CFD Online Discussion Forums

CFD Online Discussion Forums (
-   Main CFD Forum (
-   -   Staggered grids for compressible flow? (

Frank Muldoon October 21, 1998 19:08

Staggered grids for compressible flow?
Staggered grids are commonly used when solving the incompressible Navier-Stokes 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 Navier-Stokes are solved in the low Mach number limit?

John C. Chien October 22, 1998 09:40

Re: Staggered grids for compressible flow?
Who said so ? I am using this so-called widely-used compressible Navier-Stokes code using B-L 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 Navier-Stokes 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 die-hard motor oil).

Farid Moussaoui October 22, 1998 12:50

Re: Staggered grids for compressible flow?

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.


Zhong Lei October 23, 1998 00:02

Re: Staggered grids for compressible flow?

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 TVD-type is enough to suppress the velocity-pressure decoupling. I am using a compressible code with algebriac turbulence models and two-equation low-Re 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 poor-conditioned 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 velocity-pressure decoupling exists both in incompressible and in compressible flows, and may be suppressed by artificial viscosity.

C-H Kuo October 23, 1998 09:50

Re: Staggered grids for compressible flow?
If this is related to finite volume and SIMPLE (or similar) solution methods, it is possible due to the solution algorithm to cause v-p decoupling. In SIMPLE type algorithm, v components are composed to form the normal mass flux for a control volume (non-rectangular), and then discretized as p' poisson-like 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 v-p 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 v-p coupling should not be problem. But, to some extent, PISO is similar to SIMPLE, does anyone see decouple with PISO?

All times are GMT -4. The time now is 22:44.