CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Axial compressor calculation steps? (https://www.cfd-online.com/Forums/cfx/94382-axial-compressor-calculation-steps.html)

 olegmang November 14, 2011 08:39

Axial compressor calculation steps?

Dear All. I'm a newbie in CFX calculations and i need your advices concerning calculation of axial compressor stage in CFX.
I calculated axial turbine before and everything was OK. But in compressor (Stage 37), when i set the same boundary conditions (P_total_in, T_total_in and P_static_out) the flow goes in wrong direction. Solver puts wall on 100% of inlet. The only way i managed to calculate it right is by setting of "supersonic" in outlet conditions.

Could you please tell me what i'm doing wrong and what are the right steps of compressor calculation should be?

TIA, Oleg.

 Far November 14, 2011 08:43

rpm is 17188.7 or -17188.7?

 olegmang November 14, 2011 08:48

-17188.7 rpm

 Far November 14, 2011 08:49

whats inlet and outlet pressure? and flow direction (-1 axial, 0 for other directions)?

 olegmang November 14, 2011 09:05

Inlet total pressure 101.4 kPa, outlet static pressure = 138 kPa. I'm not sure what you mean on "flow direction". The flow goes in reverse direction comparing to how it shoud be (from outlet to inlet)

 Far November 14, 2011 09:08

are you using rotor or complete stage. If rotor then 138 KPa is very high value, beyond the stall point!! Even with stator case, it is still too high value, have start with 101325 Pa and gradually increase in increment of 5000

 olegmang November 14, 2011 09:14

really, i'm not sure that i'm doing as i suppose to do for compressor.

dear Far. Maybe there's some specific BC or loss model need to be set for compressor calculation? Is the task formulation that i use right and compressor should calculate OK with such scope boundary conditions an the probles is just in me?

 olegmang November 14, 2011 09:19

Quote:
 Originally Posted by Far (Post 332005) are you using rotor or complete stage. If rotor then 138 KPa is very high value, beyond the stall point!! Even with stator case, it is still too high value, have start with 101325 Pa and gradually increase in increment of 5000
I'm using comlete stage.

Thanks for the advise. While increasing pressure on 5000 Pa what should i control as convergense parameter? Mass flow or maybe something else? in other words when should i decide that I can inrease pressure?

 Far November 14, 2011 09:19

Simple. Just use 101325 pa as inlet pressure (or profile at later stages) and outlet pressure 101325, then gradually increase static pressure at outlet to

105000
110000
115000
120000
122500
125000
127000
128000
129000

 olegmang November 14, 2011 09:33

I understood about increasing outlet pressure step by step. But what parameter should i control to decide that it is the right time to increase pressure? e.g. i'm doing calculation for P_stat_out=101325, controlling what parameter i can decide that it's time for increasing presure up to 105000? Mass flow rate stabilize? or maybe some of convergense parameters go lower than some specific value?

 ghorrocks November 14, 2011 17:32

If the inlet pressure is about 101kPa and the outlet pressure is about 130kPa then you should be using a reference pressure of 101kPa and an inlet pressure of 0kPa, outlet of 29kPa. If you do not use a reference pressure you will have more round-off error and that can lead to convergence problems.

Are you using a reference pressure?

 olegmang November 15, 2011 05:33

Quote:
 Originally Posted by ghorrocks (Post 332089) If the inlet pressure is about 101kPa and the outlet pressure is about 130kPa then you should be using a reference pressure of 101kPa and an inlet pressure of 0kPa, outlet of 29kPa. If you do not use a reference pressure you will have more round-off error and that can lead to convergence problems. Are you using a reference pressure?
No i dont. I'll try.

 olegmang November 15, 2011 07:35

Dear ghorrocks.

I have a question concerning total pressure ratio. Can i plot total pressure at stage oultet while solver running the calculation in new monitor?

 Far November 15, 2011 08:34

Could you please post some pics of your domain and mesh. Also post information about total no of nodes in domain, any information about the interface between rotor and stator.
Any how, compressor flows are more difficult to handle than the turbine and you need to handle it by putting little load at start-up (in terms of rpm and pressure at outlet) and then ramp-up to desired value. Also search the forum for older posts regarding the same issue

 olegmang November 15, 2011 09:53

Thanks Far!

 olegmang November 15, 2011 10:33

1 Attachment(s)
Quote:
 Originally Posted by Far (Post 332185) Could you please post some pics of your domain and mesh. Also post information about total no of nodes in domain, any information about the interface between rotor and stator.
Number of nodes 229118. All interfaces are set as "Stage". The picture of domain is attached.

 Far November 16, 2011 00:32

This should also be noted as the no. of nodes increases compressor simulation tend to numerically stall at the higher pressure ratio than for coarse mesh. Therefore it is good idea to refine mesh further and also check the solution at lower back pressure for the current mesh.

Moreover which turbulence model you are using? What is Y+ in domain? Since appropriate Y+ should be used for each model.

Other things to be checked are (important to solution convergence and accuracy): aspect ratio, max and min angle, expansion rate

 olegmang November 16, 2011 06:29

Quote:
 Originally Posted by Far (Post 332247) This should also be noted as the no. of nodes increases compressor simulation tend to numerically stall at the higher pressure ratio than for coarse mesh. Therefore it is good idea to refine mesh further and also check the solution at lower back pressure for the current mesh. Moreover which turbulence model you are using? What is Y+ in domain? Since appropriate Y+ should be used for each model. Other things to be checked are (important to solution convergence and accuracy): aspect ratio, max and min angle, expansion rate
I'm using the SST model. On blade surface maximum Yplus is 200, on nozzle 100.
+--------------------------------------------------------------------+
| Domain Name | Orthog. Angle | Exp. Factor | Aspect Ratio |
+----------------------+---------------+--------------+--------------+
| | Minimum [deg] | Maximum | Maximum |
+----------------------+---------------+--------------+--------------+
| Rotor | 41.5 ok | 6 ok | 736 ok |
| Stage in | 85.7 OK | 1 OK | 7 OK |
| Stator | 46.0 ok | 40 ! | 52 OK |
| Global | 41.5 ok | 40 ! | 736 ok |
+----------------------+---------------+--------------+--------------+
| | %! %ok %OK | %! %ok %OK | %! %ok %OK |
+----------------------+---------------+--------------+--------------+
| Rotor | 0 <1 100 | 0 <1 100 | 0 2 98 |
| Stage in | 0 0 100 | 0 0 100 | 0 0 100 |
| Stator | 0 <1 100 | <1 1 99 | 0 0 100 |
| Global | 0 <1 100 | <1 <1 100 | 0 1 99 |
+----------------------+---------------+--------------+--------------+

 Far November 16, 2011 08:16

Use K-epsilon (also use lower pressure at outlet as discussed earlier)

 olegmang November 16, 2011 08:19

Quote:
 Originally Posted by Far (Post 332308) Use K-epsilon (also use lower pressure at outlet as discussed earlier)
Thank you. I'll try.

All times are GMT -4. The time now is 00:07.