# Where to stop with mesh

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

 September 5, 2001, 15:29 Where to stop with mesh #1 Slobodan Pazin Guest   Posts: n/a Hi Where to stop with number of cells when meshing in Gambit, because when the number of cells are biger and biger the results in Fluent are diferent and diferent. Whit adapt it is the same. Thanks in advance

 September 5, 2001, 16:01 Re: Where to stop with mesh #2 Scott Whitney Guest   Posts: n/a This depends on a few things. 1) How much of a change are you talking about. Suppose you are most interested in a result (such as temperature at a point). Is this result changing by 1%, 10%, or 100%? 2) What is your required error margin in this result? 3) If you aren't using a turbulent model you must keep increasing the cell count until your result differences are less than your required error margin. I typically try one grid, find the result. Then I make a grid with about double the cells and find the new result. Repeat until the difference is less than your required error margin. 4) If you are using a turbulence model, you must make sure you don't violate the near-wall conditions. That is you may accidently make the cells too small or too large at the walls. But as long as you don't violate this, follow step (3).

 September 6, 2001, 00:28 Re: Where to stop with mesh #3 John C. Chien Guest   Posts: n/a (1). It is sad to hear that, the solution keeps changing with refined mesh. (2). Well, there is something you must do to regain your confidence in CFD. First of all, select a few test cases, such as flow over a flat plate (laminar), flow in a lid driven cavity (laminar, say Re=400. it's a good number.), flow in the entrance of a 2-D channel (laminar). (3). If you can not get the mesh independent solution for these cases, then you should stop using the code. (or you could try to get the vendor's support engineer to solve it for you) (4). You should try to solve these problems before any attempt to solve turbulent flows. (5). I have used my own codes to solve these problems, now it is your turn to do it using the commercial code. (I didn't have the time to do it when I was using the code.)

 September 6, 2001, 14:33 Re: Where to stop with mesh #4 Kang Guest   Posts: n/a It is not sad in the sense that this is probably because that's the way the commercial codes were designed, to have maximum stability/convergence with the sacrifice of accuracy, because the code has to be coping with so many different problems -- the so-called general purpose CFD codes... The advantage of using commerical codes is to get results quickly, but on the side, there should be some other (analytical, experimental) data to make the results more convincing...

 September 6, 2001, 16:46 Re: Where to stop with mesh #5 John C. Chien Guest   Posts: n/a (1). What you are saying is that they are not "non-profit organization". For that, I can understand.

 November 4, 2001, 12:17 Re: Where to stop with mesh #6 Rikard Gebart Guest   Posts: n/a To better understand the effect of truncation errors I suggest that you read the section about grid convergence in the Ferziger & Peric CFD textbook ("Computational methods for fluid dynamics", Springer Verlag, 2001) or the book by Roache ("Verification and Validation in Computational Science and Engineering", Hermosa Publishers, 1998). This problem has been the subject of lots of research the last decade, you can find many of the references in the book by Roache. It is natural that your result changes as you refine the grid. In practice the error compared to an infinitely fine grid will often be around 5-10% both for local and global values (functionals) even with relatively fine grids. The simplest way to estimate the error is to apply Richardson extrapolation to the results from a sequence of two or three grids. You can find details about how to do this in Ferziger & Peric. When you do the extrapolation you will probably be disappointed to find that the requirements on the grids are quite strict. Often 1000000+ grid cells will be necessary to obtain a relative error less than 1%. Hope this helps, Rikard

 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 Ganesh FLUENT 13 January 22, 2014 05:11 Zymon enGrid 31 August 29, 2011 13:40 student123a ANSYS Meshing & Geometry 13 December 8, 2010 11:40 Remy Main CFD Forum 1 December 22, 2008 05:49 arya CFX 4 June 19, 2007 12:21

All times are GMT -4. The time now is 12:14.