
[Sponsors] 
April 4, 1999, 05:47 
Questions about CFD

#1 
Guest
Posts: n/a

I have some questions about CFD :
WHat is exactly Y+, formula? Physics explanation? what is the diffenrence between rampant, fluent and UNS? Is there a methods to determinate the first cells size on a meshing, with wall law? without? What is the method when you want to do hybrid mesh with geomesh and TGrid? Is using unstructured with prism for adaptation a good method? When is it better to use wall law or not, how to you know the kind of mesh would be the best? I am new to CFD and maybe those questions would look stupid or trivial, but I think they are the basis of this area Thank you for your answers and your help. Al. 

April 6, 1999, 14:23 
Re: Questions about CFD

#2 
Guest
Posts: n/a

(1). I am not sure whether you will be able to absorb all the answer. (2). The definition of Y+ is vey simple, Y+ = y * (v*) / mu, where y is the normal distance, mu is the kinematic viscosity and (v*) is the frictional velocity defined as (v*)= sqrt ( wall shear stress/ rho) . The reason behind this is the velocity profile near the wall ( sublayer region) can be written as ( U/(v*) ) = Y+, and if you define U+ =( U/(v*) ) then you get the linear sublayer velocity profile as U+ = Y+, which is valid up to Y+ =< 5. This profile comes from the experimental data, and you can read book by : Schlicting,Boundary Layer Theory(McGraw Hill,ISBN 0070553343) , Hinze,Turbulence(McGraw Hill), or Tuncer Cebeci & Peter Bradshaw, Momentum Transfer in Boundary Layers(Hemisphere/Mcgraw Hill,ISBN 0070103003) for more detail information about the law of wall universal velocity profile. (3). Rampant, Fluent and UNS are three commercial CFD codes, Rampant and UNS are unstructured mesh codes for compressible and incompressible flow, respectively. Fluent is the structured mesh code. In the new version of code, these are all included in one module under different names. (4). Once you have computed a boundary layer flow, you can plot the velocity profile using the frictional velocity defined above because the wall shear stress is known. Since the universal profile normally says that the sublayer linear profile is in the region less than Y+ =< 5, you need , say use 5 point for this region and put the first Y+ at 1. In this way, you will have enough point to cover the sublayer region. ( at least two points to draw a straight line) Now Y+ = 1.0, and with mu and (v*) know, you can solve for Y, and that is your first grid point away from the wall. ( If you don't have the solution, then you have to estimate the (v*). You could use some empirical curve fit also.) (5). In the case of using the wall function, the universal velocity profile tells you that you should be roughly in the region greater than 100 or 200. this is because the law of the wall profile exist in this region so that the matching process can be carried out. (6). The hybrid mesh approach is one way to solve the accuracy problem associated with the triangular mesh near the wall. This approach is suppose to improve the accuracy without using a lot of mesh points or cells near the wall.(the use of triangular mesh near the wall will have high skewness problem for practical problems.) (7). The mesh refinement in most cases are carried out in the unstructured triangular mesh region away from the wall. This normally depends on the code.(8).In the wall function case, you don't solve for the near wall region, you assume that the solution form is given.( you don't know whether this is your real solution, but it is one approach.) In the low Reynolds number model, you can solve the whole flow field including the sublayer region. so, you have everything. But sometimes you can't afford it. (9). The mesh is one way to obtain a solution, and in order to obtain accurate solution, it is important to refine the mesh to get the socall mesh independent solution. You don't want to make the solution as a function of the mesh used. (10). The mesh is just like the colthing, there is no such thing as a better mesh. Just like clothing, there are premade and there are custommade.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Propellar CFD Analysis Questions  Craig  FloEFD, FloWorks & FloTHERM  1  February 25, 2009 04:35 
Where do we go from here? CFD in 2001  John C. Chien  Main CFD Forum  36  January 24, 2001 22:10 
Errors in CFD  Lily Kabanj  FLUENT  8  May 1, 2000 07:52 
CFD Salary  CFD  Main CFD Forum  15  September 4, 1999 14:04 
public CFD Code development  Heinz Wilkening  Main CFD Forum  38  March 5, 1999 12:44 