CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Temperature Unbound Warning in a Transient Compressor Simulation

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 30, 2022, 08:05
Default Temperature Unbound Warning in a Transient Compressor Simulation
  #1
Member
 
TurBoris's Avatar
 
Bora
Join Date: Nov 2016
Posts: 32
Rep Power: 9
TurBoris is on a distinguished road
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.
Attached Images
File Type: jpg 2037_diverged.jpg (135.4 KB, 24 views)
File Type: jpg 2037_nozzle_Diverge.jpg (107.9 KB, 16 views)
TurBoris is offline   Reply With Quote

Old   October 8, 2022, 04:25
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,692
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   October 8, 2022, 15:51
Default
  #3
Member
 
TurBoris's Avatar
 
Bora
Join Date: Nov 2016
Posts: 32
Rep Power: 9
TurBoris is on a distinguished road
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.
TurBoris is offline   Reply With Quote

Old   October 8, 2022, 17:38
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,692
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[Other] mesh airfoil NACA0012 anand_30 OpenFOAM Meshing & Mesh Conversion 13 March 7, 2022 17:22
foamToTecplot360 thomasduerr OpenFOAM Post-Processing 121 June 11, 2021 10:05
[Gmsh] discretizer - gmshToFoam Andyjoe OpenFOAM Meshing & Mesh Conversion 13 March 14, 2012 04:35
OpenFOAM Solaris mamaly60 OpenFOAM Installation 13 May 10, 2010 21:16
Warning 097- AB Siemens 6 November 15, 2004 04:41


All times are GMT -4. The time now is 12:23.