Convergence problem with 1. mixed porous media and air system 2. rough/spiky geometry

[Traiwit]

Check these boxes if you have followed the posting rules.

• Q&A Navier Stokes is the most appropriate category for my question
• I have consulted the posting Guidelines on the Discussions front page
• I have searched the Discussions forum and my question has not been asked before
• I have searched the MOOSE website and the documentation does not answer my question
• I have formatted my post following the posting guidelines (avoid screenshots if possible, triple back quotes before/after pasted text, etc)

Question

Hi

so i'm working on flow in mine/cave material problem

1. I have hard time converging when there is a restriction in flow path:

@GiudGiud mentioned in another thread of mine

for porosity jumps: porosity smoothing layers, bernouilli pressure drop imposition on the pressure variable
for friction jumps: body force reconstruction, and friction correction with consistent scaling

currently I let all the element to be void (porosity = 1) but only assign drag term to the elements at different domain (this doesn't help much)

I tried below, but still doesn't help much

        # THESE ARE NEW to handle porosity jumps
        porosity_smoothing_layers = 20
        porosity_interface_pressure_treatment = automatic
        use_friction_correction = true
        consistent_scaling = 1e-3

        friction_blocks =  '0 1 2 3 6'
        friction_types = 'DARCY'
        friction_coeffs = 'Darcy_coefficient'
        block = '0 1 2 3 6'

        momentum_scaling = 1e-3 # not even sure what it does
        # mass_scaling = 1

below is the way I control outlet vel (not sure if this is even the right way)

    [outlet_u_Momentum_Mass]
        type = INSFVMassAdvectionOutflowBC
        boundary = 'top_B1'
        variable = pressure
        u = vel_control_top_B1
        v = superficial_vel_y
        w = superficial_vel_z
        rho = ${rho}
    []

    [outlet_u_Momentum]
        type = PINSFVMomentumAdvectionOutflowBC
        variable = pressure
        u = vel_control_top_B1
        v = superficial_vel_y
        w = superficial_vel_z
        boundary = 'top_B1'
        momentum_component = 'x'
        rho = ${rho}
        rhie_chow_user_object = 'pins_rhie_chow_interpolator'
        porosity = porosity
    []

quick note: while i'm typing I have an idea, since the cave material move down with time it will open up the flow channel, maybe I can set extremely low flow (or no flow) during the time that tunnels are blocked and ramp up the flow (both TOP inlet and outlet) when they are unblocked

but how do i do that? to only let the BC at the top active at t > a certain time

I could set function like this but i dont no enforce flow means vel = 0

    [./vel_control_top_B1_fx]
        type = ParsedFunction
        expression =  'if(t>= 1339200.01, ${u_outlet_top_B1}, 0)'
    [../]

this is only outlet, how do i control inlet in such a way as well?

note2: it some cases it converges fine ie when I let perm in cave to be higher (less friction), no flow at all at the top part, only flow in and out at the bottom, etc

---

2. This is entirely different problem, simulation wont even start if the wall of the geometry isnt somewhat smooth

for example:

during the first jacobian step it will just give this error

Linear solve did not converge due to DIVERGED_PC_FAILED iterations 0
                   PC failed due to SUBPC_ERROR 
    Finished Computing Residual                                                          [  5.12 s] [ 7691 MB]
  Nonlinear solve did not converge due to DIVERGED_FNORM_NAN iterations 0

and it will just keep repeating until the simulation stop

but when i pad it with smoother layer of element, it solves fine, i dont understand why is that the case?

so it's impossible for me to move to the cave scale where the cave elements are quick spiky

below are the solver setting that i'm using:

#   petsc_options_iname  = '-pc_type -sub_pc_type -sub_pc_factor_levels -ksp_type -ksp_gmres_restart '
#   petsc_options_value  = ' bjacobi  ilu          1                    gmres       1000             '

    petsc_options_iname = '-pc_mat_solver_package -pc_type -pc_factor_shift_type -ksp_type -ksp_gmres_restart'
    petsc_options_value ='mumps asm NONZERO gmres       750 '

Thank you!

Traiwit

Additional information

Mesh size and type: 100k-500k element
Reynolds number:
Discretization (finite element CG/DG, finite volume, etc): finite volume
Models (turbulence, porous media, etc): porous media
Solver method (fully coupled, segregated, multiapps, etc): fully coupled
Base input you started from:

[GiudGiud]

but how do i do that? to only let the BC at the top active at t > a certain time

You can use a FunctionEnableControl to do that
https://mooseframework.inl.gov/source/controls/ConditionalFunctionEnableControl.html

[GiudGiud]

This is entirely different problem, simulation wont even start if the wall of the geometry isnt somewhat smooth

did you turn on skewness correction? It's needed for your average skewed tet meshes.

so should i scale everything by this number to get realistic flow pattern?

can you do that? Seems like it would require rescaling the variables too

[Traiwit]

Hi @GiudGiud

i'm not aware of skewness correction at all, I will have a look first thing tomorrow and get back to you.

Seems like it would require rescaling the variables too

is this via mass_scaling and momentum_scaling? is there any downside if i ramp up these variable too much

Traiwit

[GiudGiud]

is this via mass_scaling and momentum_scaling?

no these parameters are for scaling equations not output variables
The output variable scaling would need to be done manually. I dont think it's a real option

[Traiwit]

hmm I see, yeh it's weird, when I ramp up the time step it just wont converge when I use drag_air = 0 with mu = 2e-5 (gas flow)

would changing time unit help? my simulation is ideally in hrly to yearly scaling, i'm still using seconds (using adaptive time stepper from 0.01 to 40k sec for each miningframe), so when the dt > 100 it becomes unstable.

is there an option that I can change time unit similar to PorousFlow module?

[GiudGiud]

hmm I see, yeh it's weird, when I ramp up the time step it just wont converge when I use drag_air = 0 with mu = 2e-5 (gas flow)

So it converges at first for small time steps?
Have you tried a viscosity rampdown? Starting with a high viscosity and reaching the nominal value before the end of the simulation

is there an option that I can change time unit similar to PorousFlow module?

no if you changed the time unit you would need to change the fluid properties.

[Traiwit]

So it converges at first for small time steps?

yes, only the first few steps

Have you tried a viscosity rampdown? Starting with a high viscosity and reaching the nominal value before the end of the simulation

this is interesting, and how would I do this, my drag/porosity map is changing, lets say, every 20000 sec (due to miningframe update)

do i spend the first 10 sec of every miningframe ramping viscosity down from 1 to 2e-5, something like this?

[GiudGiud]

do i spend the first 10 sec of every miningframe ramping viscosity down from 1 to 2e-5, something like this?

yes for example. This will help the solver, in a similar way as initializing very close to the solution.
See the viscosity_rampdown parameter of the GeneralFunctorFluidProps. I use a ParsedFunction with '1 + 1000 * exp(-100 * t)' usually