Potential incompressible flow around an aerofoil

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 24, 2001, 05:05 Potential incompressible flow around an aerofoil #1 Alberto Guest   Posts: n/a 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?

 April 24, 2001, 10:11 Re: Potential incompressible flow around an aerofo #2 Xiao Hu Guest   Posts: n/a 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.

 April 24, 2001, 12:52 Re: Potential incompressible flow around an aerofo #3 Alberto Guest   Posts: n/a 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.

 April 25, 2001, 01:19 Re: Potential incompressible flow around an aerofo #4 Dan Williams Guest   Posts: n/a 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.

 April 25, 2001, 07:08 Re: Potential incompressible flow around an aerofo #5 Jonas Larsson Guest   Posts: n/a 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.

 April 25, 2001, 09:43 Re: Potential incompressible flow around an aerofo #6 Amadou Sowe Guest   Posts: n/a 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.

 April 27, 2001, 07:08 Re: Potential incompressible flow around an aerofo #7 Alberto Guest   Posts: n/a 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.

 April 27, 2001, 07:10 Re: Potential incompressible flow around an aerofo #8 Alberto Guest   Posts: n/a Yes, it's able but do you have any difference of total pressure between inlet and outlet?

 April 27, 2001, 07:25 Re: Potential incompressible flow around an aerofo #9 Dan Williams Guest   Posts: n/a 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.

 April 27, 2001, 10:09 Re: Potential incompressible flow around an aerofo #10 Alberto Guest   Posts: n/a 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

 April 27, 2001, 10:17 Re: Potential incompressible flow around an aerofo #11 Alberto Guest   Posts: n/a 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.

 April 27, 2001, 17:55 Re: Potential incompressible flow around an aerofo #12 John C. Chien Guest   Posts: n/a (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.

 April 28, 2001, 00:36 Re: Potential incompressible flow around an aerofo #13 Dan Williams Guest   Posts: n/a 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.

 April 29, 2001, 11:28 Re: Potential incompressible flow around an aerofo #14 bulbul Guest   Posts: n/a 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.

 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 Laith Mohammed Main CFD Forum 1 November 14, 2013 12:26 pxyz Main CFD Forum 37 July 7, 2006 08:42 Hun Jung Main CFD Forum 4 August 11, 2003 10:10 Shahriar Main CFD Forum 7 March 7, 2003 09:53 A.M.Yang Main CFD Forum 1 July 3, 2002 07:58

All times are GMT -4. The time now is 09:58.

 Contact Us - CFD Online - Top