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

The Onset of Surge in a centrifugal compressor

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 15, 2009, 14:37
Question The Onset of Surge in a centrifugal compressor
  #1
Member
 
Susann
Join Date: Apr 2009
Location: Dresden
Posts: 33
Rep Power: 8
Suzzn is on a distinguished road
Hello guys,

i want to start some simulations of a full 360 centrifugal compressor using Ansys CFX. I simulate the compressor involving inlet, impeller, vaneless diffuser, volute and outlet. With different mass flow rates i want to examine the onset of surge. First i gonna do some steady state simulations with the frozen rotor interface. Afterwards i want to try the unsteady Simulation. I found this paper about the topic: http://www.ansys.com/events/proceedi...PAPERS/252.pdf
Because surge is an unsteady phenomena it cannot be modelled with a steady state simulation. Thats why the convergence rate for the calculations tends to stall near surge. Despite the fact of convergence difficulties the results for lower mass flow rates were plotted in this paper because they often matched experimental data very well. So the peak for pressure ratio in the resulting plots was used to localise the onset of surge and comparing the result with the experimental data. Is there any other way of capturing the onset of surge? Maybe calculating negative mass flow rates inside of the compressor? Did anybody setup a similar simulation or does anybody know another paper about this topic?

Best regards,
Susann
Suzzn is offline   Reply With Quote

Old   December 15, 2009, 18:35
Default
  #2
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Hi,

I'm simulating a centrifugal compressor and a vaned diffuser, with the same conditions like yours. I've found that paper at Ansys.com too. But I've got a lot of problems during my work. My compressor stage reached the surge at more lower pressure ratio, than it had to (We made measures of course). Any ramping function (wich was described in the papers), and modifying of the boundary conditions etc. couldn't help. There was a big separation started from the suction side of the impeller blades, wich closed the area. My operating pressure ratio at 116000RPM is 3.17, but we can reach only about 2.5. After that we made a periodic modell with only one blade passage, with millions of elements, in a transient simulation, where the pressure at the outlet was ramped up. So the mesh was very fine and good quality. Thus we reached the targeted PR, but this transient simulation takes a lot of time (1 week absolute simulation time).
So there is an other problem with my modell, but we don't now what exactly.

To the surge: Yes, we made surge in steady simulation. For example, at 2.4PR, the mass flow is very small. You step to 2.5PR, and the fluid is flowing back into the domain. To get this, you have to use opening boundary conditions of course. With outlet you will get convergence problems, with the message "Wall has been placed at portions of an outlet...". So I recommend to use opening. Also the Mass flow outlet wasn't helpful to avoid surge at these low pressure ratios.

Could anybody send a picture about a good mesh in cf compressor? With hexahedral mesh could I reach lower element numbers and more accurate results?

Finally, sorry for my english

Regards,
Attesz

Last edited by Attesz; December 16, 2009 at 05:11.
Attesz is offline   Reply With Quote

Old   December 16, 2009, 08:57
Default
  #3
Member
 
Susann
Join Date: Apr 2009
Location: Dresden
Posts: 33
Rep Power: 8
Suzzn is on a distinguished road
Hello Attesz,

i`m running my first steady state simulation at operating point (160.000 RPM and a massflow of 0.2kg/s, Pressure ratio of 2.7). My inlet boundary condition is Total Pressure and Temperature, outlet boundary is the massflow. But you`re right when it comes to unsteady surge effects i should use an opening boundary condition at the inlet instead! I use the frozen rotor interface between stator and rotor and wanted to start the stage model afterwards initialising the simulation with the results from the frozen rotor model. I guess this could safe some computing time....Which model are you using? So you initiated surge by changing the pressure ratio and not the mass flow? My first simulation is not ready yet...the only thing i see is that the results are oscillating but seem to converge...any idea why that is happening? From my backup file i see that the simulated pressure ratio is also much too small...there is a great loss of pressure inside of the volute and between volute and outlet it rises again abruptly. To the mesh: i have to use scripts that generate a tetra mesh for impeller and volute, for inlet and outlet i made hexameshes. I dont know if my mesh is ok. I want to make a net study first refining the mesh of impeller and volute. I think inlet and outlet dont have to get lots of elements. Hexameshes are always a better solution because you need less elements and less computing time. And you can control the number of elements in a better way! But it should have no effect on the quality of your results i think, because your solution must be approximately independent of the used mesh.

Best regards
Susann

Last edited by Suzzn; December 17, 2009 at 09:15.
Suzzn is offline   Reply With Quote

Old   December 16, 2009, 17:43
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,817
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Have you been through the basic stuff to obtain convergence? As discussed here:

http://www.cfd-online.com/Wiki/Ansys...gence_criteria
ghorrocks is online now   Reply With Quote

Old   December 19, 2009, 09:49
Default
  #5
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Hi Susann,

I'm using both frozen rotor and stage interface. With the stage interface the solver averages the values at the interface, so you can get more general values, for example in the vaned diffuser. It can help you to avoid some convergence problems caused by flow separation, but I think, it can safe not too much computing time. Stage is useful, when your geometry is periodic, and you can not use frozen rotor. But with frozen rotor, you can study the interferences between the rotor and stator (in my work, the blades of impeller and diffuser are very close together). You can get a more accurate simulation, when you make a steady simulation with frozen rotor, and then a transient simulation (with initialization from the steady of course).

Quote:
the only thing i see is that the results are oscillating but seem to converge
The flow in our problems are very difficult: compressible flow, boundary layers, high sheared regions, and rotating domains with interfaces. So reaching convergence needs a lot of time, with "oscillation". But I dont know exactly what do you mean "oscillating". The oscillation of imbalances, torque values at the blades is normal.

I've got the surge by increasing the pressure ratio, by 0.1 or lower values. With mass flow my simulation diverges near surge, but I've got a different geometry model. If I have a bit time, I will upload some pictures next week...

What is the main goal of your simulation? To get the characteristic, or just getting the surge line? I ask it because when your goal is getting the characteristic curves, i recommend you some "tricks" to get them faster. You should start your simulation at lower RPM-s, for example at 60%, and with very low PR. When you have time, it can be PR 1.0. With PR1.0 the simulation finishes fast, with a high mass flow rate. From these results, you can increasing the PR, keeping the RPM constant. At the beginning, you can use bigger steps in PR (1.0->1.5), but at higher PR-s, when you don't want to have a divergence, more lower (PR 2.4->2.5 or lower).
It is also intersting, that when I set a mass flow value I get a PR. When I set this PR, I got a different mass flow, and it was a big difference. After that I saw it's better not to use mass flow outlet boundary conditions. But I note again, my geometry is different than yours!
When you finished your simulation, please share with me the results, I'm very intresting in it.

Have a nice weekend,
Attesz
Attesz is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Centrifugal compressor mass flow error Attesz CFX 18 May 27, 2012 10:17
Doing Centrifugal Compressor Simulation? Lee FLUENT 3 March 31, 2010 05:28
centrifugal compressor Marek CFX 6 December 17, 2008 12:25
centrifugal compressor siva appanna Main CFD Forum 5 February 13, 2006 22:07
Centrifugal compressor volute Stuman CFX 2 November 29, 2005 01:25


All times are GMT -4. The time now is 01:45.