yet, since you did not mention them. So I assume you are looking for qualitative rather than quantitative results. 

February 22, 2012, 21:21 

#15 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 467
Rep Power: 9 
OK, I'm going to show my ignorance, but is FLOVENT time accurate?
I went to the web page and data sheet says "The conjugate nature of heat transfer is concurrently solved using a preconditioned conjugate residual solver together with a flexible cycle multigrid solution technique." As far as I know, multigrid methods are not time accurate unless they are used with some sort of sub iteration approach. This almost sounds like a steady state solver? Is a "preconditioned conjugate residual solver" time accurate? I'm assuming that it is not used in a time accurate sub iteration approach. Though I could be wrong. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Specifying the laminar to turbulent transition location  sylvester  OpenFOAM Running, Solving & CFD  1  May 15, 2010 11:07 
air bubble is disappear increasing time using vof  xujjun  CFX  9  June 9, 2009 07:59 
Transition from laminar to turbulence  Devang  CFX  2  June 24, 2008 02:27 
Smooth Grid Error! Help  seasoul  FLUENT  1  March 24, 2008 11:56 
Transition from laminar to turbulent flow  BJ  Main CFD Forum  2  December 19, 2003 11:39 