CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Potential incompressible flow around an aerofoil (http://www.cfd-online.com/Forums/fluent/28470-potential-incompressible-flow-around-aerofoil.html)

Alberto April 24, 2001 05:05

Potential incompressible flow around an aerofoil
 
Hi, I had a difference of average total pressure between inlet and outlet even if i set the "inviscid" solution model and apparently there is not any dissipations. Can you help me please?

Xiao Hu April 24, 2001 10:11

Re: Potential incompressible flow around an aerofo
 
That is interesting. I would check the following:

1) convergence. Note that even if the residuals satisfy the criteria, it does not necessarily mean it converges. Monitor the drag coefficient to make sure that there is no more change.

2) Use the 2nd method to increase accuracy. 2nd method is essential especially when you have tet mesh.


Alberto April 24, 2001 12:52

Re: Potential incompressible flow around an aerofo
 
I sent this case to a Fluent responsible for consulting and support and he said that fluent is not designed for this purpouse. The "Inviscid" option exists just to start the iteration. In other words Fluent is not able to solve potential flow.

Dan Williams April 25, 2001 01:19

Re: Potential incompressible flow around an aerofo
 
Whatever, there is no reason it shouldn't do it. You'll get total pressure variation simply due to numerical diffusion. So, if you run a first order advection scheme you should get more total pressure change than you do if you run a more accurate second order advection scheme.

Dan.

Jonas Larsson April 25, 2001 07:08

Re: Potential incompressible flow around an aerofo
 
As other have already say - use a better scheme (2nd order), try to improve the grid (if possible avoid tets) and make sure that you have a well-converged solution. If fluent still gives significant total pressure losses (caused by numerical diffusion) then that imples that fluent is not suitable to predict losses, drag coefficients etc.... I doubt if the support engineer would say that. He probably just tried to get off the hook. You should also look at a contour plot of total pressure to see where the loss occurs - might give you a hint of the source of the problem.

Btw, I assume that you don't have any shocks in your solution... that would of course cause total pressure losses even if you have a fully inviscid flow.

Amadou Sowe April 25, 2001 09:43

Re: Potential incompressible flow around an aerofo
 
You can tell the support engineer that flow through porous media is a typical potential flow problem. So fluent is able to solve at least some potential flow problems.

Alberto April 27, 2001 07:08

Re: Potential incompressible flow around an aerofo
 
Yes, Fluent does the calculation but in Inviscid flow simulation a variation in the total pressure is inadmisible, even if it's due to a numerical diffusion. That's why, probably, in this cases it's better using Martensen codes. I tried with second order advection and results were about the same.

Alberto April 27, 2001 07:10

Re: Potential incompressible flow around an aerofo
 
Yes, it's able but do you have any difference of total pressure between inlet and outlet?

Dan Williams April 27, 2001 07:25

Re: Potential incompressible flow around an aerofo
 
Maybe inadmissable is the wrong word here. I think what you mean to suggest is that it would be nice if one could minimise numerical diffusion when running invicsid calculations so that non-physical viscous effects will not be a factor. Unless you have found out how to violate the second law of thermodynamics, it's impossible to eliminate it completely with a finite difference or finite volume advection scheme due to the finite discretisation error. So, you have to live with some. For example, people, including myself, have been running invicid shock tube and detonation problems for years this way.

Dan.

Alberto April 27, 2001 10:09

Re: Potential incompressible flow around an aerofo
 
Of course I didn't find a way to violate the second principle of thermodynamics, I would have been enjoing the Nobel prize right now. I just found another code wich suits my case very well (air flow through aerodynamic cascade) and doesn't give me that numerical diffusion and those total pressure problems. ciao

Alberto April 27, 2001 10:17

Re: Potential incompressible flow around an aerofo
 
The code if you are interested is called Martensen codes and it's based on the surface vorticity method. It's very simple and solves a linear equations system which gives very low errors due to the discretisation.

John C. Chien April 27, 2001 17:55

Re: Potential incompressible flow around an aerofo
 
(1). I think, I like your question. If the code is not designed to solve the inviscid equation accurately, then you are not going to get the useful answer from the code. (2). As I have said several times before, a commercial code is a commercial code. Look for what it can do for you, instead of what you want from the black box. (3).In the end, it would be better to spend the same amount of time to write the code on your own, or to look for a suitable code for your problem.

Dan Williams April 28, 2001 00:36

Re: Potential incompressible flow around an aerofo
 
You have found what many before you know. A code specific to the job will do what you want. If I wanted the best solution to a shock tube problem, or a steady state potential flow problem, Fluent would be complete overkill.

Still, you have to use judgment when throwing your problem at Fluent, or any other commercial CFD code for that matter. Don't be suprised when they can't solve an inviscid flow problem without a total pressure loss. In the absence of physical diffusion, the best you can do is based on how diffusive the advection scheme is. It's just the way it is.


bulbul April 29, 2001 11:28

Re: Potential incompressible flow around an aerofo
 
My Hints:

- Potential flow is a THEORETICAL Solution and cannot imply real physical phenomenas actually - The best way to deal with it is to try to get an analytical exact solution - ANY code will give You an approximated Solution with some numerical diffusion etc... - Fluent can perform such simulations. I have simulated a dipole with success - have You considerd Kutta-Joukowski condition? - if You calculate a symmetrical profil try to simulate a half (axisymmetric) part. - How in percent deviate the Drag?

Hope to be helping You.

B.


All times are GMT -4. The time now is 04:34.