Hi, I'm am a Phd student, I'm involving in a research about a fan, but I don't know the problems that I should face (rotation of the fan, type of mesh, turbulent model, etc.), in fact till now I was interested in flow around a ship hull.

I would be grateful to you if you would give me some advice.

Giovanni

(1). Fan is a low speed device, with several blades attached to the rotating shaft. (2). With the rotating reference frame, the blade and the shaft boundary condition will be stationary, just like in any turbomachinery rotor. So, you need to work with the rotating reference frame, and the equations can be found in any turbomachinery book or Journals. (3). Then in this cylindrical coordinates, you need to be able to define the blade in 3-D. This is usually done section-by-section in the radial direction (radial cylindrical cuts). But the original blade definition can be defined in Cartesian coordinates. Basically, each section is an airfoil section. (4). The blade shape can be as simple as a finite flat plate, or it can be as complicated as a real airfoil with variable thickness and camberline. It can also be a custom defined section shape. (5). Since the local relative free stream or inlet condition depends on the radial position (Vt=r*omega), each section will have different inlet flow angle, thus the airfoil must also be design accordingly or airfoil section rotated so that the flow in the leading edge can be properly matched. This is usually called the airfoil section stacking.(in the radial direction) (6). From the symmetry consideration, one can consider only one blade sector. This is the so-called blade passage flow analysis. (7). There are two typical formulations: one is to put the airfoil in the middle of the stream, and create the periodic boundary condition along the middle of the passage from the inlet to the exit. The other is to connect a periodic boundary line from the inlet to the hi-light of the airfoil, then followed by the one side of the airfoil, then connect the trailing edge point to the exit to create another segment of the periodic condition. The direction of the periodic boundary normally follows the general flow direction, but this is not necessary. (8). So, it is really like the flow through a curved channel, you specify the inlet condition, exit condition, that's all. Well, you can also include the simulation of the hub geometry in the model. The problem is very similar to the flow over an airfoil (aircraft wing). (9). The grid can be a simple H-type, O-type, hybrid o- and H-type, unstructured hybrid prism and tet cells, etc. (10). The turbulence model selection is similar to that for the flow over an airfoil, it can be simple algebraic model or fancy low RE k-epsilon model with laminar to turbulent flow transition treatment. For a simple fan, a high Re standard k-epsilon model should be a good starting point. (11). Well, this does not prevent you from doing more advanced turbulence modelling though. Anyway, this is a relatively standard problem.

Dear Chien,

Yes, your answer is a relatively standard problem, but if the blades are installed unsymmetry in pitch, for example, variable pitch axial flow fans, how to build the CFD model in Gambit & Fluent then?

Thanks

Wason

(1). What is a variable pitch axial flow fan? (2). A blade can be cut into many sections, and each can be represented by a closed profile or segment of curves. (3). Once the curves are created, one can use several curves to create a surface patch in the radial direction. You can divide the profile into say four segments each. Then you can create four large patches in the radial direction around the airfoil. You can also use four edge curve approach to define individual surface patch. I think, the approach is fairly standard to create the surface patches from the profile curves, or edge curves. (4). In this way, you will get several patches of nose section, suction surface section, trailing edge section, and the pressure surface section in radial direction. So, the shape variation can be linear, or spline fit surface. If you have enough cuts (profile sections), or if the blade is rather simple, you can use linear interpolation between section profile curves, otherwise, try the spline surface using several section profile curves to create the surface patchs. (5). By the way, almost any general mesh generation code should have this bottom-up capability to create the surface definition. (create surface patches from point, curves up)

Dear Chien,

Sorry, I have not explicated the problem,a variable pitch axial flow fan means that the blades are distributed unsymmetry, in my opion, we have to simulate the whole fan flow. Then how to build the model by using the Gambit & Fluent?

Thanks Wason

Dear Chien, thanks for your numerous suggestion.I've not understood all them, but I must reread them with some professors. My fan is an existing one, and I have to optimize it.It is very similar to that one present in Fluent tutorial guide (#15: 2D centrifugal blower). The blade sections are costant. The tutorial uses a 2D triangular mesh, what do you think about it? You suggest an hybrid mesh, why? Are not tetra cells so good near wall, if I would use 3D mesh? Are the standard wall functions good for this kind of analysis? Thanking in advance I remain Giovanni

(1). If you can not simplify it down to single passage flow, then just build the whole model in the same way one blade a time. (2). I remember a few years back, I had to build a 3-D model, a 3-D scroll with at least 13 nozzle blades in it as a whole, to study the flow field in the scroll and at the exit.(using PREbfc, the simple stone age code) (3). In creating a model and mesh bottom up, it is necessary to plan ahead of the time. You need to study the final mesh topology and the geometry model topology carefully, because they have to work together. (this is also true, if you use other code, such as icem,etc.. )

(1). It does not matter whether it is radial or axial type, the same principle applies. (2). You can still run the flow through a single passage to get some flow field results. Or you can also try to model the whole thing. (3). You can follow the tutorial method, or you can try some other kind of meshes, it is all up to you.