[DrZoidberg]

Dear CFD community,


I want to simulate the loss coefficient in a zigzag duct. My basic case setup is:

-strucutred mesh ~1e6 elements (see image of inlet section enclosed)
-steady simulation, PBS coupled solver, kwSST, air ideal-gas
-spatial discr. all 2nd order, HOTR engaged, momentum URF 0.3, Pseudo Timestep 0.01

-adibatic walls, operating pressure 1bar, pressure inlet is varied and pressure outlet with 0Pa


Inlet pressure is varied from 100Pa to 3MPa. The loss coeff profile of this duct is used for an outlet vent in a more complex simulation.


Problem: As soon as the inlet pressure is increased beyond the choking point (somewhere around 230kPa, here Ma at the outlet becomes 0.99) the Ma at outlet becomes >1, p_outlet=1bar is no longer kept but raises, net mass flow becomes > 1% of inlet mass flow and the residuals keep oscillating.


According to Fanno, the velo may be max Ma=1 at the outlet. But there is no way to set an appropiate pressure there, right?

Is the only way to fix this problem by a more complex outlet domain, i.e. setting p_out=1bar it in the "far-field"? Do you maybe have a tip how this could be modeled or what dimensions are needed? I already tried to add a square of 40mm edge length there (and used similar mesh size like the duct), but the solver diverged right from the start with this setting.



Br

[LoGaL]

Indeed if your outlet is your throat, forcing the pressure there to be 1atm is wrong. But in any case, P would be 1atm in the farfield (as you said), not exactly at the outlet of your pipeline.

Maybe if you make a diverging section after your "real outlet", that could help the solver to stabilize.

Quick tip, such low pseudo-time step (0.01) will, most probably, not help you at all and will just make convergence time so long. You should only lower it if the problem is complicated and the CFD has numerical issues at the beginning of the simulation.

[DrZoidberg]

Originally Posted by LoGaL

Indeed if your outlet is your throat, forcing the pressure there to be 1atm is wrong. But in any case, P would be 1atm in the farfield (as you said), not exactly at the outlet of your pipeline.

Maybe if you make a diverging section after your "real outlet", that could help the solver to stabilize.

Quick tip, such low pseudo-time step (0.01) will, most probably, not help you at all and will just make convergence time so long. You should only lower it if the problem is complicated and the CFD has numerical issues at the beginning of the simulation.

Hi LoGaL,
thank you for the tip! That will save some time I tried again with an improved mesh at the outlet. Now it ran at least, but the solution is stuck at this point. Residuals oscillate around 1e-3...1e-4 and the velocity profile looks even more unphysical now. There should not be any shocks within the duct as long as it has constant cross section because there is always a subsonic inlet velocity. Another question is, if Fanno/Raleigh theory is still applicaple here. I could not find literature on such flows to assess the plausibility. Usually the textbooks cover Fanno-flow (=1D flow in straight pipe, adibatic, irreversible) or conv/div nozzles, but never a curved duct, which is already a 2D flow. Could the curvature have a similar effect on the flow like a conv/div nozzle, i.e. it may cause indeed shocks/Ma>1 even for subsonic inflow?
I found this https://doi.org/10.1063/1.5120215, which covers a 3D 90°-bend pipe, and they got Ma>1 even in the constant cross section domain. But it seems to originate from the outlet - not from the bend.



So far, I tried varying the inlet-bc to: p-inlet, massflow-inlet, v-inlet. For a p-inlet the velocities drop to almost 0 and nothing converges, although this should be the most stable bc setting . Massflow and v-inlet (I know, it should not be used in compressible) do not differ much and produce similar results like in the screenshot.

[LoGaL]

Fanno theory is alwais right, but the point is that for complex geometry the position of the throat is not alwais trivial. Are you having separation after the bends in the tube?

[DrZoidberg]

Yes, there is laminar separation in the bends. The image shows the profile in the first bends (near to inlet).

[LoGaL]

When there's separation (which is unsteady phenomenon) the steady solver has always difficulties in converging. Especially if laminar.

Nothing you can do about it. You need to go for unsteady solver.

[DrZoidberg]

Ok, now I tried more mesh settings and varied esp the outlet domain. The results look more realistic now.

The bigger the outlet domain, the better - that was the idea behind the new mesh. It is unstructured with y+ < 1 everywhere (1st layer height 3e-8) and 5e-5m in bulk volume for coarse mesh (600k elements) and 2.5e-5m for fine mesh (2kk elements).

I tried tried steady and transient pbs-coupled and dbs-AUSM/RoeFDS with timesteps 1e-8 to 1e-9. CFL < 0.1

But I observed still some odd behaviour. As often recommended I start with steady and here the solution seems to be converged (see first iterations in Residuals plot), because (1) the residuals rest at a constant value (2e-4 for momentum, 6e-6 for energy and continutity) and (2) the net-mass-flux has come down to 2% of the inlet (which is 1.5kg/s).

Once the setting is changed to transient, even with 1e-9 the residulas drop to 1e-10...1e-12 which should be sufficient, but the net-mass-flux increases no matter if pbs/dbs is used. Even worse for the net-heat flux, but it did not converge at 0 in steady neither (inlet 2792W vs. outlet -14216W).
I checked then only the net-mass-flux just in the wall-bounded duct. Here it is also at ~2% as for the steady solution. The outlet domain has reverse flow at 50% of its surface. I assume that is why the fluxes won't come down to 0. But is it even neceassary to achieve this wrt to the goal (=getting the the loss coefficient)? The loss coefficient is just dependent on p_in,p_out,v_in, rho_in but it is also far away from an asymtotic settling as shown by the figures.