Represents a datum axis feature builder. More...

Inheritance diagram for NXOpen.Features.DatumAxisBuilder:

Public Types
enum	AlternateSolution { Undefined, Tangent, Normal, Binormal, OppositeTangent, OppositeNormal, OppositeBinormal, Project }
	Specifies the alternate solution for datum axis using point on curve method only More...

enum	ConstraintType { Undefined, Coincident, Parallel, Perpendicular, Center, Tangent, Distance, Angle, Frenet }
	Specifies different constraint types for selected geometries More...

enum	CurveOption { Distance, Percent }
	Specifies the distance on the curve as absolute distance or relative distance as percentage More...

enum	CurveOrientations { Tangent, Normal, Binormal, PerpendicularToObject, ParallelToObject }
	Available orientations that the user can choose when the Datum Axis type is On Curve Vector More...

enum	DirectionOrientations { ParallelToVector, PerpendicularToVector }
	Two available direction orientations that the user can choose when the Datum Axis type is Point and Direction More...

enum	FixedType { All, X, Y, Z }
	Specifies the fixed type datum axis going thru only one specific axis or thru all axes. More...

enum	Types { Inferred, Intersection, CurveOrFaceAxis, OnCurveVector, XcAxis, YcAxis, ZcAxis, PointAndDir, TwoPoints, Fixed }
	New Datum Axis types in NX5 More...

enum	UseArcLength { NoPoint, FirstPoint, SecondPoint, AllPoints }
	Specifies points for which arclength is to be used. More...

Public Member Functions
unsafe void	EvaluatePath (NXOpen.Section section)
	Evaluate the path. More...

unsafe void	SetFixedDatumAxis (NXOpen.Features.DatumAxisBuilder.FixedType type)
	Sets type of fixed datum axis More...

unsafe void	SetGeometryAndConstraints (NXOpen.DisplayableObject geometry1, NXOpen.Features.DatumAxisBuilder.ConstraintType geometryConstraintType1, int constraintAttribute1, double constraintValue1, string constraint1, NXOpen.DisplayableObject geometry2, NXOpen.Features.DatumAxisBuilder.ConstraintType geometryConstraintType2, int constraintAttribute2, double constraintValue2, string constraint2, NXOpen.Sense direction)
	Sets two different geometric objects. More...

unsafe void	SetPointAndDirection (NXOpen.Point point, NXOpen.Direction direction)
	More...

unsafe void	SetPointOnCurve (double arcLength, string constraint, NXOpen.Features.DatumAxisBuilder.AlternateSolution alternateSolution, NXOpen.Features.DatumAxisBuilder.CurveOption option, NXOpen.ICurve curve)
	Sets curve or edge and arc length More...

unsafe void	SetPointOnCurve (double arcLength, string constraint, NXOpen.Features.DatumAxisBuilder.CurveOption option, NXOpen.ICurve curve, NXOpen.DisplayableObject secondGeometry)
	Sets Curve or Edge object and arc length with an extra geometry in picture More...

unsafe void	SetPointOnCurve (double arcLength, string constraint, NXOpen.Features.DatumAxisBuilder.CurveOption option, NXOpen.DisplayableObject secondGeometry, NXOpen.ICurve curve)
	Sets Curve or Edge object and arc length with an extra geometry in picture More...

unsafe void	SetTwoPoints (NXOpen.Point point1, NXOpen.Point point2, NXOpen.Features.DatumAxisBuilder.UseArcLength useArcLength)
	Sets two points More...

Public Member Functions inherited from NXOpen.Features.DatumBuilder
unsafe NXOpen.DatumConstraint	CreateConstraint ()
	Creates a new empty constraint object. More...

unsafe NXOpen.DatumConstraint[]	GetConstraints ()
	Gets the contraint objects that define the positioning of this datum. More...

unsafe void	SetConstraints (NXOpen.DatumConstraint[] constraints)
	Sets the contraint objects that define the positioning of this datum. More...

Public Member Functions inherited from NXOpen.Features.FeatureBuilder
unsafe NXOpen.Features.Feature	CommitFeature ()
	Commits the feature parameters and creates the feature More...

unsafe NXOpen.Features.Feature	GetFeature ()
	Returns the feature currently being edited by this builder. More...

unsafe void	HideInternalParentFeatureAfterEdit (NXOpen.Features.Feature parentFeature)
	Re-suppress an internal parent feature (a slave feature) after it has been edited. More...

unsafe void	SetParentFeatureInternal (NXOpen.Features.Feature parentFeature)
	Set the parent features which would be internal or slaves to the feature being created or commited More...

unsafe void	ShowInternalParentFeatureForEdit (NXOpen.Features.Feature parentFeature)
	Unsuppress an internal parent feature (a slave feature) so it can be edited. More...

unsafe void	UnsetParentFeatureInternal (NXOpen.Features.Feature parentFeature)
	Set the internal parent feature of the feature being edited to external More...

Public Member Functions inherited from NXOpen.Builder
unsafe NXOpen.NXObject	Commit ()
	Commits any edits that have been applied to the builder. More...

unsafe void	Destroy ()
	Deletes the builder, and cleans up any objects created by the builder. More...

unsafe NXOpen.NXObject[]	GetCommittedObjects ()
	For builders that create more than one object, this method returns the objects that are created by commit. More...

unsafe NXOpen.NXObject	GetObject ()
	Returns the object currently being edited by this builder. More...

unsafe void	ShowResults ()
	Updates the model to reflect the result of an edit to the model for all builders that support showing results. More...

unsafe bool	Validate ()
	Validate whether the inputs to the component are sufficient for commit to be called. More...

Public Member Functions inherited from NXOpen.TaggedObject
void	PrintTestData (String variableName)
	<exclude> More...

void	PrintTestData (String variableName, int lineNumber)
	<exclude> More...

override string	ToString ()
	Returns a String that represents the current Object. More...

Public Member Functions inherited from NXOpen.Utilities.NXRemotableObject
IMessageCtrl	AsyncProcessMessage (IMessage msg, IMessageSink replySink)
	Asynchronously processes the given message. More...

IMessage	SyncProcessMessage (IMessage msg)
	Synchronously processes the given message. More...

Properties
unsafe NXOpen.Features.DatumAxisBuilder.AlternateSolution	AlternateSolutionType `[get, set]`
	Returns or sets the alternate solution type. More...

unsafe NXOpen.GeometricUtilities.OnPathDimensionBuilder	ArcLength `[get]`
	Returns the arc length. More...

unsafe NXOpen.SelectICurve	Curve `[get]`
	Returns the curve or edge. More...

unsafe NXOpen.SelectNXObject	CurveOrFace `[get]`
	Returns the curve or face . More...

unsafe NXOpen.Features.DatumAxisBuilder.CurveOrientations	CurveOrientation `[get, set]`
	Returns or sets the orientation of vector on a curve. More...

unsafe NXOpen.Features.DatumAxisBuilder.DirectionOrientations	DirectionOrientation `[get, set]`
	Returns or sets the direction orientation. More...

unsafe bool	IsAssociative `[get, set]`
	Returns or sets the associativity. More...

unsafe bool	IsAxisReversed `[get, set]`
	Returns or sets the datum axis direction. More...

unsafe NXOpen.SelectNXObject	Object1 `[get]`
	Returns the first object (i. More...

unsafe NXOpen.SelectNXObject	Object2 `[get]`
	Returns the second object (i. More...

unsafe NXOpen.SelectNXObjectList	Objects `[get]`
	Returns the objects to define Datum Axis. More...

unsafe NXOpen.SelectNXObject	OrientationObject `[get]`
	Returns the orientation object. More...

unsafe NXOpen.Point	Point `[get, set]`
	Returns or sets the point. More...

unsafe NXOpen.Point	Point1 `[get, set]`
	Returns or sets the first point. More...

unsafe NXOpen.Point	Point2 `[get, set]`
	Returns or sets the second point. More...

unsafe double	ResizedEndDistance `[get, set]`
	Returns or sets the resized distance for the end point. More...

unsafe bool	ReverseDirection `[get, set]`
	Returns or sets More...

unsafe NXOpen.Section	Section `[get]`
	Returns the section. More...

unsafe NXOpen.Features.DatumAxisBuilder.Types	Type `[get, set]`
	Returns or sets the Datum Axis type More...

unsafe NXOpen.Direction	Vector `[get, set]`
	Returns or sets the vector. More...

Additional Inherited Members
Protected Member Functions inherited from NXOpen.TaggedObject
new void	initialize ()
	<exclude> More...

Detailed Description

Represents a datum axis feature builder.

Provides methods to create datum axis thru two points, point and direction and point on curve. Also provides generic method for creation of datum axis feature

To create a new instance of this class, use NXOpen.Features.FeatureCollection.CreateDatumAxisBuilder

Created in NX3.0.0

Member Enumeration Documentation

enum NXOpen.Features.DatumAxisBuilder.AlternateSolution

Specifies the alternate solution for datum axis using point on curve method only

Enumerator
Undefined	Not defined
Tangent	Indicates the datum axis at tangent to curve
Normal	Datum axis at normal to curve
Binormal	Datum axis at binormal to curve
OppositeTangent	Datum axis at opposite to tangent to curve
OppositeNormal	Datum axis at opposite to normal to curve
OppositeBinormal	Datum axis at opposite to binormal to curve
Project	This direction is calculated by projecting a point selected along a curve to a line, a datum axis, an edge of a solid, a planar face or a datum plane

enum NXOpen.Features.DatumAxisBuilder.ConstraintType

Specifies different constraint types for selected geometries

Enumerator
Undefined	Not defined
Coincident	Coincident constraint
Parallel	Parallel constraint
Perpendicular	Perpendicular constraint
Center	Center constraint
Tangent	Tangent constraint
Distance	Distance constraint
Angle	Angle constraint
Frenet	Frenet constraint

enum NXOpen.Features.DatumAxisBuilder.CurveOption

Specifies the distance on the curve as absolute distance or relative distance as percentage

Enumerator
Distance	Absolute distance
Percent	Relative distance as percentage

enum NXOpen.Features.DatumAxisBuilder.CurveOrientations

Available orientations that the user can choose when the Datum Axis type is On Curve Vector

Enumerator
Tangent	Orientation at tangent to curve
Normal	Orientation at normal to curve
Binormal	Orientation at binormal to curve
PerpendicularToObject	Orientation at perpendicular to object
ParallelToObject	Orientation at parallel to object

enum NXOpen.Features.DatumAxisBuilder.DirectionOrientations

Two available direction orientations that the user can choose when the Datum Axis type is Point and Direction

Enumerator
ParallelToVector	Orientation parallel to Direction
PerpendicularToVector	Orientation perpendicular to Direction

enum NXOpen.Features.DatumAxisBuilder.FixedType

Specifies the fixed type datum axis going thru only one specific axis or thru all axes.

Enumerator
All	Fixed datum axis thru all Axis
X	Fixed datum axis thru X Axis
Y	Fixed datum axis thru Y Axis
Z	Fixed datum axis thru Z Axis

enum NXOpen.Features.DatumAxisBuilder.Types

New Datum Axis types in NX5

Enumerator
Inferred	Inferred
Intersection	Datum axis at the intersection of objects
CurveOrFaceAxis	Datum axis at the curve or face axis
OnCurveVector	Datum axis at vector on curve
XcAxis	Datum axis thru X axis
YcAxis	Datum axis thru Y axis
ZcAxis	Datum axis thru Z axis
PointAndDir	Datum axis thru a point and parallel or perpendicular to direction
TwoPoints	Datum axis thru two point
Fixed	Indicate the datum axis is fixed

enum NXOpen.Features.DatumAxisBuilder.UseArcLength

Specifies points for which arclength is to be used.

Percentage of arclength is used for points for which arclength option is not selected. Specified for creation of datum axis using thru two points method.

Enumerator
NoPoint	All points use percentage of arclength
FirstPoint	Only first point uses arclength
SecondPoint	Only second point uses arclength
AllPoints	Both points use arclength

Member Function Documentation

unsafe void NXOpen.Features.DatumAxisBuilder.EvaluatePath ( NXOpen.Section section )

inline

Evaluate the path.

If there is no path, create it, otherwise evaluate it. This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.OnCurveVector

Created in NX8.0.0

License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

section

unsafe void NXOpen.Features.DatumAxisBuilder.SetFixedDatumAxis ( NXOpen.Features.DatumAxisBuilder.FixedType type )

inline

Sets type of fixed datum axis

Created in NX3.0.0

License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

type	Indicates fixed datum axis type

unsafe void NXOpen.Features.DatumAxisBuilder.SetGeometryAndConstraints	(	NXOpen.DisplayableObject	geometry1,
		NXOpen.Features.DatumAxisBuilder.ConstraintType	geometryConstraintType1,
		int	constraintAttribute1,
		double	constraintValue1,
		string	constraint1,
		NXOpen.DisplayableObject	geometry2,
		NXOpen.Features.DatumAxisBuilder.ConstraintType	geometryConstraintType2,
		int	constraintAttribute2,
		double	constraintValue2,
		string	constraint2,
		NXOpen.Sense	direction
	)

inline

Sets two different geometric objects.

Possible combinations are:

If first constrain is Through Point, then the second contraint can be:
- Solid Body Vertex (endpoint)
- Edge Midpoint
If first constrain is Intersection of Plane, then the second contraint can be:
- Through the straight edge formed by the intersection of two planes
If first constrain is Through Curve, then the second contraint can be:
- Used with Through Point constraint and along a curve
If first constrain is Perpendicular to object, then the second contraint can be:
- Through Curve and Through Point perpendicular to lines, linear edge, datum planes, datum axis, or planar faces

Created in NX3.0.0

License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

geometry1	First geometric object
geometryConstraintType1	Constraint type of first geometry
constraintAttribute1	Constraint attribute value of first geometry VRH alternate_solution_only - only for point on curve
constraintValue1	Constraint value parameter of first geometry
constraint1	Constraint attached with first geometric object. Set to "0.0" in case value is not specified
geometry2	Second geometric object
geometryConstraintType2	Constraint type of second geometry
constraintAttribute2	Constraint attribute value of second geometry
constraintValue2	Constraint value parameter of second geometry
constraint2	Constraint attached with second geometric object. Set to "0.0" in case value is not specified
direction	Flag to specify datum axis direction

unsafe void NXOpen.Features.DatumAxisBuilder.SetPointAndDirection	(	NXOpen.Point	point,
		NXOpen.Direction	direction
	)

inline

Created in NX3.0.0

License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

point
direction

unsafe void NXOpen.Features.DatumAxisBuilder.SetPointOnCurve	(	double	arcLength,
		string	constraint,
		NXOpen.Features.DatumAxisBuilder.AlternateSolution	alternateSolution,
		NXOpen.Features.DatumAxisBuilder.CurveOption	option,
		NXOpen.ICurve	curve
	)

inline

Sets curve or edge and arc length

Created in NX3.0.0

License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

arcLength	Arc length
constraint	Constraint expression. Usually same as arc_length
alternateSolution	Alternate solution
option	Absolute distance or relative distance
curve	Curve or Edge object

unsafe void NXOpen.Features.DatumAxisBuilder.SetPointOnCurve	(	double	arcLength,
		string	constraint,
		NXOpen.Features.DatumAxisBuilder.CurveOption	option,
		NXOpen.ICurve	curve,
		NXOpen.DisplayableObject	secondGeometry
	)

inline

Sets Curve or Edge object and arc length with an extra geometry in picture

Created in NX3.0.0

License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

arcLength	Arc length
constraint	Constraint expression. Usually same as arc_length
option	Absolute distance or relative distance
curve	Curve or Edge object
secondGeometry	Second geometric object

unsafe void NXOpen.Features.DatumAxisBuilder.SetPointOnCurve	(	double	arcLength,
		string	constraint,
		NXOpen.Features.DatumAxisBuilder.CurveOption	option,
		NXOpen.DisplayableObject	secondGeometry,
		NXOpen.ICurve	curve
	)

inline

Sets Curve or Edge object and arc length with an extra geometry in picture

Created in NX3.0.0

License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

arcLength	Arc length
constraint	Constraint expression. Usually same as arc_length
option	Absolute distance or relative distance
secondGeometry	Second Geometric object
curve	Curve or Edge object

unsafe void NXOpen.Features.DatumAxisBuilder.SetTwoPoints	(	NXOpen.Point	point1,
		NXOpen.Point	point2,
		NXOpen.Features.DatumAxisBuilder.UseArcLength	useArcLength
	)

inline

Sets two points

Created in NX3.0.0

License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

point1
point2
useArcLength	Specify points which use arclength instead of percentage of arclength

Property Documentation

unsafe NXOpen.Features.DatumAxisBuilder.AlternateSolution NXOpen.Features.DatumAxisBuilder.AlternateSolutionType

getset

Returns or sets the alternate solution type.

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.OnCurveVector

Created in NX5.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

unsafe NXOpen.GeometricUtilities.OnPathDimensionBuilder NXOpen.Features.DatumAxisBuilder.ArcLength

get

Returns the arc length.

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.OnCurveVector

Created in NX5.0.0

License requirements: None.

unsafe NXOpen.SelectICurve NXOpen.Features.DatumAxisBuilder.Curve

get

Returns the curve or edge.

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.OnCurveVector

Created in NX5.0.0

License requirements: None.

unsafe NXOpen.SelectNXObject NXOpen.Features.DatumAxisBuilder.CurveOrFace

get

Returns the curve or face .

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.CurveOrFaceAxis

Created in NX5.0.0

License requirements: None.

unsafe NXOpen.Features.DatumAxisBuilder.CurveOrientations NXOpen.Features.DatumAxisBuilder.CurveOrientation

getset

Returns or sets the orientation of vector on a curve.

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.OnCurveVector

Created in NX5.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

unsafe NXOpen.Features.DatumAxisBuilder.DirectionOrientations NXOpen.Features.DatumAxisBuilder.DirectionOrientation

getset

Returns or sets the direction orientation.

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.PointAndDir

Created in NX5.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

unsafe bool NXOpen.Features.DatumAxisBuilder.IsAssociative

getset

Returns or sets the associativity.

If true, the Datum Axis is associative

Created in NX5.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

unsafe bool NXOpen.Features.DatumAxisBuilder.IsAxisReversed

getset

Returns or sets the datum axis direction.

If true, the Datum Axis direction is reversed

Created in NX5.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

unsafe NXOpen.SelectNXObject NXOpen.Features.DatumAxisBuilder.Object1

get

Returns the first object (i.

e. a planar face or datum plane). This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.Intersection

Created in NX5.0.0

License requirements: None.

unsafe NXOpen.SelectNXObject NXOpen.Features.DatumAxisBuilder.Object2

get

Returns the second object (i.

e. a planar face or datum plane). This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.Intersection

Created in NX5.0.0

License requirements: None.

unsafe NXOpen.SelectNXObjectList NXOpen.Features.DatumAxisBuilder.Objects

get

Returns the objects to define Datum Axis.

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.Inferred

Created in NX5.0.0

License requirements: None.

unsafe NXOpen.SelectNXObject NXOpen.Features.DatumAxisBuilder.OrientationObject

get

Returns the orientation object.

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.OnCurveVector

Created in NX5.0.0

License requirements: None.

unsafe NXOpen.Point NXOpen.Features.DatumAxisBuilder.Point

getset

Returns or sets the point.

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.PointAndDir

Created in NX5.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

unsafe NXOpen.Point NXOpen.Features.DatumAxisBuilder.Point1

getset

Returns or sets the first point.

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.TwoPoints

Created in NX5.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

unsafe NXOpen.Point NXOpen.Features.DatumAxisBuilder.Point2

getset

Returns or sets the second point.

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.TwoPoints

Created in NX5.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

unsafe double NXOpen.Features.DatumAxisBuilder.ResizedEndDistance

getset

Returns or sets the resized distance for the end point.

If the value is 0.0, then this datum axis is not resized at end point

Created in NX5.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

unsafe bool NXOpen.Features.DatumAxisBuilder.ReverseDirection

getset

Returns or sets

Created in NX4.0.0

License requirements to get this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

unsafe NXOpen.Section NXOpen.Features.DatumAxisBuilder.Section

get

Returns the section.

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.OnCurveVector

Created in NX8.0.0

License requirements: None.

unsafe NXOpen.Features.DatumAxisBuilder.Types NXOpen.Features.DatumAxisBuilder.Type

getset

Returns or sets the Datum Axis type

Created in NX5.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

unsafe NXOpen.Direction NXOpen.Features.DatumAxisBuilder.Vector

getset

Returns or sets the vector.

This is used only if the Datum Axis type is Features.DatumAxisBuilder.Types.PointAndDir

Created in NX5.0.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

The documentation for this class was generated from the following file:

Features_DatumAxisBuilder.cs

Public Types

Public Member Functions

Properties

Additional Inherited Members

Detailed Description

Member Enumeration Documentation

Member Function Documentation

Property Documentation