Simple test 3D cad reading/halo using cylinder reading The cad file was generated using FreeCad and exported as a .stp file. When exporting the mesh, select Meter from the “Units for export of STEP” in preferences to ensure the mesh is in SI units.

compressibleFlow/compressibleFlowCadExample.yaml

---
test:
  # a unique test name for this integration tests
  name: compressibleFlowCadExample
  # the cad software in PETSc does not clean up after itself so ignore the error
  environment: "ASAN_OPTIONS=detect_leaks=0"
  # create a list of asserts to compare
  assert:
    # create a default assert that compares the log file
    "inputs/compressibleFlow/compressibleFlowCadExample/compressibleFlowCadExample.txt"

environment:
  title: _compressibleFlowCadExample
  tagDirectory: false
arguments: { }
timestepper:
  # setup default controls for the time stepper
  arguments:
    ts_type: rk
    ts_max_time: 100000
    ts_max_steps: 10
    ts_dt: 1.0E-10
    ts_adapt_safety: 0.9
  # io controls how often the results are saved to a file for visualization and restart
  io:
    interval: 0 # results are saved at every step.  In real simulations this should be much larger.

  # load in a cad file directly and then create a surface mesh then volumetric mesh from the cad geometry
  domain: !ablate::domain::CadFile
    name: exampleNozzle
    path: cylinder.stp
    # Options to be applied to the volumetric geometry
    options:
      dm_refine: 3
      dm_plex_check_all: true
    modifiers:
      # label all boundary faces as "marker" to allow extruding
      - !ablate::domain::modifiers::TagMeshBoundaryFaces
        region:
          name: marker
      # extrude all boundaries to add needed ghost cells for the boundary solver
      - !ablate::domain::modifiers::ExtrudeLabel
        # extrude the boundary cells marked
        regions:
          - name: marker
        # 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
        thickness: 0.001

      # if using mpi, this modifier distributes cells
      - !ablate::domain::modifiers::DistributeWithGhostCells
        ghostCellDepth: 2

      # tag the inlet boundary
      - !ablate::domain::modifiers::CreateLabel
        region:
          name: inletBoundaryCells
        function: "z < 0 ? 1.0 : 0"

      # repeat for the outlet
      - !ablate::domain::modifiers::CreateLabel
        region:
          name: outletBoundaryCells
        function: "z > 0.1 ? 1.0 : 0"

        # there are two example ways to apply the wall boundary conditions.  Only one should be selected but both are
        # presented for example illustration
        # example 1: define a geometry that tags only the boundary wall cells
        #- !ablate::domain::modifiers::CreateLabel
        #  region:
        #    name: wallBoundaryCells
        #  function: !ablate::mathFunctions::geom::CylinderShell
        #    start: [0.0, 0.0, 0.0]
        #    end: [0.0, 0.0, .1]
        #    radiusMin: 0.01
        #    radiusMax: 10

      # example 2: create a wall boundary that is all boundary cells minus inlet/outlet
      - !ablate::domain::modifiers::SubtractLabel
        differenceRegion:
          name: wallBoundaryCells
        minuendRegion:
          name: boundaryCells
        subtrahendRegions:
          - name: outletBoundaryCells
          - name: inletBoundaryCells

    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
        eos: !ablate::eos::PerfectGas &eos
          parameters:
            gamma: 1.4
            Rgas: 287.0
  # set the initial conditions of the flow field
  initialization:
    - !ablate::finiteVolume::fieldFunctions::Euler
      state: &initFlowState
        eos: *eos
        pressure: 101325.0
        temperature: 300
        velocity: !ablate::mathFunctions::geom::Cylinder
          start: [ 0.0, 0.0, -1 ]
          end: [ 0.0, 0.0, .05 ]
          radius: 0.005
          insideValues: "0.0, 0.0, 100.0"
          outsideValues: "0.0, 0.0, 0.0"

    # when extruding from a tet mesh, the boundary cells must be explicitly set as well
    - !ablate::finiteVolume::fieldFunctions::Euler
      region:
        name: boundaryCells
      state: *initFlowState
solvers:
  - !ablate::finiteVolume::CompressibleFlowSolver
    id: vortexFlowField
    # only apply this solver to the flowRegion
    region:
      name: flowRegion

    additionalProcesses:
      - !ablate::finiteVolume::processes::PressureGradientScaling
        &pgs
        eos: *eos
        alphaInit: 10.0
        maxAlphaAllowed: 100.0
        domainLength: 0.2
        log: !ablate::monitors::logs::StdOut

    # a flux calculator must be specified to so solver for advection
    fluxCalculator: !ablate::finiteVolume::fluxCalculator::AusmpUp
      pgs: *pgs

    # the cfl is used to compute the physics time step
    parameters:
      cfl: 0.25

    # set the eos and transport
    eos: *eos
    transport: !ablate::eos::transport::Sutherland
      eos: *eos

    monitors:
      # output time step information for each time step
      - !ablate::monitors::MaxMinAverage
        field: velocity

  # use a boundary solver to update the cells in the wallBoundaryCells region to represent standard wall
  - !ablate::boundarySolver::BoundarySolver
    id: wallBoundary
    region:
      name: wallBoundaryCells
    fieldBoundary:
      name: boundaryFaces
    mergeFaces: true
    processes:
      - !ablate::boundarySolver::lodi::IsothermalWall
        eos: *eos
        pgs: *pgs
  # use a boundary solver enforce an inlet
  - !ablate::boundarySolver::BoundarySolver
    id: inlet
    region:
      name: inletBoundaryCells
    fieldBoundary:
      name: boundaryFaces
    mergeFaces: true
    processes:
      - !ablate::boundarySolver::lodi::Inlet
        eos: *eos
        pgs: *pgs

  # use a boundary solver allow outward flow
  - !ablate::boundarySolver::BoundarySolver
    id: outlet
    region:
      name: outletBoundaryCells
    fieldBoundary:
      name: boundaryFaces
    mergeFaces: true
    processes:
      - !ablate::boundarySolver::lodi::OpenBoundary
        eos: *eos
        reflectFactor: 0.0
        referencePressure: 101325.0
        maxAcousticsLength: 0.1
        pgs: *pgs