CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Axial compressor map (https://www.cfd-online.com/Forums/cfx/95106-axial-compressor-map.html)

 olegmang December 6, 2011 07:10

Axial compressor map

1 Attachment(s)
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?:confused:
What have i done wrong?

Maybe someone could give me algorithm of compressor map calculating in CFX or at least some tips :o

 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

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 (Post 334910) 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 :o).

 olegmang December 7, 2011 05:45

Quote:
 Originally Posted by ghorrocks (Post 334932) 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 (Post 334974) 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 :o).
It is meaningless to have such a coarse mesh. Atleast try 200000 elements.

 olegmang December 7, 2011 11:19

Quote:
 Originally Posted by Far (Post 335009) 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

2 Attachment(s)
Quote:
 Originally Posted by ghorrocks (Post 335065) 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

3 Attachment(s)
Quote:
 Originally Posted by ghorrocks (Post 335112) 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 (Post 335110) 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 (Post 335163) 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?:p Just kidding

 Far December 11, 2011 03:53

Quote: