[TurBoris]

Hi All,

I have been performing a full-wheel 2-staged centrifugal compressor with a choked nozzle connected to downstream of it to control the mass flow rate (as in test rigs). The outlet is set as supersonic.

Every monitor was normal until compressor did 7 revolutions. After that I observed a drop in the average Mach number at nozzle outlet and eventually massflow. Then, in the out file temperature unbound warning appeared.

Before this warning the average temperature in the nozzle exit was about 500 K . Then the temperature locally exceeded this value and spreaded half of the nozzle ring eventually.

I attached some visuals. In the first one, the left figure is before the warning. On the right, the temperature rised and covered the exit.

What would be a cause of this ? Might it be related to time step size ? I go with a coarse time step (200 time step per rev) to reduce the computing time since the domain and number of elements are very large. The RMS Courant is about 40.

Or would it be related to material data. I use ideal gas with a CEL function of Cp. I apply reasonable bounds for temperature and pressure in table generation.

Thank you for any help.

[ghorrocks]

Your simulation has diverged and the results are rubbish. You will need to rerun it and improve the numerical stability to it converges. This FAQ has some tips: https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F

In your case definitely first run this with ideal gas with a fixed Cp. If that converges OK then you can use this run as an initial condition for the variable Cp case.

[TurBoris]

Hi Glenn,

Thank you for your comment.

The results were useless as you said so I stopped the simulation after I had seen this.

The instability arose in the nozzle region where the flow accelerates and becomes sonic. I investigated the flow field in this region and I realized that flow field had some gradients in circumferential direction (even in temperature). I associated the error with this type of flow field and used mixing-plane interface between the last stationary vanes and nozzle region instead of the default general connection interface.

I rerun the new setup and its been solving very stable for 6 days without a temperature error. The only change is the interface type.

Before this I had tried to impose temperature damping with an under relaxation of 0.2 (without knowing its theory well). This hindered the temperature error in nozzle, however caused very large mass flow fluctuations in the interfaces between blade rows. Thats why quit using it.

[ghorrocks]

While this sounds promising, make sure you are aware of the implications of the different interface types. They all have different physical models behind them, so make sure the one you are using is suitable for what you want to do. Read the section of the CFX documentation on interface types.