[FutureCX]

Hi, I am simulating the pressure change caused by the sudden velocity increase in the pipe with a surge tank as the following picture. I set a transient table at velocity inlet and atmosphere pressure at two pressure outlets. By using transient simulation, the wave was observed, and wave reflections appeared among inlet boundary, surge tank and outlet boundary. But the problem is that wave would reflect again when it reached the inlet and outlet boundaries. Ideally, I want the wave to pass the boundaries without any reflection.



This wave reflection is defined as non-physical wave reflection in Ansys User's Guide. The guide suggests to use NRBC (Non-reflecting boundary condition) to eliminate this reflection. I can only set NRBC at pressure outlet boundary to remove the wave reflection at outlet, but there is no such option for velocity inlet boundary. Does anyone know how to eliminate the wave reflection at velocity inlet boundary? Thanks in advance.

[anjelicamove]

Hello Everyone
Here are some excellent PC components for you gaming PCs. Just click the link and you will get what you will want https://betasimracing.com/processor/
Stay Blessed

[LuckyTran]

It shouldn't be an isssue as long as you use the NRBC at the outlet. The wave won't reflect at the outlet back towards the inlet anymore and there won't be a wave passsing back towards the inlet (to be reflected) that needs to be transmitted.


An nrbc inlet is non-trivial and afaik is not implemented in Fluent.

[FutureCX]

Originally Posted by LuckyTran

It shouldn't be an isssue as long as you use the NRBC at the outlet. The wave won't reflect at the outlet back towards the inlet anymore and there won't be a wave passsing back towards the inlet (to be reflected) that needs to be transmitted.


An nrbc inlet is non-trivial and afaik is not implemented in Fluent.

Thanks for your reply. Maybe I need to describe the problem in more detail.

When the inlet velocity changes suddenly, a pressure wave can be generated at inlet boundary and propagate to the downstream (outlet boundary). Once the wave arrives at the surge tank, a part of wave will be reflected and go back to upstream (inlet boundary) while the rest continues propagation toward downstream.

When the reflected wave arrives at the inlet boundary, it will be reflected again and go to surge tank. But for the wave propagating to the downstream without reflection, it will disappear at outlet boundary because of the NRBC at pressure outlet boundary.

I'd like to set NRBC at inlet boundary to eliminate the wave reflection, but there isn't such option for velocity inlet boundary. So I wonder how I can figure out the wave reflection at velocity inlet boundary. I hope that my description is understandable

[LuckyTran]

Unless there is a nrbc in the latest version of Fluent that I'm not aware of, then you need to find a workaround. A fixed velocity boundary condition, as if you have experienced, is perfectly reflecting.

You could use a freestream inlet to soften up the inlet boundary but it will kind of only get you half way there.

Another workaround is to apply an acoustic sponge via momentum and/or energy sources. Create a region in your domain around the inlet and define a sink that is proportional to the difference in the actual, instantaneous flow velocity and your desired plug velocity. Preferably, you would initialize your case with the wave already having propagated past the sponge if you get what I mean. You might want to extend your inlet upstream if your current setup doesn't have any room for this sponge.

For proprietary reasons, I cannot tell you how to implement a non-reflecting velocity condition except to tell you to go look it up in the literature and do it yourself. I've been begging the Fluent (and other CFD software) developers to implement this boundary condition for well over a decade.

[FutureCX]

Originally Posted by LuckyTran

Unless there is a nrbc in the latest version of Fluent that I'm not aware of, then you need to find a workaround. A fixed velocity boundary condition, as if you have experienced, is perfectly reflecting.

You could use a freestream inlet to soften up the inlet boundary but it will kind of only get you half way there.

Another workaround is to apply an acoustic sponge via momentum and/or energy sources. Create a region in your domain around the inlet and define a sink that is proportional to the difference in the actual, instantaneous flow velocity and your desired plug velocity. Preferably, you would initialize your case with the wave already having propagated past the sponge if you get what I mean. You might want to extend your inlet upstream if your current setup doesn't have any room for this sponge.

For proprietary reasons, I cannot tell you how to implement a non-reflecting velocity condition except to tell you to go look it up in the literature and do it yourself. I've been begging the Fluent (and other CFD software) developers to implement this boundary condition for well over a decade.

I really appreciate for your instruction. In the latest Fluent, I can add a sponge layer at velocity inlet boundary. For this sponge layer, I need to define the far-field density, ramping distance and total thickness. But the User's Guide only gives a rough definition about the ramping distance and the total thickness.

I have tried this function in my simulation, it did work. But the solution could be different. Also, the continuity equation couldn't get converged. Do you know how to set this sponge layer properly? Thanks.

[LuckyTran]

The sponge layer must be tuned for each individual case because it depends on the frequencies and wavelengths of the acoustic wave. The ramping distance smooths the sponge so that it isn't a hard cutoff, making the numerics play a bit nicer. The sponge distance controls the strength of the absorption. The thicker the sponge the more your bonudary is non-reflecting, but the more the sponge the more the solution can drift from your desired set constraint. You have to figure it out by doing several trials. Without knowing the details of the geometry, I cannot make any recommendations on what the appropriate thickness ought to except that it is proportional to the wavelength of the wave you need to absorb.

[FutureCX]

Originally Posted by LuckyTran

The sponge layer must be tuned for each individual case because it depends on the frequencies and wavelengths of the acoustic wave. The ramping distance smooths the sponge so that it isn't a hard cutoff, making the numerics play a bit nicer. The sponge distance controls the strength of the absorption. The thicker the sponge the more your bonudary is non-reflecting, but the more the sponge the more the solution can drift from your desired set constraint. You have to figure it out by doing several trials. Without knowing the details of the geometry, I cannot make any recommendations on what the appropriate thickness ought to except that it is proportional to the wavelength of the wave you need to absorb.

Thank you for such a detailed answer. I think I can start from tuning the sponger layer. Besides, I have the last question about the sponge layer. Can sponge layer at velocity inlet affect the initial generated pressure wave? In my simulation, I noticed that the pressure value of the generated wave showed a distinct linear drop once the sponge layer was added. I am not sure if this pressure drop was caused by the sponge layer.

[LuckyTran]

Yes. Consider a stationary step function (your initial condition effectively) is a combination of a rightward traveling impulse and a leftward traveling expansion wave. This expansion wave is now non-reflecting due to your new treatment.

[FutureCX]

Originally Posted by LuckyTran

Yes. Consider a stationary step function (your initial condition effectively) is a combination of a rightward traveling impulse and a leftward traveling expansion wave. This expansion wave is now non-reflecting due to your new treatment.

That makes sense. Anyway, I really appreciate for your kind help. And I will start from the setting of sponge layer first.

Kind regards.

[LuckyTran]

I briefly mentioned but just to explain it a little bit better. The sponge layer has a damping curve which is generally strongly damping at high frequencies (and short wavelengths) and less effective at low frequencies (and long wavelengths). The damping curve is rather smooth and very broadband.

You just need the damping to be effective for your particular wave, which means you just need to be in the right ballpark for the sponge length with respect to the wavelength of the reflected wave(s). The tuning can be very coarse and does not need to be very fine. For example if my wave has wavelength of 2 m, I would try 1 m, 5 m, and 10 m. You don't need to test small deltas like 1.1, 1.2, 1.3 m. Think orders of magnitude or scales proportional to quarter-wavelengths.

[FutureCX]

Originally Posted by LuckyTran

I briefly mentioned but just to explain it a little bit better. The sponge layer has a damping curve which is generally strongly damping at high frequencies (and short wavelengths) and less effective at low frequencies (and long wavelengths). The damping curve is rather smooth and very broadband.

You just need the damping to be effective for your particular wave, which means you just need to be in the right ballpark for the sponge length with respect to the wavelength of the reflected wave(s). The tuning can be very coarse and does not need to be very fine. For example if my wave has wavelength of 2 m, I would try 1 m, 5 m, and 10 m. You don't need to test small deltas like 1.1, 1.2, 1.3 m. Think orders of magnitude or scales proportional to quarter-wavelengths.

Got it. That's why the User's Guide suggests the total thickness should be the twice length of the wavelength at least. And the coarse test should be enough to ensure the proper setting.

[FutureCX]

Originally Posted by LuckyTran

I briefly mentioned but just to explain it a little bit better. The sponge layer has a damping curve which is generally strongly damping at high frequencies (and short wavelengths) and less effective at low frequencies (and long wavelengths). The damping curve is rather smooth and very broadband.

You just need the damping to be effective for your particular wave, which means you just need to be in the right ballpark for the sponge length with respect to the wavelength of the reflected wave(s). The tuning can be very coarse and does not need to be very fine. For example if my wave has wavelength of 2 m, I would try 1 m, 5 m, and 10 m. You don't need to test small deltas like 1.1, 1.2, 1.3 m. Think orders of magnitude or scales proportional to quarter-wavelengths.

Hi LuckyTran, thanks for your previous help on my case. I am using VOF model with the same geometry to simulate the air hammer caused by a sudden velocity increase of water flow at the inlet boundary. Right now, I am facing two problems.
(1). For air phase, should I use compressible liquid or idea gas law considering an isothermal condition?
(2). As the speed of pressure wave is much faster than the local velocity, how can I ensure the courant number below 1 as tiny time step can slow down simulation too much?
Any suggestions could be appreciated.