# Periodic compressor simulation

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

 February 17, 2010, 08:01 Periodic compressor simulation #1 Senior Member     Attesz Join Date: Mar 2009 Posts: 355 Rep Power: 9 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

 February 18, 2010, 15:43 #2 New Member   Join Date: Dec 2009 Posts: 13 Rep Power: 8 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.

 February 18, 2010, 17:58 #3 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 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.

 February 23, 2010, 06:49 #4 Senior Member     Attesz Join Date: Mar 2009 Posts: 355 Rep Power: 9 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

 March 3, 2010, 06:42 transient rotor-stator interface #5 Senior Member     Attesz Join Date: Mar 2009 Posts: 355 Rep Power: 9 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

 March 3, 2010, 06:54 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 You cannot use frozen rotor in a transient simulation. It is only valid for steady state flows. You can use TRS interfaces with periodicity.

 March 3, 2010, 07:27 #7 Senior Member     Attesz Join Date: Mar 2009 Posts: 355 Rep Power: 9 Ok, good news, thanks! Regards, Attesz

March 24, 2010, 10:16
#8
Senior Member

Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 9
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.

Attesz
Attached Images
 periodic.jpg (81.1 KB, 43 views)

Last edited by Attesz; March 24, 2010 at 10:19. Reason: inserting picture

 October 19, 2010, 08:36 #9 Senior Member     Attesz Join Date: Mar 2009 Posts: 355 Rep Power: 9 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

 October 19, 2010, 17:42 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98