what is the Raynolds number for the transition from laminar to turtulent
 

For HVAC systems.
Can I assume that 30000 is still a laminar flow?
thanks
Sivan :D

Transition in a pipe happens at approximately 3*10^3

this is not a pipe but a large room with air flow

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 high-speed 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.cfd-online.com/Wiki/Intro...nt_shear_flows

To answer your question; I doubt you can assume the flow is laminar.

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 (K-e) 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

In general, I would say a RANS solver is inappropriate for this type of flow.

Heat transfer is a higly turbulence-dependant 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?

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.

Are you just solving NS equations with laminar air coming uniformly from the inlet, or considering nonuniform flow from the inlet or the heat/mass transfer due to temperature differences in the room as well?

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?

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 K-e solver?
what should I take?
what is the process of solving such a problem?

thanks
Sivan

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

what is the difference between URANS and RANS?

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

I gather you already solved for a laminar and turbulent case. The RANS equations differ from the laminar NS equations by a term that is a function of eddy viscosity (nu_t) and the turbulence kinetic energy (k). These two values are picked up from the turbulence model. I believe the eddy viscosity is the dominant term. I know the Spalart Allmaras model, which neglects the turbulence kinetic energy seems to do OK. So, I suggest plotting the eddy viscosity for the turbulent case. Hopefully your code allows it. In the areas that the eddy viscosity is much less than the molecular (which is sometimes called the laminar) viscosity the equations are basically the laminar NS equations. Sometimes the eddy viscosity will be non-dimensionalized by molecular viscosity, in which case the eddy viscosity should be compared to 1.0. Take a look at the eddy viscosity next to the wall and take a look at the eddy viscosity in the vicinity of the inlets. You can also take a look at the turbulence kinetic energy. But I don't know what constitutes a small value.

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 k-e 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.

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 multi-grid solution technique." As far as I know, multi-grid 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.