hello,

i`m an undergraduated of mechanical engineers and started working with fluent last year.

case :

i want to simulate the internal flow through very thin duct. it consists of an nozzle and a diffusor. indeed it is a model for an air gap in a compressor with a gap depth of 0.4 mm (nozzle > gap > diffusor. inlet pressure is 2 bar and outlet pressure 1 bar

experience data :

as we detected from experience there is a transient flow. as the flow-speed increases and reaches the gap, there appears a shock that is refleceted at the walls several times

questions :

- is it possible to simulate such small geometries with fluent ?

- i got flow-speed over 1 Ma (sound-velo), but shocks does not appear very sharp and are not reflected at the walls (i`m using viscoud, turbulent models, a very fine mesh with about 50.000 cells, steadz simulation). during the simulation shocks are formed but dissapear again... is unsteady simulation necessary ?

- as i see in cfd-online, shocks are not easy to handle. does fluent5.3 uses density-based solution-progress ? should i use other boundary-condition ?

- do i have to consider any other aspects ? (hint, tips ...)

many thanks for helping

dirk (university of dortmund, germany)

Are you doing a 2D or a 3D simulation? If it is a 3D simulation then 50,000 cells doesn't sounds like very much.

Make sure you use the coupled implicit solver (not the segregated) - the coupled solver gives better resolution of shocks. Also use 2nd order schemes for all variables. Be careful with the standard k-epsilon model - it can behave quite badly if you have strong shocks. Try the realizable model or the RNG model instead. However, since your geometry is so small you might even have laminar flow - estimate the typical Reynolds number to see if the flow is likely to be laminary, if it is you shouldn't use any turbulence model - just run laminar.

If the flow is inherently unstable you might get convergence problems if you try to do a steady simulation of it. The solution to this of course is to do an unsteady simulation instead.

Unsteady effects like this are often caused by shock-boundary layer interaction - be aware that this is not easy to predict correctly with CFD!

Thanks for your advice Mr Larsson.

i`m doing 2D simulation. and the dimension of my geometry is about 0.06 m x 0.04m. i am using the coupled solver and 2nd order schemes for all variables.

i`ve checked the Reynolds numbers. indeed, at the inlet until the narrow gap the cell Reynolds numbers are about 2e+02 - 2e+03. then in the very small gap, the cell Reynolds numbers are about 3e-03 !!!. should this mean i have to use laminar flow ?

in the book "computational methods for fluid dynamcis" by Ferziger and Peric, there are shocks and the reflection of them presented on page 288ff. so i think and hope, this should be reached by cfd.

if you or anybody else is interested in this problem, you can see some details at :

http://mbfem4.maschinenbau.uni-dortm...tarbeiter.html

once more - special thanks to you

respectfully

dirk (university of dortmund, germany)

hello to all members of the cfd-family,

here some more details for interested "cfd-er" :

- i`m using a quadrilateral mesh

- are 50.000 cells for this dimension of the geometry really not enough ? (my experience with cfd are extremly small)

- the flow behaves like the one in a LAVAL-nozzle, known from turbomachinery

- should i use a different courant number for the detecting of shocks ? (at the moment using : 1)

- shouldn`t i use the explicit solver ?

with best regards

Dirk (university of dortmund, germany)

(1). Whether the code has the capability to solve your problem or not, is hard to know or answer. (2). A better way to do is: find a nozzle test case which has been used and reported in paper, and then try to use the code to solve that problem first. (3). If you can solve that test case (with test data given in the paper), then you can systematically change or reduce the geometry and run additional cases to see if you can obtain good solutions. (4). With this approach, you can reach your goal step-by-step, if the code does have the capability. (5). You are likely to run into several problems: (a). Shock resolution problem. (b). Oblique shock resolution related to the mesh alignment problem. (c). Normal shock/boundary layer interaction. (d). Oblique shock/ boundary layer interaction. (e). Reynolds number effect.(laminar, turbulent, transitional) (6). Each time you run a case, make sure that you have the mesh independent solution. This is especially important when shocks are involved.

I also agree that shock/boundary layer interaction is one of the most difficult flow to obtain accuratly by cfd simulation.

You should carefully check your mesh in order to have a good capture of the shocks. You may use adaptation of the mesh at each time step. This may give very long simulation but I think that it is a good way to have accurate transient simulation of this kind of flow.

Be also carefull with the kind of descritisation scheme you use and not only the order (Upwind, QUICK, ...).

In my experience of this kind of flow explicit solver often give a better result than implicit ones but I hardly know the implicit coupled solver of FLUENT 5.

At last, good luck...

Alain

again thanks for all your advice.

correction : the correct adress (without searching) with the current case i´m working on and showing the problem is described is here :

http://www.fem.mb.uni-dortmund.de/fo...schlieren.html

have a nice weekend

and best regards

dirk (university of dortmund, germany)

(1). There is another way you can do to check the result of the calculation as well as the test data. That is, you can use the MOC (method of Characteristics) to compute the supersonic portion of the 2-D nozzle flow field. (2). As a first approximation, you can ignore the boundary layer effects (displacement, or interactions). Many standard gasdynamics text should have the information about how to use MOC for 2-D supersonic nozzle flow. (3). Once you have some ideas about the exact or approximate locations of the normal and oblique shock wave system, you can then concentrate on the mesh generation to learn how to improve the solution with multiple shocks. (4). Similar to the turbulent, separated flow over a smooth airfoil, this is another extremely tough problem to solve, because an internal flow problem is always more difficult to solve, since the only controlling boundary condition is far away at the inlet. (5). Because of the non-linear nature of the fluid dynamic equations, simple geometry normally does not have simple solution. It has direct effect on the mass conservation, but very little control of momentum and energy conservation, locally. (6). My suggestion is: do some mesh generation studies along with the MOC solution. (Such shock system in transonic nozzle is likely to be oscillating in nature. But for now, you can forget about it, and come back to it after you have some good result with new meshes.) (7). It is always nice to see the focused research approach in mechanical design.

hi..... I have just started to study on Fluent I want to model F-16 wing section which has NACA 64A204 airfoil.But ý couldn't get nodal data of NACA 64A204 airfoil.Where can ý get these nodal data.I also want to learn that, can ý model a wing by extruding the aýrfoil face geometry in gambit. if it is so, how can i describe geometric angles (sweep angle..etc)of the wing .

I look forward your massages impatiently.

thanks..

Serhat Kilerci (Eskisehir/TURKEY)