This is an example of setting up a 2D SlabBurner Simulation using the gMsh python api with a series of derived slab burner points.
Mesh Generation Script
- Open the slabBurner2DMeshGen.py python
- Update the geometry if necessary
- To preview the resulting mesh run with the
--previewargument - Generate the slabBurner2DMesh.msh mesh file by running without the preview argument.
slabBurner2D/slabBurner2D.yaml
---
test:
# a unique test name for this integration tests
name: slabBurner2DTchem
# run on multiple mpi ranks
ranks: 2
# create a list of asserts to compare
assert:
# create a default assert that compares the log file
"inputs/slabBurner2D/expectedOutput.txt"
# metadata for the simulation
environment:
title: _slabBurner2DTchem
tagDirectory: false
# global arguments that can be used by petsc
arguments:
# The gmsh arguments must be global because they are used before the mesh options are parsed
dm_plex_gmsh_use_regions: true
# set up the time stepper responsible for marching in time
timestepper:
# time stepper specific input arguments
arguments:
ts_type: rk
ts_max_time: 100000
ts_max_steps: 100
ts_dt: 1.0E-10
ts_adapt_safety: 0.9
ts_adapt_type: physicsConstrained
# io controls how often the results are saved to a file for visualization and restart
io: !ablate::io::Hdf5MultiFileSerializer
interval: 10 # results are saved at every 5 steps. In real simulations this should be much larger.
# load in the gmsh produced mesh file
domain: !ablate::domain::MeshFile
path: slabBurner2DMesh.msh
options:
dm_plex_check_all: true # check to make sure the mesh if valid from gMsh
dm_distribute: false # turn off default dm_distribute so that we can extrude label first
dm_plex_hash_location: true # enable the fast look up particle locations
# specify any modifications to be performed to the mesh/domain
modifiers:
- # GMsh/dm_plex_gmsh_use_regions creates individual labels with their separate values. By collapsing the labels to the default values
# this input file does not need to individually specify each one for boundary conditions
!ablate::domain::modifiers::CollapseLabels
regions:
- name: inlet
- name: wall
- name: outlet
- name: slab
- name: main
- # use the newly collapsed labels to extrude the boundary. Do not extrude the main mesh
!ablate::domain::modifiers::ExtrudeLabel
regions:
- name: inlet
- name: wall
- name: outlet
- name: slab
# mark all the resulting boundary faces with boundaryFaces label
boundaryRegion:
name: boundaryFaces
# tag the original mesh as the flow region
originalRegion:
name: flowRegion
# tag the new boundary cells for easy boundary condition specifications
extrudedRegion:
name: boundaryCells
# if using mpi, this modifier distributes cells
- !ablate::domain::modifiers::DistributeWithGhostCells
ghostCellDepth: 2
# remove the slabBurnerFace from the flowRegion so that the ablate::boundarySolver::physics::Sublimation can handle the boundary condition
- !ablate::domain::modifiers::SubtractLabel
differenceRegion:
name: interiorFlowRegion
minuendRegion:
name: flowRegion
subtrahendRegions:
- name: slab
incompleteLabel: true # allow the faces to be removed the flowRegion
# this can be enabled to print a domain summary
# - !ablate::domain::modifiers::PrintDomainSummary
fields:
# all fields must be defined before solvers. The ablate::finiteVolume::CompressibleFlowFields is a helper
# class that creates the required fields for the compressible flow solver (rho, rhoE, rhoU, ...)
- !ablate::finiteVolume::CompressibleFlowFields
# The soot equation of state is an extension of the tChem eos with support for a simple soot model
eos: !ablate::eos::TChem &eos
mechFile: MMAReduced.soot.yml
options:
# set a minimum temperature for the chemical kinetics ode integration
thresholdTemperature: 560
# use a higher order field for the conserved field transport options
conservedFieldOptions:
petscfv_type: leastsquares
petsclimiter_type: vanleer
# create a conserved field to track ndd
- !ablate::finiteVolume::ExtraVariable
name: "Progress"
components: [ "NDD" ]
# by adding a pressure field the code will compute and output pressure
- !ablate::domain::FieldDescription
name: pressure
type: FV
location: aux
# set the initial conditions of the flow field
initialization:
# initialize the flow the entire domain with the default values using the flow state. The flow state can be used to compute
# both ablate::finiteVolume::fieldFunctions::Euler and ablate::finiteVolume::fieldFunctions::DensityMassFractions consistently
- !ablate::finiteVolume::fieldFunctions::Euler
# the ablate::finiteVolume::fieldFunctions::CompressibleFlowState defines a field given T, P, vel, and Yi
state: &flowFieldState
eos: *eos
# use a sphere geometry to set up an ignition kernel
temperature: !ablate::mathFunctions::geom::Sphere
center: [ 0.0182024, 0.007 ]
radius: 0.005
insideValues: 1673.15
outsideValues: 300
# set the entire domain to atmospheric pressure
pressure: 101325.0
# set the velocity everywhere to zero
velocity: "0.0, 0.0"
# the eos requires mass fractions to compute initial conditions
other: !ablate::finiteVolume::fieldFunctions::MassFractions
&oxMassFrac
eos: *eos
values:
- fieldName: O2
field: 1.0
# using the same CompressibleFlowState set the initial conserved mass fractions
- !ablate::finiteVolume::fieldFunctions::DensityMassFractions
state: *flowFieldState
# Set the soot number density to zero
- fieldName: densityProgress
field: "0.0"
# Set the boundary cells for the slab to a different initial condition
- !ablate::finiteVolume::fieldFunctions::Euler
# slab Burner
region:
name: slab
state: &fuelFieldState
eos: *eos
# the fuel is assumed to be at 653.0K
temperature: 653.0 #fuel temperature
pressure: 101325.0
velocity: "0.0, 0.0"
# set the mass fractions in the fuel boundary cells to 100% mma
other: !ablate::finiteVolume::fieldFunctions::MassFractions
&fuelMassFrac
eos: *eos
values:
- fieldName: MMETHAC_C5H8O2 # The fuel boundary condition
field: 1.0
# using the fuelFieldState set the initial conserved mass fractions in the boundary slab region
- !ablate::finiteVolume::fieldFunctions::DensityMassFractions
region:
name: slab
state: *fuelFieldState
# list the solvers that apply over the main mesh and the boundary cells
solvers:
# The compressible flow solver will solve the compressible flow equations over the interiorCells
- !ablate::finiteVolume::CompressibleFlowSolver
id: flowField
# the flow solver should only operate over the interiorFlowRegion. This does not include boundary cells or slab boundary faces
region:
name: interiorFlowRegion
# set the cfl constraint to be used by the physicsConstrained time stepper
parameters:
cfl: 0.45
# the flow solver requires access to the eos
eos: *eos
# the primary transport model applies to everything but the extra variables.
transport: !ablate::eos::tChemSoot::SootSpeciesTransportModel
# the SootSpeciesTransportModel adjusts the diffusion coefficient to carbon appropriately
transport: !ablate::eos::transport::Sutherland
eos: *eos
# if specified, the evTransport is used for the ndd transport
evTransport: !ablate::eos::tChemSoot::SootProgressTransportModel
transport: !ablate::eos::transport::Sutherland
eos: *eos
# additional monitors can be added to the flow solver.
monitors:
# The time step monitor outputs the current timestep and dt every 10 steps
- !ablate::monitors::TimeStepMonitor
interval: 10
# The TurbFlowStats monitor starts to take statistics after 0.01 seconds every 25 time steps
- !ablate::monitors::TurbFlowStats
fields: [ velocity, temperature ]
eos: *eos
interval: !ablate::io::interval::DelayInterval
interval: 25
minimumSimulationTime: .01 #about 1 flow
# The mixture fraction calculator outputs zMix and Yi everytime the serializer saves
- !ablate::monitors::MixtureFractionMonitor
mixtureFractionCalculator: !ablate::monitors::MixtureFractionCalculator
eos: *eos
massFractionsFuel: *fuelMassFrac
massFractionsOxidizer: *oxMassFrac
# additional processes can be added to the flow solver
additionalProcesses:
# in addition to the default process PressureGradientScaling can be used to speed up the simulation.
# the pgs must be supplied to other components to keep consistent calculations
- !ablate::finiteVolume::processes::PressureGradientScaling
&pgs
eos: *eos
alphaInit: 5.0
maxAlphaAllowed: 100.0
domainLength: 0.165354
# the chemistry process is used to compute the species and energy source terms from the reactions
- !ablate::finiteVolume::processes::Chemistry
eos: *eos
# ThermophoreticDiffusion diffusion controls the diffusion of solid carbon and ndd
- !ablate::finiteVolume::processes::ThermophoreticDiffusion
transport: !ablate::eos::transport::Sutherland
eos: *eos
# use ablate::finiteVolume::processes::Soot to compute ndd and carbon source terms
- !ablate::finiteVolume::processes::Soot
eos: *eos
# set a minimum temperature for the chemical kinetics ode integration
thresholdTemperature: 560
# a flux calculator must be specified to so solver for advection
fluxCalculator: !ablate::finiteVolume::fluxCalculator::AusmpUp
pgs: *pgs
# each boundary can be updated with a separate boundary solver
- !ablate::boundarySolver::BoundarySolver
id: inlet
# works over the extruded cells that were labeled inlet in gMsh
region:
name: inlet
fieldBoundary:
name: boundaryFaces
mergeFaces: true
processes:
# The LODI inlet boundary can adjust velocity over time
- !ablate::boundarySolver::lodi::Inlet
eos: *eos
pgs: *pgs
# The velocity is specified with a nested, nested formula to simplify specifying a radius based function
velocity: !ablate::mathFunctions::Formula
formula: "max(0.0, min(vel, t*vel/.001)), 0.0"
nested:
vel: !ablate::mathFunctions::Formula
formula: velFac*(1 - r/(dia/2.0))^(1/7)
constants:
dia: 0.0254
velFac: 6.16223189034601 # .153 m3/min
nested:
r: !ablate::mathFunctions::Formula
formula: sqrt((x-xc)^2 + (y-yc)^2)
constants:
yc: 0.0127
xc: 0.0
# the outlet boundary uses a reference pressure and maxAcousticsLength
- !ablate::boundarySolver::BoundarySolver
id: outlet
region:
name: outlet
fieldBoundary:
name: boundaryFaces
mergeFaces: true
processes:
- !ablate::boundarySolver::lodi::OpenBoundary
referencePressure: 101325.0
maxAcousticsLength: 0.165354
reflectFactor: 1.5
pgs: *pgs
eos: *eos
# The no slip/isothermal walls are applied everywhere except the slab
- !ablate::boundarySolver::BoundarySolver
id: walls
region:
name: wall
fieldBoundary:
name: boundaryFaces
mergeFaces: true
processes:
- !ablate::boundarySolver::lodi::IsothermalWall
eos: *eos
pgs: *pgs
# The slab boundary id used to couple the flow and heat/mass transfer from the fuel
- !ablate::boundarySolver::BoundarySolver
id: slabboundary
region:
name: slab
fieldBoundary:
name: boundaryFaces
processes:
# the sublimation boundary solver is responsible for predicting mass release and flow source terms
- !ablate::boundarySolver::physics::Sublimation
# the transport model is enforce to update the zero slip wall condition
transportModel: !ablate::eos::transport::Sutherland
eos: *eos
# the eos/pgs is used tor pressure boundary condition
pgs: *pgs
eos: *eos
# the specified mass fractions are assumed off-gassed by the fuel
massFractions: *fuelMassFrac
# the radiviative heat flux to the surface is updated every 10 flow time steps
radiationInterval: 10
# The sublimation model is used to compute mass flux rate from the surface, the default is complete sublimation
sublimationModel:
# the latent heat of fusion of PMMA is used to predict the mass release from heating
latentHeatOfFusion: 840890
#density of pmma used to output reg rate
solidDensity: 1190.0
# a surface radiation solver is used to compute heat flux to the surface
radiation: !ablate::radiation::SurfaceRadiation
id: surfaceflux
# the region is used to describe the area in which the flow solver is valid
region:
name: flowRegion
rays: 25
# the properties are a function of both gas and soot
properties: !ablate::eos::radiationProperties::Sum
- !ablate::eos::radiationProperties::Zimmer
eos: *eos
- !ablate::eos::radiationProperties::SootMeanProperties
eos: *eos
parameters:
emissivity: 0.9
monitors:
# the boundary solver monitor is used to record regression rate and heat flux to the surface
- !ablate::monitors::BoundarySolverMonitor
# the volume radiation solver compute the gas/gas energy transfer within the gas phase
- !ablate::radiation::VolumeRadiation
id: radiationSolver
# this is the region for which the solver operates (no boundary cells)
region:
name: flowRegion
# update the entire radiation solver every 10 flow steps
interval: 10
# The radiation solver and the associated region
radiation: !ablate::radiation::Radiation
id: volRad
region:
name: flowRegion
rays: 5
properties: !ablate::eos::radiationProperties::Sum
- !ablate::eos::radiationProperties::Zimmer
eos: *eos
- !ablate::eos::radiationProperties::SootMeanProperties
eos: *eos