[filo-gor]

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?

[dlahaye]

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.

[filo-gor]

Originally Posted by dlahaye

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?

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

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. Overshot.jpg

Originally Posted by dlahaye

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 agree with you, this bc should solve my problem, maybe I made some mistake in the set up.
Pressure:

    Outlet
    {
     	type            waveTransmissive;
        field           p;
        gamma           1.67;
        psi             thermo:psi;
        lInf            1;
        fieldInf        1e-4;
    }

Temperature:

   Outlet
    {
     	type            waveTransmissive;
        field           T;
        gamma           1.67;
        psi             thermo:psi;
    }

U:

  Outlet
    {
     	type            waveTransmissive;
        field           U;
        gamma           1.67;
        psi             thermo:psi;
        lInf            1;
        fieldInf        (0 0 0);
    }

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.

[dlahaye]

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?

[filo-gor]

Originally Posted by dlahaye

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?

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.

Originally Posted by dlahaye

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

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

[dlahaye]

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.

[filo-gor]

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

[dlahaye]

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)?

[filo-gor]

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

[dlahaye]

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?

[filo-gor]

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.

[filo-gor]

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.

[dlahaye]

Cool!

Could you post some imagine? Thx!

[filo-gor]

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

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

I hope it helps!

[dlahaye]

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!