Axial compressor map

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

December 6, 2011, 07:10
Axial compressor map
#1
Member

Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 7
Hi guys! Its me again. Still practicing in axial compressor calculation by calculating NASA 37 stage. The problem that I faced with is compressor map calculation. I tried to compare data from NASA report (TP-1659) with clalculation in CFX. Calculation was done in 3 steps for coarse (50000 elements) and fine meshes (900000 elements):
1) Points enclosed with red (see attached). I increased static pressure ratio step by step and everytihg was fine (more or less). k-e turbulence model was used on this step. But with this settings i couldnt reach desired pressure ratio (calculation was keeping to fall apart - MFR converged to 0).
2) Then i switched to SST model and it helped to calculate higher pressure ratios (see points enclosed with blue). But when it get to the point where the MFR ought to decrease (at least i think so) it become to fall apart again (MFR converges to 0).
3) Then i decided to change boundary conditions: MFR and total temperature at inlet and static pressure at oulet. Calculated 3 points with different outlet pressure (points enclosed with pink). And confused completely because pressure ratio depend on the pressure i set. Therefore i could choose outlet static pressure to fit experimental point. But i think it not qiute right because what should i do if i didnt have experimental map and wanted to create it?
What have i done wrong?

Maybe someone could give me algorithm of compressor map calculating in CFX or at least some tips
Attached Images
 Stage 37 performance.jpg (21.5 KB, 135 views)

 December 6, 2011, 15:29 #2 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,352 Blog Entries: 6 Rep Power: 45 you are simulating with 14000 elements only? or atleast for the map shown here

 December 6, 2011, 19:43 #3 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,808 Rep Power: 107 Two comments: 1) There is a rotating machinery best practises guide in the CFX documentation. Have you read it? 2) For general accuracy issues see this FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

December 7, 2011, 05:27
#4
Member

Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 7
Quote:
 Originally Posted by Far you are simulating with 14000 elements only? or atleast for the map shown here
As i mentioned before i calculated 2 cases with coarse (14000 elements) and fine (879616 elements) meshes. Its just on this map i showed curve for coarse mesh. For fine mesh curve looks even worse. So i decided not to show it (shy of my inexperience ).

December 7, 2011, 05:45
#5
Member

Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 7
Quote:
 Originally Posted by ghorrocks Two comments: 1) There is a rotating machinery best practises guide in the CFX documentation. Have you read it? 2) For general accuracy issues see this FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
Yes, i have read best practice guide and i read that post too. But as you can see unfortunately it didnt helped me. Please forgive me if i missed something. This is the reason why i post this thread. I wanted to ask people who are more experienced than i am what is wrong in my calculation (mesh, boundary conditions or something else)?

December 7, 2011, 09:09
#6
Super Moderator

Sijal
Join Date: Mar 2009
Posts: 4,352
Blog Entries: 6
Rep Power: 45
Quote:
 Originally Posted by olegmang As i mentioned before i calculated 2 cases with coarse (14000 elements) and fine (879616 elements) meshes. Its just on this map i showed curve for coarse mesh. For fine mesh curve looks even worse. So i decided not to show it (shy of my inexperience ).
It is meaningless to have such a coarse mesh. Atleast try 200000 elements.

December 7, 2011, 11:19
#7
Member

Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 7
Quote:
 Originally Posted by Far It is meaningless to have such a coarse mesh. Atleast try 200000 elements.
I wrote you that i also used fine mesh - 879616 elements in stator and rotor, but it crashes as i reach total pressure ratio 1.7.

 December 7, 2011, 18:25 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,808 Rep Power: 107 Your curve looks very wrong. Something is seriously wrong in your setup. Can you post some images of what you are modeling and the CCL?

December 8, 2011, 05:27
#9
Member

Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 7
Quote:
 Originally Posted by ghorrocks Your curve looks very wrong. Something is seriously wrong in your setup. Can you post some images of what you are modeling and the CCL?
Of course. I've attached the CCL file and the screenshot of CFX Pre window with the mesh. I couldnt attach the CCL file so i've added .doc to its extension. If I should do something else to attach it in the right way please tell.
Attached Images
 Pre screenshot.jpg (94.7 KB, 84 views)
Attached Files
 Stage 37_PSR.ccl.doc (34.8 KB, 71 views)

 December 8, 2011, 06:25 #10 Member   DB Join Date: Apr 2011 Posts: 81 Rep Power: 8 Hi, I found a small doubt in your CCl , correct me if I am wrong. I see there is no counter rotating wall B. C. applied to your hub and casing in the rotor region. Have you not given any tip gap to rotor ? and is the hub rotating as well. Rotor tip gap have huge effect on losses and flow separation at the tips especially if they are given zero. A slight tip gap as compared to zero has huge effect on the performance. Check the tip gap __________________ -D.B

 December 8, 2011, 06:37 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,808 Rep Power: 107 Also you have viscous work turned on. This almost certainly is insignificant but may add to simulation time and possibly instability. Turn it off. Can you show some images of post processing of the flow?

December 8, 2011, 08:31
#12
Member

Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 7
Quote:
 Originally Posted by ghorrocks Also you have viscous work turned on. This almost certainly is insignificant but may add to simulation time and possibly instability. Turn it off. Can you show some images of post processing of the flow?
Sure. If you need something else please ask. Also i've noticed that there are some strange lines in outlet domain. But i'm not sure what does it mean.
Attached Images
 Streamlines.jpg (72.0 KB, 65 views) Mach number.jpg (41.2 KB, 51 views) Velocity.jpg (80.5 KB, 50 views)

December 8, 2011, 13:10
#13
Member

Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 7
Quote:
 Originally Posted by D.B Hi, I found a small doubt in your CCl , correct me if I am wrong. I see there is no counter rotating wall B. C. applied to your hub and casing in the rotor region. Have you not given any tip gap to rotor ? and is the hub rotating as well. Rotor tip gap have huge effect on losses and flow separation at the tips especially if they are given zero. A slight tip gap as compared to zero has huge effect on the performance. Check the tip gap
You're right. I've decided to calculate without radial clearance to exclude it effect (because i thought it would calculate more stable).

 December 8, 2011, 13:19 #14 Member   Oleg Join Date: Nov 2011 Location: Ukraine, Kharkov Posts: 57 Rep Power: 7 The main problem is that i cant get right shape of performance curve (i'm not even dreaming about matching the experimental data). I thought that maybe i used some wrong boundary condition or or maybe there is something completely wrong with model settings. Or everything seems OK in calculation settings and i should look for a problem in a mesh? PS. Sorry for bothering you guys with my stupid questions but my professor wants me to do this and i'm stuck

 December 8, 2011, 13:26 #15 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,352 Blog Entries: 6 Rep Power: 45 Try this time scale factor = 1 Reference pressure = 0 Use average static pressure boundary condition at outlet What is the maximum yplus in domain?

 December 8, 2011, 13:43 #16 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,352 Blog Entries: 6 Rep Power: 45 pls attach residual plots

 December 8, 2011, 17:26 #17 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,808 Rep Power: 107 Your simulation shows a separation. This will change the result substantially. Is it real? Separations are very sensitive to mesh, turbulence model and upstream conditions, and they cause major effects to the end result.

December 9, 2011, 09:23
#18
Super Moderator

Sijal
Join Date: Mar 2009
Posts: 4,352
Blog Entries: 6
Rep Power: 45
Quote:
 Originally Posted by olegmang PS. Sorry for bothering you guys with my stupid questions but my professor wants me to do this and i'm stuck
This is requirtment of your professor to ask stupid questions? Just kidding

December 11, 2011, 03:53
#19
Super Moderator

Sijal
Join Date: Mar 2009
Posts: 4,352
Blog Entries: 6
Rep Power: 45
Quote:
 Your simulation shows a separation
The separation at hub is present in rotor 37 by design. There is huge literature on this aspect of rotor 37.
What I am not understanding is that " Why compressor map has jumps from one point to another point. Looks like choked flow after two to three operation points"

 December 11, 2011, 19:01 #20 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,808 Rep Power: 107 Ok, if this design has separations by design then the presence or not, and the size of the separation will have large effects on the result. And when the separation reaches critical points (eg is long enough to reach the full blade chord) it will cause jumps in the pump curve. I suspect accurate modelling of this separation is the key for this model.

 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 user0314 FLUENT 1 May 27, 2016 12:30 wildli FLUENT 0 July 17, 2010 15:54 Nicola Viscanti CFX 3 March 17, 2010 05:15 student CFX 0 February 28, 2006 05:20 HanCheolHeui Main CFD Forum 0 September 8, 1998 10:13

All times are GMT -4. The time now is 23:00.

 Contact Us - CFD Online - Privacy Statement - Top