I am making my predegree thesis, and look for a profile of a convergent nozzle that reaches an equal mach 1, in the throat, by using software Ansys, the problem is that I am not able to optimize the amount of element which is due to use in the analysis, I have already proven from 1000 elements to 70000 elements and the results do not become stabilized, each elements variation throws an different answer, for the same exercise, with the same boundering conditions .

please if something knows, answer me, the truth I almost have been a year in this thesis and not that I must make to finish it , thanks..

Dear Diego,

Your question is missing important information regarding the model details:

- Laminar or Turbulent ?

- Slip, or Non-Slip walls?

- Viscous, or inviscid (mu ~ 0)

- specific heat ratio = 1.4 ?

- pressure ratio = 0.5283 ?

Besides that, you still must do a mesh refinement study to guarantee your solution is independent of the mesh size. How are you measuring your "element variations"? Based on a given measure, what is the value that gives you confidence? On which variable are you applying the measure?

Opaque

thanks for the quick answer, I am working with flow convergent, in the turbulent zone, adiabatic and steady state, the fluid is the air, specific heat ratio = 1,4, pressure ratio = 0,5357, I am doing pressure deltas of 50 kpa, with an initial pressure of 1400 kpa until arriving at the pressure critical, according to the equations the pressure of the throat, where the mach = 1, with those pressure delta I can calculate the radius of the nozzle in that point of pressure I specify until arriving at the pressure critical that it gives the critical radius

and what I want to look for it is a profile with all these pressure delta to that the mach is 1. and to know as it is the length of each pressure delta, with the help software ansys. I am making the study for the refinement of the mesh, but the problem is that if increase the amount of elements or nodes, leaves an error much to me that is density negative, and the simulation stops, I am using the standard turbulent model k-e, I don`t know is the model is good for this simulation

Why are you running a pressure ratio of 0.5? A good designed laval nozzle is designed for a pressure ratio of 0.12. Here's some good advice and a design tool (non-cfd):

http://www.engapplets.vt.edu/fluids/...le/cdinfo.html

Below a pressure ratio of 0.5 you will have choked flow (reaching Mach=1 in the throat). Few things: 1. Use total inlet boundary conditions (total pressure and total temperature) 2. Make sure your outlet boundary (average pressure imposed) is NOT near the throat. 3. Use a small initial velocity with local timestepping. After you can apply physical timestepping (typically 1e-4 [s] I would say) 3. Start with a coarse mesh to get a solution fast and a good starting condition for you fine mesh solution 4. Use the SST turbulence model 5. Apply inflation layers (in your final mesh you should aim for a low (<<100) y+ and a minimum of 10 layers in the boundary layer. 6. Maybe apply the expert parameter (max continuity loops=2)

This is a simple standard calculation and should give the proper result in no time.

Bart

thanks for the replaced one, Dr flow squad, but the truth I do not understand to him very well how to use the results obtained with a coarse mesh, I am using an inlet pressure of 1400 kpa and 750 kpa in the throat , I do not understand if these conditions are forcing the model, when analyzing it, in the tutorials says that is a good option, for convergent flows, but also it says that you can use two conditions in the inlet and the outlet don`t use anything, but I try to analyze with these condition, and I took root and the results did not seem logical to me, the graphs of speed and mach, etc.

maybe I must use last conditions of entrance , that would be pressure and speed inlet and in the exit don`t use condition of boundary, and varying the length of the nozzle so that I varied the conditions of the exit like the mach and the speed, I am not being placed a speed of zero in the walls of the nozzle, as the ANSYS help recommends, serious to vary the length for each pressure delta , until obtaining a good result near to mach 1, of course that the result depends the inlet conditions ,if you modify themselves, they would have change and create another different profile.

excuse by my English, the truth I do not have much practices in the writing

Dear Diego,

whatever you do, do NOT put a pressure boundary at the throat itself. You really have to put it more downstream. The behaviour of the flow in the nozzle is mainly determined what the solution is in the throat (mass flow and hence velocity). Let the code find the solution in the throat, do not try to impose it via a pressure boundary.

Bart

Mr. Bart Prast in the help of ANSYS, suggests for convergent flow, can be used two forms of conditions of boundary, first is pressure entered inlet and the outlet, and the other form is pressure and speed to the inlet, and the outlet don`t using anything, but when doing the analysis of this form, the outlet condition is going to take the atmospheres conditions , the atmospheric pressure, I don´t know what do you to think for this analysis, this is coherent ?

These settings for your boundary conditions will give a solution. However as you are looking at choked flow in a nozzle I would recommend using total inlet conditions. This way the solver can return the mass flow connected to these inlet boundary conditions. At the exit we normally impose static pressure. However, the flow is very sensitive to what happends in the throat of the nozzle. Therefore you should never put a boundary condition in such a critical region. If you nozzle is cut-off at the throat and exhausts in a much larger space, I would construct a larger box around the exhaust (may be a box or a sphere), at the surface of this space you can than impose you atmosferic conditions away from the throat.

Bart