CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Compressible flow in nozzle (http://www.cfd-online.com/Forums/fluent/35412-compressible-flow-nozzle.html)

rawin January 8, 2005 10:35

Compressible flow in nozzle
 
hi; My case is 2-D Compressible Flow in a C-D Nozzle. Inlet and throat area of the nozzle are 0.8 and 0.05 meter. When I use complete model (i.e with it's top and bottom walls) very high speed flow after throat turn to the bottom wall.But when I use half model ,with symmetry boundary condition Fluent Solve Flow field correctly and High speed Flow after throat,stay on the center line. I use Coupled implicit and standard k-e to solve it. How can i use complete model and solve it correctly. thanks.

Jason January 8, 2005 17:53

Re: Compressible flow in nozzle
 
A common reason for asymmetries in the flow is an asymmetric model. Since the walls you are meshing are symmetric (I'm assuming) it only leaves that the mesh is asymmetric, and this small asymmetry is introducing enough error to change your flow. I'm running into a similar problem in 3D right now. Perfectly symmetric models become sensitive to asymmetric meshes. If you can, go with a structured mesh and don't use sizing functions. The background grid tends to be splotchy and causes curvatures in your mesh that you don't want. If you can't do that, then only mesh half of the model in Gambit, then mirror it and connect the overlaying edges so that the two halves now share a common edge. Another option is to try refining your mesh, and eventually the error becomes so small from cell to cell that you can't see any change in the flow (but it'll still be there).

Hope this helps, and goodluck Jason

rawin January 11, 2005 02:33

Re: Compressible flow in nozzle
 
HI; Thank you Jason.It was helpful and solved my problem .But residauls after 15000 iter are between 1 and 0.1.what should i do?

Jason January 11, 2005 08:18

Re: Compressible flow in nozzle
 
What are you trying to get out of the nozzle? The residuals you are looking at are normalized based on the initial guess. It's possible that you model can be converged without dropping three orders of magnitude. Figure out the main parts of the model you're trying to solve for (forces, mass flow rate, pressure at a point, etc...) and monitor those over the solution process. When the residuals have leveled off and the data you're monitoring has leveled off, then you can call your model converged.

A common problem is that people watch the monitors looking for convergence. One of two things can happen... there can be dynamics in the model that the steady state solver is having problems dealing with (usually indicates a mesh problem... even bluff bodies can be solved with a proper mesh) and the residuals will level off to some point, but the pressure distribution will change and cause your forces to change. The other problem is that the residuals hit the default convergence criteria and people go "I'm done, it's converged!" but if they were monitoring the forces they might see that they haven't reached a truly converged solution.

What I'm trying to get at is that for convergence, monitor the residuals, but also monitor the information that is most important to you. If you're going to be reporting forces, then monitor the forces to show that they did converge. Compare your results to published or experimental data too. Make sure your solution makes sense.

Hope this helps, and goodluck Jason

rawin January 12, 2005 03:40

Re: Compressible flow in nozzle
 
thank you jason Refining mesh makes results better.But i have a question.Mach number at the nozzle exit is 2.7 and this exit flow enters to a L shap circular duct.Then i model this duct and the nozzle flow as a sudden expansiuon.But that error comes again and nozzle exit jet turns to the wall.How can i solve this problem in nonasymmetric model?

Jason January 12, 2005 08:01

Re: Compressible flow in nozzle
 
I have a couple of questions.

Your nozzle... does it have a circular or rectangular cross section?

I'm guessing the L shape is the side view and when you say circular, you are talking about the cross section, is that right? You said it's a sudden expansion, so I'm guessing that the flow goes from right to left on the L (L <-- flow direction) and that the exit of the nozzle is at the small part of the L.

This could be an issue. If the cross section is circular, then you can use a 2D model, but know that you're introducing error. The 2D model assumes a straight extrusion of your model into and out of the screen. The flow is going to be slightly different from a rectangular (what Fluent assumes) to a circular cross section. The problem comes in when you change the cross section. Decreasing the height by 2" on a rectangular cross section has less of an impact than changing the diameter of a circular cross section by 2".

If it is a circular cross section, then you can run a 2D axisymmetric model, but then the centerlines for the entire nozzle and duct have to be coincident.

The last option is to model it in 3D.

Again, I'm assuming a couple of things here, so feel free to correct me. Also, if you e-mail me a couple images of your problem I might be better able to help. Maybe a picture showing the overall model and flow characteristics, and another showing a close-up of the problem you're having.

Goodluck, Jason

rawin January 19, 2005 02:04

Re: Compressible flow in nozzle
 
Hi jason I send it.what do you think about it?would you help me? thaks.

Jason January 19, 2005 08:33

Re: Compressible flow in nozzle
 
Sorry about that, I got caught up in work-related things. I just responded to your e-mail. For your setup, you have a pressure ratio (P0/P) at the inlet of 1.01, which correlates to a Mach number of 0.12. For this low-speed, I would not use the Coupled solver because it is a density based solver and you are no where near the compressible region so the solver will have trouble dealing with this model. I would use the Segregated solver since it is a pressure based solver. Also, watch your mass flow rates at the inlet and outlet. Make sure they match, otherwise your solution isn't converged no matter what the residuals tell you.

Goodluck, Jason


All times are GMT -4. The time now is 23:23.