modeling potential flow
Hi,
I wonder if anyone can suggest that, whether it is possible to model a flow domain defined by potential flow theory i.e. irrotational flow using FLUENT. If so, how? Thnx. 
Yes. Use the inviscid model for your viscous model.
Potential flow and inviscid flows are the same, depending on what background you have in fluids they are called one or the other or both. 
Are you sure? To my knowledge, potential flow can be viscous and inviscid depending upon the viscosity condition implemented in the flow. So, the point I would like to mention that, in FLUENT, all option to define a flow is kind of realistic approach. However, potential flow is sort of simplistic approach with sum assumption that makes it irrotational, which I don't know if at all feasible in practice and so, if FLUENT can model it, that is my question? If possible in FLUENT, what to select under DEFINE>MODELS>SOLVER and under DEFINE>MODELS>VISCOUS?
Thnx. 
Quote:
Fluent allows you to model inviscid flows, the inviscid potential flows, by selecting the inviscid flow model under viscous models. You can use either solver, but the pressurebased solver is cheaper, simpler, and should suffice. 
Ok. Thnx Lucky.

I would be hesitant using fluent inviscid solver to solve a potential flow. The reason for that is that fluent solves the NS equations, which when viscosity is omitted reduce to the Euler equations.
Now, Euler equations can be solved using potential flow theory, assuming the flow is irrotational and steady state. Generally it is valid to assume so, since if there is no viscosity, there is no reason for the fluid elements to start rotating, right? However, since fluent does not solve the potential flow model, but the Euler equations, the inherent numerical viscosity of the used schemes (even if you use the highest order schemes possible, which will limit numerical viscosity), will produce viscosity and vorticity effects, which will give a totally different answer from the expected, when solving pure potential flow (Δφ=0, solve for φ and then spatial derivatives of φ give u,v,w). A simple experiment to check this would be to solve flow over a cylinder with the fluent inviscid model (steady state). You will see that pressure will not be fully recovered after the cylinder (D' alamberts paradox : http://en.wikipedia.org/wiki/D%27Alembert%27s_paradox), as it would be expected from a pure potential flow solver. On the other hand you will get small vortices after the cylinder and eventually you will get drag (again contrary to what you would expect from potential flow). To sum up, using inviscid fluent for potential flow is, according to my opinion, inaccurate (inaccurate here means that you won't get the expected, from potential theory, results  the results you'll get will be closer to reality, than the potential theory, though). You should use another software for that (for example Comsol has the ability to solve Laplace equation, which is used for potential flow). However, using inviscid fluent solver, can still give you an initial flow field for more complex physics. Any comments are welcome. 
Quote:

Ehm, sorry but solving the Euler equations does not mean that there is no numerical dissipation. Numerical dissipation (or numerical viscosity) comes from the truncation of the Taylor expansion at the derivative approximations and it is inherent in any numerical scheme.
Increased resolution and higher order schemes will limit numerical dissipation, but it will always be there. According to my experince, trying to solve inviscid flow (Euler equations) with Fluent will not result to the same results as a potential flow solver and, from my experience again, results will differ substantially. I don't know if anyone else has any experience with the inviscid flow solver, but if you perform the small numerical experiment I described above you'll see what I mean when I say that fluent is not appropriate for simulating potential flow. See also this post: http://www.cfdonline.com/Forums/flu...aerofoil.html (It is somewhat old, but I don't think that fluent's numerics on inviscid solver changed much) or this one: http://www.cfdonline.com/Forums/mai...ulerflow.html Again any comments welcome. 
Quote:

Quote:

All times are GMT 4. The time now is 11:15. 