# Outlet BC in a micro channel? waveTransmissive?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 30, 2021, 05:07 Outlet BC in a micro channel? waveTransmissive? #1 New Member   Join Date: Dec 2019 Posts: 9 Rep Power: 6 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? Last edited by filo-gor; May 1, 2021 at 05:24.

 April 30, 2021, 13:23 #2 Senior Member   Domenico Lahaye Join Date: Dec 2013 Posts: 736 Blog Entries: 1 Rep Power: 17 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.

May 1, 2021, 04:15
#3
New Member

Join Date: Dec 2019
Posts: 9
Rep Power: 6
Quote:
 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

Quote:
 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:
Code:
    Outlet
{
type            waveTransmissive;
field           p;
gamma           1.67;
psi             thermo:psi;
lInf            1;
fieldInf        1e-4;
}
Temperature:
Code:
   Outlet
{
type            waveTransmissive;
field           T;
gamma           1.67;
psi             thermo:psi;
}
U:
Code:
  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.

Last edited by filo-gor; May 1, 2021 at 05:23.

 May 2, 2021, 14:04 #4 Senior Member   Domenico Lahaye Join Date: Dec 2013 Posts: 736 Blog Entries: 1 Rep Power: 17 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?

May 3, 2021, 05:33
#5
New Member

Join Date: Dec 2019
Posts: 9
Rep Power: 6
Quote:
 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.

Quote:
 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

 May 3, 2021, 06:07 #6 Senior Member   Domenico Lahaye Join Date: Dec 2013 Posts: 736 Blog Entries: 1 Rep Power: 17 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 likes this.

 May 3, 2021, 06:19 #7 New Member   Join Date: Dec 2019 Posts: 9 Rep Power: 6 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

 May 3, 2021, 06:47 #8 Senior Member   Domenico Lahaye Join Date: Dec 2013 Posts: 736 Blog Entries: 1 Rep Power: 17 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)?

 May 4, 2021, 09:07 #9 New Member   Join Date: Dec 2019 Posts: 9 Rep Power: 6 I don't get this point, what is the interest in doing so?

 May 4, 2021, 09:18 #10 Senior Member   Domenico Lahaye Join Date: Dec 2013 Posts: 736 Blog Entries: 1 Rep Power: 17 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?

 May 4, 2021, 09:25 #11 New Member   Join Date: Dec 2019 Posts: 9 Rep Power: 6 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.

 May 6, 2021, 05:11 #12 New Member   Join Date: Dec 2019 Posts: 9 Rep Power: 6 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 likes this.

 May 6, 2021, 10:27 #13 Senior Member   Domenico Lahaye Join Date: Dec 2013 Posts: 736 Blog Entries: 1 Rep Power: 17 Cool! Could you post some imagine? Thx!

 May 6, 2021, 11:15 #14 New Member   Join Date: Dec 2019 Posts: 9 Rep Power: 6 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 likes this.

 May 6, 2021, 11:54 #15 Senior Member   Domenico Lahaye Join Date: Dec 2013 Posts: 736 Blog Entries: 1 Rep Power: 17 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!

 Tags boundary condition, outlet, rhocentralfoam, wavetransmissive bc

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post [ANSYS Meshing] Meshing Micro Channel with surface Roughness jonheb ANSYS Meshing & Geometry 3 February 14, 2018 06:31 aqibaziz76 FLUENT 0 February 8, 2014 16:45 Agad15 FLUENT 0 January 24, 2014 04:54 Fonta Fluent Multiphase 0 September 30, 2013 08:04 sepidehkavousi Main CFD Forum 2 January 6, 2012 07:01

All times are GMT -4. The time now is 09:50.

 Contact Us - CFD Online - Privacy Statement - Top