Greetings, I'm running a CFD model of an entire wind tunnel. The solution converges but my velocity profiles are not comparable to experiment.

I have B.C's for all the walls as inviscid, the floor as viscid , the inlet prssure condition and outlet pressure condition.

Any suggestions?

(1). What do you mean by the "entire wind tunnel"?

By entire wind tunnel I mean the exact geometry from entrance cone to exit cone (200 ft long).

(1). So, it is not a closed loop wind tunnel. (2). And the entrance cone must be the air inlet. The exit cone must be the air outlet. (3). Hopefully, there is a large fan or compressor somewhere. And a test section in between? (4). Or it could be a blow-down wind tunnel, with pressure supply at the inlet? (5). Anyway, the internal flow, such as the flow in a long duct of varying area, is sensitive to the boundary layer development. The displacement effect will affect directly the centerline velocity and the wall pressure distribution. (because it is internal flow, and mass has to be conserved) (6). So, there are two problems: (a). the boundary layer has to be included at the wall, and the displacement effect is always there, (b). if there is area change, like diffuser,etc. then the turbulence model must be able to handle the adverse pressure gradient accurately.(which has been difficult in the past) This affects the boundary layer thickness in the adverse pressure gradient flow field, which in turn affect the centerline or the wall pressure distribution.

Thank you. I did consider that my turbulence models would have to be tweaked. My problem is in the boundary layer thickness about 6" from the flow. I'm getting fresstream velocities way to close to the floor.

(1). you will have to say more about your wind tunnel geometry first before we can help you locate the problem. This is because there are many different types of wind tunnel in operation.

It's a sub-sonic wind tunnel with a 7x10 test section. It has an entrance cone that elliptically smooths to a test section to a diffuser section.

I have boundary layer data at the center of the test section.

The tunnel conditions are q=12 psf, V=99 ft/s.

Please let me know what else you need to know. I appreciate the help.

(1). I can only assume that there is a bellmouth at the entrance of the wind tunnel inlet. (2). The inlet section is "elliptic" shape? Anyway, it doesn't matter whether it is rectangular or elliptic. (3). The most important thing is, whether you have a bellmouth at the inlet or not. This will determine how a wind tunnel actually work. This will determine where you should place your inlet condition. (4). Anyway, if you have a bellmouth inlet, then you should create a box much larger than the bellmouth (to enclose the bellmouth) and set the inlet condition there. (5). So, where is your inlet location and conditions? (6). When you run a wind tunnel, the air will come from all directions into the inlet. The bellmouth is there to avoid the inlet flow separation. (7). So, one thing at a time, what is your inlet shape of your wind tunnel?

It's a bell mouth...

I placed pressure(p0) and temperature(T0) bc's at the inlet.

(1). Since the bellmouth is an object in the flow field, the free stream is away from the bellmouth. (2). Something like a sphere which enclose the bellmouth. (3). Some flow will come from the area in front of the bell mouth, and some flow will come in from behind the bellmouth. (4). The boundary layer will start from the lip of the bell mouth. (5). In other words, you can create a large shpere which enclose the bellmouth, acting like the far field inlet. (6). You can't specify the condition at the bellmouth, because it is unknown during the testing. (7). I am assuming that you don't have a screen or something like that in the inlet section, because it will create additional problems. and I am assuming that the fan is at the back end of the duct (wind tunnel).

>I have B.C's for all the walls as inviscid, the floor
:as viscid
:I'm getting fresstream velocities way to close to the
: floor.

The walls as inviscid and the floor as viscid? What do you mean by this?

The bc's are set as slip(inviscid)on the walls and slip(viscid) on the floor

Why? I don't see why you would want to set either of these conditions. Shouldn't all the walls be set as non-slip?

There was typo on my last message. The walls are all non-slip, but the floor is slip to resolve the boundary layer. What are your suggestions for b.c's at the inlet and outlet.

What are you modelling? If you are modelling ground effect (is this why have the ground slip?) then you really need the ground moving to get an accurate simulation. What happens in the wind tunnel? What are you currently using as inlet and outlet BCs?

I'm using the tunnel to simulate flow over a vehicle. At the inlet I have pressure and temperature. At the outlet I have pressure ratio. Firstly, I'm trying to compare the boundary layer data I have for the real tunnel then put in the vehicle.

(1). Well, you can always use the flow over a flat plate data (or formula) to calculate the boundary layer thickness at the test section from the inlet.(2). Formula from the "boundary layer theory" by Schlichting, gives delta(x) = 0.37 * x * (U * x / nu)^(-0.2) (3). If you don't have enough mesh points in the boundary layer from the inlet, you are not going to see the boundary layer. (4). Use the formula in item-(2) to give you the boundary layer thickness distribution from the inlet. (5). Put in some 30 mesh points inside this boundary layer all around the wall, from the inlet. This will provide you adequate mesh distribution to capture the boundary layer. You could start with fewer mesh points and refine it step-by-step. (6). To capture the boundary layer profile and development, use 30 points when using wall function, use 60 points when using low Reynolds number model.(if available) (7). In the empty wind tunnel, all you are trying to do is to compute the turbulent boundary layer development.

Thank you. When the vehicle is placed in the tunnel should the same distribution be followed off the wall.

(1). Yes. (2). You can always check the Y+ values on the wall to see if it is within the limit specified by the turbulent model you are using. (3). You can just put in a simple rectangular box first to simulate the vehicle, and check the effect. (4). With blockage due to the vehicle (depend on the relative size), you will have flow acceleration in the test section and thinner wall boundary layer. (5). But as a first cut, keep the mesh near the wall the same.