PyIntact manual

Overview

• Introduction to the API

  This document provides a comprehensive guide to using our Python API for Intact.Simulation. The API allows users to define geometries, material properties, components, assemblies, and boundary conditions. Users can specify units, create simulation scenarios, execute the simulation, and query the results. The simulations can be run with different solver types and the results can be written to a file for visualization. The document also provides Python code examples and snippets for each step of the simulation process.

• Key features and capabilities

  • Physics Support

    • Stress

    • Modal

    • Thermal

    • Linear Buckling

  • Geometry Support

    • Brep: Surface mesh

    • VDB volume

Getting Started

• A simple example of running a structural simulation. Any geometry files used in these examples are available in the examples/ folder.

  • Import Intact Module

  from PyIntact import *
  

  • Create Geometry

  beam_geometry = MeshModel("beam.stl")
  beam_geometry.instance_id = "simple_cantilever"
  beam_geometry.refine(0.02) # refine stl for smoother visualization
  

  • Create Material (Properties are in MKS unit system)

  material = IsotropicMaterialDescriptor() # steel
  material.density = 7800.0 # kg/m^3
  material.poisson_ratio = 0.3
  material.youngs_modulus = 2.1e11 # Pa
  

  • Create Restraints and Loads

  # Create a fixed boundary condition at one end of the beam
  fixed_boundary = FixedBoundaryDescriptor()
  fixed_boundary.boundary = MeshModel("restraint.stl")
  
  # Create a pressure load at the free end of the beam
  pressure_load = PressureForceDescriptor()
  pressure_load.units = UnitSystem.MeterKilogramSecond
  pressure_load.magnitude = 1000  # Applying pressure in Pascals
  pressure_load.boundary = MeshModel("load.stl")
  

  • Setup simulation and solve

  # Setup the simulation scenario descriptor
  scenario = LinearElasticScenarioDescriptor()
  scenario.materials = {"Steel": material}
  scenario.metadata.resolution = 10000
  scenario.metadata.units = UnitSystem.MeterKilogramSecond
  scenario.boundary_conditions = [fixed_boundary, pressure_load]
  
  # Associate the material with the model
  component = MaterialDomain(beam_geometry, "Steel", scenario)
  assembly = [component]
  
  # Initialize and run the simulator
  simulator = StressSimulator(assembly, scenario)
  simulator.solve()
  

  • Query result and create output file to visualize

  # Query results for stress distribution
  results = QueryResult(assembly)
  stress_query = FieldQuery(Field.VonMisesStress)
  simulator.sample(stress_query, results)
  
  # Write results to a file (unit system is saved as a metadata in the vtu file)
  results.writeVTK("cantilever_beam_results.vtu", UnitSystem.MeterKilogramSecond)
  

How To

Creating Simulation Input

Units

The default Unit System is MKS or MeterKilogramSecond. We allow the following customizations:

• Specify custom unit for geometry through the Scenario unit (default MKS)

• Specify custom unit for loads (default MKS)

• Specify custom unit for materials (default MKS)

Unit System Keywords	Mass	Force	Stress	Length
MeterKilogramSecond	kg	N	Pa	m
CentimeterGramSecond	g	dyne	dyne/cm²	cm
MillimeterMegagramSecond	Mg	N	MPa	mm
FootPoundSecond	slug	lbf	lbf/ft²	ft
InchPoundSecond	lbf s²/in	lbf	psi	in

Geometry

Geometry is specified through a Model object

• MeshModel from surface mesh can be defined in two ways.

  • filename to define mesh from a file (STL, PLY)

    • instance_id a unique name

    mesh_geometry = MeshModel(filename="beam.stl")
    mesh_geometry.instance_id = "beam"
    

  • Constructing mesh face-by-face

    # define an empty mesh
    mesh_geometry = MeshModel()
    mesh_geometry.instance_id = "fixed_boundary"
    
    # add vertices to the mesh and get the vertex id as output
    v0 = mesh_geometry.addVertex([0.0, 0.0, 0.0])
    v1 = mesh_geometry.addVertex([1.0, 0.0, 0.0])
    v2 = mesh_geometry.addVertex([0.0, 1.0, 0.0])
    
    # add faces defined by the vertex id
    mesh_geometry.addFacet(v0, v1, v2)
    

  • Mesh refinement (usually used for finer interpolation of results during visualization). Uses MeshModel.refine with refinement_level as an input which is the largest allowed triangle edge as a ratio of the bounding box diagonal.

    # mesh geometry created above is further refined
    mesh_geometry.refine(refinement_level=0.02)
    

• VDB Model

  • Using a .vdb file

    vdb_geometry= VDBModel("box.vdb")
    

  • In memory using a VDB object

    import pyopenvdb as vdb
    
    #create a vdb double grid object
    cube = vdb.DoubleGrid()
    cube.fill(min=(100, 100, 100), max=(199, 199, 199), value=1.0)
    
    #create an Intact Model from VDB object
    vdb_geometry = PyIntact.VDBModel(cube)
    
    #create a tesselation of the vdb to get a MeshModel and its list of vertices for sampling
    mesh = vdb_geometry.tesselate() # mesh is a MeshModel()
    num_vertices = mesh.vertexCount()
    print(num_vertices)
    

Material Properties

• Structural

  • IsotropicMaterialDescriptor to create an Isotropic material. (Unit is MeterKilogramSecond)

    • density is the material density

    • youngs_modulus is the elastic modulus

    • poisson_ratio is the Poisson ratio

    steel_structural = IsotropicMaterialDescriptor()
    
    # Set the density to 7845 kg/m^3, modulus to 200 GPa and poison ratio to 0.29
    steel_structural.density = 7845
    steel_structural.youngs_modulus = 200e9
    steel_structural.poisson_ratio = 0.29
    

  • OrthotropicMaterialDescriptor to create an Orthotropic material. Orthotropic materials are often used to represent composites and wood, where the material properties along one axis are significantly different from the properties along the other axes. (Unit is MeterKilogramSecond)

  • density is the material density

  • Ex is the elastic modulus in the material’s x-direction

  • Ey is the elastic modulus in the material’s y-direction

  • Ez is the elastic modulus in the material’s z-direction

  • Gxy is the shear modulus in the xy plane

  • Gxz is the shear modulus in the xz plane

  • Gyz is the shear modulus in the yz plane

  • vxy is the poisson ratio in the xy plane

  • vxz is the poisson ratio in the xx plane

  • vyz is the poisson ratio in the yz plane

  • transform is the optional material transform to arbitrarily rotate the axes along which the material properties are defined. Specified as a list of 9 floating point numbers corresponding to a 3x3 matrix. Note the first 3 floating point numbers corresponds to the first row.

  # Create an orthotropic material (Red Pine)
  material = OrthotropicMaterialDescriptor()
  material.density = 460.0             # kg/m³
  material.Ex = 11.2e9                 # Pa
  material.Ey = 492.8e6                # Pa
  material.Ez = 985.6e6                # Pa
  material.Gxy = 907.2e6               # Pa
  material.Gxz = 1.08e9                # Pa
  material.Gyz = 123.2e6               # Pa
  material.vxy = 0.315
  material.vxz = 0.347
  material.vyz = 0.308
  material.transform = [1.0, 0.0, 0.0,
                      0.0, 1.0, 0.0,
                      0.0, 0.0, 1.0] # optional in this case
  

• Thermal

  • ThermalMaterialDescriptor to create a thermal material. (Default unit is MeterKilogramSecond)

    • density is the material density

    • conductivity is the conductivity of the material

    • specific_heat is the specific heat of the material

    thermal_material = ThermalMaterialDescriptor()
    
    # Set the density, conductivity, and specific heat of the material
    thermal_material.density = 2700.0 # kg/m^3
    thermal_material.conductivity = 170  # W/(m·K)
    thermal_material.specific_heat = 500  # J/(kg·K)
    

Component and Assembly

• A Component is created as a MaterialDomain and takes three inputs

  • A Model object (MeshModel or VDBModel specifically)

  • A material name

  • A ScenarioDescriptor object

  bar1_structural = MaterialDomain(mesh_geometry, "Steel", structural_scenario)
  bar2_structural = MaterialDomain(vdb_geometry, "Steel", structural_scenario)
  

• Assembly is a list of components that are bonded together

  structural_assembly = [bar1_structural, bar2_structural]
  

Boundary Conditions

• Restraints

  • Fixed Boundary A “Fixed Boundary” restraint fixes the selected geometry in all directions.

    The fixed boundary only has one input:

    • the boundary surface to be fixed

    fixed = FixedVectorDescriptor()
    
    # Set the geometry "restraint.ply" to be fixed
    fixed.boundary = MeshModel("restraint.ply")
    

  • Fixed Vector A “Fixed Vector” restraint allows for each direction to be optionally set to a specified displacement value, 0 being fixed and ‘None’ being un-restrained. Note that a structural problem must have all three directions restrained somewhere to be valid. Also, note that this boundary condition doesn’t take custom units and it’s always in the units of the scenario metadata.

    A fixed vector requires four inputs:

    • the boundary surface to be fixed

    • the x_value to set the displacement for the x-axis direction (optional)

    • the y_value to set the displacement for the y-axis direction (optional)

    • the z_value to set the displacement for the z-axis direction (optional)

    fixed_vector = FixedVectorDescriptor()
    
    # Set the geometry "restraint.stl" to be restrained
    fixed_vector.boundary = MeshModel("restraint.stl")
    
    # Set the displacements in each direction
    fixed_vector.x_value = 0.2  # X-direction displacement of 0.2 m
    fixed_vector.y_value = None # un-restrained in the Y-direction at this surface
    fixed_vector.z_value = 0.0  # fixed Z-direction
    

  • Sliding Restraint A “Sliding Restraint” allows for motion tangential to a specified surface, but fixes motion normal to the specified surface.

    A sliding restraint only has one input:

    • the boundary surface for the sliding restraint condition

    sliding_boundary = SlidingBoundaryDescriptor()
    
    # Set the geometry "restraint.stl" for the sliding restraint condition
    sliding_boundary.boundary = MeshModel("restraint.stl")
    

• Structural Loads (TractionDescriptor)

  • Vector Force

    “Vector Force” load is a surface load applied to a face in a specified direction. An example of this load is pressing on the top of a book to push it across a table.

    A vector load requires four inputs:

    • the boundary surfaces where the load is applied

    • the direction vector of the force

    • the UnitSystem that applies to the magnitude

    • the magnitude of the force.

    load = VectorForceDescriptor()
    
    # Set the geometry "load.stl" the vector load is applied to
    load.boundary = MeshModel("load.stl")
    
    # Set the vector load direction to be in the -Z direction with a magnitude of 100 lbf
    load.direction = [0, 0, -1]
    load.units = UnitSystem.InchPoundSecond
    load.magnitude = 100 # lbf
    

  • Torque

    “Torque” load is a surface load that applies a twisting force around an axis. The direction of the torque is determined using the right-hand rule: using your right hand, point your thumb in the direction of the axis. A positive torque value applies a torque acting in the direction the fingers of your right hand would wrap around the axis. The torque load is applied among the load faces with a distribution that varies linearly from zero at the axis.

    A Torque load requires five inputs:

    • the boundary surfaces where the load is applied

    • the axis of rotation about which the torque acts

    • origin is the starting point of the axis of rotation

    • the UnitSystem that applies to the magnitude

    • magnitude of the torque.

    torque_load = TorqueForceDescriptor()
    
    # Set the geometry "load.stl" the torque load is applied to
    torque_load.boundary = MeshModel("load.stl")
    
    # Set the axis of the torque axis
    torque_load.origin = (10, 1, 1)
    torque_load.axis = [1, 0, 0] # Set the torque to be about the +X (right-hand rule)
    torque_load.units = UnitSystem.MeterKilogramSecond
    torque_load.magnitude = 10 # Set the torque magnitude to 10 N*m
    

  • Pressure

    A “Pressure” load is a surface load specified in terms of force per unit area. Positive pressures ‘push’ into the surface, and negative pressures ‘pull’.

    A Pressure Load requires three inputs:

    • the boundary surfaces where the load is applied

    • the UnitSystem that applies to the magnitude

    • the magnitude of the pressure.

    pressure_load = PressureForceDescriptor()
    
    # Set the geometry "load.stl" the pressure load is applied to
    pressure_load.boundary = MeshModel("load.stl")
    
    # Set the pressure magnitude to 10 Pa
    pressure_load.units = UnitSystem.MeterKilogramSecond
    pressure_load.magnitude = 10
    

  • Bearing Force

    A “Bearing Force” is a surface load applied to a (typically) cylindrical face to approximate the effects of a shaft pressing against the side of a hole. The applied force gets converted to a varying pressure distribution on the portion of the face experiencing compressive pressure. The pressure distribution is computed automatically to achieve the specified overall bearing force.

    A Bearing Force requires three inputs:

    • the boundary surfaces where the load is applied

    • the direction vector of the bearing force

    • the UnitSystem that applies to the magnitude

    • the magnitude of the force

    bearing_load = BearingForceDescriptor()
    
    # Set the geometry "load.stl" the bearing load is applied to
    bearing_load.boundary = MeshModel("load.stl")
    
    # Set the loading direction to be in the -Z
    bearing_load.direction = [0, 0, -1]
    
    # Set the magnitude of the load to 100 N
    bearing_load.units = UnitSystem.MeterKilogramSecond
    bearing_load.magnitude = 100
    

• Thermal Loads

  • Fixed Boundary (Fixed Temperature)

    A “Fixed Boundary” load fixes the selected geometry to a specified temperature when the value is specified and non-zero.

    The fixed boundary has two inputs:

    • the boundary surface to be fixed

    • the value of the temperature to fix at the boundary surface

    fixed = FixedBoundaryDescriptor()
    
    # Set the geometry "fixed_temp.ply" to set a fixed temperaure of 320 K
    fixed_boundary.boundary = MeshModel("fixed_temp.ply")
    fixed_boundary.value = 320  # Kelvin
    

  • Convection

    A “Convection” load specifies the transfer of heat from a surrounding medium.

    A thermal convection boundary condition requires three inputs:

    • the boundary surface(s) where the convection is applied.

    • the heat transfer coefficient

    • the environment_temperature of the surrounding medium

    • the units (default MKS)

    # Create an instance of ConvectionDescriptor
    convection = ConvectionDescriptor()
    convection.units = UnitSystem.MeterKilogramSecond
    
    # Set the geometry "face.ply" the convection is applied to
    convection.boundary = MeshModel("face.ply")
    
    # Set the heat transfer coefficient to 25 W/m^2K and environment temperature
    convection.coefficient = 25  # W/m^2K
    convection.environment_temperature = 300  # Kelvin
    

  • Surface Flux

    Surface “Thermal or Heat Flux” specifies the heat flow per unit of surface area.

    A surface thermal flux requires two inputs:

    • the boundary surface(s) where the flux is applied.

    • the magnitude of the heat flux

    • the units (default MKS)

    # Create an instance of ConstantFluxDescriptor
    flux = ConstantFluxDescriptor()
    flux.units = UnitSystem.MeterKilogramSecond
    
    # Set the geometry "face.ply" the constant flux is applied to
    flux.boundary = MeshModel("face.ply")
    
    # Set the flux magnitude to 500 W/m^2
    flux.magnitude = 500  # W/m^2
    

• Body Loads/Internal Conditions

  Add body load to the scenario as shown below. (see Scenario Setup section for more details)

  scenario.internal_conditions = [rotational_load, gravity_load]
  

  • Body Load (Linear Acceleration, Gravity)

    Body loads comprise forces that are distributed over a solid volume. They are specified by entering the components of a linear acceleration vector field in which the body is immersed. The material in the body will tend to be pulled in the direction of the acceleration vector.

    The inputs to the body load are:

    • the direction vector of the acceleration field

    • the UnitSystem that applies to the magnitude

    • the magnitude of acceleration

    # Example for a "gravity load"
    body_load = BodyLoadDescriptor()
    
    # Set the direction vector to be downward (-Z)
    body_load.direction = [0, 0, -1]
    
    # Set the magnitude to 9.80655 m/s^2
    body_load.units = UnitSystem.MeterKilogramSecond
    body_load.magnitude = 9.80665
    

  • Rotational Load

    Rotational body loads simulate the effect of a body rotating around an axis. Two contributions are considered in a rotational body load: angular velocity and angular acceleration. The angular velocity term simulates the centrifugal effects that tend to throw a body’s material away from the axis of rotation. The angular acceleration term simulates the effect of a rotational acceleration field around the axis of rotation. A positive angular acceleration tends to drag the body’s material in the positive rotational direction according to the right-hand rule.

    A rotational body load has 4 inputs:

    • origin point for the axis of rotation

    • vector defining the axis of rotation

    • angular_velocity (in radians/sec)

    • angular_acceleration (in radians/sec²)

    rotational_load = RotationalLoadDescriptor()
    
    # Set the origin at the coordinate system origin
    rotational_load.origin = (0, 0, 0)
    
    # Set the axis of rotation about the y-axis
    rotational_load.axis = [0, 1, 0]
    
    # Set angular velocity to 10 rad/s and angular acceleration to 0.5 rad/s^2
    rotational_load.angular_velocity = 10
    rotational_load.angular_acceleration = 0.5
    

• Thermal Loads

  • Constant Heat

    A “Constant Heat” or body heat flux load applies uniform heat generation over a specified volume.

    Constant heat flux has 2 inputs

    • the instance_id of the components which are producing heat flux

    • the magnitude of the body heat flux

    • the units (default MKS)

    constant_heat = ConstantHeatDescriptor()
    constant_heat.units = UnitSystem.MeterKilogramSecond
    
    # Set the heat generation to -200,000 W/m^3 for a beam component
    constant_heat.instance_id = "beam"
    constant_heat.magnitude = -200000.0  # W/m^3
    

Simulation Scenario Setup and Solution

• Scenario Setup using ScenarioDescriptor

  • Linear Elasticity scenario is created using LinearElasticScenarioDescriptor. It takes the following inputs:

    • boundary_conditions, a list of boundary conditions

    • internal_conditions, a list of internal conditions (body loads)

  • Scenario Metadata, metadata, a set of solver parameters to control the accuracy and speed of the simulation:

    • resolution is the target number of finite elements. An iterative process determines a cell_size that achieves approximately the specified number of elements. You can directly specify the cell_size instead of resolution. Note that decreasing cell_size can quickly result in large numbers of finite elements and long solve times. resolution is recommended for most cases.

    • units sets the unit of the scenario (geometry and results will be in this unit) for example, a geometry in ‘MKS’ that is 6 m long would be 6 mm long when set to ‘MMS’

    • basis_order is the type of finite element used. The default is 1, which would be linear elements. 2 is for quadratic elements.

    • solver_type is the solver type used in the simulation with the following options:

      • MKL_PardisoLDLT (default) is the direct solver and is typically faster for lower resolution (< 200K cells on 32 GB memory), but gets slower and consumes more memory at higher resolutions

      • AMGCL_amg_rigid_body is the iterative solver which is typically faster at high resolution.

    scenario = LinearElasticScenarioDescriptor()
    scenario.materials = {"Aluminum 6061-T6": material}
    scenario.boundary_conditions = [fixed_boundary, vector_load, torque_load]
    scenario.internal_conditions = [body_load]
    
    scenario.metadata.resolution = 10000
    scenario.metadata.units = UnitSystem.MeterKilogramSecond
    
    # Optional settings
    scenario.metadata.basis_order = 2 # 2 = quadratic elements
    scenario.metadata.solver_override = Solver.AMGCL_amg_rigid_body # iterative solver
    

  • Similarly, Modal scenario is created using ModalScenarioDescriptor which takes boundary_conditions, a list of boundary conditions, as input.

    • The metadata is the same as for the linear elastic scenario except there is necessary input modal_metadata.desired_eigenvalues that takes in an integer for the number of eigenvalues.

    # Setup the modal simulation scenario
    modal_scenario = ModalScenarioDescriptor()
    modal_scenario.materials = {"Aluminum 6061-T6": material}
    modal_scenario.boundary_conditions = [fixed_boundary]
    
    modal_scenario.metadata.resolution = 10000
    modal_scenario.modal_metadata.desired_eigenvalues = 10
    
    # Optional settings
    modal_scenario.metadata.basis_order = 2 # 2 = quadratic elements
    modal_scenario.metadata.solver_override = Solver.AMGCL_amg_rigid_body  #iterative solver
    

  • Similarly, Linear Buckling scenario is created using LinearBucklingScenarioDescriptor which takes boundary_conditions, a list of boundary conditions, as input. A linear buckling scenario first performs a linear elasticity simulation, and then solves a generalized eigenvalue problem to determine the critical load factors.

    • The metadata is the same as for the linear elastic scenario except there is necessary input modal_metadata.desired_eigenvalues that takes in an integer for the number of eigenvalues.

    # Setup the linear buckling simulation scenario
    buckling_scenario = LinearBucklingScenarioDescriptor()
    buckling_scenario.materials = {"Aluminum 6061-T6": material}
    buckling_scenario.boundary_conditions = [fixed_boundary]
    
    buckling_scenario.metadata.resolution = 10000
    # Generally, the first critical load factor from a buckling analysis is most useful,
    # a small number of additional buckling modes may be useful to examine.
    buckling_scenario.modal_metadata.desired_eigenvalues = 3
    
    # Optional settings
    buckling_scenario.metadata.basis_order = 2 # 2 = quadratic elements
    # Use iterative solver for the linear elasticity simulation
    buckling_scenario.metadata.solver_override = Solver.AMGCL_amg_rigid_body
    

  • Similarly, a Thermal scenario is created using StaticThermalScenarioDescriptor which takes a list of boundary_conditions and a list of internal_conditions as input. Note that the material must be a thermal material for this scenario type.

    • The metadata is the same as for the linear elastic scenario with additional input thermal_metadata.environment_temperature which specifies the temperature of the environment.

    # Setup the thermal simulation scenario
    thermal_scenario = StaticThermalScenarioDescriptor()
    thermal_scenario.materials = {"Aluminum 6061-T6": material}
    thermal_scenario.boundary_conditions = [fixed_temp, convection]
    thermal_scenario.internal_conditions = [constant_heat]
    thermal_scenario.thermal_metadata.environment_temperature = 0.0
    
    thermal_scenario.metadata.resolution = 10000
    
    # Optional settings
    thermal_scenario.metadata.basis_order = 2 # 2 = quadratic elements
    thermal_scenario.metadata.solver_override = Solver.AMGCL_amg # iterative solver
    

• Finalize Simulation Setup and Execute

  • Stress Simulation is created using StressSimulator. It takes the following inputs:

    • An assembly or the list of MaterialDomains

    • LinearElasticScenarioDescriptor that describes the simulation scenario

    # Initialize and run the linear elastic scenario
    simulator = StressSimulator(assembly, scenario)
    simulator.solve()
    

  • Modal Simulation is created using ModalSimulator. It takes the following inputs:

    • An assembly or the list of MaterialDomains

    • ModalScenarioDescriptor that describes the simulation scenario

    # Initialize and run the modal scenario
    modal_simulator = ModalSimulator(assembly, modal_scenario)
    modal_simulator.solve()
    

  • Linear Buckling Simulation is created using LinearBucklingSimulator. It takes the following inputs:

    • An assembly or the list of MaterialDomains

    • LinearBucklingScenarioDescriptor that describes the simulation scenario

    # Initialize and run the linear buckling scenario
    buckling_simulator = LinearBucklingSimulator(assembly, buckling_scenario)
    buckling_simulator.solve()
    

Query and Result Output

• Create a QueryResult object that specifies the domain to be sampled. It takes a single component or an assembly as input

  assembly = [component_1, component_2]
  
  results = QueryResult(component_1) # sample only the defined component
  results = QueryResult(assembly) # sample on the full assembly
  

• Specify a query class & type that defines what quantity you are querying. The query classes and types available are as follows :

  • Global Query is for querying quantities defined for the entire domain or structure. The available GlobalQueryType``s are ``Compliance for linear elasticity simulations, Frequency for modal simulations, CriticalLoadFactor for linear buckling simulations, and ThermalCompliance for static thermal simulations.

  # GlobalQuery example
  # Create a GlobalQuery to query the first mode
  results = QueryResult(assembly)
  frequency_query = GlobalQuery(GlobalQueryType.Frequency, DiscreteIndex(0))
  
  # Sample the simulation for the specified query
  freq_1 = simulator.sample(mode1_query, results)
  print(freq_1.get(0,0)) # Print out the first mode in Hz
  
  # Example use to get the first 10 modes
  # Note, the simulator would need this:
  # modal_scenario.modal_metadata.desired_eigenvalues = 10
  
  for i in range(10):
      # Create the query for the current mode
      query = GlobalQuery(GlobalQueryType.Frequency, DiscreteIndex(i))
  
      # Sample the query using the simulator
      r = simulator.sample(query, results)
  
      # Append the value obtained from result.get(0, 0) to a list
      values.append(r.get(0, 0))
      print(values) # list of first 10 modes in Hz
  

  • Field Query is for querying field quantities defined at any point in the domain. This depends on the physics type.

    • For Stress Simulation, the following FieldType inputs are available

      • Displacement tuple of dimension 3 for each point

        [x-displacement, y-displacement, z-displacement]
        

      • Strain and Stress are each a tuple of dimension 6 for each point

        [stress_xx, stress_yy, stress_zz, stress_yz, stress_xz, stress_xy]
        [strain_xx, strain_yy, strain_zz, strain_yz, strain_xz, strain_xy]
        

      • TopologicalSensitivity, StrainEnergyDensity, and VonMisesStress are each a tuple of dimension 1 for each point

    • For Modal Simulation and Linear Buckling Simulation, the only FieldType available is Displacement, which corresponds to the mode shape information and requires an index for the specified mode.

      # Create a field query for the displacement/mode shape of mode 1
      mode_num = 0 # first mode
      modal_field_query = FieldQuery(f=Field.Displacement, scheme=DiscreteIndex(mode_num))
      

    • For Thermal Simulation, the available FieldType are * Temperature which is a tuple of dimension 1

      • HeatFlux which is a tuple of dimension 3

    • Field Query Interface usage

      # FieldQuery example
      # Create a FieldQuery to query displacement
      results = QueryResult(assembly)
      displacement_query = FieldQuery(f=Field.Displacement)
      
      # Create a FieldQuery with optional input to query the y-component
      y_displacement_query = FieldQuery(f=Field.Displacement, component=1)
      
      # FieldQuery with optional input to query the norm of displacement
      displacement_magnitude_query = FieldQuery(f=Field.Displacement, norm=True)
      
      # Sample the simulation with the given query to create a VectorArray
      # * more info on VectorArrays are provided in the subsequent section *
      displacement_VectorArray1 = simulator.sample(displacement_query, results)
      displacement_VectorArray2 = simulator.sample(y_displacement_query, results)
      displacement_VectorArray3 = simulator.sample(displacement_magnitude_query, results)
      
      displacement1 = displacement_VectorArray1.get(i, j); # jth component of the displacement (0 = X, 1 = Y, or 2 = Z) at the ith sampling point
      displacement2 = displacement_VectorArray2.get(1, 0); # y-displacement value at the second sampling point
      displacement3 = displacement_VectorArray3.get(1, 0); # displacement magnitude at the second sampling point
      

Sample and Export Results

• Sampling results in-memory

  • Methods to sample results of the simulation and store/print VectorArray results from the queries created above.

    # Query results
    results = QueryResult(assembly)
    stress_query = FieldQuery(f=Field.Stress) # a field is needed to create a field query
    stress_VectorArray = simulator.sample(stress_query, results)
    

  • This sampling is stored in a VectorArray of size n_tuple by dimension, n_tuple is the number of points sampled in the component/assembly and dimension depends on the query type. For example, FieldQuery(Field.Displacement) has a dimension of 3 for each displacement component, thus VectorArray.get(i, 2) would get the z-displacement of point i.

    # Get the number of tuples (vectors) in the VectorArray (one per point results are sampled at)
    n_tuples = stress_VectorArray.n_tuples()
    
    # Get the dimension of each vector - in this case 6, one value for each stress component
    dimension = stress_VectorArray.dimension()
    
    stress_xx = stress_VectorArray.get(i, 0); # stress_xx at i-th sample point
    stress_yy = stress_VectorArray.get(i, 1); # stress_yy at i-th sample point
    stress_ij = stress_VectorArray.get(i, j); # jth stress component (0, 1, 2, 3, 4, or 5) of the ith tuple
    

• Export results to a file: Once the query is created, results can be used to write a .vtu file which contains all solution fields via results.writeVTK which has two inputs:

  • file name "*.vtu"

  • UnitSystem is an attribute in the *.vtu ( Note that this argument is just metadata in the *.vtu file. The result magnitudes are in the unit of the scenario regardless of the unit system specified. )

  # Write results to a file (unit system is saved as a metadata in the vtu file)
  results = QueryResult(assembly)
  stress_query = FieldQuery(Field.VonMisesStress)
  simulator.sample(stress_query, results)
  
  # Write results to a file (unit system is saved as a metadata in the vtu file)
  results.writeVTK("cantilever_beam_results.vtu", UnitSystem.MeterKilogramSecond)
  

Sampling on Custom Geometries

• Another important functionality is the ability to specify a point set to sample on. This can be done by creating a new sampling_component consisting of vertices at the desired sampling locations. Note that the sampling_component is not to be included in the assembly that is being simulated.

  # Create an empty MeshModel to store vertices for desired sampling locations
  sampling_geometry = MeshModel()
  
  # Add the desired sampling point locations and store their ID for later use
  test_index1 = sampling_geometry.addVertex([6.0, 0.0, 0.0])
  test_index2 = sampling_geometry.addVertex([3.0, 0.0, 0.0])
  
  sampling_component = MaterialDomain(sample_geometry, "material_name", scenario)
  
  # Define the assembly to be simulated (note that the sampling_component is not included)
  component = MaterialDomain(component_geometry, "material_name", scenario)
  assembly = [component]
  simulator = StressSimulator(assembly, scenario)
  simulator.solve()
  
  displacement_query = FieldQuery(f=Field.Displacement)
  sampled_results = QueryResult(sampling_component) # sample only the custom point set
  sampled_VectorArray = simulator.sample(displacement_query, sampled_results)
  
  displacement_index1 = sampled_VectorArray.get(test_index1, 0) # x-displacement at above specified index1
  displacement_index2 = sampled_VectorArray.get(test_index2, 1) # y-displacement at above specified index2
  

Installation

Prerequisites

PyIntact can be installed when running Python 3.10 or 3.11, and requires the openmpi-devel package to be installed.

Installation

Install PyIntact, the python interface to Intact.Simulation, by downloading the Python wheel and then using pip to install, as in the following example:

pip install PyIntact.whl

PyIntact API

class PyIntact.Geometry(self: PyIntact.Geometry, value: int)

Members:

VDB

Mesh

property name

class PyIntact.Model

property instance_id

The instance ID of the model. We enforce that this must be unique per run.

mass(self: PyIntact.Model) -> float

Returns the mass of the model

property model_name

This is used for debugging purposes. It need not be filled out in general.

projectField(self: PyIntact.Model, field: Callable[[Annotated[list[float], FixedSize(3)]], Intact::Tensor]) -> None

Sets tensors according to a user-provided callback

Parameter field:

The field

setDensities(self: PyIntact.Model, densities: list[float]) -> None

Sets tensors as 1x1-dimensional data, AKA densities. This is a convenience wrapper around setTensors.

Parameter densities:

The densities

setTensors(self: PyIntact.Model, tensors: list[Intact::Tensor]) -> None

Set the tensors for all voxels.

Parameter tensors:

The tensors for all voxels.

tensor(self: PyIntact.Model, id: int) -> Intact::Tensor

Returns the tensor at the given index

Parameter id:

The id (typically point ID) for the tensor

class PyIntact.MeshModel(*args, **kwargs)

Bases: Model

Overloaded function.

1. __init__(self: PyIntact.MeshModel) -> None

Construct an empty MeshModel.

1. __init__(self: PyIntact.MeshModel, other: PyIntact.MeshModel) -> None

Construct a MeshModel from an existing MeshModel.

Parameter other:

A MeshModel.

1. __init__(self: PyIntact.MeshModel, filename: str) -> None

Load MeshModel from file.

Parameter filename:

File must be a VTU, PLY, or STL file.

addFacet(self: PyIntact.MeshModel, vertex_1: int, vertex_2: int, vertex_3: int) -> int

Add a new facet to the MeshModel.

Parameter vertex_1:

Index of the first vertex in the facet.

Parameter vertex_2:

Index of the second vertex in the facet.

Parameter vertex_3:

Index of the third vertex in the facet.

Returns:

The index of the new facet.

addVertex(self: PyIntact.MeshModel, vertex: Annotated[list[float], FixedSize(3)]) -> int

Add new vertex to the MeshModel.

Parameter vertex:

The position of the vertex.

Returns:

The index of the new vertex for use with facets.

facet(self: PyIntact.MeshModel, facet_index: int) -> Annotated[list[int], FixedSize(3)]

Get a specific facet.

Parameter facet_index:

The facet identifier.

Returns:

The facet.

facetCount(self: PyIntact.MeshModel) -> int

Get the number of facets in the MeshModel.

refine(*args, **kwargs)

Overloaded function.

1. refine(self: PyIntact.MeshModel, threshold: float) -> None

Refine the input mesh, by splitting every facet edge that is larger than (threshold) * (bounding box size of mesh). Refining the input mesh increases sampling density.

Parameter threshold:

The fraction of the bounding box size of the mesh.

1. refine(self: PyIntact.MeshModel) -> None

Refine the input mesh, by splitting every facet edge that is larger than 2% of bounding box size of mesh.

vertex(self: PyIntact.MeshModel, vertex_index: int) -> Annotated[list[float], FixedSize(3)]

Get a specific vertex.

Parameter vertex_index:

The vertex identifier.

Returns:

The vertex.

vertexCount(self: PyIntact.MeshModel) -> int

Get the number of vertices in the MeshModel.

writePLY(self: PyIntact.MeshModel, output_filename: str) -> None

Write the MeshModel to file in PLY format.

Parameter output_filename:

The output filename.

writeVTU(self: PyIntact.MeshModel, output_filename: str) -> None

Write the MeshModel to file in VTU (VTK unstructured grid) format.

Parameter output_filename:

The output filename.

class PyIntact.Tensor(self: PyIntact.Tensor, arg0: list[float], arg1: int, arg2: int)

cols(self: PyIntact.Tensor) -> int

raw_data(self: PyIntact.Tensor) -> list[float]

rows(self: PyIntact.Tensor) -> int

class PyIntact.VDBModel(*args, **kwargs)

Bases: Model

Represents a model based on an openVDB volume.

Overloaded function.

1. __init__(self: PyIntact.VDBModel, filename: str) -> None

Load a VDBModel from a file.

Parameter filename:

The VDB file.

1. __init__(self: PyIntact.VDBModel, grid: openvdb::v7_2::Grid<openvdb::v7_2::tree::Tree<openvdb::v7_2::tree::RootNode<openvdb::v7_2::tree::InternalNode<openvdb::v7_2::tree::InternalNode<openvdb::v7_2::tree::LeafNode<double, 3u>, 4u>, 5u> > > >) -> None

Construct a VDBModel an existing DoubleGrid.

Parameter grid:

The existing DoubleGrid.

tessellate(self: PyIntact.VDBModel) -> `PyIntact.MeshModel <#PyIntact.MeshModel>`_

Create a mesh from the VDBModel, using the OpenVDB volumeToMesh method.

Returns:

A MeshModel.

class PyIntact.MaterialDomain(self: PyIntact.MaterialDomain, model: PyIntact.Model, material_name: str, scenario_descriptor: Intact::AbstractScenarioDescriptor)

Construct a MaterialDomain from a model, material name, and scenario descriptor. This constructor ensures the material units are consistent with scenario units and should be used.

Parameter model:

The model

Parameter material_name:

The material name

Parameter scenario_descriptor:

The scenario descriptor

class PyIntact.Field(self: PyIntact.Field, value: int)

Members:

Displacement

Strain

Stress

TopologicalSensitivity

StrainEnergyDensity

VonMisesStress

Temperature

HeatFlux

property name

class PyIntact.Query

class PyIntact.FieldQuery(*args, **kwargs)

Bases: Query

This class describes a query over a field. This query can be for a specific field component, or the norm of the field.

Overloaded function.

1. __init__(self: PyIntact.FieldQuery, *, f: PyIntact.Field, norm: bool = False) -> None

Parameter f:

The field to sample

Parameter norm:

Whether to compute the norm of the field.

1. __init__(self: PyIntact.FieldQuery, *, f: PyIntact.Field, scheme: Intact::IndexScheme, norm: bool = False) -> None

Parameter f:

The field to sample

Parameter scheme:

The indexing scheme for the field

Parameter norm:

Whether to compute the norm of the field.

1. __init__(self: PyIntact.FieldQuery, *, f: PyIntact.Field, component: int) -> None

Parameter f:

The field to sample

Parameter component:

The field component to sample

1. __init__(self: PyIntact.FieldQuery, *, f: PyIntact.Field, component: int, scheme: Intact::IndexScheme) -> None

Parameter f:

The field to sample

Parameter component:

The field component to sample

Parameter scheme:

The indexing scheme for the field

class PyIntact.StatisticalQuery(*args, **kwargs)

Bases: Query

This class describes a query for a statistic over a field. This query can be for the minimum, maximum or mean value of the field.

Overloaded function.

1. __init__(self: PyIntact.StatisticalQuery, *, f: PyIntact.Field, s: PyIntact.StatisticalQueryType, norm: bool = False) -> None

Parameter f:

The field to sample.

Parameter s:

The statistic to query for.

Parameter norm:

Whether to compute the norm of the field.

1. __init__(self: PyIntact.StatisticalQuery, *, f: PyIntact.Field, component: int, s: PyIntact.StatisticalQueryType) -> None

Parameter f:

The field to sample.

Parameter component:

The field component to sample.

Parameter s:

The statistic to query for.

1. __init__(self: PyIntact.StatisticalQuery, *, f: PyIntact.Field, s: PyIntact.StatisticalQueryType, scheme: Intact::IndexScheme, norm: bool) -> None

Parameter f:

The field to sample.

Parameter s:

The statistic to query for.

Parameter scheme:

The indexing scheme for the field

Parameter norm:

Whether to compute the norm of the field.

1. __init__(self: PyIntact.StatisticalQuery, *, f: PyIntact.Field, component: int, s: PyIntact.StatisticalQueryType, scheme: Intact::IndexScheme) -> None

Parameter f:

The field to sample.

Parameter component:

The field component to sample.

Parameter s:

The statistic to query for.

Parameter scheme:

The indexing scheme for the field

class PyIntact.IndexScheme

class PyIntact.DiscreteIndex(self: PyIntact.DiscreteIndex, arg0: int)

Bases: IndexScheme

class PyIntact.NullIndex

Bases: IndexScheme

class PyIntact.VectorArray(*args, **kwargs)

This class represents an array of constant-sized vector data. It wraps a flat std::vector<double> for cache performance, but structures the queries so that indexing errors are unlikely.

Overloaded function.

1. __init__(self: PyIntact.VectorArray) -> None

2. __init__(self: PyIntact.VectorArray, arg0: int, arg1: int) -> None

3. __init__(self: PyIntact.VectorArray, arg0: list[float], arg1: int) -> None

dimension(self: PyIntact.VectorArray) -> int

get(self: PyIntact.VectorArray, arg0: int, arg1: int) -> float

Get the component at the given index.

Parameter index:

The index

Parameter component:

The component

Returns:

Returns the component at the given index value.

n_tuples(self: PyIntact.VectorArray) -> int

Gives the number of tuples stored in this vector array.

Returns:

The full size of the raw data divided by the vector m_dimension.

raw_data(self: PyIntact.VectorArray) -> list[float]

class PyIntact.QueryResult(*args, **kwargs)

This class describes a query result. The buffer contains a list of scalar values, however the amount of data depends on the query type that produced it.

Overloaded function.

1. __init__(self: PyIntact.QueryResult, model: PyIntact.MaterialDomain) -> None

Constructs a new query result over the given material domain. Note that if the underlying model is a VoxelModel, the data will be sampled at the centroids of each voxel, and the data will be persisted in the same order as the voxels themselves. Otherwise, the data will be sampled at the points of the model and persisted in the same order as the points.

1. __init__(self: PyIntact.QueryResult, assembly: list[PyIntact.MaterialDomain]) -> None

Constructs a new query result over the given assembly. Note that if the underlying model is a VoxelModel, the data will be sampled at the centroids of each voxel, and the data will be persisted in the same order as the voxels themselves. Otherwise, the data will be sampled at the points of the model and persisted in the same order as the points.

addData(self: PyIntact.QueryResult, arg0: PyIntact.Query, arg1: PyIntact.VectorArray) -> None

Adds the result of computing query to this object.

Parameter query:

The query being computed.

Parameter data:

The data result of the query.

getData(self: PyIntact.QueryResult, arg0: PyIntact.Query) -> `PyIntact.VectorArray <#PyIntact.VectorArray>`_

Returns the vector-valued data indexed by the given query. Note that this method can throw an error if the query data has not been precomputed. Use hasData to ensure that such data has been computed.

Parameter query:

The query whose results are to be returned

Returns:

The vector-valued output of the query.

hasData(self: PyIntact.QueryResult, arg0: PyIntact.Query) -> bool

Determines if data exists for a given query.

Parameter query:

The query whose results we are checking on.

Returns:

True if data has been computed, False otherwise.

writeVTK(self: PyIntact.QueryResult, filename: str, unit_system: Intact::UnitSystemType) -> None

Writes a vtk file containing the results that have been stored on this object.

Parameter filename:

The filename to write to. If it does not end in “.vtu”, the “.vtu” will be appended to the filename.

Parameter unit_system:

The Unitsystem to use when attaching units to the sampled data.

class PyIntact.UnitSystem(self: PyIntact.UnitSystem, value: int)

Members:

MeterKilogramSecond

CentimeterGramSecond

MillimeterMegagramSecond

FootPoundSecond

InchPoundSecond

property name

class PyIntact.Metadata

property basis_order

The order of basis function approximation to use. We support linear (= 1) and quadratic (= 2).

property cell_size

The exact simulation cell size to use.

Warning: Setting the cell_size overrides the resolution.

property integrator_override

For some physics types, there may be multiple integrator implementations available. This field allows you to override the default solver.

property max_iterations_multiplier

max_iterations_multiplier is used to control the maximum number of iterations of a solver from the AMG family of solvers. Use a value less than 1 to reduce the maximum number of iterations and reduce the solver runtime.

property moment_order

moment_order is the order of moments computed for integration. Use lower for faster runtime, at an accuracy cost. This number must be at least 2 and can be as high as 6-7. The default is 3.

property resolution

resolution is the number of finite elements to compute over. Note that Intact will only approximate the target number of cells. Either this member or the cell_size must be set, or else Intact will throw an error.

property solver_override

For some integrator types, there are multiple sparse linear solvers available. Please see the user’s manual for information about the available options. The default is AMGCL_amg.

property tolerance

The tolerance of the linear solver. Use a smaller tolerance for more accurate simulations and longer runtime. Use a larger tolerance for less accurate simulations and shorter runtime. Default is 1e-8.

class PyIntact.ThermalMetadata

property environment_temperature

The temperature of the environment.

class PyIntact.ModalMetadata

property desired_eigenvalues

The number of eigenvalues or natural frequencies to calculate.

class PyIntact.Solver(self: PyIntact.Solver, value: int)

Members:

AMGCL_cg : Iterative conjugate gradient solver without preconditioner.

AMGCL_ilu0_cg : Iterative conjugate gradient solver with ilu0 preconditioner.

AMGCL_damped_jacobi_cg : Iterative conjugate gradient solver with damped jacobi preconditioner.

AMGCL_amg : Iterative AMG based solver with smoothed aggregation. This is the default solver for thermal scenarios.

AMGCL_amg_rigid_body : Iterative AMG based solver with rigid body modes based coarsening. This is the default solver for linear elasticity. This solver cannot be used with thermal scenarios.

Eigen_SparseLU : Direct solver that uses LU decomposition.

MKL_PardisoLDLT : PardisoLDLT is proprietary direct solver provided by Intel through MKL. Use Intact::mklPresent() to check whether this feature is available.

MKL_PardisoLLT : PardisoLLT is proprietary direct solver provided by Intel through MKL. Use Intact::mklPresent() to check whether this feature is available.

MKL_PardisoLU : PardisoLU is proprietary direct solver provided by Intel through MKL. Use Intact::mklPresent() to check whether this feature is available.

property name

class PyIntact.Integrator(self: PyIntact.Integrator, value: int)

Members:

IntactModal

IntactLinearElasticity

MPCLinearElasticity

MPCStaticThermal

LinearBuckling

property name

class PyIntact.AbstractBoundaryConditionDescriptor

property boundary

The boundary where the boundary condition is applied.

property units

The unit system. If not set, then the default value is MeterKilogramSecond.

class PyIntact.TractionDescriptor

Bases: AbstractBoundaryConditionDescriptor

class PyIntact.VectorForceDescriptor(self: PyIntact.VectorForceDescriptor)

Bases: TractionDescriptor

Describes a vector force applied uniformly over the specified boundary.

property direction

The direction of the force.

property magnitude

The magnitude of the force.

class PyIntact.HydrostaticForceDescriptor(self: PyIntact.HydrostaticForceDescriptor)

Bases: TractionDescriptor

Simulates a body submerged in liquid.

property density

The density of the liquid in which the body is submerged.

property height

The height the liquid rises above the z=0 plane.

class PyIntact.PressureForceDescriptor(self: PyIntact.PressureForceDescriptor)

Bases: TractionDescriptor

Describes a pressure load (force per unit area) applied normal to the boundary.

property magnitude

The magnitude of the pressure load.

class PyIntact.TorqueForceDescriptor(self: PyIntact.TorqueForceDescriptor)

Bases: TractionDescriptor

Describes a torque load applied to the boundary.

property axis

The axis of rotation of the torque load.

property magnitude

The magnitude of the torque load.

property origin

The origin of the axis of rotation of the torque.

class PyIntact.BearingForceDescriptor(self: PyIntact.BearingForceDescriptor)

Bases: TractionDescriptor

Describes a load at the contact between two curved surfaces. The contact pressure is not uniform. It is scaled by the angle of the contact relative to the angle of the force.

property direction

The direction of the force.

property magnitude

The magnitude is the total force applied over the entire surface.

class PyIntact.FixedBoundaryDescriptor(self: PyIntact.FixedBoundaryDescriptor)

Bases: AbstractBoundaryConditionDescriptor

This class describes a fixed solution quantity (also known as a Dirichlet boundary condition). In order to set the value to fix the solution, set the value member. Note that not all scenarios support inhomogeneous Dirichlet conditions.

property value

The value of the boundary condition.

class PyIntact.FixedVectorDescriptor(self: PyIntact.FixedVectorDescriptor)

Bases: AbstractBoundaryConditionDescriptor

Describes a fixed vector quantity.

A fixed vector boundary condition can represent fixing displacement at some non-zero value, or it can represent partial restraints, also known as axis-aligned sliding restraints.

Displacement is a three dimensional field, and each displacement component can optionally be specified. Any axis not specified will not be restrained.

property x_value

The value of the boundary condition in the x-direction.

property y_value

The value of the boundary condition in the y-direction.

property z_value

The value of the boundary condition in the z-direction.

class PyIntact.SlidingBoundaryDescriptor(self: PyIntact.SlidingBoundaryDescriptor)

Bases: AbstractBoundaryConditionDescriptor

Describes a sliding boundary condition, which prevents displacement in the direction normal to the specified surface, and permits displacement tangential to the surface.

class PyIntact.ConvectionDescriptor(self: PyIntact.ConvectionDescriptor)

Bases: AbstractBoundaryConditionDescriptor

Describes the convective transfer of heat from a surrounding medium.

property coefficient

The coefficient of convection.

property environment_temperature

The temperature of the surrounding medium.

class PyIntact.ConstantFluxDescriptor(self: PyIntact.ConstantFluxDescriptor)

Bases: AbstractBoundaryConditionDescriptor

Describes a constant flux per unit surface area.

property magnitude

The magnitude of the flux.

class PyIntact.AbstractInternalConditionDescriptor

property instance_id

The instance id of the Model that this internal condition is applied to. If not set, then this internal condition is applied to every instance.

property units

The unit system. If not set, then the default value is MeterKilogramSecond.

class PyIntact.BodyLoadDescriptor(self: PyIntact.BodyLoadDescriptor)

Bases: AbstractInternalConditionDescriptor

Describes body load caused by linear acceleration.

property direction

The direction of the acceleration.

property magnitude

The magnitude of the acceleration.

class PyIntact.RotationalLoadDescriptor(self: PyIntact.RotationalLoadDescriptor)

Bases: AbstractInternalConditionDescriptor

Describes a rotational load on a body.

property angular_acceleration

The angular acceleration.

property angular_velocity

The angular velocity.

property axis

The axis of rotation of the rotational load.

property origin

The origin of the axis of rotation of the rotational load.

class PyIntact.ConstantHeatDescriptor(self: PyIntact.ConstantHeatDescriptor)

Bases: AbstractInternalConditionDescriptor

Describes the uniform generation of heat within a body.

property magnitude

The magnitude of the body heat flux.

class PyIntact.AbstractMaterialDescriptor

An abstract description of a material.

property density

The material density.

property units

The unit system. If not set, then the default value is MeterKilogramSecond.

class PyIntact.IsotropicMaterialDescriptor(self: PyIntact.IsotropicMaterialDescriptor)

Bases: AbstractMaterialDescriptor

Describes an isotropic material, which has the same behavior no matter the direction of the forces applied.

property compressive_strength

The ultimate strength in compression of the material.

property poisson_ratio

The Poisson ratio of the material.

property tensile_strength

The ultimate strength in tension of the material.

property yield_strength

The yield strength of the material.

property youngs_modulus

The Young’s modulus of the material.

class PyIntact.OrthotropicMaterialDescriptor(self: PyIntact.OrthotropicMaterialDescriptor)

Bases: AbstractMaterialDescriptor

property Ex

The elastic modulus in the x-direction

property Ey

The elastic modulus in the y-direction

property Ez

The elastic modulus in the z-direction

property Gxy

The shear modulus in the xy plane.

property Gxz

The shear modulus in the xz plane.

property Gyz

The shear modulus in the yz plane.

property transform

A transformation matrix to change the material orientation.

property vxy

The poisson ratio in the xy plane.

property vxz

The poisson ratio in the xz plane.

property vyz

The poisson ratio in the yz plane.

class PyIntact.ThermalMaterialDescriptor(self: PyIntact.ThermalMaterialDescriptor)

Bases: AbstractMaterialDescriptor

Describes the thermal properties of an isotropic material.

property conductivity

The thermal conductivity.

property expansion_coefficient

The coefficient of thermal expansion (optional).

property specific_heat

The specific heat of the material.

class PyIntact.AbstractScenarioDescriptor

property boundary_conditions

The collection of boundary conditions to be applied.

property materials

The mapping of a material identifier, usually the material name, to the material.

property metadata

Metadata about the simulation to be performed.

class PyIntact.LinearElasticScenarioDescriptor(self: PyIntact.LinearElasticScenarioDescriptor)

Bases: AbstractScenarioDescriptor

Describes a linear elastic scenario to be simulated.

property internal_conditions

The collection of the internal conditions, such as a gravity load, to be applied.

class PyIntact.ModalScenarioDescriptor(self: PyIntact.ModalScenarioDescriptor)

Bases: AbstractScenarioDescriptor

class PyIntact.LinearBucklingScenarioDescriptor(self: PyIntact.LinearBucklingScenarioDescriptor)

Bases: AbstractScenarioDescriptor

Describes a linear buckling scenario to be simulated.

property internal_conditions

The collection of the internal conditions, such as a gravity load, to be applied.

class PyIntact.StaticThermalScenarioDescriptor(self: PyIntact.StaticThermalScenarioDescriptor)

Bases: AbstractScenarioDescriptor

class PyIntact.Simulator

Generic Simulation Manager

cellComplex(self: PyIntact.Simulator) -> list[tuple[Annotated[list[float], FixedSize(3)], Annotated[list[float], FixedSize(3)]]]

Get the simulation grid.

Returns:

A vector of pairs of points that represent the minimum and maximum of the bounding box of each cell in the simulation grid.

cellCount(self: PyIntact.Simulator) -> int

Get the number of cells in the simulation grid.

cellSize(self: PyIntact.Simulator) -> float

Get the size of each cell in the simulation grid.

sample(*args, **kwargs)

Overloaded function.

1. sample(self: PyIntact.Simulator, query: PyIntact.Query, result: PyIntact.QueryResult) -> PyIntact.VectorArray

Sample the given query over the domain provided.

Parameter query:

The result to query for.

Parameter result:

The query result.

Returns:

The values of the query.

1. sample(self: PyIntact.Simulator, sample_points: list[Annotated[list[float], FixedSize(3)]], material_name: str, field_queries: list[PyIntact.FieldQuery]) -> list[PyIntact.VectorArray]

Sample at the given points, producing results for each query

Parameter sample_points:

The sample points

Parameter material_name:

Name of the material associated with points

Parameter field_queries:

The field queries to be answered

Returns:

The values of the field queries at the query points, in order

solve(self: PyIntact.Simulator) -> PyIntact.SolutionStats

Solve the simulation that has been constructed.

Returns:

The number of iterations performed by the solver and the error.

class PyIntact.StressSimulator(*args, **kwargs)

Bases: Simulator

Simulation Manager for Stress Scenarios

Overloaded function.

1. __init__(self: PyIntact.StressSimulator, assembly: list[PyIntact.MaterialDomain], descriptor: PyIntact.LinearElasticScenarioDescriptor) -> None

Construct a linear elastic scenario

Parameter assembly:

A collection of MaterialDomains.

Parameter descriptor:

A LinearElasticScenarioDescriptor that describes the simulation.

1. __init__(self: PyIntact.StressSimulator, arg0: list[PyIntact.MaterialDomain], arg1: PyIntact.LinearElasticScenarioDescriptor, arg2: Intact::StaticThermalSimulator) -> None

Construct a linear elastic scenario

Parameter assembly:

A collection of MaterialDomains.

Parameter descriptor:

A LinearElasticScenarioDescriptor that describes the simulation.

class PyIntact.ModalSimulator(self: PyIntact.ModalSimulator, arg0: list[PyIntact.MaterialDomain], arg1: PyIntact.ModalScenarioDescriptor)

Bases: Simulator

Simulation Manager for Modal Scenarios

Construct a modal elastic scenario.

Parameter assembly:

A collection of MaterialDomains.

Parameter descriptor:

A ModalScenarioDescriptor that describes the simulation.

class PyIntact.LinearBucklingSimulator(self: PyIntact.LinearBucklingSimulator, arg0: list[PyIntact.MaterialDomain], arg1: PyIntact.LinearBucklingScenarioDescriptor)

Bases: Simulator

Simulation Manager for linear buckling scenarios

Construct a linear buckling scenario.

Parameter assembly:

A collection of MaterialDomains.

Parameter descriptor:

A LinearBucklingScenarioDescriptor that describes the simulation.

class PyIntact.StaticThermalSimulator(self: PyIntact.StaticThermalSimulator, arg0: list[PyIntact.MaterialDomain], arg1: PyIntact.StaticThermalScenarioDescriptor)

Bases: Simulator

Simulation Manager for Static Thermal Scenarios

Construct a static thermal scenario

Parameter assembly:

A collection of MaterialDomains.

Parameter descriptor:

A StaticThermalScenarioDescriptor that describes the simulation.

PyIntact.setupLogging(log_level: int, catch_sig: bool = True) -> None

Initialize logging

Parameter log_level:

The max log level: 0 is info, -1 is warning, -2 is errors

Parameter catch_sig:

Whether Intact should gracefully handle signals. For testing purposes where exit code of the program is important, set to false.