CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

Questions about CFD

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 4, 1999, 05:47
Default Questions about CFD
  #1
Lebeau alexandre
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.
  Reply With Quote

Old   April 6, 1999, 14:23
Default Re: Questions about CFD
  #2
John C. Chien
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 ( sub-layer region) can be written as ( U/(v*) ) = Y+, and if you define U+ =( U/(v*) ) then you get the linear sub-layer 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 0-07-055334-3) , Hinze,Turbulence(McGraw Hill), or Tuncer Cebeci & Peter Bradshaw, Momentum Transfer in Boundary Layers(Hemisphere/Mcgraw Hill,ISBN 0-07-010300-3) 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 so-call 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 pre-made and there are custom-made.
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 15:00.