impeller symmetry
 

Hi everyone :)

i've been simulating an impeller, and i notice some lack of symmetry, especialy when i measure the total presure, the impeller is rotating at 2500 RPM which make me think that something is wrong

The image 1 is a contour of the blades, hub and shroud
https://imgur.com/s8SbTal
https://imgur.com/s8SbTal https://imgur.com/s8SbTal
now as you can see, i highlight 2 zones, where is evident a lack of symmetry, what i mean is that the total pressure is different in this two zones, actually is different in every zone.
i've read the information about the inlet zone, and I used an inlet chanel of 100[mm] but that's the result that i'm getting.



i got 2 more questions 1 regarding to the parameter set in the inlet-outlet, and the other one about an imbalance in the monitor plot but i'm not really sure if I'm able to ask different topics in the same thread.


Thank you very much for you time, and help.
have a nice day :)

I assume the conditions you are applying are symmetrical.

Have you checked your model is adequately converged by doing a sensitivity analysis? Looking at the results of an inadequately converged simulation is pointless. While you are at it, also do a sensitivity check on the mesh resolution.

And don't forget that fluid mechanics often generates non-symmetric results from symmetric flows. The Von Karman vortex street is a classic example.

Right, Coanda effect is another example of the asymmetry which I have seen an several models.

thank you very much for your answers and time.

currently i'm performing a sensitivity analisys using the information that you guys post in the forum.

well, i did a sensitivity test and i didn't find a lot of difference between the models, i change the mesh size and add 2 monitors in my setup, also i increase the relevance in the critical areas. in the next figure you can se how do i improve the symmetry.

The other concern are the boundary conditions, for the inlet and outlet i'm using mass flow i have seen in the tutorials and videos in youtube, that for impellers they use pressure for the inlet and mass flow for the outlet, i used only mass flow because i'm only examinating the impeller not the impeller as a system, i'm not really sure about it but my teacher says it's ok.


Again guys, thank you very much fot the help

Could be a weaker form of rotating stall. Flow-field in a channel influencing the incidence angles of adjacent blades thus resulting in an inherently asymmetric and transient phenomenon. Would be interesting to view the circular motion of pressure and velocity in a transient simulation.

Video of rotating stall:
https://www.youtube.com/watch?v=5ppMtNLw0yo

A paper on rotating stall in centrifugal compressors:
https://link.springer.com/article/10...494-017-9877-z

thank you for the answer, i'm going to check the rotatig stall.
also, what do you think about the boundary conditions that i used? is that ok?

Well the boundary conditions depend on what you know about the case you want to simulate. So if you want to simulate for a certain pressure ratio, then total pressure inlet and static pressure outlet it is. If you want to simulate for a certain mass flow then I'd choose total pressure inlet and mass flow outlet. In both cases I'd go for total pressure inlet, because that's something you probably know (ambient total pressure * inlet efficiency).

Mass flow both at inlet and outlet seams redundant to me in a stationary simulation, because they should be the same anyway (mass continuity).
I didn't even know that that is a possibility so i can't tell you if it's ok (the simulation did converge though, so it should be ok?)

Here is a link to recommended boundary conditions:
https://www.sharcnet.ca/Software/Ans.../i1300679.html

Well the simulation converge when I choose 1e-4 as the RMS convergence criteria, but the imbalances are pretty high, then i choose to decrease the convergence criteria to 5e-5 and it didn't converge but the imbalances are really low, i'm suspecting about the mass, actually the mass keeps almost constan at 2% in the imbalance monitor, although, it's low i'm not pretty sure about that result.

Well if you define mass flow at inlet and outlet to be the same and constant, then mass flow imbalance should be zero by definition. But i can't believe this setup is stable and sufficient. I don't know all the parameters for massflow inlet/outlet of my head, did you define pressure and temperature (total or static) in atleast one of them? If not then there is no way for the solver to know at which pressure/temperature level he is at. See this thread:
https://www.cfd-online.com/Forums/cf...condition.html

If the imbalance stays positive or negative then that's a hint that something is off here. You would expect an oscillation of the imbalances around 0%.

In this thread everything is explained, just read through it and everything should be clear.
https://www.cfd-online.com/Forums/cf...-boundary.html

- It is difficult is say something regarding the influence of the inlet and the outlet on the symmetry of your solution without knowing your geometry and the amount of flow compared to the flow generated by the impeller. Can you share the full geometry?
- Don't trust the default convergence criterium 1e-4. In general that is not enough. Go as low as it gets.
- Create monitoring points on the impeller where you monitor pressure, velocity and tke. If these show flatlines, your solution might be converged.
- The pressure given in your first picture is 6e5. That is quite a lot for an impeller. What velocities do you generate?
- Connected to that, what about Y-Plus? And is your inflation layer the same everywhere?
- Currently I perform a calculation on an impeller which should also provide me a symmetrical solution, based on the geometry given. But CFX can't find one because of transient effects, like other members already mentioned. Below my impeller I observe a vortex to the bottom of the vessel. This vortex is never in the center of my vessel but wiggling around. Don't you have something similar?

well guys thank you very much for all the information that you are giving me, it's really helpful, I'm quite sure the problem is using the mass flow as boundary condition in the inlet and outlet, i was using an isothermal model and water at 4°C asumming that the density changes due to pressure wouldn't be relevant, that's why i choose those boundary conditions. Also, I don't really have to much information about the geometry because I created something quite different from the conventional. so i can't really calculate an inlet efficiency or any other parameter ralated to the geometry.
again thank you guys for everything, have a nice day :D