Outlet BC in a micro channel? waveTransmissive?
 

Hello Foamers! I'm facing some trouble in setting correct BC in my problem, I briefly descrive my problem:

I have a cylindrical micro channel with a diameter of 200m and 6cm long full of Argon at prescribed T and p. A cylindrical portion, set with setFields utility, of this channel is hit with a laser that immediately increase temperature (4000K) and pressure of the gas.
I want to study the expansion of the gas through two outlets (cylinder bases), in my first analysis no inlet is present.

The problem is axisymmetric and I use small wedge for the simulation, I use rhoCentralFoam as solver since I'm dealing with compressible unsteady simulation.
What are the correct BC for p, T and U at the outlets? I want a pressure of 1e-4 Pa at the outlet.
I tried the combination fixedValue for p, zeroGradient for T and U but I get overshoot for p and rho in the cells next to outlets.
Then I tried waveTransmissive for p, T and U that, in my opinion, can give the correct representation of the problem, but I get unphysical result: some axial pressure waves that run till the center of the channel...I'm confident that they shouldn't be there. It's like the wave is reflected and I don't want to.

Any suggestion? Is it correct waveTransmissive bc for this problem? :confused:

I fail to understand the problem set-up as much as I would like to.

What do you mean by "no inlets are present", by "overshoots for p and rho in cells near the outlet" and by desiring a pressure value at the outlet?

My understanding is that imposing a fixed pressure at the outlet will cause pressure waves to reflect back into the domain. Wave transmissive boundary conditions should render the outlet patch transparent for incoming pressure waves.

I would like to understand your problem set-up better than I currently do.

The micro channel is filled with argon, at start time the gas has U=0, p=41572 Pa and T= 300K
Attachment 84120
The geometry is a small wedge, here I scaled 50x in x-direction for better understanding Attachment 84121

When I said overshot for p and rho I mean that in the cells in proximity of outlets I get some results that are unphysical, pressure and density increase dramatically and I don't understand why. Attachment 84122

I agree with you, this bc should solve my problem, maybe I made some mistake in the set up.
Pressure:
Temperature:
U:
I've also tried different combination with zeroGradient for temperature and velocity, changing lInf to different values but nothing changed.
with waveTransmissive I get a strange behaviour and I don't understand if everything is set correctly, in particular I want a velocity that is supersonic, but in my simulations U is purely subsonic.

I thank you in advance for the attention.

Thank you so much for your further elaboration.

I do remain confused, I am afraid do say.

Your post mentions a constraint pressure while your figure shows pressure with a radial gradient (from center axis to wall). Any idea why this gradient arises?

What is the mechanism that drives the flow? Are the boundary conditions compatible with this mechanism?

The simulation start with a radial pressure and temperature gradient, this arises because argon is hit by a laser that increase temperature and pressure locally(T=4000K and p = , thanks to setFields I set this initial condition, in the rest of the channel we have U=0, p=41572 Pa and T= 300K.

I can say that there are two types of phenomena (that are not coupled):
- radial cylindrical shockwaves due to pressure gradient that are damped in the order of 1e-6 s
- flow that goes towards outlets emptying the channel (slower than the previous one)

I want to study expansion of the gas, in particular how much time i need before pressure inside the channel is lower than a certain threshold.
I expect a flow that is supersonic at the outlet, but this do not happen...probably I made some mistake defining the bc. Should I try something different?

I hope this further elaboration make the problem clearer

This does clarify, thanks.

I imagine the the solver has a hard time in handling the shock, i.e., the sudden transition in T and p from rest/background values to values induced by the laser beam. I imagine that a fine mesh in space and time is required to solve the sudden off/on transition that you try to capture.

I am curious to understand whether the solver is able to capture a smoother (less sudden) transition in which the laser emits less power first. Once you are comfortable with this situation, you could potentially try a harder case.

The solver is rhocentralfoam that is explicit and I need to set an extremely low deltaT of 1e-10s to capture the shocks, i will try a simpler case and let you know. Thanks for helping :)

I am happy to help.

My interest is in seeing how the wave-transmissive boundary conditions would work in this case. Is is feasible to make the pressure reflect from one lateral patch (by imposing a fixed value) and leave the domain on the other one (by imposing a wave-transmissive condition)?

I don't get this point, what is the interest in doing so?

I'm sorry to cause confusing.

My interest is in seeing how fixed value and wave-transmissive boundary conditions influence the computed fields.

Does this make sense?

Ok thanks for make it clearer.

I will try this and let you know, but my concern is to understand if I'm imposing the waveTransmissive condition in the right way.
Maybe for this run I should use an higher pressure at outlets to avoid strange behaviour in the solution.

I come to a solution imposing lInf = 10 and fieldInf = 100
In this way no reflection happen in my domain.

I also understood that fixedValue is a wrong condition to impose in a compressible problem, reflection wave are strong and affect calculation domain. :)

I initially thought I made some mistake defining the condition, but I cannot have a strong supersonic flow since the outlet is chocked.

Cool!

Could you post some imagine? Thx!

I start saying I chose a not well refined grid, a study on grid convergence will follow Attachment 84218
As you can see at t=0 I use setFields to set a strong pressure and temperature gradient inside the channel Attachment 84219
The simulation start and after 1e-6 seconds the radial cylindrical shock wave effects drop Attachment 84220 (I can be more specific if you are interested).
The simulation run till 1e-4 s and the result is the following Attachment 84221

Mach number is sonic at the outlet, as I would expect, no reflection wave occur in the domani :)

I hope it helps!

How does a solution with fixed value for pressure at the boundaries at t=1e-4 look like?

What is your Mach number?

Could you perform a simulation at subsonic conditions, at Mach = 0.5 say?

Thx!