
[Sponsors] 
October 21, 1998, 19:08 
Staggered grids for compressible flow?

#1 
Guest
Posts: n/a

Staggered grids are commonly used when solving the incompressible NavierStokes to avoid the problem of pressure velocity decoupling. Collocated grids are always used when solving the compressible Navier_stokes. Why does the problem of pressure velocity decoupling not occur when the compressible NavierStokes are solved in the low Mach number limit?


October 22, 1998, 09:40 
Re: Staggered grids for compressible flow?

#2 
Guest
Posts: n/a

Who said so ? I am using this socalled widelyused compressible NavierStokes code using BL turbulence model and a lot of artificial viscosity, and I am having difficulties in getting converged solution at inlet Mach number =0.1. The flow just refuse to settle down to uniform condition. It is oscillating there all the time. In other region of the flow, the Mach number is higher and the flow is stable. Without special treatment, the compressible NavierStokes program is always hard to converge at low Mach number. ( There must be a reason why codes always come with artificial viscosity treatment something like TV Ads of diehard motor oil).


October 22, 1998, 12:50 
Re: Staggered grids for compressible flow?

#3 
Guest
Posts: n/a

Hi,
Compressible codes are inaccurate at low Mach mach number. We can restore the accuracy by using a precondionned approach a la Turkel. At low Mach number, it is possible to use a staggered approach as in the incompressible case. But the formulation is valid only at low Mach because at high Mach ( M>0.3) you must get some kind of upwinding of the density. I know that Wesseling proposed an approach based on staggered grids to compute low Mach flows. Good Luck. Farid 

October 23, 1998, 00:02 
Re: Staggered grids for compressible flow?

#4 
Guest
Posts: n/a

John,
At the same Reynolds number, there is no reason to say the solution is converged at high Mach number while it is disconverged at low Mach number. I think if the solution can not converged at inlet Mach number =0.1, it can not converged at inlet Mach number =0.3, too. For incompressible flow, the two solutions must be the same. I have got a converged solution of low Mach number flow without any special treatment. The artificial viscosity of TVDtype is enough to suppress the velocitypressure decoupling. I am using a compressible code with algebriac turbulence models and twoequation lowRe models to study separation bubble flow, but I havenot found the oscillation difficulty. As my experience, the oscillation disappears when grids are fine enough both in the cross direction of streamwise AND in streamwise. Especially for separaion flow, the spatial step of the streamwise is as important as that of the cross direction because in the sepration region, u is in the same order of v. The problem resulting from low Mach number is the convergence rate because of the poorconditioned coefficient matrices. There are some ways to overcome this problem, for example, precondition approach, multigrid method. Some other problem, such as inaccurate computation becomes severe when Mach number is extremely small. The velocitypressure decoupling exists both in incompressible and in compressible flows, and may be suppressed by artificial viscosity. 

October 23, 1998, 09:50 
Re: Staggered grids for compressible flow?

#5 
Guest
Posts: n/a

If this is related to finite volume and SIMPLE (or similar) solution methods, it is possible due to the solution algorithm to cause vp decoupling. In SIMPLE type algorithm, v components are composed to form the normal mass flux for a control volume (nonrectangular), and then discretized as p' poissonlike equations. p' solutions are used to modify v', and thus in each iteration continuity will be exactly satisfied. In this process it involves compose and decompose of v. There is no guarantee that vp will be coupled, unless special care is taken to minimize the decoupling. Colocated or staggered grid should have the same problem. Usually, strong convective flow will not have the decoupling problem, but in the small votex area oscillation might happen depending on discretization scheme. The very local and small oscillation might also occur when the mesh is very fine and cause long time to drive convergence, and usually we can ignore it if it doesn't affect major flow field.
For compressible flow, PISO or other coupled solution methos are used, the vp coupling should not be problem. But, to some extent, PISO is similar to SIMPLE, does anyone see decouple with PISO? 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
problem related to staggered grids  zhu  Main CFD Forum  10  October 27, 2001 22:30 
CFD Modeling of Twophase Flow in Small Dia.Tubes  Eric Poindexter  Main CFD Forum  2  September 22, 2000 09:21 
mass flow inlet  Denis Tschumperle  FLUENT  7  August 9, 2000 02:19 
Help: Poiseulle flow benchmariking  Mohammad Kermani  Main CFD Forum  1  November 12, 1999 17:15 
Question on 3D potential flow  Adrin Gharakhani  Main CFD Forum  13  June 21, 1999 05:18 