Divergence problem with a pipe

[Anonymous]

Hello i have a little problem with my simulation.

I have a pipe with a diameter of 2 inches; seven nozzle on the side and the end of the pipe is closed.
The boundary conditions are: Inlet massflow with 1925g/s; the seven outlet 0bar pressure.
And i use the turbulence model k_epsilon and i tried all advection from 1 to 5.
Well i thinking the combination of ADV5 and this turbulence modell is the best variation.
But in every simulation the plot begins to swing and the simulation ends on the basis of divergenz.
Behind the nozzle are areas (looks like a tube; only air) to measure the massflow on the seven outlet and check the balance sheet.

Please take a look on the following images.

Maybe you can help me to find a solution with this problem!

[srhusain]

Perform the following steps to verify that you have applied the pressure boundary conditions correctly:

1. Run the model 5 iterations
2. Open the summary file and verify that you have 7 outlets and 1 inlet. If this is not the case, then something in the geometry is preventing the boundary conditions at the openings from being properly applied, in which case you need to ensure that these openings do not have duplicate surfaces.

If you have seven outlets and one inlet indicated in the summary file, then the problem lies elsewhere- could be excessively coarse mesh, or you are using variable properties. Make sure you have a mesh that is fine enough to capture the flow gradients, and that the material environment is fixed, that is, the density is constant. Also ensure that you are running the problem as incompressible.

Attach the zipped support file if you are still having difficulty getting a converged solution.

Hope this helps.

[Anonymous]

Well i´m thinking the simulation is fine, but i would appreciate it very much when  you can have a look at this following file.

The files are too large!
Maybe can i send the file to your email address or something else?

[srhusain]

You should be able to reproduce the problem with a smaller model. Alternatively, you can log a support case.

[Anonymous]

With a smaller model  (mesh) unfortunately I could not solve the problem.

[srhusain]

Can you be more specific on how you failed to solve the problem? Was it divergence? Unrealistic results? Look in the status file for any warnings or errors.

[srhusain]

I see that you have set it up as compressible flow, in which case you should apply the "unknown" BC at all outlets and zero gauge pressure at the inlet. Have you tried running the problem incompressible?

[srhusain]

Here is a screen shot of your model which auto-converged at 842 iterations. The boundary conditions were modified as unknowns at the 7 outlets and zero gauge pressure at the inlet, running compressible flow. The mesh enhancement layer factor was set to 1.2 and the mesh gradation was set to 1.25.

[srhusain]

Correction- the only boundary condition change made was to add a zero gauge pressure (static) at the inlet- see the tree on the left side of the image.

[Anonymous]

I have not been able to try that, but I will give a message as soon as I have found.

[Anonymous]

I tried this version, but I must say that I do not trust this.
The pressure is too low at the beginning and later too high compared to other simulations.

I really want to know is if I specify a mass flow at the inlet as spread the mass flows at the outputs.

The other simulations was simulated successfully with 5,5 bar inlet pressure and 0 bar outlet pressure.

[srhusain]

The pressure boundary conditions you used to get successful simulation is a good alternative to specifying the mass flow rate- I was merely trying to help achieve a resolution to your divergence problem.

So, using the inlet and exit pressure BC approach, you could adjust the inlet pressure to help achieve the flow rate that you desire. Of course, this is a trial and error approach but a valid one.