I am running a MFR problem composed of a single blade centered rotor slice and a single stator section. It has roughly 350k nodes and skews are greater than 20 deg., etc. The boundary surface on the rotor side of the stage interface is experiencing convergence difficulty and I can not get below a rms on the order of e-2 locally there. Any ideas? I am using the 2.10 ggi interface on TASCflow.

Thanks

(1). If the mesh and the geometry are consistent with the solution, and assuming that the numerical scheme in the code is good enough (you don't have much choice there), then you should get converged solution if the solution is steady-state. (2). The possibility number one: the solution is un-steady, it is oscillating, because it is part of the solution,or because there is flow separation somewhere. (3). The possibility number two: the solution does not like your mesh, or even your geometry. So, this is the place you can do something. Change the mesh first, in anyway you like, and observe the results. You should see the difference, unless your solution is already in the mesh-independent regime.(unlikely, I guess) (4). The possibility number three: you are giving the code a very hard time by solving a very complex geometry problem. This is easy to spot, look for any tutorial examples first and find one which is similar to your geometry. If you can't find one, then you could do your analysis "backward", that is make your geometry less severe step-by-step, and try to see whether the code can give you a converged solution. Also try to use a geometry which you think will give you flow field without "separation". (5). Remember that you are using someone's black box, so you need to move away from the good geometry step-by-step toward your geometry until the code fails. (6). The other way to do is to reduce the time step. But I guess, you should have done so already. (7). On the other hand, if you are having convergence problem, then it could mean that your existing design is not nice and smooth. Perhaps, you don't have choice either in geometry . You can easily verify that by calculating a simpler geometry case. (I don't even know the geometry of your problem.)

Thanks John,

I will try step-by-step on mesh. It just seemed strange due to its location at the interface, although the pitch change across is 40 to 27.69 degrees. Have tried time step,etc. Looking at the non-converged 'solution' at the stage interface boundary yields inflow unexpected for this point of operation...

Will investigate further. Thanks.

Non-convergence man,

How close are your rotor and stator (ie %chord)?

If your stator leading edge is located close to the interface it can lead to convergence problems. Try adding the parameter STAGE_PCONSTANT_FACTOR = 0.9 to your PRM file and run again. As for your timestep, use DTIME = 1.0/abs(omega1).

Let us know how it works.

Regards, Robin

I did the mesh over and 'apparently' have a similar issue in that I am getting inflow at this stage interface. The stator is 2 chord lengths away from the interface, however the rotor is.375" away from the interface. I am going to test another grid with rotor closer and farther away from the interface... any thoughts? At this point of operation much of the flow is tangential so I realize it may be hard to converge, but ...

Did not try that PCONSTANT factor yet... would it be appropriate if the ROTOR is close to the interface?

Thanks again-

Non-convergence guy,

I assume by your statement that .375" is close? Try moving the interface farther from the rotor. If you can, put the interface 1/2 chord from the outlet of the rotor.

Having reversed flow across a stage interface is plausible. Where is the recirculation occurring?

What kind of pump is it?

Robin

Robin,

Thanks for your help. In process of moving interface away from rotor as recommended.

Recirculation zone is plausible in at this point of operation, just assuming this is why it is not converging...

Mixed Flow pump...

thnaks

Robin,

Thanks for your help. In process of moving interface away from rotor as recommended.

Recirculation zone is plausible in at this point of operation, just assuming this is why it is not converging...

Mixed Flow pump...

thanks

Amazingly with the stage interface farther downstream the solution converged... now to check out the results...

I was lucky in that I could move it downstream... what if I couldn't have?

Thanks all

(1). Good comment. (2). If you don't say, nobody will know.

Non-convergence guy,

If you couldn't have moved it, you could still use the stage_pconstant_factor = 0.9 flag to help.

Regards, Robin

I am currently running a stage case (600K nodes) with 1/4 chord gap between rotor and stator which means the interface is only 1/8 chord from the blades. It runs great.

If your real machine has a relatively steady operating point, you will be able to get a reasonable stage solution. One little trick (haven't tested it rigorously but I think it helps at times) is to put the last couple of nodes (id-2:id,j=1:jd,k=1)) near the interface on the hub of the rotor (shroud too if it's rotating) as stationary walls in the absolute frame. That saves the code having to deal with stage averaging, a frame change, and a wall speed change all at one place. That's a tall order for any numerical scheme I think.

(1). Stator/rotor interaction is a strong function of the stage design. (2). For the turbine blades, the blade turning angle and the shape can be such that the flow at some distance ahead of the rotor (assuming there is no stator) will sense the existence of the rotor. (3). There is also a very complex vortex system and flow separation ahead and around the blade. It extends further upstream of the blade geometric leading edge. (4). In other words, there is a complex separation system ahead of the blade, which can easily extend into the upstream stator passage area. (5). So, the interface plane treatment is the key to avoid this problem in the steady state solution. If the interface plane allow the reverse flow or nearly zero flow , then it will present a problem to the rotor side calculation, because there is reverse flow at the inlet. (6). To, avoid this, the transient flow calculation with sliding interface can be used. But it is time consuming. (7). So, there are still unresolved basic problems in turbomachinery simulation. (single row is fine, but stage or multi-stage can be troublesome. because of the physics of the real flow)