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.

rpm is 17188.7 or -17188.7?

-17188.7 rpm

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

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)

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

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?

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?

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

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?

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.

Thank you for advice.

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?

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

Thanks Far!

Number of nodes 229118. All interfaces are set as "Stage". The picture of domain is attached.

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 |
+----------------------+---------------+--------------+--------------+

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

Thank you. I'll try.

Also wanted to ask. Do you advise me K-epsilon because calculation of compressor converges better (it should be used for hardconverging cases) with it than SST model. Or it is common practice for compressors to use K-epsilon?

I feel for a standard case like this these issues might not be the problem. 1st question I would like to ask you is for how many iteration do you get the 100 % blockage ?

For a lot of my cases I have seen is that mostly there is something horrendously wrong with the solution set up and not so much with choice of turbulence models or y+.

If your solution crashes after a lot of simulations with 100% wall block then double check your setup ( especially if your axis is correct ) and if you can post your out file here so someone can find out the error.

What is the advection scheme you are using ? and also what point on the performance curve are you trying to simulate, if it is near stall point you will have to tread carefully, especially with the choice of advection scheme. Also check the timescale in your simulation setup. Hope this helps.

well, the SST model in better in performance but it tends to over predict the separation zone and therefore likely to have numerical stall at lower pressure ratio than in real. second problem is that with automatic wall treatment solution become unstable with hybrid wall functions (automatic wall treatment in CFX) at large values of Y+. See paper of knopp (DLR) in J. Computational Physics 2006

K-epsilon model is designed for wall function meshes therefore it should not problem with this model. Another advantage (you can say it weakness :D) is that, due to under prediction of separation (even no separation at all) this model tends to be more robust near the stall point and should give you decent solution in extreme conditions. This model should be your first choice if you are not interested in separation, losses and just want to predict the overall solution like mass flow rate, pressure ratio and efficiency (yes you heard right I am saying efficiency, with advance models like SST, RSMBSL it is normally under predicted due to higher losses).

As I have pointed out earlier in this thread that with coarse mesh (as you have like 0.1 million cells in each component), you should get the required pressure ratio with less back pressure at outlet. So if you are specifying the higher pressure ratio beyond the stall point then CFX must always fail. So reduce your static pressure by factor of 2 and rerun case again.


As DB said if your set-up is wrong then we can not be of any help to you, since we assume that you have setup problem correctly, so it is the time to double check every thing in CFX pre.

Hi Far,
I am unable to download that paper ( knopp (DLR) in J. Computational Physics 2006 ) can you email a copy of it to me. my email id is bhatiadinesh05@gmail.com.

Thanks in Advance

Dear D.B
I get 100% blokage all the time when i set pressure drop 29kPa. MFR converges to 0 :)
When i'm rumping-up on pressure at outlet (with the same settings), as Far suggested me, everything goes OK.
I'm using high resolution advection scheme. i tried to simulate Design point. Now i decided to simulate point from performance map (reading 4188) to have an opportunity to compare with spanwise experimental data.

What do you advise as for advection scheme and timescale when calculating point near stall? And can i calculate e.g. compressor on coarse mesh and then caclulate in on fine mesh? Will it help to increase speed of calculation if i start from fine mesh with coarse mesh as initial guess or from fine mesh without initial guess? i.e. time for coarse mesh calc + time for fine mesh calc with coarse as initial guess <:confused:> time for fine mesh calc without any initial guess

You can run fresh case with fine mesh. No need for initial conditions. Initial guess is necessary when convergence is very difficult like for differential Reynolds stress turbulence models or flows with stiff numerics.

Time to get convergence for both settings should be typically same

sent two papers on hybrid wall functions

1) Knopp (DLR) 2006 J.Computational Physics
2) Kalitzin (Stanford University, Turbulence Research Centre) 2005 J. Computational Physics

This is known as numerical stall and may occur before actual stall due to numerical solution instability.

What do you mean by rumping up the pressure ? and by OK do you mean you are getting correct results or you are not getting back flow ? If your simulation is correct at design point then only go for higher pressure ratios.

I apologise,
I didn't have a great deal of idea about rotor 37 first, Now I have seen that it is a transonic rotor. So there could be some shocks ( I don't have the details so I can't say for sure ) and compressibility is definitely a factor. First confirm about the correctness of you converged simulation at design point and don't just compare the mass flow rate but try to see if you are getting a physically feasible solution.

As far as your simulation strategy goes first ensure that your grid is fine enough to resolve any shocks that might be present ( read literature to see if there are any ) and though I have never simulated transonic rotors I would think going for high advection scheme directly might be a bad idea ( not sure :D) , go for specific blend factor option, start from a value of say 0.6 early on and then slowly increase it in steps to value of 0.98-1.0, If you want after that taking this result as the initial file simulate with high resolution scheme.

I would say for timescale you can start by a guess of 1/w or 1.5/w. But I would seriously suggest for you to look at the grid, I think in this case it would be very important, try reading the literature for the kind of mesh you need.

Thanks................................

what do you say about domains meshes (picture attached). On picture below, from left to right, end of inlet domain, blade domain, nozzle domain. The mesh of inlet domain id much coarser than on rotor and stator domains. The question is should i remesh (increase number of elements) inlet domain?

As I told you I am not too experienced in transonic rotor simulations ( and your rotor -stator mesh is hardly visible ), but in any case there is a huge difference in your mesh density in your inlet domain and rotor-stator domains, I think this difference should have some implications especially if there are some non-linearities in the flow. Also in general such stark difference in mesh sizes should be avoided.

For inlet domain (which is not important for your simulation, it has only function to ease the solution right?) use coarse mesh and specify hub and casing as inviscid wall (wall with zero shear or slip wall). For rotor and stator at least use 0.3 million to 0.4 million nodes for each component for your serious simulation. For learning purpose it is OK to use coarse mesh.

I would recommend use the mesh of 1.0 million cells or higher for each component (while keeping the same mesh for the inlet part) and use SST model with Y+ = 1 to 15 (lower the better but also take care of aspect ratio) but this may be implemented at later stage when you very fully comfortable with your requirements like what to compare, at which location, tip clearance flow study or you want to implement some casing treatments for stall control.

And what about blade and nozzle. Should i set No slip or Free slip wall?

For blade and nozzle (Nozzle = stator, We should rather use the compressor terminology as opposed to turbine terminology) use the standard conditions on walls i.e. no slip.

Thanks again for helping to a newcommer not to lost in CFD labyrinth. And pardon for my english because it not on the level i wanted it to be. hope it wasnt hard to understand me :o

Dear Far, should I use "edit run in progress" button in solver manager for ramping up pressure gradually?
Because if I do this, then original value in cfx pre setup doesn't change. So , is it correct?

yes. It will just the conditions in the solver file not in pre file

dear friend: I am trying to simulate Unsteady case of Rotor 67. i am doing periodic rotation of rotor as i dont have stator blades. My concern is to get pressure difference on Harmonic balance (when transient simulation repeats same kinds of graphs).
How may i get it?
Secondly kindly share boundary conditions for the unsteady rotor case?
Third What equation is use for Pressure inlet distortion on steady case?