[Bananenflanke]

Hi,

I would like to investigate the acoustic behaviour of a centrifugal pump. For this purpose I want to generate a wave in front of the non-driven pump and determine which part of the wave is reflected by the pump and which part is transmitted by the pump. Some preliminary studies have shown that this probably requires very small time steps (10^-5...10^-6 s) and a fine grid. Probably the computational effort will therefore be very large, so I wonder how I can reduce the effort?

My thoughts so far:
- I should do sensitivity analyses for the time step and the grid.
- I should check how long the pipes before and after the pump have to be, so that the boundary conditions imposed at the pipe ends do not influence the results. Perhaps the pipe length can be further reduced by using boundary conditions that allow the development of a transverse profile. For example by using the average pressure condition instead of the static pressure condition at the outlet or the total pressure condition instead of a uniform velocity at the inlet.
- Another idea would be to simulate only one blade channel instead of the entire impeller and to work with the rotational periodicity for interfaces, although I am not sure about this. As I understood it, with this simulation approach the flow in each blade channel would be exactly the same. But since the surrounding of the impeller (volute) is not rotationally symmetric, the flow in reality should be slightly different in each blade channel. Therefore it seems to me that this approach is not correct. Is my understanding of rotational periodicity and my conclusion correct?

Does anyone have further ideas how to reduce the calculation effort?

Greetings!

[Stel]

- Sensitivity tests for grid and time step are actually important in every serious CFD problem but it will be particularly critical to yours. Only by testing is how you will be able to tell how fine your grid and time step will have to be for you to obtain physically consistent results without prohibitive computational time.
- True, you do also have to test not just how far your inlets and outlets will have to be positioned from your region of interest to minimize effects on results, but also the most phisically consistent one (or the most robust one). Usually, total pressure (and temperature) conditions are the more robust for this kind of problem. One thing with transonic problems (if that is the case) is that velocities are so high that solving boundary layers becomes impractical. However, unless the boundary layer flow interferes decisively with your problem (I mean, the acoustic one you are interested in), you could very well neglect solving it. You could do that for instance by assuming free-slip walls everywhere, that would significantly reduce grid refinement requirements and the problem should also converge faster. This is quite a reasonable assumption for FFT analysis of rotating machinery working at very high rotating speeds (such as turbines), for example. But again, only testing will tell.
- Yes, assuming only one channel together with rotational periodic conditions will mean, by definition, that the flow you solve within this channel is representative of the flow through all channels. For symmetric or periodic components (such as an impeller interacting with a pipe upstream and with a diffuser with the same number of blades downstream), that assumption works very well for evaluating Head, Efficiency, and other global parameters, and also quite well for local properties. Of course, there is also how you treat the interface between components, since transient rotor-stator analysis gives a more realistic impeller-stator interaction than frozen rotor or stage connections. But for largely asymmetric components (such as volutes), the rotational periodic assumption will certainly not be ideal. I guess that it will conceptually affect your objectives at some degree, since analyzing acoustics depends upon how different components interact through a rotating machinery assembly. BUT, as always, this could be also subject to testing. You could start with just one passage interacting with the volute, then you add another one, then another one, then you assume the whole 360, and then you compare solutions to investigate how they behave. In the end, the kind of response you expect will help you to decide which approach will be the best one for you in terms of the trade-off between accuracy and computational effort. In any case, considering transient rotor-stator interfaces here seems to be important.

As for assumptions, in general: people are sometimes afraid to adopt many of them because they read something very general about them in manuals and books, without even testing them in the first place to understand what they actually do or to see how they fit (or not) to their problem. My personal opinion: it is the duty of CFD engineers to simplifiy their problems as much as they can, according to the very kind of response they expect from their model. So, by now you already see that my suggestion here is for you to test all of those assumptions, it may happen that some of them which look too simplistic for you would work just as fine as a more complex one, given your interests.

Good luck.

[ghorrocks]

Stel's comments are important for the CFD side of things, I want to make a few points about acoustics modelling specifically:

Acoustics modelling is a specialised sub-section of CFD modelling. It is common in automotive applications and many other industries where noise levels are important.

You really should read some acoustics textbooks before doing any acoustics modelling. For instance, a common approach is to use CFD to model the near-field behaviour and interface to a acoustics simulation package some distance away from the object. Acoustics simulation packages use much simpler mathematical models of wave propagation than the Navier Stokes equations, meaning you can model out to the far field easily. Packages like SYSNOISE are commonly used for this.

If you are modelling acoustics in the pipes around your machine be aware that the traditional approach of moving the boundary conditions far enough away that they do not affect the result is likely to not be possible. Acoustic waves propagate a VERY long way (which is why you can hear aircraft from kilometres away). The waves in the pipe will reflect from whatever is in the pipe, even if it is a long way away. You will need to think carefully about boundary conditions for pipes. Normal inlets and outlets are not appropriate and do not reflect waves correctly for most applications.

[Bananenflanke]

Hi Stel,

thank you for your detailed suggestions! Regarding the treatment of the interface between the impeller and the volute, I have one more question. Since the impeller does not rotate in the simulation, I can imagine that the frozen rotor approach can work as well. Is there maybe a reason why this should not work or is this another possibility I can test to reduce the computational effort?

Hi ghorrocks,

thank you for sharing your thoughts on the acoustic aspects!

Regarding the coupling of cfd and an acoustics simulation package:
As Gülich describes it in his book "centrifugal pumps", the hydrodynamic near-field in a centrifugal pump is created by the unsteady flow in front of the impeller and the uneven velocity distribution over the outlet of the impeller. Furthermore, all structures near the impeller inlet and outlet (i.e. in the near field) act as secondary sound sources. In my opinion, therefore, most of the computational domain (pump and pipes) should be calculated using cfd, partly because the spatial transition between near and far field is unclear. Therefore I wonder whether the effort of coupling cfd and an acoustics simualtion package (implementation, calculation time) is worth it, or whether the savings in calculation are used up, for example by the data transfer between cfd and the acoustic simulation package. Even if this is probably not possible without further information, can you or someone else estimate whether it would be worthwhile?

Regarding the boundary conditions:
As boundary conditions I want to try the non-reflecting boundary conditions, which are implemented as a beta function in CFX, and if that does not work, I want to coarsen my mesh in the area of boundary conditions.

[ghorrocks]

You will find the mesh and time steps required to model acoustics to the far field are prohibitive. You will already have a crazy big mesh when it is fine enough to just model the near field behaviour. The only practical way in most cases to model out to far field is to couple to the far simpler acoustic equations and use the acoustic solver to go out to far field.

But don't take my word for it, do a little demonstration simulation where you put a noise source in the middle of the domain, and do mesh and time step independence checks to see what mesh and time step you need to model the waves. You will find you won't be able to model very far before you max out the world's biggest supercomputer.

Non-reflecting boundary conditions: Keep in mind there is no such thing as a non-reflecting boundary condition, just a boundary condition which reflects less others. Also, keep in mind what this means: an ideal non-reflecting boundary condition means a far field condition (ie reflections never come back). In reality you do get reflections in acoustics from the far field (think echoes off a distant cliff line). If you are modelling acoustics in pipes then you get reflections off objects huge distances away. Are you sure a non-reflecting boundary is what you want? (I don't know what you are doing so cannot say)

[Bananenflanke]

Thank you for your further thoughts.

Your suggestion to put a sound source in the domain center seems like a good way to test what is possible. Thanks!

The goal is to find out what happens when a wave hits a pump. Which part of the wave is reflected by the pump and which part is transmitted. Therefore it would be advantageous if (almost) no reflections occur at the boundaries. Nevertheless, it would also be possible to use reflective boundary conditions, but the evaluation of the data would then be more difficult because standing waves would then occur in the pipes before and after the pump.

[ghorrocks]

If you are not modelling the generation of the sound, just the reflection of the wave on the surface then forget CFD and do it all in an acoustics simulation software. As long as the acoustics waves are in the linear region then the acoustics models will work fine and CFD is not required. It will run in a flash and is simple and easy to get working as they are linear equations compared to the non-linear Navier Stokes equations.

[ghorrocks]

Also, the structural response of the pump may be important as well. If you need to include this it is a FSI thing, not just CFD.

[Stel]

Originally Posted by Bananenflanke

Hi Stel,

thank you for your detailed suggestions! Regarding the treatment of the interface between the impeller and the volute, I have one more question. Since the impeller does not rotate in the simulation, I can imagine that the frozen rotor approach can work as well. Is there maybe a reason why this should not work or is this another possibility I can test to reduce the computational effort?

Oh, so your impeller is static... I didn't understand that part in your first post, sorry.

Well, if it is static so there is no need to use another type of interface connection because your rotor is literally frozen. The transient rotor-stator will only make sense when you have relative motion. But in ANSYS CFX in particular if you assume only one blade channel you still need to use Frozen Rotor instead of a general fluid-fluid connection not because of the "Frozen Rotor" itself, but actually because of the Pitch Change, so that CFX will calculate the pitch scale to transfer information through the two sides of the interface which will not be equivalent in area.

[Bananenflanke]

@ghorrocks
Thank you very much for the hints!

The plan was to transfer the mesh, the results and the experiences of the simulation described here to a subsequent simulation later on, which will be about the generation of sound. Either way, a cfd simulation will be necessary. However, as soon as enough experience has been gathered, the sole use of acoustic software for the simulation described here looks promising.
I have not yet dealt with the theory of FSI simulation, but it would probably be even more complex than the approaches discussed so far? Nevertheless, it is probably the next step if the hardware resources are sufficient and the results obtained before are not accurate enough.

@Stel
Thanks for the clarification!

[ghorrocks]

The plan was to transfer the mesh, the results and the experiences of the simulation described here to a subsequent simulation later on, which will be about the generation of sound. Either way, a cfd simulation will be necessary.

This comment does not make sense based on what you appear to be doing is just modelling the reflection of linear waves. You are trying to do this the really, really hard way if you do it by CFD. But whatever, it is your analysis not mine

I have not yet dealt with the theory of FSI simulation, but it would probably be even more complex than the approaches discussed so far?

Yes, it sure is. You should do some experiments or analysis to see if this effect is significant before starting on it because it is a very expensive simulation to do. There is a good chance it is not significant and then it can be ignored.

[Bananenflanke]

You are certainly right that using an acoustic simulation to model the reflection and transmission of linear waves to and through a pump would be much easier. But the results of this simulation are needed for a further simulation. In this simulation the near field (and far field) of the pump has to be investigated, for which at least partly a cfd simulation has to be used. The intention to use cfd for the first simulation is to determine as early as possible whether the project can be successful. If it turns out that it is not possible to find out the transmission and reflection behaviour of the pump using a cfd simulation, then it would probably not be possible to investigate the generation of sound in the pump in a subsequent simulation. Furthermore, I would not have to worry about two completely different simulations in the beginning. But if it turns out that the cfd simulation is possible, it would make sense to do the first simulation with an acoustic simulation to save time in the future. In this way, one could also compare the results of cfd simulation with those of acoustic simulation and determine whether the assumption of linear waves is justified. I hope that the intention of the procedure has now become somewhat clearer and it makes sense.

But probably it is better if I first try it out on a simpler model and clarify some uncertainties.

[ghorrocks]

CFX certainly can model the acoustics you are talking about, and it can also model the sound generation as well.

it is good to hear you are doing some simpler models to clarify things before doing the complex model. This will help sort out the technique in a reasonable time.

Don't forget my comment about using CFD to model the near field and interface to an acoustics model for the far field. This is the standard way of doing these sort of simulations as you will find doing it in CFD all the way to far field is going to be impossibly large. But hopefully your preliminary simple model will demonstrate this.