[Khaza]

Hi Everyone.

I have problem in simulating unsteady flow around a super tall building (300 m ). The main problem is the building is like a tower .See the image in attachment. I am using Ansys fluent 16.0 and I used the Hexmeshing and got the skewness for body mesh as 0.849 (acceptable). I am fine upto this.

The Real problem comes in Solving part. I mean what reynolds number I should use for this building(Please note that it is not like a cylinder problem where u just choose reynolds number for whole geometry) ? How do I choose reynolds number at different parts of my geometry( I have 70m diameter cylinder at bottom and 15 m all the top and then sphere of 25m dia at the very top)?

My domain size in mesh is ( 1750m from inlet to building, 5250m from building to outlet ,2100m from building to top ) . I defined inlet,oulet,and wall functions for topsurface,ground and building in my domain.

Please help me with following questions?

1. What reynolds no. should I use for different parts of my model and how should I apply as a whole?

2.What model should I use ( Laminar or (turbulence since I have super tall building and large domain )?

3.what courant number Should I use?

4.I am defining wind profile by own ,will it create any problems?

5.I can calcaulate timestep once I calculate strouhal number. but again I need Reynolds number to calculate strouhal .

Please help me if I miss any significant step in my modelling process.

Thanks a lot in advance.

[Quek]

Hi,

I having problem for my meshing. Can I take a look at your meshing? I'm too doing airflow around tall buildings. For me i using existing results to compare see whether my Cd or Cl values are at the correct range. I using Re = 20 which gives me velocity, v, of 0.00029m/s.

[FMDenaro]

The Reynolds number that characterizes your problem depends on the lenght you want to use but does not change the physics of your problem. Aren't working with dimensional variable in Fluent?

I am quite sure you have a turbulent problem, you should think that over a real building the flow coming on is itself alreay in turbulent condition. Actually, one of the problems is in defining a suitable inlet condition.

What formulation you want to use, URANS?

[Quek]

I will be using RANS, k-espilon

[FMDenaro]

But the title of the post is "unsteady"

[Quek]

Originally Posted by FMDenaro

The Reynolds number that characterizes your problem depends on the lenght you want to use but does not change the physics of your problem. Aren't working with dimensional variable in Fluent?

I am quite sure you have a turbulent problem, you should think that over a real building the flow coming on is itself alreay in turbulent condition. Actually, one of the problems is in defining a suitable inlet condition.

What formulation you want to use, URANS?

Originally Posted by FMDenaro

But the title of the post is "unsteady"

Sorry mine is a different topic from this person post. Im just going around asking for help regards of RANS.

[Khaza]

Originally Posted by FMDenaro

The Reynolds number that characterizes your problem depends on the lenght you want to use but does not change the physics of your problem. Aren't working with dimensional variable in Fluent?

I am quite sure you have a turbulent problem, you should think that over a real building the flow coming on is itself alreay in turbulent condition. Actually, one of the problems is in defining a suitable inlet condition.

What formulation you want to use, URANS?

Hey! Thanks for the reply. Yeah Re Depends on characteristic length. But my problem here is ( Re = rho * v* D / Mu) . If you see the formula , my D value varies along the building since it is not cylinder all the way or it is not rectangle all the way. It is a tower whose diameter is varying along its height. Then how to take reynolds number? Let say if I assume (Re for Laminar flow as 150) ,then I will get different viscosity values from different diameter values. How should I input all viscosity values (Since one option to adjust Re is changing viscosity for fluid(air) Property.

I hope you understand my problem.

and What do you mean defining suitable inlet condition? I defined velocity inlet condition after finishing mesh part?

Thanks in advance

[FMDenaro]

Viscosity has one value for air!
You can use the height of the tower as characteristic lenght or an average diameter of the tower, no matter about the physics of the problem.


As the inflow is concerned, You must prescribe a suitable BL- based profile

[Khaza]

Originally Posted by FMDenaro

Viscosity has one value for air!
You can use the height of the tower as characteristic lenght or an average diameter of the tower, no matter about the physics of the problem.


As the inflow is concerned, You must prescribe a suitable BL- based profile

Do you mean I should take the height of tower - 300 m as characteristic length and calculate the viscosity value? Not Clear again

Let say Re = (rho * v*d )/ u => u = rho*v*d / Re => ( 1.225 * 64.4479*300m/(what is Re value here)) . Then I will get u value very high (whats the meaning of it)

Please clear my doubts. If possible can u write it down on a paper and paste it here. Thanks so much !

Yes I defined ABL (Atmospheric boundary layer profile) while solving.

[FMDenaro]

the viscosity for the air is a thermodinamic property

http://www.engineeringtoolbox.com/dr...ies-d_973.html

the dimension of the tower is known, therefore, if you know the characteristic velocity you compute the Re number (and viceversa)

[flotus1]

There are two possibilities here:
1) You are trying to re-create some measurement or simulation with a specific Reynolds number. In this case, use the same characteristic length that was used there.
2) You are doing your own simulation: In this case the physical parameters should be fixed (velocity, density, viscosity) and you can define whatever characteristic length you want. It will change the Reynolds number, but it will not change the flow.

@Quek: Start your own thread and stop posting here. Hijacking other peoples threads is generally considered rude.

[adrin]

I second Alex with his response. Khaza, with due respect, your difficulty at this stage is not with CFD but with understanding the very basics of fluid dynamics. The Reynolds number is a parameter that forms after the Navier Stokes is non-dimensionalized using the kinematic viscosity of the fluid, and (key point) _arbitrary_ reference values of U and D. Whereas the kinematic viscosity is dictated by the fluid itself (you have zero control over it), the choices for U and D are entirely up to you. As others have mentioned, this choice will _not_ affect the flow physics. Having said that, one has to select _representative_ values of U and D so that one can make sense out of the results and/or even be able to set up the CFD simulation properly. In your case, the best U would be the peak free stream velocity (if it is unsteady), and the best D would be the largest width that is "normal" to the incoming flow (think of a long cylinder; D is still the diameter and not the cylinder length, because flow physics is determined primarily by D).

Since you have an unsteady flow, depending on the frequency of unsteadiness and depending on what it is that you're trying to accomplish (which dictates the accuracy of your unsteady simulation; i.e., tilmestep size), you also have the option to use a typical T (time) for non-dimensionalization. Note that given a U and D, your T is fixed via T = D/U (so you don't have control over it). But, you could use, say, D and T for non-dimensionalization, in which case your U would be D/T. In such a scenario, your Reynolds number would be D^2/T.nu. Again, it all depends on what you're trying to accomplish.

In the case of your tall building, the flow is fully turbulent, so the choice of D will be relatively irrelevant. The problem is with multi-regime flows where regions of laminar, transitional, and turbulent flow may coexist. In this case, the choice for non-dimensionalization becomes critical, and, anyway, traditional turbulence models would be useless. But, you don't have this problem.

One last but crucial comment. Making a statement such as "the Reynolds number of a flow is, say, 1000" is absolutely meaningless, even for simple geometries like a circular cylinder. One has to ALWAYS accompany that statement with a clarification of the references used. That is, the correct statement would be "the Reynolds number based on the, say, base of the building and the peak free stream velocity is 1000".

adrin

[Khaza]

Originally Posted by adrin

I second Alex with his response. Khaza, with due respect, your difficulty at this stage is not with CFD but with understanding the very basics of fluid dynamics. The Reynolds number is a parameter that forms after the Navier Stokes is non-dimensionalized using the kinematic viscosity of the fluid, and (key point) _arbitrary_ reference values of U and D. Whereas the kinematic viscosity is dictated by the fluid itself (you have zero control over it), the choices for U and D are entirely up to you. As others have mentioned, this choice will _not_ affect the flow physics. Having said that, one has to select _representative_ values of U and D so that one can make sense out of the results and/or even be able to set up the CFD simulation properly. In your case, the best U would be the peak free stream velocity (if it is unsteady), and the best D would be the largest width that is "normal" to the incoming flow (think of a long cylinder; D is still the diameter and not the cylinder length, because flow physics is determined primarily by D).

Since you have an unsteady flow, depending on the frequency of unsteadiness and depending on what it is that you're trying to accomplish (which dictates the accuracy of your unsteady simulation; i.e., tilmestep size), you also have the option to use a typical T (time) for non-dimensionalization. Note that given a U and D, your T is fixed via T = D/U (so you don't have control over it). But, you could use, say, D and T for non-dimensionalization, in which case your U would be D/T. In such a scenario, your Reynolds number would be D^2/T.nu. Again, it all depends on what you're trying to accomplish.

In the case of your tall building, the flow is fully turbulent, so the choice of D will be relatively irrelevant. The problem is with multi-regime flows where regions of laminar, transitional, and turbulent flow may coexist. In this case, the choice for non-dimensionalization becomes critical, and, anyway, traditional turbulence models would be useless. But, you don't have this problem.

One last but crucial comment. Making a statement such as "the Reynolds number of a flow is, say, 1000" is absolutely meaningless, even for simple geometries like a circular cylinder. One has to ALWAYS accompany that statement with a clarification of the references used. That is, the correct statement would be "the Reynolds number based on the, say, base of the building and the peak free stream velocity is 1000".

adrin

Thanks adrin for your comment. I will keep all points in mind and will get back to you soon.

[adrin]

Just a correction: I said "the best D would be the largest width that is "normal" to the incoming flow (think of a long cylinder; D is still the diameter and not the cylinder length, because flow physics is determined primarily by D)"

In 3-D there would be two "normals" to the free stream. So, what I said above is confusing or even misleading. The more correct answer would have been to consider the physics of the problem. If you have a bluff body (like your building) the relevant dimension is the one that causes (dominant) flow separation, vortex shedding, and unsteady wake behind the body. If you have a finite-span bluff body, the _shorter_ side of the plane normal to the free stream would be the more relevant dimension; it's because the longer dimension affects the flow primarily at the ends (it's a secondary, 3-D effect).

Viewed differently, ask yourself the question, if you were to cut any of the three sides of the body at its plane of symmetry with a 2D plane, which 2-D flow in one of these 2D planes would provide you a first-guess estimate of the whole 3-D flow? That 2D plane is the relevant plane for you, and now the side in that plane that is normal to the free stream is the relevant non-dimensionalization parameter.

I hope I made sense to you.

adrin

[Khaza]

Originally Posted by adrin

Just a correction: I said "the best D would be the largest width that is "normal" to the incoming flow (think of a long cylinder; D is still the diameter and not the cylinder length, because flow physics is determined primarily by D)"

In 3-D there would be two "normals" to the free stream. So, what I said above is confusing or even misleading. The more correct answer would have been to consider the physics of the problem. If you have a bluff body (like your building) the relevant dimension is the one that causes (dominant) flow separation, vortex shedding, and unsteady wake behind the body. If you have a finite-span bluff body, the _shorter_ side of the plane normal to the free stream would be the more relevant dimension; it's because the longer dimension affects the flow primarily at the ends (it's a secondary, 3-D effect).

Viewed differently, ask yourself the question, if you were to cut any of the three sides of the body at its plane of symmetry with a 2D plane, which 2-D flow in one of these 2D planes would provide you a first-guess estimate of the whole 3-D flow? That 2D plane is the relevant plane for you, and now the side in that plane that is normal to the free stream is the relevant non-dimensionalization parameter.

I hope I made sense to you.

adrin

Thanks for all the info! I have roughly drawn and attached here. Please see it .

[adrin]

The average kinematic viscosity of (dry) air is roughly 1.6E-5 m^2/s. So, Re based on your suggested U~65m/s and D~75m is Re ~ 3.1E8. Of course, you realize that all your dimensions should now be normalized by D=75 and your inlet velocity should be normalized by U~65.

D=75m is all good and acceptable, and it also helps decide on your grid sizes (it's always easier to work in normalized units where the maximum value is 1). But since you are interested in vortex shedding properties, the relevant geometry in this case is the "cylinder" in your tower. So, I would personally choose D=15m for your particular problem. With this choice your Strouhal number would correspond to that of a 2D cylinder more closely (that's just a hunch). By the way, the Re vs St relationship you show in your right-up is most probably irrelevant to your most complex geometry.

I have to add here that going from a steady computation to transient is a smart step. However, very tall buildings are (hopefully) non-rigid and probably sway by quite large deflections in response to gusts. So, if you have the computational resources (both software and hardware) I would urge you to view this as a Fluid-Structure Interaction problem. I am sure the results will be quite different compared to a rigid building. You can/should start with a rigid body as a matter of good science (and for benchmarking), but should then move to FSI.

adrin