Axial compressor map

olegmang · December 6, 2011, 07:10

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

Far · December 6, 2011, 15:29

you are simulating with 14000 elements only? or atleast for the map shown here

ghorrocks · December 6, 2011, 19:43

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

olegmang · December 7, 2011, 05:27

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

).

olegmang · December 7, 2011, 05:45

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)?

Far · December 7, 2011, 09:09

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.

olegmang · December 7, 2011, 11:19

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.

ghorrocks · December 7, 2011, 18:25

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?

olegmang · December 8, 2011, 05:27

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.

D.B · December 8, 2011, 06:25

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

ghorrocks · December 8, 2011, 06:37

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?

olegmang · December 8, 2011, 08:31

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.

olegmang · December 8, 2011, 13:10

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).

olegmang · December 8, 2011, 13:19

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

Far · December 8, 2011, 13:26

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 · December 8, 2011, 13:43

pls attach residual plots

ghorrocks · December 8, 2011, 17:26

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.

Far · December 9, 2011, 09:23

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

Far · December 11, 2011, 03:53

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"

ghorrocks · December 11, 2011, 19:01

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.

December 8, 2011, 06:25		#10
D.B Member DB Join Date: Apr 2011 Posts: 87 Rep Power: 15	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

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
axial and z-velocity difference?	user0314	FLUENT	1	May 27, 2016 13:30
how to plot out circumferentially mass averaged axial velocity in a rotor?	wildli	FLUENT	0	July 17, 2010 16:54
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 11:13

December 6, 2011, 15:29		#2
Far Senior Member Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,558 Blog Entries: 6 Rep Power: 54	you are simulating with 14000 elements only? or atleast for the map shown here

December 6, 2011, 19:43		#3
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	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, 18:25		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	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, 06:37		#11
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	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, 13:19		#14
olegmang Member Oleg Join Date: Nov 2011 Location: Ukraine, Kharkov Posts: 57 Rep Power: 15	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
Far Senior Member Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,558 Blog Entries: 6 Rep Power: 54	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
Far Senior Member Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,558 Blog Entries: 6 Rep Power: 54	pls attach residual plots

December 8, 2011, 17:26		#17
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	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 11, 2011, 19:01		#20
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	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.