
[Sponsors] 
February 14, 2000, 07:46 
Model problem

#1 
Guest
Posts: n/a

I am using a CFD software to calculate the coefficient of lift and coefficient of drag for NACA 23012 airfoil.
My model is like this: The airfoil is located at the centre of a rectangular domain with inlet at the left and outlet at the right. The leading edge of the airfoil is facing the inlet. The calculation is based on the concept of wind tunnel. My questions are: Generally, what should be the distance of the leading edge to the inlet and the distance of the trailing edge to the outlet? And what should be the distance of the upper surface of the airfoil to the cealing of the domain and the distance of the lower surface of the airfoil to the bottom of the domain? Because I found that as the distance changed, I get different answer. 

February 14, 2000, 10:58 
Re: Model problem

#2 
Guest
Posts: n/a

For external flow problems, the boundary conditions can affect the solution if the boundaries are close enough to the body to influence the solution. There are some rules of thumb that I've used on external flow problems, but they are not absolutes. The best thing for you to do is start with a grid based on rules of thumb, and then rerun the problem with a slightly larger computational domain. If the solution does not change (or changes an acceptable amount, like 1%) then you've got a lagre enough domain.
For external, incompressible flow, I have used the following rules of thumb: * The inlet should be two chord (body) lengths upstream of the leading edge of the body. * The outlet should be four chord lengths downstream of the trailing edge of the body. You may have to lengthen the domain downstream if the body produces a strong wake (like a blunt body). * The symetry or outflow boundaries above, below, and to the side of the body should be two chord lengths away. A computational domain based on these rules should give you a good starting point for determining exactly how large a domain you need. 

February 14, 2000, 14:00 
Re: Model problem

#3 
Guest
Posts: n/a

i assume you are running a subsonic problem. if you read journals you'll often see that the airfoil is just a speck in the centre of the domain. this is because in subsonic flow the effect of the airfoil is felt far away from it. from a potential flow analysis you can show that the P/Pinf ratio is still about 1.1 when you are on the order of 10 diameters upstream of a cylinder. that gives you some idea about the appropriate size for your grid.


February 14, 2000, 23:08 
Re: Model problem

#4 
Guest
Posts: n/a

(1) With uniform values of free stream, the life does not converge evenif the far boundary is vary far (100 chord). Because the perturbence of the arifoil in the far field is of the firstorder which can not be neglected, the lift has an approximate relation Cl=Cl0A/R where R is the distance of the far boundary and Cl0 is the real lift and A>0. So the vortex correct should be used (See Pulliam AIAA 850360) (2) Or you may set uniform values at the inlet, and interpolate the other boundaries in the far field.


February 14, 2000, 23:21 
Re: Model problem

#5 
Guest
Posts: n/a

The second discoussion in my last message should be explained as: set the uniform values at the inlet, while calculate values at the upper, lower and outlet by linear extrapolation or Riemann invariants.


February 15, 2000, 13:04 
Re: Model problem

#6 
Guest
Posts: n/a

external flow is not my speciality, but from my understanding for subsonic problems it's probably better to use some kind of nonreflecting boundary condition or Riemann invariant condition to allow properties on unspecifiable boundaries. for references you can try Kevin Thompson's paper in Journal of Computational Physics vol 89 pp 439461, 1990. there are other references to bc of this type such as Poinsot and Lele in J Comp Phys vol 101, 1992. also Hirsch's "Numerical Computation of Internal and External Flows" is a good reference on riemann invariant BC.
the problem with constant upstream values is that flow angle often has to be specified which requires the upstream boundary to be quite far (as you said even 100 chords is typical) from the body. so it is probably better to specify bc which allow the flow direction to be free. the same is true for outlet conditions. it is typical in nozzle/turbomachinery flows to specify outlet static pressure. however viscous simulations usually include outflowing wakes which tend to be smeared out by this bc. often the results depend on outlet boundary placement and accurate solutions require the outlet to be placed far downstream which is unphysical. nonreflecting outlet conditions have been used to obtain reliably accurate results with outlet boundaries placed in a mechanically accurate position. unfortunately many commercial and other codes don't have a sufficient variety of these 'free' boundary conditions so users are required to make their domains bigger than necessary. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
kw SST transitional model problem  shanon  ANSYS  0  September 21, 2010 09:00 
Problem with turbulence model  akonduri  OpenFOAM  2  September 17, 2010 00:49 
Turbulence model for mixing problem???  nileshjrane  Main CFD Forum  7  September 14, 2010 04:57 
multiphase mixing Problem with MRF model in MixSim  Srinivas  FLUENT  0  October 17, 2005 06:35 
Non premixed model  combustion validation problem  David  FLUENT  2  October 24, 2003 10:06 