# centrifugal compressor

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 December 7, 2008, 17:54 centrifugal compressor #1 Marek Guest   Posts: n/a Hi! I want to simulate centrifugla compressor in CFX-10.0. First I made hand calculations. I used total pressure on inlet and mass flow on outlet for BC. Although I calculated that Mach number at outlet is 0.77 solver crashed because of high Mach number. For timescale I set 1/omega. I also try to gradually increase mass flow. First I set half final mass flow. Solution almost converged. Than I set 10% bigger mass flow. Solution did't converged. Does anybody has any practical advice?! This is my first compressor simulation except tutorial. Best regards! Marek

 December 13, 2008, 11:25 Re: centrifugal compressor #2 Georg Guest   Posts: n/a Perhaps you get high Mach number near blade surface (leading edge). I recommend you to check mesh quality of whole model and especially in this zone. May be your elements are too big. In CFX Post you can verify 1) shape of elements â€" several criterions (you'll find information about in CFX Help); 2) Y+ variable on walls (it should be less then 200 if you use default k-epsilon turbulence model).

 December 13, 2008, 20:15 Re: centrifugal compressor #3 Marek Guest   Posts: n/a Georg, thanks for reply Actually the high Mach number is on outlet. I changed BC to mass flow on inlet and total pressure on outlet. But minimum MAX residual I can get is 5E-4. First I used timescale 1/omega and than I reduced them to 1/(2*omega).

 December 15, 2008, 10:52 Re: centrifugal compressor #4 CycLone Guest   Posts: n/a Hi Marek, You can't specify total pressure at an outlet, did you mean static pressure? Go back to having a total pressure at the inlet and set the relative pressure at the outlet to zero (i.e. equal to your inlet). This should run fine and return the choke mass flow rate. Compare this to your desired mass flow rate to see if it is indeed achievable. Some common mistakes to check: 1. Geometry scale; it's not uncommon to have created the mesh in the wrong units. 2. Direction of rotation; use right-hand rule. 3. Component vs. full machine; did you apply the full machine mass flow on a single component? 4. Initial guess; if you entered an initial guess, try deleting it and letting the solver do it automatically. Good intentions can lead to undesirable results. Generally good advice: If the flow is near choke, use a pressure outlet. Away from choke, use mass flow rate. See the turbomachinery best practices guide in the documentation for more help. -CycLone

 December 16, 2008, 07:47 Re: centrifugal compressor #5 Marek Guest   Posts: n/a CycLone, thanks for useful reply! Yes, it was mistake (late hour). I set static pressure at an outlet. I will set pressures as you said. Thanks also for common mistakes list. I checked all the things (except No.4) and everything is OK. best regards Marek

 December 17, 2008, 10:04 Re: centrifugal compressor #6 Marek Guest   Posts: n/a I set total pressure (relative pressure to 0Pa) at an inlet and Average static pressure (relative pressure 0Pa)at an outlet. I set reference pressure to 1atm. The mass flow I get is the choke mass flow. Is this correct? Now I have new question. I made three meshes. Compressor inlet, compressor and difusor. I am not sure how to make domain interface between the inlet and compressor and between compressor and difusor. Inlet and difusor domain is stationary but compressor is rotating domain. Any useful advices are welcome! Thanks in advance! Marek

 December 17, 2008, 12:25 Re: centrifugal compressor #7 Sonja Guest   Posts: n/a There are 3 different interfaces which you can use to connect stationary to rotating domains. They are called Stage, Frozen Rotor and transient Stator-Rotor Interface. They are described well in the cfx manual. hope this helps you!

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Attesz CFX 18 May 27, 2012 10:17 Mitpostdoc ANSYS Meshing & Geometry 8 February 25, 2011 11:51 murthy pnvr CFX 3 November 12, 2010 12:13 Suzzn CFX 4 December 19, 2009 09:49 siva appanna Main CFD Forum 5 February 13, 2006 22:07

All times are GMT -4. The time now is 06:09.

 Contact Us - CFD Online - Top