# compressible flow computation

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

 June 24, 2003, 09:23 compressible flow computation #1 amv Guest   Posts: n/a Sponsored Links hello everybody From the (legendry) book of Suhas Patankar we know the formulation of the flow computation for in-compressible flow. I have myself written codes for constant density and variable density in-compressible flows but can somebody tell me how to compute "COMPRESSIBLE" flow ? My flow is sub-sonic so much consideration abt transonic etc is not required. Also can somebody tell me how FLUENT computes COMPRESSIBLE flow ? The only ref I could get is "PhD thesis of KC Karki" which was written under guidance of Suhas Patankar only. THANKING YOU.

 June 25, 2003, 06:38 Re: compressible flow computation #2 John Guest   Posts: n/a There are 2 issues involved to extend to compressible flow: 1. density treatment in continuity equation (density change in other transport equations is the same as variable-density incompressible flow) and 2. boundary conditions. When deriving pressure correction equation, you have u_new=u_old+u', and density_new=density_old+density' so mass flux = density_new*u_new*area = mass_flux_old + density_old*u'*area + u_old*density'*area + density'*u'*area The last term can be neglected, and compared to incompressible flow, you have extra term and you can link density' to p' by ideal gas law. Boundary conditions: for example subsonic inlet - you have to have 2 types of inlets: fixed mass and fixed velocities. The pressure at inlet is extrapolated from interior, and since temperature is fixed, you have changing density. If mass fixed, then normal velocity to the inlet surface has to change. If velocity fixed, then mass flux has to change. Just the idea.

 June 25, 2003, 07:24 Re: compressible flow computation #3 Abhijeet M Vaidya Guest   Posts: n/a Thank you Mr John. Actually with the above concepts I derived the pressure correction equation but it does not satisfy the condition aP= aE + aW + aN + aS . this is because we have rho_e, rho_n etc like terms which bring P'_e , P'_n etc like terms and no matter whether one uses central differencing or upwinding for density , one gets an equation where aP is slightly different from aE + aW + aN + aS . Am I write ? Also in FLUENT , they use some " density equation" but I wonder how do they derive it ?

 June 26, 2003, 01:31 Re: compressible flow computation #4 Rami Guest   Posts: n/a Abhijeet, I guess the following paper may be helpful: K.C. Karki, S.V. Patankar, "Pressure Based Calculation Procedure for Viscous Flows at All Speeds in Arbitrary Configurations", AIAA J v27 n9, 1989. > Also in FLUENT , they use some " density equation" but I wonder how do they derive it ? I am not familiar with Fluent, but it may refer to the other possibility of solving compressible flows (usually with M>0.3). In this method, in contrast to the pressure-based methods, density (rather than pressure) is one of the solved variables - it is the conserved variable in the continuity equation. This method is straightforward, but difficulties are encountered for incompressible flows, where density is constant, and it is not linked to the pressure via an equation of state. The same applies (to a lesser degree) for low-Mach flows as well. This was the motivation for devising the pressure-based methods.

 June 26, 2003, 01:58 Thanks to Rami & John #5 AMV Guest   Posts: n/a

 June 27, 2003, 07:27 Re: compressible flow computation #6 John Guest   Posts: n/a AP is NOT equal to AE+AW+AN+AS in compressible flow formula. Indeed using your structured mesh concept, AP is equal to AE_of_WEST_CELL + AW_of_EAST_CELL + AN_of_SOUTH_CELL + AS_of_NORTH_CELL and the matrix is no longer symmetry.

 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 student4326 OpenFOAM Running, Solving & CFD 7 November 2, 2015 12:34 beguxa FLUENT 4 June 8, 2013 16:17 BBG Main CFD Forum 1 November 19, 2008 15:05 James FLUENT 2 June 20, 2007 04:22 atit Main CFD Forum 8 July 31, 2000 13:19