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

Periodic compressor simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 17, 2010, 08:01
Cool Periodic compressor simulation
  #1
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Hi all,

I'm doing a centrifugal compressor simulation. To speed up the simulation, I want to use only a blade passage instead of the whole geometry. To get this, I have to slice the geom to a periodic piece. What is the recommend way?
1. Slice between the blades, so I get a geometry bounded by periodic boundary conditions with a blade in the middle, or
2. Slice at the centroid of the blade, so I get a clear blade passage, bounded by blade walls.

I found examples for the type 1., but the second one seems to be good too.

Thanks for any advice,
Attesz
Attesz is offline   Reply With Quote

Old   February 18, 2010, 15:43
Default
  #2
New Member
 
Join Date: Dec 2009
Posts: 13
Rep Power: 7
puga is on a distinguished road
I'm relatively new to CFD, but would suggest the first option. Let me put it this way: a periodic boundary is only going to increase the local complexity of the problem. That being said, would you rather have the possible error from this near the object of interest (the airfoil), or away? I'd go with the latter. It seems to be the general practice from what I've seen.

Alternatively, you could do a 2-airfoil passage and get the best of both worlds, but sacrifice run some run time.
puga is offline   Reply With Quote

Old   February 18, 2010, 17:58
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,960
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The boundary layer on the blade is often critical to accurate models. To get a good boundary layer you need a good mesh with no interuptions and so it is usual to move anything boundaries away from these areas. That is why option 1 is normal chosen. But if the periodic boundary is 1 to 1 option 2 can work. If it is a GGI that is not recommended.
ghorrocks is offline   Reply With Quote

Old   February 23, 2010, 06:49
Smile
  #4
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Hi,

thanks to all, I will do the 1. type, because the periodic surface mesh is not 1:1, and the compressor has tip gap. Fortunately, I could slice the geometry in DesingModeller (I couldn't believe in this before) so this way can work.

Thanks again for the answers,
Attesz
Attesz is offline   Reply With Quote

Old   March 3, 2010, 06:42
Question transient rotor-stator interface
  #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 all,
i've done with the geometry, It works fine in steady state simulation (with wrong results unfortunately). We want to do a transient simulation, in first step with frozen rotor interfaces, and then with the transient rotor-stator. My question is: can CFX use well the transient rotor-stator interface with periodic geometry? Because here the domain will be physically rotated...

Thank you,
Attesz
Attesz is offline   Reply With Quote

Old   March 3, 2010, 06:54
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,960
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You cannot use frozen rotor in a transient simulation. It is only valid for steady state flows.

You can use TRS interfaces with periodicity.
ghorrocks is offline   Reply With Quote

Old   March 3, 2010, 07:27
Default
  #7
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Ok, good news, thanks!

Regards,
Attesz
Attesz is offline   Reply With Quote

Old   March 24, 2010, 10:16
Default
  #8
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Hi all,
Glenn wrote that I cannot use frozen rotor, but in transient simulation, I can set the interfaces to Frozen Rotor, it's allowed. But, it's not physically valid, mostly when the periodicity in the rotor and stator has not the same angle. I think, stage option is better. But, if I use huge difference between the periodicity angles or pitch, I can get wrong results with stage also? Is there a recommened upper/lower value for pitch change? In my case the pitch change between stator& rotor is 2. Is it more suitable to use 2 blade passages from impleller to get pitch change to 1? Using this means more cells and computational time.

Thanks for any advice,
Attesz
Attached Images
File Type: jpg periodic.jpg (81.1 KB, 39 views)

Last edited by Attesz; March 24, 2010 at 10:19. Reason: inserting picture
Attesz is offline   Reply With Quote

Old   October 19, 2010, 08:36
Default
  #9
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Hi all,

i have a question in the simulation project of this thread, but it can be a general one as well.
So I'm running a steady simulation on a centrifugal compressor-diffuser stage, and when I increase the pressure ratio, the massflows converge hardly. Also the RMS residuals are increasing, while the MAX residuals are high from the beginning. I use a fine, unstructured tetra mesh, SST k-w model, 120deg periodic geometry with frozen rotor interfaces. The increase in RMS occurs under the operational point, so it is far from surge too. the outlet boundary condition is average static pressure. Now, i've switched to mass flow outlet, and the residuals are going down, as you can see on the picture. Why is this happened?

An other question, because of the increased Timescale Factor, the convergence can be poor when i would use lower factors? Is there any upper limit for that factor? Currently i'm using 50 and 100, but there is no significant difference in between.

conv.JPG

Thanks,
Attesz
Attesz is offline   Reply With Quote

Old   October 19, 2010, 17:42
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,960
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
http://www.cfd-online.com/Wiki/Ansys...gence_criteria
ghorrocks is offline   Reply With Quote

Reply

Tags
blade, compressor, periodic

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
Periodic boundary condition Arif FLUENT 2 January 17, 2014 07:48
Why can't I make the boundaries periodic? Alina FLUENT 5 April 12, 2012 14:06
[TGrid] unable to find periodic twin ?? aeroosso ANSYS Meshing & Geometry 1 September 21, 2009 18:29
Must periodic oscillation give periodic results? zonexo Main CFD Forum 6 May 13, 2007 15:36
construct a periodic boundary condition in Gambi? Daniel FLUENT 0 October 17, 2006 10:28


All times are GMT -4. The time now is 13:10.