# Flat plate trouble

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

 October 16, 2001, 16:10 Flat plate trouble #1 Chetan Kadakia Guest   Posts: n/a Sponsored Links I am modelling a flat plate, but I am having difficulties acheiving a reasonable number for the Cd. Could someone advise what I could be doing wrong. My Cd should be in at the magnitude of 10^-3, but Fluent is showing a magnitude of about 10^4. If anyone has worked the flat plate in Fluent, please let me know what you have done to make it work. Thanks.

 October 16, 2001, 17:23 Re: Flat plate trouble #2 John C. Chien Guest   Posts: n/a (1). First of all, put your flat plate leading edge in the middle of your computational domain. On the left side, you have empty free stream. (2). Stretch the mesh in both directions centered around the leading edge. In this way, you have very fine mesh at the leading edge. And the mesh size increases in both direction (left and right). (3). Stretch the mesh in the normal to the plate direction, higher density near the leading edge. This should gradually increase in spacing downstream of the flat plate. Basically, you are trying to capture the boundary layer development and the thickening of the boundary layer. (4). Try to use both the high Reynolds number model and the low Reynolds number model. And follow the model guidelines in terms of Y+ at the wall setting. (5). If you still have problems, try to use uniform mesh near the wall, and along the plate. (stretching in x-direction will change the solution in my systematic tests a couple of years ago, using tri-mesh) You should try quad-cell near the wall also. (6). Flat plate case is the most fundamental test case, because the turbulence models are all supposed to re-create the result. Unfortunately, there is no guarantee when using a commercial code. (I am not saying they are useless, I am saying that each case must be validated for accuracy)

 October 19, 2001, 03:05 Re: Flat plate trouble #3 dimitris Guest   Posts: n/a 7 orders of magnitude is too much, to be accounted by modelling, meshing or other physical/numerical reasons. You are probably haven't set the correct reference values in the "Report/Reference Values" panel (see User's Guide). Dimitris

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post recon9 CFX 1 January 20, 2011 22:09 vsun FLUENT 0 October 3, 2010 07:56 Far FLUENT 0 May 18, 2010 04:57 mc Main CFD Forum 0 April 24, 2007 22:38 Simon Mizzi Main CFD Forum 1 December 16, 2003 02:26