# Non-orthogonal correction in SimpleFOAM

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

 May 28, 2010, 02:10 Non-orthogonal correction in SimpleFOAM #1 Member   Jinbiao Xiong Join Date: Oct 2009 Location: China/Japan Posts: 50 Rep Power: 7 I am using a non-orthogonal mesh in the calculation. I tried to put the nonorthogonal as 1 to add some correction. But when I read the code of simpleFoam. I can not understand what difference it can make. It seems the correction just solve the matrix one more time, with little change in the matrix. The change of the matrix is only from pEqn.setReference(pRefCell, pRefValue) So I cannot understand what is going on with the non-orthogonal correction. Can any one explain it? Thanks a lot. Best, __________________ Jinbiao

 May 28, 2010, 08:10 #2 Member   Cedric Van Holsbeke Join Date: Dec 2009 Location: Belgium Posts: 81 Rep Power: 7 Non-orthogonal correction is not recommended for steady-state solvers as it is not needed to have a converged solution every time-step. Just put it to 0 and set limiters in your fvSchemes file in order to handle a non-orthogonal mesh. songwukong and sharonyue like this.

 May 29, 2010, 02:43 #3 Member   Jinbiao Xiong Join Date: Oct 2009 Location: China/Japan Posts: 50 Rep Power: 7 Hi Cedric, Thanks for your reply. Do you mean I only need to apply the correction in the laplacian terms. For example laplacian (phi, *) Gauss linear corrected Thanks a lot. Best, __________________ Jinbiao

 May 29, 2010, 03:20 #4 Member   Cedric Van Holsbeke Join Date: Dec 2009 Location: Belgium Posts: 81 Rep Power: 7 If your max orthogonality is < 60, you can indeed use "Gauss linear corrected" for your laplacian scheme, if higher you can use "Gauss linear limited 0.333". Your snGradScheme has to be edited accordingly (either corrected or limited 0.333). You can also limit the other schemes. For example: Code: gradSchemes { default cellLimited Gauss linear 1; } divSchemes { default none; div(phi,U) Gauss linearUpwind cellLimited Gauss linear 1; ... } laplacianSchemes { default Gauss linear limited 0.333; } snGradSchemes { default limited 0.333; } lakeat, kiddmax, fumiya and 3 others like this.

 May 30, 2010, 00:14 #5 Member   Jinbiao Xiong Join Date: Oct 2009 Location: China/Japan Posts: 50 Rep Power: 7 Thanks a lot, Cedric. In your example, you used gradSchemes { default cellLimited Gauss linear 1; } This is my first time to know there is a cellLimited scheme. I am curious about the difference between cellLimited and other limited schemes? If possible, could you also explain what is the function of the numbers following the limited scheme. Thanks again. Best, __________________ Jinbiao

August 26, 2014, 03:52
#6
Member

Pratik Nanavati
Join Date: May 2014
Location: Munich, Germany
Posts: 40
Rep Power: 2
Quote:
 Originally Posted by JinBiao Thanks a lot, Cedric. In your example, you used gradSchemes { default cellLimited Gauss linear 1; } This is my first time to know there is a cellLimited scheme. I am curious about the difference between cellLimited and other limited schemes? If possible, could you also explain what is the function of the numbers following the limited scheme. Thanks again. Best,
Limited versions of any of these 3 base gradient schemes (Gauss, leastSquares and fourth) can be selected by preceding the discretisation scheme by cellLimited (or faceLimited),

e.g. a cell limited Gauss scheme,

for more details you can refer http://www.openfoam.org/docs/user/fvSchemes.php (4.4.3 Gradient schemes)

 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 herenger OpenFOAM Running, Solving & CFD 7 July 11, 2013 06:27 7islands OpenFOAM Running, Solving & CFD 4 December 9, 2012 23:54 Alan OpenFOAM Running, Solving & CFD 10 April 6, 2012 14:02 Pierpaolo OpenFOAM 1 May 8, 2010 03:08 Subhra Datta Main CFD Forum 2 November 24, 2003 14:11

All times are GMT -4. The time now is 05:00.