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

Axial compressor map

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 6, 2011, 07:10
Default Axial compressor map
  #1
Member
 
Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 5
olegmang is on a distinguished road
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
File Type: jpg Stage 37 performance.jpg (21.5 KB, 85 views)
olegmang is offline   Reply With Quote

Old   December 6, 2011, 15:29
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
you are simulating with 14000 elements only? or atleast for the map shown here
Far is offline   Reply With Quote

Old   December 6, 2011, 19:43
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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
ghorrocks is offline   Reply With Quote

Old   December 7, 2011, 05:27
Default
  #4
Member
 
Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 5
olegmang is on a distinguished road
Quote:
Originally Posted by Far View Post
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 ).
olegmang is offline   Reply With Quote

Old   December 7, 2011, 05:45
Default
  #5
Member
 
Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 5
olegmang is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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)?
olegmang is offline   Reply With Quote

Old   December 7, 2011, 09:09
Default
  #6
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by olegmang View Post
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.
Far is offline   Reply With Quote

Old   December 7, 2011, 11:19
Default
  #7
Member
 
Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 5
olegmang is on a distinguished road
Quote:
Originally Posted by Far View Post
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.
olegmang is offline   Reply With Quote

Old   December 7, 2011, 18:25
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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?
ghorrocks is offline   Reply With Quote

Old   December 8, 2011, 05:27
Default
  #9
Member
 
Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 5
olegmang is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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
File Type: jpg Pre screenshot.jpg (94.7 KB, 58 views)
Attached Files
File Type: doc Stage 37_PSR.ccl.doc (34.8 KB, 45 views)
olegmang is offline   Reply With Quote

Old   December 8, 2011, 06:25
Default
  #10
D.B
Member
 
DB
Join Date: Apr 2011
Posts: 62
Rep Power: 6
D.B is on a distinguished road
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
D.B is offline   Reply With Quote

Old   December 8, 2011, 06:37
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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?
ghorrocks is offline   Reply With Quote

Old   December 8, 2011, 08:31
Default
  #12
Member
 
Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 5
olegmang is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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
File Type: jpg Streamlines.jpg (72.0 KB, 43 views)
File Type: jpg Mach number.jpg (41.2 KB, 32 views)
File Type: jpg Velocity.jpg (80.5 KB, 35 views)
olegmang is offline   Reply With Quote

Old   December 8, 2011, 13:10
Default
  #13
Member
 
Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 5
olegmang is on a distinguished road
Quote:
Originally Posted by D.B View Post
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).
olegmang is offline   Reply With Quote

Old   December 8, 2011, 13:19
Default
  #14
Member
 
Oleg
Join Date: Nov 2011
Location: Ukraine, Kharkov
Posts: 57
Rep Power: 5
olegmang is on a distinguished road
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
olegmang is offline   Reply With Quote

Old   December 8, 2011, 13:26
Default
  #15
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Try this
time scale factor = 1
Reference pressure = 0
Use average static pressure boundary condition at outlet

What is the maximum yplus in domain?
Far is offline   Reply With Quote

Old   December 8, 2011, 13:43
Default
  #16
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
pls attach residual plots
Far is offline   Reply With Quote

Old   December 8, 2011, 17:26
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   December 9, 2011, 09:23
Default
  #18
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by olegmang View Post

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
Far is offline   Reply With Quote

Old   December 11, 2011, 03:53
Default
  #19
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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"
Far is offline   Reply With Quote

Old   December 11, 2011, 19:01
Default
  #20
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks 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
axial and z-velocity difference? user0314 FLUENT 0 August 25, 2011 17:18
how to plot out circumferentially mass averaged axial velocity in a rotor? wildli FLUENT 0 July 17, 2010 15:54
Transient axial rotor/stator convergence issue? Nicola Viscanti CFX 3 March 17, 2010 05:15
axial and azimuthally averaged profiles student CFX 0 February 28, 2006 05:20
About the design of axial fans HanCheolHeui Main CFD Forum 0 September 8, 1998 10:13


All times are GMT -4. The time now is 16:18.