HELP! Small Turbomachinery Diffuser Turbulence Modeling
 

Hello, I am trying to model a small jet engine (70mm centrifugal compressor) in an attempt to evaluate diffuser performance to compare one design to another. The fluid volume is from the outlet of the compressor to the inlet of the combustor. I am having trouble getting the model to converge which I think is attributable to using the default turbulence parameters. Can anybody suggest a range of suitable parameters for turbulence and or any suggestions for the rest of the model?

My enabled models are as follows:
All y + Wall Treatment
SST (Menter) K Omega
K Omega Turbulence
Reynolds Averaged Navier Stokes
Turbulent
Coupled Energy
Ideal Gas
Coupled Flow
Gas
Steady
Three Dimensional


It is a rotational periodic interface about 24 degrees

Velocity Inlet (from compressor)
Flow Direction: (121.3,337.6,0) Cylindrical Coordinate frame
Static Temperature: 372.2239
Turbulence Intensity: 0.1
Turbulent Length Scale: 0.01m
Velocity Magnitude: 358.8m/s


Pressure Outlet (To Combustor)
Pressure: 0 (Reference Pressure 2.0942BAR)
Static Temperature: 409.861K
Turbulent Intensity 0.01
Turbulent Viscosity Ratio: 10
I tried Target Mass Flow Rate Option but it caused sudden divergence after 200 iterations

http://itechdandm.com/innovaero/cfdmesh.JPG

What version of Star-CCM are you using?

I did not find any glaring errors in your setup yet. However, your modelling is fairly complex with a coupled solver and ideal gas. How are you initializing the simulation? You will need a fairly good initialization for the simulation to not diverge.

I'm assuming you've already tried lowering the under relaxation factors.

Try running without all the complicated setups right off the bat. For starters I would turn off the target mass flow rate option initially and let the solution settle a bit. Next I would start with cutting back on ideal gas and use constant density. Help the solver as much as you can!

Again the most important question is: HOW DID YOU JUDGE CONVERGENCE? How long did you run it and how big is the model? Are your sure, your mesh is suitable to capture all important flow phenomena?

A lot of people complain about a not converging simulation but don't judge convergence the right way.

Lucky,
Im using Version 6.04. By initializing the solution do you mean initial conditions? I have:
pressure = 0
Static Temp = 300K
Turbulence Intensity = 0.01
Turbulent Velocity Scale = 1m/s
Turbulent Viscosity Ratio= 10
Velocity=0

I have not tried any under relaxation factors.

Abdul, the volume mesh is 2420377 cells, 15413936 faces and the residual plot is below. Also, a pressure scaler plot will continue to change as the iterations continue. As for if my mesh is suitable for capturing all important flow phenomena, unfortunately I have no idea, but I would appreciate some insight.
http://itechdandm.com/innovaero/cfdresiduals.JPG

Your initialization is terrible. They are nothing like what the flow is even at the inlet. Your flow is incoming at 358 m/s but you initialize it with 0 m/s? Your inlet static temperature is 370+ K and you initialized it with 300K. It is no surprise that it diverged, you tried to use target mass flow rate yet you initialized it with no flow!

The geometry is a bit complex, so giving a good initialization will be hard without writing your own field functions. But as I said before, you need to help the solver anyway you can.

You need to monitor the solution periodically and check that they even make sense.

And you should run it longer

This.

If it works, grid sequencing initialization is excellent. That said, it doesnt always work for me depending on my geometry.

Make sure you try ramps on your courant number & relaxation factors

Well, it doesn't look too bad. Of course, better initialisation would help, but it also should work without doing anything.

Maybe it just needs more than 1500 iterations? At least the residual plot doesn't look too bad since the residuals are not exploding but still slightly decreasing.
Maybe it's an unsteady flow while your're running steady? (There are not many really steady flows in the real world). That would cause the pressure plots to change forever, although important engineering values would be okay when averaging them over some iterations.

The target mass flow option is useless when using a velocity inlet. You fix the incoming mass to a specific value, calculated from inlet velocity, area of your inlet boundary and density. Now imagine, that doesn't meet the desired outlet mass flow (might be due to numerical issues since most of the values are just single precision). The solver might ramp the outlet pressure up (or down) to reach it's target mass flow, but that could never be achieved without violating the mass conservation. So it will continue to rise (or lower) the outlet pressure, giving you unphysical values or sudden divergence.

Therefore this option should only be used when using a pressure outlet in combination with a stagnation inlet or something similar, giving an additional degree of freedom to the solver. And even when using the target mass flow option, it shouldn't be switched on unless the flow pattern more or less meets the expected flow pattern. Otherwise it could get unstable.

For the initialisation, I wouldn't bother too much with this, since your geometry is too complicated to reliable predict the flow behaviour. It's not your job to know the solution to initialise the simulation, it's the solver's job to get the solution from some initial values. Of course, a better initialisation will help to solver to get the solution quicker and more stable, but for a steady flow, it should even work with a poor initialisation.
I would just ramp up the inlet velocity with a field function over some hundred iterations. That should help enough to stabilise the solution, but of course it will take longer to get a converged state.
Grid sequencing mentioned by rwryne might also be a good idea, but it's not guaranteed to work well for internal flows. It was desinged to be used mainly with external flows. The more complex and winding your domain the more propably it will not work.

Maybe you can set the static initialisation temperature to meet some expected average temperature in your domain. But don't bother too much about this. Ramping up the velocity and / or Courant number should help enough.

And please monitor some engineering values like inlet pressure, volume averaged turbulent kinetic energy etc. and wait until they are leveled out or start oscillating around a constant value while the residuals don't ddrop anymore. This will be the point to judge the simulation to be converged.

Should I keep going or call this good?

Look at your actual pressure and kinetic energy plots. They are not converged by any means, there are large and rampant changes in their values.
Verdict: Not converged