# Staggered grids for compressible flow?

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

 October 21, 1998, 19:08 Staggered grids for compressible flow? #1 Frank Muldoon Guest   Posts: n/a Sponsored Links 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?

 October 22, 1998, 09:40 Re: Staggered grids for compressible flow? #2 John C. Chien Guest   Posts: n/a 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).

 October 22, 1998, 12:50 Re: Staggered grids for compressible flow? #3 Farid Moussaoui 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 Zhong Lei 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 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.

 October 23, 1998, 09:50 Re: Staggered grids for compressible flow? #5 C-H Kuo 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 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?

 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 zhu Main CFD Forum 10 October 27, 2001 22:30 Eric Poindexter Main CFD Forum 2 September 22, 2000 09:21 Denis Tschumperle FLUENT 7 August 9, 2000 02:19 Mohammad Kermani Main CFD Forum 1 November 12, 1999 17:15 Adrin Gharakhani Main CFD Forum 13 June 21, 1999 05:18