6 solid_mechanics_definitions#(struct:traverse-element #<procedure:...lib/render-cond.rkt:38:12>)

6 solid_mechanics_definitions (release)

Contains all the definitions specific to a solid mechanics procedure.

Name	Type	Description	Default
boundary_conditions (release) [optional]	LIST	A boundary condition object defines a static or kinematic displacement type boundary condition. Boundary conditions can be applied to sets representing both boundaries and bodies.
load_conditions (release) [optional]	LIST	The load_conditions object defines applied loads. Loads can be applied to sets representing boundaries and bodies.
initial_conditions (alpha) [optional]	LIST	An initial condition definition defines a condition of the procedure at its start time.
outputs (release) [optional]	LIST	The outputs object holds all output objects, identified by user defined identifiers, each of which define an output for this procedure. If a chosen set was specified as an immersed set during geometry creation, that set must the only item in the sets list. If an immersed set is selected the output command will produce two separate files. The main file will include a tessellated surface representation of the boundary. The second file (with suffix envelope), will include a smooth volumetric output of the U-spline envelope domain for the immersed set. When viewing results on the envelope domain take care that only values on the interior of the model of interest are considered as values at the extremities of this representation may not exhibit physically relevant behavior. Not all elements from the original mesh used may be shown, in general only those that intersect the model of interest will be included.
probes (release) [optional]	LIST	The probes object holds all user defined probe_variables. Probe variables are used to track quantities of interest at specific locations in a model over time. For example, a user may want to track von Mises stress at a specific location in a model over time.
interactions (release) [optional]	LIST	Each object in the interaction definitions array defines an interaction for the procedure. Currently the supported interactions are mechanical_contact and tied_constraint.
interaction_search_parameters (beta) [optional]	LIST	Each object in the interaction search definitions array defines search parameters to be used in an interaction. Currently the supported search definitions is a sensor-based layout.
interaction_properties (beta) [optional]	LIST	The interaction property definition allows the user to define the type of friction and movement that occurs once contact is initiated.

6.1 boundary_conditions (release)

A boundary condition object defines a static or kinematic displacement type boundary condition. Boundary conditions can be applied to sets representing both boundaries and bodies.

Name	Type	Description	Default
label	STRING	A user defined identifier for this boundary condition.
displacement (release) \| velocity (beta) \| acceleration (beta)	SUB OBJECT \| SUB OBJECT \| SUB OBJECT	One of the given keywords must be defined to specify kinematic variable to be constrained by this boundary condition
part \| set	STRING \| STRING	Defines the set or part to be operated on
penalty (beta) [optional]	SUB OBJECT	See linked documentation
quadrature_options (beta) [optional]	SUB OBJECT	See linked documentation

Example Usage:
boundary_conditions: [ { label: "hold_bottom", displacement: { components: [ "x", "y", "z" ], scale_factor: [ 0 ], function: "constant_1" }, set: "hold_surface", penalty: {value: 24000000000, dimensionless: false}, quadrature_options: { quadrature: "QP1"} } ]

6.1.1 displacement (release)

Name	Type	Description	Default
components	[ “x” \| “y” \| “z”, ... ]	Specifies which degrees-of-freedom components are active.
scale_factor [optional]	[ DOUBLE, ... ]	A scalar value or vector of the same length as components which scales the function.	1.0
function	STRING	The user defined identifier of the temporal function.

Example Usage:
displacement: { components: [ "x", "y", "z" ], scale_factor: [ 0 ], function: "constant_1" }

6.1.2 velocity (beta)

Name	Type	Description	Default
components (beta)	[ “x” \| “y” \| “z”, ... ]	Specifies which degrees-of-freedom components are active.
scale_factor [optional] (beta)	[ DOUBLE, ... ]	A scalar value or vector of the same length as components which scales the function.	1.0
function (beta)	STRING	The user defined identifier of the temporal function.

6.1.3 acceleration (beta)

Name	Type	Description	Default
components (beta)	[ “x” \| “y” \| “z”, ... ]	Specifies which degrees-of-freedom components are active.
scale_factor [optional] (beta)	[ DOUBLE, ... ]	A scalar value or vector of the same length as components which scales the function.	1.0
function (beta)	STRING	The user defined identifier of the temporal function.

6.1.4 part | set

Defines the set or part to be operated on

Name	Type	Description	Default
part	STRING	The user defined label of the part that defines the set.
set	STRING	The user defined identifier of the geometric set.

6.1.5 penalty (beta)

Options for penalty enforcement of a boundary condition or other type of constraint. When penalty values are calculated from a dimensionless scale using material properties and element size on two sides of a material or contact interface, the smaller of the two values is selected.

Name	Type	Description	Default
value (beta)	DOUBLE	The value of the penalty parameter, in the range $[0,\infty)$ , determining how strongly the constraint is enforced. The precise interpretation of this value depends on the choice of the parameter dimensionless, whose documentation provides a more detailed discussion. Note that the default value assumes that dimensionless is also set to its default value of true.	1e1
dimensionless (beta)	true\|false	If this parameter is true, then the penalty value is interpreted as the dimensionless constant $C$ in the formula $\beta = CEh^{c-2}$ , where $E$ is a scalar estimate of the material stiffness (i.e., the Young's modulus in elasticity or the thermal conductivity in heat conduction), $h$ is a measure of element size (with units of length), and $c$ is the co-dimension of the constrained set, i.e., 0 for volumes, 1 for surfaces, 2 for curves, or 3 for points. If this parameter is false, then the penalty value is instead interpreted as the dimensional value of $\beta$ directly. The dimensionless option is recommended for most use cases. To interpret the dimensionless penalty value for the common case of constrained boundaries and interfaces ( $c=1$ ) in elasticity, it is roughly the ratio of a single element's change in length under a given tensile load to the error allowed in the consraint. Note that, for any positive value, the constraint error will go to zero as the mesh is refined, since the specimen's overall change in length is distributed over more elements. Selecting too large of a penalty value makes the discrete problem harder to solve. The default value represents a good balance between accuracy and efficiency for most practical applications, but higher values may be appropriate for certain situations, such as calibrating material models with single-element patch tests.	true

6.1.6 quadrature_options (beta)

Name	Type	Description	Default
quadrature [optional] (beta)	“QP1” \| “QP0” \| “Q1” \| “Q2” \| “Q3” \| “Q4” \| “Q5” \| “Q6” \| “Q7” \| “Q8” \| “Q9” \| “Q10”	Quadrature type enumeration. The quadrature type determines the point layout over a patch or patch element. The schemes following the pattern “Q#” specify that a Gauss quadrature scheme with #-points will be used. The schemes following the pattern “QP#” specify that a Gauss quadrature scheme with $(P+\#)$ -points will be used, where $P$ is the degree of the patch's or patch element's basis.	QP1
optimized_cut_quadrature_strategy [optional] (beta)	“match_uncut” \| “reduce_from_uncut” \| “match_basis”	Strategy to choose the degree of accuracy for quadrature on cut cells. The default strategy of chooses quadrature rules with similar numbers of points as those used on uncut cells, as specified by ; it has lower formal accuracy (integrating tensor products of monomials up to degree $N-1$ for uncut quadrature $N$ ), but is a good default choice for practical calculations. The strategy match_uncut matches the formal accuracy of the quadrature on uncut cells, but is significantly more costly. The strategy match_basis chooses a rule that exactly integrates the basis functions; this is equivalent to reduce_from_uncut if the uncut cells use the default quadrature of QP1, but may differ for other choices of uncut quadrature.	reduce_from_uncut
optimized_cut_quadrature_degree [optional] (beta)	NONNEGATIVE INTEGER	If provided, this value overrides optimized_cut_quadrature_strategy by specifying an explicit polynomial degree of accuracy for optimized quadrature rules on cut cells.
optimization_method [optional] (beta)	“tet_pruning” \| “grid_doubling” \| “linear_programming”	Specifies the preferred method of quadrature generation for cut cells. If the preferred method fails on a particular cell, the other methods will be used in an attempt to recover.	tet_pruning
optimization_residual_tolerance [optional] (beta)	DOUBLE	The absolute residual tolerance used in quadrature optimization on cut cells. A smaller value will result in a more accurate quadrature rule, but may increase the time to compute quadrature rules for cut cells.	1e-12
optimization_lawson_hanson_solve_completion [optional]	true\|false	An experimental option that controls the convergence behavior of quadrature optimization. For best results it is recommended to set this value to true. If set to true this causes each iteration of quadrature optimization to solve to the highest accuracy possible. The results at each iteration are then checked against the optimization_residual_tolerance to determine if a sufficient rule has been found. If this value is set to false then the optimization_residual_tolerance is passed to the solve at each iteration and can cause the solve step to terminate more quickly which can result in faster execution and a lower number of quadrature points. However the quality and accuracy of the resulting rule may be suspect.	true

6.2 load_conditions (release)

The load_conditions object defines applied loads. Loads can be applied to sets representing boundaries and bodies.

Name	Type	Description	Default
label	STRING	User defined identifier for this load condition.
temperature_distribution (alpha) \| surface_traction (release) \| surface_pressure (release) \| point_force (release) \| line_traction (release) \| body_force (release)	SUB OBJECT \| SUB OBJECT \| SUB OBJECT \| SUB OBJECT \| SUB OBJECT \| SUB OBJECT	One of the given keywords must be defined to specify the class of load condition
part \| set	STRING \| STRING	Defines the set or part to be operated on
follower [optional] (beta)	true\|false	If true, the load direction will follow the loaded region as it deforms and the current surface area will be used. If false, load direction and magnitude will remain unchanged as the domain deforms.	false
quadrature_options (beta) [optional]	SUB OBJECT	See linked documentation

Example Usage:
load_conditions: [ { label: "push_top", surface_pressure: { scale_factor: 2307.86806, function: "linear_ramp" }, set: "load_surface", follower: false, quadrature_options: { quadrature: "QP1"} } ]

6.2.1 temperature_distribution (alpha)

Name	Type	Description	Default
scale_factor [optional] (alpha)	DOUBLE	A scalar value which scales the function.	1.0
function (alpha)	STRING	The user defined identifier of the temporal function.

6.2.2 surface_traction (release)

Define a surface traction load

Name	Type	Description	Default
components	[ “x” \| “y” \| “z”, ... ]	Specifies which degrees-of-freedom components are active.
scale_factor [optional]	[ DOUBLE, ... ]	A scalar value or vector of the same length as components which scales the function.	1.0
function	STRING	The user defined identifier of the temporal function.

Example Usage:
surface_traction: { components: [ "x", "y" ], scale_factor: [ 1, 1 ], function: "traction" }

6.2.3 surface_pressure (release)

Define a pressure load, a load which is always normal to the surface

Name	Type	Description	Default
scale_factor [optional]	DOUBLE	A scalar value which scales the function.	1.0
function	STRING	The user defined identifier of the temporal function.

Example Usage:
surface_pressure: { scale_factor: 2307.86806, function: "linear_ramp" }

6.2.4 point_force (release)

Define a point force

Name	Type	Description	Default
components	[ “x” \| “y” \| “z”, ... ]	Specifies which degrees-of-freedom components are active.
scale_factor [optional]	[ DOUBLE, ... ]	A scalar value or vector of the same length as components which scales the function.	1.0
function	STRING	The user defined identifier of the temporal function.

6.2.5 line_traction (release)

Define a point force

Name	Type	Description	Default
components	[ “x” \| “y” \| “z”, ... ]	Specifies which degrees-of-freedom components are active.
scale_factor [optional]	[ DOUBLE, ... ]	A scalar value or vector of the same length as components which scales the function.	1.0
function	STRING	The user defined identifier of the temporal function.

6.2.6 body_force (release)

User must use the ’part’ option when defining sets for a body force

Name	Type	Description	Default
components	[ “x” \| “y” \| “z”, ... ]	Specifies which degrees-of-freedom components are active.
scale_factor [optional]	[ DOUBLE, ... ]	A scalar value or vector of the same length as components which scales the function.	1.0
function	STRING	The user defined identifier of the temporal function.

6.2.7 part | set

Defines the set or part to be operated on

Name	Type	Description	Default
part	STRING	The user defined label of the part that defines the set.
set	STRING	The user defined identifier of the geometric set.

6.2.8 quadrature_options (beta)

Name	Type	Description	Default
quadrature [optional] (beta)	“QP1” \| “QP0” \| “Q1” \| “Q2” \| “Q3” \| “Q4” \| “Q5” \| “Q6” \| “Q7” \| “Q8” \| “Q9” \| “Q10”	Quadrature type enumeration. The quadrature type determines the point layout over a patch or patch element. The schemes following the pattern “Q#” specify that a Gauss quadrature scheme with #-points will be used. The schemes following the pattern “QP#” specify that a Gauss quadrature scheme with $(P+\#)$ -points will be used, where $P$ is the degree of the patch's or patch element's basis.	QP1
optimized_cut_quadrature_strategy [optional] (beta)	“match_uncut” \| “reduce_from_uncut” \| “match_basis”	Strategy to choose the degree of accuracy for quadrature on cut cells. The default strategy of chooses quadrature rules with similar numbers of points as those used on uncut cells, as specified by ; it has lower formal accuracy (integrating tensor products of monomials up to degree $N-1$ for uncut quadrature $N$ ), but is a good default choice for practical calculations. The strategy match_uncut matches the formal accuracy of the quadrature on uncut cells, but is significantly more costly. The strategy match_basis chooses a rule that exactly integrates the basis functions; this is equivalent to reduce_from_uncut if the uncut cells use the default quadrature of QP1, but may differ for other choices of uncut quadrature.	reduce_from_uncut
optimized_cut_quadrature_degree [optional] (beta)	NONNEGATIVE INTEGER	If provided, this value overrides optimized_cut_quadrature_strategy by specifying an explicit polynomial degree of accuracy for optimized quadrature rules on cut cells.
optimization_method [optional] (beta)	“tet_pruning” \| “grid_doubling” \| “linear_programming”	Specifies the preferred method of quadrature generation for cut cells. If the preferred method fails on a particular cell, the other methods will be used in an attempt to recover.	tet_pruning
optimization_residual_tolerance [optional] (beta)	DOUBLE	The absolute residual tolerance used in quadrature optimization on cut cells. A smaller value will result in a more accurate quadrature rule, but may increase the time to compute quadrature rules for cut cells.	1e-12
optimization_lawson_hanson_solve_completion [optional]	true\|false	An experimental option that controls the convergence behavior of quadrature optimization. For best results it is recommended to set this value to true. If set to true this causes each iteration of quadrature optimization to solve to the highest accuracy possible. The results at each iteration are then checked against the optimization_residual_tolerance to determine if a sufficient rule has been found. If this value is set to false then the optimization_residual_tolerance is passed to the solve at each iteration and can cause the solve step to terminate more quickly which can result in faster execution and a lower number of quadrature points. However the quality and accuracy of the resulting rule may be suspect.	true

6.3 initial_conditions (alpha)

An initial condition definition defines a condition of the procedure at its start time.

Name	Type	Description	Default
label (alpha)	STRING	User defined identifier for this initial condition.
velocity (alpha)	SUB OBJECT	See linked documentation
part \| set	STRING \| STRING	Defines the set or part to be operated on

6.3.1 velocity (alpha)

Name	Type	Description	Default
components (alpha)	[ “x” \| “y” \| “z”, ... ]	Specifies which degrees-of-freedom components are active.
scale_factor [optional] (alpha)	[ DOUBLE, ... ]	A scalar value or vector of the same length as components which scales the function.	1.0

6.3.2 part | set

Defines the set or part to be operated on

Name	Type	Description	Default
part	STRING	The user defined label of the part that defines the set.
set	STRING	The user defined identifier of the geometric set.

6.4 outputs (release)

The outputs object holds all output objects, identified by user defined identifiers, each of which define an output for this procedure. If a chosen set was specified as an immersed set during geometry creation, that set must the only item in the sets list. If an immersed set is selected the output command will produce two separate files. The main file will include a tessellated surface representation of the boundary. The second file (with suffix envelope), will include a smooth volumetric output of the U-spline envelope domain for the immersed set. When viewing results on the envelope domain take care that only values on the interior of the model of interest are considered as values at the extremities of this representation may not exhibit physically relevant behavior. Not all elements from the original mesh used may be shown, in general only those that intersect the model of interest will be included.

Name	Type	Description	Default
label	STRING	The user defined identifier for this output definition.
tessellate [optional]	true\|false	The output should be tessellated to hdf5 files for consumption by third party tools.
field (release) \| history (release)	SUB OBJECT \| SUB OBJECT	One of the given keywords must be defined to specify the class of output

Example Usage:
outputs: [ { label: "field_results", field: { database_name: "results", interval: "output_interval", part: "cframe", variables: { displacement: [ "x", "y", "z" ], stress: [ "all" ] }, element_variable_output_strategy: "interpolate", include_integration_point_output: false } }, { label: "probe_results", history: { interval: "output_interval", probe_variables: [ "stress_probe", "load_reaction_force" ] } } ]

6.4.1 field (release)

The field object is primarily useful for visualization and explorative analysis of the results. In addition to the result values, field output exports information needed to construct a visualization of the model.

Name	Type	Description	Default
database_name	STRING	The file name prefix of the output file that will be written to disk. The field output is written out in the ParaView *.pvd format.
interval	STRING	The user defined identifier of the interval to use for this output. This interval will specify when the output should be written, as determined by the time_increment or step_increment values within the interval. A time_increment of 0 acts the same as a step_increment of either 0 or 1, writing output after each intermediate solution step. A negative value for time_increment or step_increment will output only at the bounds of the interval.
part \| set	STRING \| STRING	Defines the set or part to be operated on. If nothing is specified, it is equivalent to including every part.
variables	SUB OBJECT	See linked documentation
element_variable_output_strategy [optional]	“max” \| “min” \| “average” \| “interpolate”	This specifies how values are calculated within each cell. min, max, and average take the minimum, maximum, or average component point values at the integration points and report them across the entire cell. interpolate interpolates the component values from the integration points.	interpolate
include_integration_point_output [optional]	true\|false	Whether to include output at integration points. Output at integration points is not included by default.	false

Example Usage:
field: { database_name: "results", interval: "output_interval", part: "cframe", variables: { displacement: [ "x", "y", "z" ], stress: [ "all" ] }, element_variable_output_strategy: "interpolate", include_integration_point_output: false }

6.4.1.1 part | set

Defines the set or part to be operated on. If nothing is specified, it is equivalent to including every part.

Name	Type	Description	Default
part	STRING	The user defined label of the part that defines the set.
set	STRING	The user defined identifier of the geometric set.

6.4.1.2 variables

The variable to output.

Name		Type		Description		Default
displacement \| velocity (beta) \| acceleration (beta) \| stress \| nominal_strain (beta) \| plastic_strain (beta) \| deformation_gradient (alpha) \| failure_indicator (alpha)		[ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ] \| [ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ] \| [ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ] \| [ “all” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz” \| “von_mises” \| “tresca” \| “pressure” \| “triaxiality” \| “octahedral” \| “total_measure” \| “min_principal” \| “mid_principal” \| “max_principal” \| “invariant_I1” \| “invariant_I2” \| “invariant_I3” \| “invariant_J2” \| “invariant_J3”, ... ] \| [ “all” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz”, ... ] \| [ “equivalent”, ... ] \| [ “all” \| “xx” \| “xy” \| “xz” \| “yx” \| “yy” \| “yz” \| “zx” \| “zy” \| “zz” \| “determinant”, ... ] \| [ “value”, ... ]		Any of the given options can be defined

Example Usage:
variable: { stress: [ "xx", "yy", "zz" ] }

6.4.1.3 displacement | velocity | acceleration | stress | nominal_strain | plastic_strain | deformation_gradient | failure_indicator

Any of the given options can be defined

Name	Type	Description	Default
displacement	[ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ]
velocity (beta)	[ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ]
acceleration (beta)	[ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ]
stress	[ “all” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz” \| “von_mises” \| “tresca” \| “pressure” \| “triaxiality” \| “octahedral” \| “total_measure” \| “min_principal” \| “mid_principal” \| “max_principal” \| “invariant_I1” \| “invariant_I2” \| “invariant_I3” \| “invariant_J2” \| “invariant_J3”, ... ]
nominal_strain (beta)	[ “all” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz”, ... ]
plastic_strain (beta)	[ “equivalent”, ... ]
deformation_gradient (alpha)	[ “all” \| “xx” \| “xy” \| “xz” \| “yx” \| “yy” \| “yz” \| “zx” \| “zy” \| “zz” \| “determinant”, ... ]
failure_indicator (alpha)	[ “value”, ... ]

6.4.2 history (release)

Define a history object to extract time-history data from specific regions of interest. The history object is primarily useful for analysis at known regions of interest (ROI), especially when a high-temporal resolution is required to gain useful information from the results. Field output on the entire domain of the model is often intractable in these situations as writing the entire field at a high sample rate can negatively impact performance, especially when using explicit time-integration, and can quickly generate enormous files that are cumbersome to process. History output writes a minimal set of information at user define probe_variable locations to an HDF5 file format that is easy to process in any number of downstream tools such as Excel, Matlab, or Python.

Name	Type	Description	Default
interval	STRING	The user defined identifier of the interval to use for this output.
probe_variables	[ STRING, ... ]	The user-defined probe_variables that should be included in the output file.

Example Usage:
history: { interval: "output_interval", probe_variables: [ "stress_probe", "load_reaction_force" ] }

6.5 probes (release)

The probes object holds all user defined probe_variables. Probe variables are used to track quantities of interest at specific locations in a model over time. For example, a user may want to track von Mises stress at a specific location in a model over time.

Name	Type	Description	Default
label	STRING	The user defined identifier for this probe definition.
field (release) \| integrated_surface_quantity (release) \| integrated_volume_quantity (beta) \| l2_error_norm (release)	SUB OBJECT \| SUB OBJECT \| SUB OBJECT \| SUB OBJECT	One of the given keywords must be defined to specify the class of probe

Example Usage:
probes: [ { label: "stress_probe", field: { single_point: { location: [ 0, -1.5, -4.25 ] }, location_configuration: "reference", field_variable_configuration: "reference", variables: { stress: [ "max_principal" ] } } }, { label: "load_reaction_force", integrated_surface_quantity: { variables: { reaction_force: [ "x", "y", "z" ] }, part: "cframe", use_set_from_load_condition: "push_top" } } ]

6.5.1 field (release)

Defines a probe that extracts field variable data.

Name	Type	Description	Default
set \| single_point (release) \| along_line (release) \| along_curve (release) \| extremum (release)	STRING \| SUB OBJECT \| SUB OBJECT \| SUB OBJECT \| SUB OBJECT	One of the given keywords must be defined to specify the class of field probe
location_configuration	“reference”	Defines the configuration of the probe location. The reference configuration will track the same material point through time. The current configuration will track the field_variable at a specific spatial location. If no part of the model covers the location when tracking the current configuration then zero values will be returned. Currently, only reference is supported.
field_variable_configuration	“reference”	The configuration of the output coordinate system. Currently, only reference is supported.
variables	SUB OBJECT	See linked documentation

Example Usage:
field: { single_point: { location: [ 0, -1.5, -4.25 ] }, location_configuration: "reference", field_variable_configuration: "reference", variables: { stress: [ "max_principal" ] } }

6.5.1.1 set | single_point | along_line | along_curve | extremum

One of the given keywords must be defined to specify the class of field probe

Name	Type	Description	Default
set	STRING	Specifies the user defined identifier of the set in the Flex model.
single_point (release)	SUB OBJECT	See linked documentation
along_line (release)	SUB OBJECT	See linked documentation
along_curve (release)	SUB OBJECT	See linked documentation
extremum (release)	SUB OBJECT	See linked documentation

6.5.1.2 single_point (release)

Define a probe at a coordinate location

Name		Type		Description		Default
location		[ DOUBLE, DOUBLE, DOUBLE ]		The coordinate location of the probe.

Example Usage:
single_point: { location: [ 0, -1.5, -4.25 ] }

6.5.1.3 along_line (release)

Define a series of probes along a straight line

Name	Type	Description	Default
start_location	[ DOUBLE, DOUBLE, DOUBLE ]	The coordinate location of the first probe.
stop_location	[ DOUBLE, DOUBLE, DOUBLE ]	The coordinate location of the last probe.
num_points	NONNEGATIVE INTEGER	The number of probes between the first and last probe location (minimum 2).

6.5.1.4 along_curve (release)

Define a series of probes at arbitrary coordinate locations

Name		Type		Description		Default
locations		[ [ DOUBLE, ... ], ... ]		The evaluated coordinate locations of all probes along the curve

6.5.1.5 extremum (release)

Name	Type	Description	Default
set [optional]	STRING	Specifies the user defined identifier of the set in the Flex model in which the extremum value is to be found. If not defined then the entire model will be used.
minimum (release) \| maximum (release)	SUB OBJECT \| SUB OBJECT	One of the given keywords must be defined to specify the type of extremum probe

6.5.1.6 minimum (release)

The variable to track for the extremum.

Name		Type		Description		Default
displacement \| velocity (beta) \| acceleration (beta) \| stress \| plastic_strain (beta) \| deformation_gradient (alpha) \| failure_indicator (alpha)		“x” \| “y” \| “z” \| “magnitude” \| “x” \| “y” \| “z” \| “magnitude” \| “x” \| “y” \| “z” \| “magnitude” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz” \| “von_mises” \| “tresca” \| “pressure” \| “triaxiality” \| “octahedral” \| “total_measure” \| “min_principal” \| “mid_principal” \| “max_principal” \| “invariant_I1” \| “invariant_I2” \| “invariant_I3” \| “invariant_J2” \| “invariant_J3” \| “equivalent” \| “xx” \| “xy” \| “xz” \| “yx” \| “yy” \| “yz” \| “zx” \| “zy” \| “zz” \| “determinant” \| “value”		Only one of the given keywords my be defined

6.5.1.7 displacement | velocity | acceleration | stress | plastic_strain | deformation_gradient | failure_indicator

Only one of the given keywords my be defined

Name	Type	Description	Default
displacement	“x” \| “y” \| “z” \| “magnitude”
velocity (beta)	“x” \| “y” \| “z” \| “magnitude”
acceleration (beta)	“x” \| “y” \| “z” \| “magnitude”
stress	“xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz” \| “von_mises” \| “tresca” \| “pressure” \| “triaxiality” \| “octahedral” \| “total_measure” \| “min_principal” \| “mid_principal” \| “max_principal” \| “invariant_I1” \| “invariant_I2” \| “invariant_I3” \| “invariant_J2” \| “invariant_J3”
plastic_strain (beta)	“equivalent”
deformation_gradient (alpha)	“xx” \| “xy” \| “xz” \| “yx” \| “yy” \| “yz” \| “zx” \| “zy” \| “zz” \| “determinant”
failure_indicator (alpha)	“value”

6.5.1.8 maximum (release)

The variable to track for the extremum.

Name		Type		Description		Default
displacement \| velocity (beta) \| acceleration (beta) \| stress \| plastic_strain (beta) \| deformation_gradient (alpha) \| failure_indicator (alpha)		“x” \| “y” \| “z” \| “magnitude” \| “x” \| “y” \| “z” \| “magnitude” \| “x” \| “y” \| “z” \| “magnitude” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz” \| “von_mises” \| “tresca” \| “pressure” \| “triaxiality” \| “octahedral” \| “total_measure” \| “min_principal” \| “mid_principal” \| “max_principal” \| “invariant_I1” \| “invariant_I2” \| “invariant_I3” \| “invariant_J2” \| “invariant_J3” \| “equivalent” \| “xx” \| “xy” \| “xz” \| “yx” \| “yy” \| “yz” \| “zx” \| “zy” \| “zz” \| “determinant” \| “value”		Only one of the given keywords my be defined

6.5.1.9 displacement | velocity | acceleration | stress | plastic_strain | deformation_gradient | failure_indicator

Only one of the given keywords my be defined

Name	Type	Description	Default
displacement	“x” \| “y” \| “z” \| “magnitude”
velocity (beta)	“x” \| “y” \| “z” \| “magnitude”
acceleration (beta)	“x” \| “y” \| “z” \| “magnitude”
stress	“xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz” \| “von_mises” \| “tresca” \| “pressure” \| “triaxiality” \| “octahedral” \| “total_measure” \| “min_principal” \| “mid_principal” \| “max_principal” \| “invariant_I1” \| “invariant_I2” \| “invariant_I3” \| “invariant_J2” \| “invariant_J3”
plastic_strain (beta)	“equivalent”
deformation_gradient (alpha)	“xx” \| “xy” \| “xz” \| “yx” \| “yy” \| “yz” \| “zx” \| “zy” \| “zz” \| “determinant”
failure_indicator (alpha)	“value”

6.5.1.10 variables

The variable to output.

Name		Type		Description		Default
displacement \| velocity (beta) \| acceleration (beta) \| stress \| nominal_strain (beta) \| plastic_strain (beta) \| deformation_gradient (alpha) \| failure_indicator (alpha)		[ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ] \| [ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ] \| [ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ] \| [ “all” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz” \| “von_mises” \| “tresca” \| “pressure” \| “triaxiality” \| “octahedral” \| “total_measure” \| “min_principal” \| “mid_principal” \| “max_principal” \| “invariant_I1” \| “invariant_I2” \| “invariant_I3” \| “invariant_J2” \| “invariant_J3”, ... ] \| [ “all” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz”, ... ] \| [ “equivalent”, ... ] \| [ “all” \| “xx” \| “xy” \| “xz” \| “yx” \| “yy” \| “yz” \| “zx” \| “zy” \| “zz” \| “determinant”, ... ] \| [ “value”, ... ]		Any of the given options can be defined

Example Usage:
variable: { stress: [ "xx", "yy", "zz" ] }

6.5.1.11 displacement | velocity | acceleration | stress | nominal_strain | plastic_strain | deformation_gradient | failure_indicator

Any of the given options can be defined

Name	Type	Description	Default
displacement	[ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ]
velocity (beta)	[ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ]
acceleration (beta)	[ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ]
stress	[ “all” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz” \| “von_mises” \| “tresca” \| “pressure” \| “triaxiality” \| “octahedral” \| “total_measure” \| “min_principal” \| “mid_principal” \| “max_principal” \| “invariant_I1” \| “invariant_I2” \| “invariant_I3” \| “invariant_J2” \| “invariant_J3”, ... ]
nominal_strain (beta)	[ “all” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz”, ... ]
plastic_strain (beta)	[ “equivalent”, ... ]
deformation_gradient (alpha)	[ “all” \| “xx” \| “xy” \| “xz” \| “yx” \| “yy” \| “yz” \| “zx” \| “zy” \| “zz” \| “determinant”, ... ]
failure_indicator (alpha)	[ “value”, ... ]

6.5.2 integrated_surface_quantity (release)

Sum a variable on a specified surface.

Name	Type	Description	Default
variables (release)	SUB OBJECT	See linked documentation
part [optional]	STRING	Specifies the user-defined label of the part in the FRM model in which the surface for integrating is on.
use_set_from_boundary_condition \| use_set_from_load_condition \| use_set_from_interaction (beta)	STRING \| STRING \| STRING	The set for this probe must come from a user defined boundary condition, load condition or interaction.

Example Usage:
integrated_surface_quantity: { variables: { reaction_force: [ "x", "y", "z" ] }, part: "cframe", use_set_from_load_condition: "push_top" }

6.5.2.1 variables (release)

The variables to integrate.

Name		Type		Description		Default
reaction_force		[ “x” \| “y” \| “z” \| “magnitude”, ... ]		Definitions of the type of variables to integrate.

Example Usage:
variables: { reaction_force: [ "x", "y", "z" ] }

6.5.2.2 reaction_force

Definitions of the type of variables to integrate.

Name		Type		Description		Default
reaction_force		[ “x” \| “y” \| “z” \| “magnitude”, ... ]

6.5.2.3 use_set_from_boundary_condition | use_set_from_load_condition | use_set_from_interaction

The set for this probe must come from a user defined boundary condition, load condition or interaction.

Name	Type	Description	Default
use_set_from_boundary_condition	STRING	Specifies the set used in the boundary condition with this user-defined label. Used to get reaction forces associated with boundary conditions.
use_set_from_load_condition	STRING	Specifies the set used in the load condition with this user-defined label. Used to get net forces from load conditions.
use_set_from_interaction (beta)	STRING	Specifies the set used in the interaction with this user-defined label. Used to get contact reaction forces.

6.5.3 integrated_volume_quantity (beta)

Sum a variable on a specified volume.

Name	Type	Description	Default
variables (beta)	SUB OBJECT	See linked documentation
part [optional] (beta)	STRING	Specifies the part with this user-defined label. If not defined, all the parts are selected.

6.5.3.1 variables (beta)

The variables to integrate.

Name		Type		Description		Default
momentum (beta) \| energy (alpha)		[ “x” \| “y” \| “z” \| “magnitude”, ... ] \| [ “plastic_work”, ... ]		Definitions of the type of variable to integrate

6.5.3.2 momentum | energy

Definitions of the type of variable to integrate

Name	Type	Description	Default
momentum (beta)	[ “x” \| “y” \| “z” \| “magnitude”, ... ]
energy (alpha)	[ “plastic_work”, ... ]	Specifies the type of energy to integrate. Currently, only the plastic work is available for neo-Hookean isotropic plasticity. The plastic work is define as $\int_{t_0}^{t} \dot{\mathbf{\varepsilon}^p}:\mathbf{\sigma} d{\tau}$ , where $\dot{\mathbf{\varepsilon}^p}$ and $\mathbf{\sigma}$ denote the plastic strain rate and Cauchy stress, respectively.

6.5.4 l2_error_norm (release)

Calculate an L2 error norm, over a given set, between the computed solution and a user-provided solution. The error is calculated from the difference between a given user function and the computed values for stress or displacement components. The error is defined as the square root of the sum of the squares of the given components.

Name	Type	Description	Default
part \| set	STRING \| STRING	Defines the set or part to be operated on
function	STRING	The user defined identifier of the function to use for this error calculation. The function should return the reference values that the solution will be compared with in an array ordered to match the provided components of displacement or stress.
variable	SUB OBJECT	See linked documentation

Example Usage:
l2_error_norm: { part: "plate_with_hole", function: "stress", variable: { stress: [ "xx", "yy", "zz" ] } }

6.5.4.1 part | set

Defines the set or part to be operated on

Name	Type	Description	Default
part	STRING	The user defined label of the part that defines the set.
set	STRING	The user defined identifier of the geometric set.

6.5.4.2 variable

The variable to output.

Name		Type		Description		Default
displacement \| velocity (beta) \| acceleration (beta) \| stress \| nominal_strain (beta) \| plastic_strain (beta) \| deformation_gradient (alpha) \| failure_indicator (alpha)		[ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ] \| [ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ] \| [ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ] \| [ “all” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz” \| “von_mises” \| “tresca” \| “pressure” \| “triaxiality” \| “octahedral” \| “total_measure” \| “min_principal” \| “mid_principal” \| “max_principal” \| “invariant_I1” \| “invariant_I2” \| “invariant_I3” \| “invariant_J2” \| “invariant_J3”, ... ] \| [ “all” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz”, ... ] \| [ “equivalent”, ... ] \| [ “all” \| “xx” \| “xy” \| “xz” \| “yx” \| “yy” \| “yz” \| “zx” \| “zy” \| “zz” \| “determinant”, ... ] \| [ “value”, ... ]		Only one of the given keywords my be defined

Example Usage:
variable: { stress: [ "xx", "yy", "zz" ] }

6.5.4.3 displacement | velocity | acceleration | stress | nominal_strain | plastic_strain | deformation_gradient | failure_indicator

Only one of the given keywords my be defined

Name	Type	Description	Default
displacement	[ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ]
velocity (beta)	[ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ]
acceleration (beta)	[ “all” \| “x” \| “y” \| “z” \| “magnitude”, ... ]
stress	[ “all” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz” \| “von_mises” \| “tresca” \| “pressure” \| “triaxiality” \| “octahedral” \| “total_measure” \| “min_principal” \| “mid_principal” \| “max_principal” \| “invariant_I1” \| “invariant_I2” \| “invariant_I3” \| “invariant_J2” \| “invariant_J3”, ... ]
nominal_strain (beta)	[ “all” \| “xx” \| “yy” \| “zz” \| “xy” \| “yz” \| “xz”, ... ]
plastic_strain (beta)	[ “equivalent”, ... ]
deformation_gradient (alpha)	[ “all” \| “xx” \| “xy” \| “xz” \| “yx” \| “yy” \| “yz” \| “zx” \| “zy” \| “zz” \| “determinant”, ... ]
failure_indicator (alpha)	[ “value”, ... ]

6.6 interactions (release)

Each object in the interaction definitions array defines an interaction for the procedure. Currently the supported interactions are mechanical_contact and tied_constraint.

Name	Type	Description	Default
label	STRING	User defined identifier for this interaction definition.
quadrature_options (beta) [optional]	SUB OBJECT	See linked documentation
tied_constraint (release) \| material_interface (release) \| mechanical_contact (beta) \| interference_fit (beta) \| rotational_constraint (alpha)	SUB OBJECT \| SUB OBJECT \| SUB OBJECT \| SUB OBJECT \| SUB OBJECT	One of the given keywords must be defined to specify the type of interaction

Example Usage:
interactions: [ { label: "all_interfaces", quadrature_options: { quadrature: "QP1"}, material_interface: { interface: "all_interfaces", penalty: {value: 28000000000, dimensionless: false} } } ]

6.6.1 quadrature_options (beta)

Name	Type	Description	Default
quadrature [optional] (beta)	“QP1” \| “QP0” \| “Q1” \| “Q2” \| “Q3” \| “Q4” \| “Q5” \| “Q6” \| “Q7” \| “Q8” \| “Q9” \| “Q10”	Quadrature type enumeration. The quadrature type determines the point layout over a patch or patch element. The schemes following the pattern “Q#” specify that a Gauss quadrature scheme with #-points will be used. The schemes following the pattern “QP#” specify that a Gauss quadrature scheme with $(P+\#)$ -points will be used, where $P$ is the degree of the patch's or patch element's basis.	QP1
optimized_cut_quadrature_strategy [optional] (beta)	“match_uncut” \| “reduce_from_uncut” \| “match_basis”	Strategy to choose the degree of accuracy for quadrature on cut cells. The default strategy of chooses quadrature rules with similar numbers of points as those used on uncut cells, as specified by ; it has lower formal accuracy (integrating tensor products of monomials up to degree $N-1$ for uncut quadrature $N$ ), but is a good default choice for practical calculations. The strategy match_uncut matches the formal accuracy of the quadrature on uncut cells, but is significantly more costly. The strategy match_basis chooses a rule that exactly integrates the basis functions; this is equivalent to reduce_from_uncut if the uncut cells use the default quadrature of QP1, but may differ for other choices of uncut quadrature.	reduce_from_uncut
optimized_cut_quadrature_degree [optional] (beta)	NONNEGATIVE INTEGER	If provided, this value overrides optimized_cut_quadrature_strategy by specifying an explicit polynomial degree of accuracy for optimized quadrature rules on cut cells.
optimization_method [optional] (beta)	“tet_pruning” \| “grid_doubling” \| “linear_programming”	Specifies the preferred method of quadrature generation for cut cells. If the preferred method fails on a particular cell, the other methods will be used in an attempt to recover.	tet_pruning
optimization_residual_tolerance [optional] (beta)	DOUBLE	The absolute residual tolerance used in quadrature optimization on cut cells. A smaller value will result in a more accurate quadrature rule, but may increase the time to compute quadrature rules for cut cells.	1e-12
optimization_lawson_hanson_solve_completion [optional]	true\|false	An experimental option that controls the convergence behavior of quadrature optimization. For best results it is recommended to set this value to true. If set to true this causes each iteration of quadrature optimization to solve to the highest accuracy possible. The results at each iteration are then checked against the optimization_residual_tolerance to determine if a sufficient rule has been found. If this value is set to false then the optimization_residual_tolerance is passed to the solve at each iteration and can cause the solve step to terminate more quickly which can result in faster execution and a lower number of quadrature points. However the quality and accuracy of the resulting rule may be suspect.	true

6.6.2 tied_constraint (release)

Defines interaction properties for a surface to surface tied constraint.

Name	Type	Description	Default
target_set	STRING	Specifies the target interaction surface.
source_set	STRING	Specifies the source interaction surface.
region_search_method	STRING	Specifies the object in interaction-search-parameters to define the constraint search method.
penalty (beta) [optional]	SUB OBJECT	See linked documentation
offset [optional]	true\|false	A tied constraint property that, if true, will use a formulation that approximately maintains the initial gap distance. If false, the tied constraint formulation will not maintain gap distances under rotation, but is less expensive to compute.	true

6.6.2.1 penalty (beta)

Options for penalty enforcement of a boundary condition or other type of constraint. When penalty values are calculated from a dimensionless scale using material properties and element size on two sides of a material or contact interface, the smaller of the two values is selected.

Name	Type	Description	Default
value (beta)	DOUBLE	The value of the penalty parameter, in the range $[0,\infty)$ , determining how strongly the constraint is enforced. The precise interpretation of this value depends on the choice of the parameter dimensionless, whose documentation provides a more detailed discussion. Note that the default value assumes that dimensionless is also set to its default value of true.	1e1
dimensionless (beta)	true\|false	If this parameter is true, then the penalty value is interpreted as the dimensionless constant $C$ in the formula $\beta = CEh^{c-2}$ , where $E$ is a scalar estimate of the material stiffness (i.e., the Young's modulus in elasticity or the thermal conductivity in heat conduction), $h$ is a measure of element size (with units of length), and $c$ is the co-dimension of the constrained set, i.e., 0 for volumes, 1 for surfaces, 2 for curves, or 3 for points. If this parameter is false, then the penalty value is instead interpreted as the dimensional value of $\beta$ directly. The dimensionless option is recommended for most use cases. To interpret the dimensionless penalty value for the common case of constrained boundaries and interfaces ( $c=1$ ) in elasticity, it is roughly the ratio of a single element's change in length under a given tensile load to the error allowed in the consraint. Note that, for any positive value, the constraint error will go to zero as the mesh is refined, since the specimen's overall change in length is distributed over more elements. Selecting too large of a penalty value makes the discrete problem harder to solve. The default value represents a good balance between accuracy and efficiency for most practical applications, but higher values may be appropriate for certain situations, such as calibrating material models with single-element patch tests.	true

6.6.3 material_interface (release)

Name	Type	Description	Default
interface	STRING	The label of the interaction in the geometry/interactions array.
penalty (beta) [optional]	SUB OBJECT	See linked documentation
region_search_method [optional] (beta)	STRING	The search paramaters to use.
offset [optional] (beta)	true\|false	A material interface property that, if true, will use a formulation that approximately maintains any initial gap due to a small geometric mismatch at the material interface. If false, the tied constraint formulation may be less robust to geometry error, but is less expensive to compute.	true

Example Usage:
material_interface: { interface: "all_interfaces", penalty: {value: 28000000000, dimensionless: false} }

6.6.3.1 penalty (beta)

Options for penalty enforcement of a boundary condition or other type of constraint. When penalty values are calculated from a dimensionless scale using material properties and element size on two sides of a material or contact interface, the smaller of the two values is selected.

Name	Type	Description	Default
value (beta)	DOUBLE	The value of the penalty parameter, in the range $[0,\infty)$ , determining how strongly the constraint is enforced. The precise interpretation of this value depends on the choice of the parameter dimensionless, whose documentation provides a more detailed discussion. Note that the default value assumes that dimensionless is also set to its default value of true.	1e1
dimensionless (beta)	true\|false	If this parameter is true, then the penalty value is interpreted as the dimensionless constant $C$ in the formula $\beta = CEh^{c-2}$ , where $E$ is a scalar estimate of the material stiffness (i.e., the Young's modulus in elasticity or the thermal conductivity in heat conduction), $h$ is a measure of element size (with units of length), and $c$ is the co-dimension of the constrained set, i.e., 0 for volumes, 1 for surfaces, 2 for curves, or 3 for points. If this parameter is false, then the penalty value is instead interpreted as the dimensional value of $\beta$ directly. The dimensionless option is recommended for most use cases. To interpret the dimensionless penalty value for the common case of constrained boundaries and interfaces ( $c=1$ ) in elasticity, it is roughly the ratio of a single element's change in length under a given tensile load to the error allowed in the consraint. Note that, for any positive value, the constraint error will go to zero as the mesh is refined, since the specimen's overall change in length is distributed over more elements. Selecting too large of a penalty value makes the discrete problem harder to solve. The default value represents a good balance between accuracy and efficiency for most practical applications, but higher values may be appropriate for certain situations, such as calibrating material models with single-element patch tests.	true

6.6.4 mechanical_contact (beta)

A physics based contact between two surfaces (paired) or in a single surface (self).

Name	Type	Description	Default
base_contact (beta) \| sets (beta)	SUB OBJECT \| [ STRING, ... ]
interaction_properties [optional] (beta)	STRING	The name of the user defined interaction property to use for this interaction.
unintentional_overclosures (beta) [optional]	SUB OBJECT	See linked documentation
activation_distance (beta) [optional]	SUB OBJECT	See linked documentation
penalty (beta) [optional]	SUB OBJECT	See linked documentation
tessellation_subdivision_count [optional] (beta)	NONNEGATIVE INTEGER	An integration cell is subdivided by the maximum of this value and the degree of spline. When aiming to achieve better accuracy in contact, it is recommended to consider increasing this value. However, the larger the value, the greater the memory usage and the slower the computation. Therefore, it is generally recommended that this value not exceed 4.	2
effective_distance_smoothing (beta) [optional]	SUB OBJECT	See linked documentation
collision_search_filter (beta) [optional]	SUB OBJECT	See linked documentation
contact_force_scaling (beta) [optional]	SUB OBJECT	See linked documentation

6.6.4.1 base_contact | sets

Name	Type	Description	Default
base_contact (beta)	SUB OBJECT	See linked documentation
sets (beta)	[ STRING, ... ]	Specifies the interaction part, volume or surface sets that will participate in surface to surface contact. Will overrides the base_contact interaction.

6.6.4.2 base_contact (beta)

Specifies the general contact interactions. Any base interaction is overriden by any other set interactions. Only one interaction of this type should be defined.

Name	Type	Description	Default
sets [optional] (beta)	[ STRING, ... ]	Specifies the part, volume, or surface sets to be included in general contact interactions.
complement (beta)	true\|false	Takes the complement of the sets of the part, volume, or surface sets specified by base_contact so they are excluded from base contact interactions.	false

6.6.4.3 unintentional_overclosures (beta)

Name		Type		Description		Default
offset (beta)		SUB OBJECT

6.6.4.4 offset (beta)

Name		Type		Description		Default
distance (beta)		DOUBLE

6.6.4.5 distance

Name		Type		Description		Default
distance (beta)		DOUBLE		The signed effective distance is offset by this value in a unit of length. It is recommended to consider increasing this value when unintentional initial overclosures produce nonnegligible stress, leading to difficulty in the initial nonlinear convergence. This value should not exceed half of the activation distance.

6.6.4.6 activation_distance (beta)

Specifies the distance within which to search for contacting points. When it is observed that some contact surfaces lose interaction, a larger-than-default value may be required.

Name	Type	Description	Default
value (beta)	DOUBLE	Specifies the distance within which to search for contacting points. Larger values are more robust, but also potentially more expensive. The precise interpretation of this depends on the value of dimensionless, with more detail given in its documentation. Note that the default value assumes that dimensionless is also set to its default value of true.	0.5
dimensionless (beta)	true\|false	If this is set to true, then value is understood as a dimensionless fraction of the element size. If it is set to false, then value is interpreted as a length scale, and must be selected in a way that is consistent with the length units used elsewhere. When manually specifying an activation distance, it is recommended to keep it on the same order as element size, as reflected in the default dimensionless value.	true

6.6.4.7 penalty (beta)

Options for penalty enforcement of a boundary condition or other type of constraint. When penalty values are calculated from a dimensionless scale using material properties and element size on two sides of a material or contact interface, the smaller of the two values is selected.

Name	Type	Description	Default
value (beta)	DOUBLE	The value of the penalty parameter, in the range $[0,\infty)$ , determining how strongly the constraint is enforced. The precise interpretation of this value depends on the choice of the parameter dimensionless, whose documentation provides a more detailed discussion. Note that the default value assumes that dimensionless is also set to its default value of true.	1e1
dimensionless (beta)	true\|false	If this parameter is true, then the penalty value is interpreted as the dimensionless constant $C$ in the formula $\beta = CEh^{c-2}$ , where $E$ is a scalar estimate of the material stiffness (i.e., the Young's modulus in elasticity or the thermal conductivity in heat conduction), $h$ is a measure of element size (with units of length), and $c$ is the co-dimension of the constrained set, i.e., 0 for volumes, 1 for surfaces, 2 for curves, or 3 for points. If this parameter is false, then the penalty value is instead interpreted as the dimensional value of $\beta$ directly. The dimensionless option is recommended for most use cases. To interpret the dimensionless penalty value for the common case of constrained boundaries and interfaces ( $c=1$ ) in elasticity, it is roughly the ratio of a single element's change in length under a given tensile load to the error allowed in the consraint. Note that, for any positive value, the constraint error will go to zero as the mesh is refined, since the specimen's overall change in length is distributed over more elements. Selecting too large of a penalty value makes the discrete problem harder to solve. The default value represents a good balance between accuracy and efficiency for most practical applications, but higher values may be appropriate for certain situations, such as calibrating material models with single-element patch tests.	true

6.6.4.8 effective_distance_smoothing (beta)

Name	Type	Description	Default
distance_smoothing_factor (beta)	DOUBLE	Specifies a fraction of the user-specified activation distance. The discontinuity in the effective signed distance gradients at a distance of zero is regularized over an interval equal to the activation distance multiplied by this factor. While this option aids in nonlinear convergence, it allows more penetration because the effective contact stiffness becomes smaller near the effective distance of zero. When less penetration is desired, it is suggested to reduce this value. When experiencing difficulty in achieving nonlinear convergence, it is suggested to try increasing this value. It is generally not recommended for this value to exceed 1.0.	0.25
edge_smoothing_factor [optional] (beta)	DOUBLE	Specifies a fraction of the user-specified activation distance. The discontinuities in the effective signed distance gradients around the edges of the contact surface integration cells are regularized over an interval equal to the activation distance multiplied by this factor. While this option facilitates easier nonlinear convergence, it can increase unintentional overclosures. Therefore, it is recommended to use this option with caution, particularly when bodies are initially touching each other.
corner_smoothing [optional] (beta)	true\|false	The signed effective distance is additionally smoothed around the vertices of the contact surface integration cells. While this option facilitates easier nonlinear convergence, it can increase unintentional overclosures. Therefore, it is recommended to use this option with caution, particularly when bodies are initially touching each other.

6.6.4.9 collision_search_filter (beta)

Name	Type	Description	Default
angle_filter (beta) [optional]	SUB OBJECT	See linked documentation
area_filter (beta) [optional]	SUB OBJECT	See linked documentation
spurious_self_contact_filter (beta) [optional]	SUB OBJECT	See linked documentation

6.6.4.10 angle_filter (beta)

Name		Type		Description		Default
threshold_angle (beta)		DOUBLE		In order to improve performance for continuation/implicit dynamics, A pair of triangles will be removed from the collision candidate set if the angle between their surface normals is under this threshold that, in degrees, ranges from 0 to 90, with a recommended value of approximately 30 degrees. This option is automatically turned off for explicit dynamics.		30

6.6.4.11 area_filter (beta)

Name		Type		Description		Default
threshold_area_ratio (beta)		DOUBLE		In order to improve performance for continuation/implicit dynamics by avoiding an excessive amount of collision candidates when solution is diverging, the collision search will be skipped if the ratio of the surface triangle's current area to its area at the last successful time step exceeds this value. This option is automatically turned off for explicit dynamics.		2

6.6.4.12 spurious_self_contact_filter (beta)

Name		Type		Description		Default
use (beta)		true\|false		If true, will not consider the interaction between integration cells from the same body when they are initially penetrate each other to avoid spurious self-contact. When this option is turned on, intentional self-overclosures cannot be applied.		true

6.6.4.13 contact_force_scaling (beta)

Name		Type		Description		Default
closest_point_penetration_based (beta)		SUB OBJECT

6.6.4.14 closest_point_penetration_based (beta)

The contact force is adjusted using a multiplicative scaling factor, which is a function of the penetration depth from the closest point on a contact surface. This adjustment helps avoid the development of spurious contact forces under certain geometry.

Name		Type		Description		Default
regularization_factor (beta)		DOUBLE		Specifies a fraction of the user-specified activation distance. The scaling factor is zero at the contact surface and ramps up to one over the interval of the activation distance multiplied by this value. This option allows more penetration because the effective contact stiffness becomes smaller near the effective distance of zero. It is recommended to use a value between 0.05 and 0.1 to avoid excessive penetration.

6.6.5 interference_fit (beta)

A physics based contact between two surfaces (paired) or in a single surface (self).

Name	Type	Description	Default
sets	[ STRING, ... ]	Specifies the interaction part, volume or surface sets that will participate in surface to surface interference fit. Will overrides the base_contact interaction defined in mechanical_contact.
interaction_properties [optional]	STRING	The name of the user defined interaction property to use for this interaction.
activation_distance (beta) [optional]	SUB OBJECT	See linked documentation
penalty (beta) [optional]	SUB OBJECT	See linked documentation
initial_activation_distance	DOUBLE	Specifies the initial activation distance for interference fit resolution. The initial activation distance should be large enough for the contact surfaces can see each other with an initially large overclosure. It is suggested that this value be chosen 2 to 4 times larger than the maximum overclosure initially present. The activation distance is then linearly ramped down to within with a ramp function $a(t) = a_0 + \frac{t}{t_r}(a - a_0)$ where $a(t)$ , $a_0$ , $a$ , and $t_r$ denote the activation distance at time $t$ , initial_activation_distance, activation_distance, and ramp_time_interval. If this value is smaller than the activation_distance, it will be set to activation_distance.
initial_penalty_ratio [optional]	DOUBLE	Specifies the ratio of the penalty to . This value should be small enough compared to to ensure nonlinear convergence, especially with large initial overclosure. The penalty value is exponentially ramped up to within with a ramp function $\frac{\kappa (t)}{\kappa} = r^{1 - t/t_r}$ where $\kappa(t)$ , $\kappa$ , $r$ , and $t_r$ denote the penalty value at time $t$ , penalty, initial_penalty_ratio, and ramp_time_interval. If the nonlinear calculation diverges, it is recommended to lower this value. If the solution converges but the interaction is lost during the simulation, it is recommended to increase this value.	1e-5
ramp_time_interval	DOUBLE	The activation distance and the contact stiffness are ramped over this time interval. If you set initial_penalty_ratio to a fairly small number but still experience nonlinear divergence, it may be due to the ramping occurring over too few time steps. In that case, it is recommended to either increase the ramp_time_interval or ensure there are at least 5 time steps within this interval.
tessellation_subdivision_count [optional]	NONNEGATIVE INTEGER	An integration cell is subdivided by the maximum of this value and the degree of spline.	2
effective_distance_smoothing (beta) [optional]	SUB OBJECT	See linked documentation
collision_search_filter (beta) [optional]	SUB OBJECT	See linked documentation
contact_force_scaling (beta) [optional]	SUB OBJECT	See linked documentation

6.6.5.1 activation_distance (beta)

Specifies the distance within which to search for contacting points. When it is observed that some contact surfaces lose interaction, a larger-than-default value may be required.

Name	Type	Description	Default
value [optional] (beta)	DOUBLE	Specifies the distance within which to search for contacting points. Larger values are more robust, but also potentially more expensive. The precise interpretation of this depends on the value of dimensionless, with more detail given in its documentation. Note that the default value assumes that dimensionless is also set to its default value of true.	0.5
dimensionless [optional] (beta)	true\|false	If this is set to true, then value is understood as a dimensionless fraction of the element size. If it is set to false, then value is interpreted as a length scale, and must be selected in a way that is consistent with the length units used elsewhere. When manually specifying an activation distance, it is recommended to keep it on the same order as element size, as reflected in the default dimensionless value.	true

6.6.5.2 penalty (beta)

Options for penalty enforcement of a boundary condition or other type of constraint. When penalty values are calculated from a dimensionless scale using material properties and element size on two sides of a material or contact interface, the smaller of the two values is selected.

Name	Type	Description	Default
value (beta)	DOUBLE	The value of the penalty parameter, in the range $[0,\infty)$ , determining how strongly the constraint is enforced. The precise interpretation of this value depends on the choice of the parameter dimensionless, whose documentation provides a more detailed discussion. Note that the default value assumes that dimensionless is also set to its default value of true.	1e1
dimensionless (beta)	true\|false	If this parameter is true, then the penalty value is interpreted as the dimensionless constant $C$ in the formula $\beta = CEh^{c-2}$ , where $E$ is a scalar estimate of the material stiffness (i.e., the Young's modulus in elasticity or the thermal conductivity in heat conduction), $h$ is a measure of element size (with units of length), and $c$ is the co-dimension of the constrained set, i.e., 0 for volumes, 1 for surfaces, 2 for curves, or 3 for points. If this parameter is false, then the penalty value is instead interpreted as the dimensional value of $\beta$ directly. The dimensionless option is recommended for most use cases. To interpret the dimensionless penalty value for the common case of constrained boundaries and interfaces ( $c=1$ ) in elasticity, it is roughly the ratio of a single element's change in length under a given tensile load to the error allowed in the consraint. Note that, for any positive value, the constraint error will go to zero as the mesh is refined, since the specimen's overall change in length is distributed over more elements. Selecting too large of a penalty value makes the discrete problem harder to solve. The default value represents a good balance between accuracy and efficiency for most practical applications, but higher values may be appropriate for certain situations, such as calibrating material models with single-element patch tests.	true

6.6.5.3 effective_distance_smoothing (beta)

Name	Type	Description	Default
distance_smoothing_factor (beta)	DOUBLE	Specifies a fraction of the user-specified activation distance. The discontinuity in the effective signed distance gradients at a distance of zero is regularized over an interval equal to the activation distance multiplied by this factor. While this option aids in nonlinear convergence, it allows more penetration because the effective contact stiffness becomes smaller near the effective distance of zero. When less penetration is desired, it is suggested to reduce this value. When experiencing difficulty in achieving nonlinear convergence, it is suggested to try increasing this value. It is generally not recommended for this value to exceed 1.0.	0.25
edge_smoothing_factor [optional] (beta)	DOUBLE	Specifies a fraction of the user-specified activation distance. The discontinuities in the effective signed distance gradients around the edges of the contact surface integration cells are regularized over an interval equal to the activation distance multiplied by this factor. While this option facilitates easier nonlinear convergence, it can increase unintentional overclosures. Therefore, it is recommended to use this option with caution, particularly when bodies are initially touching each other.
corner_smoothing [optional] (beta)	true\|false	The signed effective distance is additionally smoothed around the vertices of the contact surface integration cells. While this option facilitates easier nonlinear convergence, it can increase unintentional overclosures. Therefore, it is recommended to use this option with caution, particularly when bodies are initially touching each other.

6.6.5.4 collision_search_filter (beta)

Name	Type	Description	Default
angle_filter (beta) [optional]	SUB OBJECT	See linked documentation
area_filter (beta) [optional]	SUB OBJECT	See linked documentation
spurious_self_contact_filter (beta) [optional]	SUB OBJECT	See linked documentation

6.6.5.5 angle_filter (beta)

Name		Type		Description		Default
threshold_angle (beta)		DOUBLE		In order to improve performance for continuation/implicit dynamics, A pair of triangles will be removed from the collision candidate set if the angle between their surface normals is under this threshold that, in degrees, ranges from 0 to 90, with a recommended value of approximately 30 degrees. This option is automatically turned off for explicit dynamics.		30

6.6.5.6 area_filter (beta)

Name		Type		Description		Default
threshold_area_ratio (beta)		DOUBLE		In order to improve performance for continuation/implicit dynamics by avoiding an excessive amount of collision candidates when solution is diverging, the collision search will be skipped if the ratio of the surface triangle's current area to its area at the last successful time step exceeds this value. This option is automatically turned off for explicit dynamics.		2

6.6.5.7 spurious_self_contact_filter (beta)

Name		Type		Description		Default
use (beta)		true\|false		If true, will not consider the interaction between integration cells from the same body when they are initially penetrate each other to avoid spurious self-contact. When this option is turned on, intentional self-overclosures cannot be applied.		true

6.6.5.8 contact_force_scaling (beta)

Name		Type		Description		Default
closest_point_penetration_based (beta)		SUB OBJECT

6.6.5.9 closest_point_penetration_based (beta)

The contact force is adjusted using a multiplicative scaling factor, which is a function of the penetration depth from the closest point on a contact surface. This adjustment helps avoid the development of spurious contact forces under certain geometry.

Name		Type		Description		Default
regularization_factor (beta)		DOUBLE		Specifies a fraction of the user-specified activation distance. The scaling factor is zero at the contact surface and ramps up to one over the interval of the activation distance multiplied by this value. This option allows more penetration because the effective contact stiffness becomes smaller near the effective distance of zero. It is recommended to use a value between 0.05 and 0.1 to avoid excessive penetration.

6.6.6 rotational_constraint (alpha)

Name	Type	Description	Default
penalty (beta) [optional]	SUB OBJECT	See linked documentation
reference_axis_origin (alpha)	[ DOUBLE, ... ]
axis_orientation (alpha)	[ DOUBLE, ... ]
axis_origin_displacement (alpha)	SUB OBJECT	See linked documentation
part \| set	STRING \| STRING	Defines the set or part to be operated on

6.6.6.1 penalty (beta)

Options for penalty enforcement of a boundary condition or other type of constraint. When penalty values are calculated from a dimensionless scale using material properties and element size on two sides of a material or contact interface, the smaller of the two values is selected.

Name	Type	Description	Default
value (beta)	DOUBLE	The value of the penalty parameter, in the range $[0,\infty)$ , determining how strongly the constraint is enforced. The precise interpretation of this value depends on the choice of the parameter dimensionless, whose documentation provides a more detailed discussion. Note that the default value assumes that dimensionless is also set to its default value of true.	1e1
dimensionless (beta)	true\|false	If this parameter is true, then the penalty value is interpreted as the dimensionless constant $C$ in the formula $\beta = CEh^{c-2}$ , where $E$ is a scalar estimate of the material stiffness (i.e., the Young's modulus in elasticity or the thermal conductivity in heat conduction), $h$ is a measure of element size (with units of length), and $c$ is the co-dimension of the constrained set, i.e., 0 for volumes, 1 for surfaces, 2 for curves, or 3 for points. If this parameter is false, then the penalty value is instead interpreted as the dimensional value of $\beta$ directly. The dimensionless option is recommended for most use cases. To interpret the dimensionless penalty value for the common case of constrained boundaries and interfaces ( $c=1$ ) in elasticity, it is roughly the ratio of a single element's change in length under a given tensile load to the error allowed in the consraint. Note that, for any positive value, the constraint error will go to zero as the mesh is refined, since the specimen's overall change in length is distributed over more elements. Selecting too large of a penalty value makes the discrete problem harder to solve. The default value represents a good balance between accuracy and efficiency for most practical applications, but higher values may be appropriate for certain situations, such as calibrating material models with single-element patch tests.	true

6.6.6.2 axis_origin_displacement (alpha)

Name	Type	Description	Default
components (alpha)	[ “x” \| “y” \| “z”, ... ]	Specifies which degrees-of-freedom components are active.
scale_factor [optional] (alpha)	[ DOUBLE, ... ]	A scalar value or vector of the same length as components which scales the function.	1.0
function (alpha)	STRING	The user defined identifier of the temporal function.

6.6.6.3 part | set

Defines the set or part to be operated on

Name	Type	Description	Default
part	STRING	The user defined label of the part that defines the set.
set	STRING	The user defined identifier of the geometric set.

6.7 interaction_search_parameters (beta)

Each object in the interaction search definitions array defines search parameters to be used in an interaction. Currently the supported search definitions is a sensor-based layout.

Name	Type	Description	Default
label (beta)	STRING	User defined identifier for this interaction search definition.
sensor_based (beta)	SUB OBJECT	See linked documentation

6.7.1 sensor_based (beta)

Defines properties for sensor-based interaction search method. The layout of sensors is determined by the quadrature rule specified in the material interface or tied constraint using these search parameters. For each sensor (quadrature point) on the source surface, the nearest point is found on the target surface using the given parameters.

Name	Type	Description	Default
max_iterations (beta)	NONNEGATIVE INTEGER	Specifies the maximum iterations for the search.	10
relative_tolerance (beta)	DOUBLE	Specifies the relative search tolerance.	1e-8
bounding_box_extension (beta)	DOUBLE	Specifies the extension of the bounding box for the interaction search.	1e-3

6.8 interaction_properties (beta)

The interaction property definition allows the user to define the type of friction and movement that occurs once contact is initiated.

Name	Type	Description	Default
label (beta)	STRING	The user defined identifier for this interaction property definition.
frictionless (beta) \| coulomb_friction (beta)	SUB OBJECT \| SUB OBJECT	One of the given keywords must be defined to specify the class of interaction property

6.8.1 frictionless (beta)

A tangential interaction property, signifying no friction will be enforced. This object has no input variables.

Name

Type

Description

Default

6.8.2 coulomb_friction (beta)

A tangential interaction occurs, governed by the coulomb friction.

Name		Type		Description		Default
coefficient_with_regularization (beta)		SUB OBJECT		Defines how the friction is described.

6.8.2.1 coefficient_with_regularization (beta)

A constant friction coefficient is applied with regularization.

Name	Type	Description	Default
friction_coefficient (beta)	DOUBLE	Friction coefficient.
regularization_velocity (beta)	DOUBLE	The friction_coefficient is multiplied by a regularization factor. The regularization factor is zero when the tangential velocity is zero. It monotomically increases and reaches to one when the magnitude of the tangential velocity becomes regularization_velocity. regularization_velocity can be interpreted as the maximum slip velocity allowed during what should nominally be static friction.

contents ← prev up next →

1	An Overview of Coreform IGA
2	General Terminology
3	iga
4	procedures (release)
5	flex_ models (release)
6	solid_ mechanics_ definitions (release)
7	heat_ transfer_ definitions (alpha)
8	structural_ modal_ analysis_ definitions (alpha)
9	materials (release)
10	time_ steppers (release)
11	nonlinear_ equation_ solvers (beta)
12	linear_ equation_ solvers (release)
13	functions (release)
14	intervals (release)

6.1	boundary_ conditions (release)
6.2	load_ conditions (release)
6.3	initial_ conditions (alpha)
6.4	outputs (release)
6.5	probes (release)
6.6	interactions (release)
6.7	interaction_ search_ parameters (beta)
6.8	interaction_ properties (beta)