NX Open C++ Reference Guide
Public Types | Public Member Functions
NXOpen::Features::DatumAxisBuilder Class Reference

Represents a datum axis feature builder. More...

Inheritance diagram for NXOpen::Features::DatumAxisBuilder:
NXOpen::Features::DatumBuilder NXOpen::Features::FeatureBuilder NXOpen::Builder NXOpen::TaggedObject NXOpen::GeometricUtilities::IComponentBuilder

List of all members.

Public Types

enum  AlternateSolution {
  AlternateSolutionUndefined, AlternateSolutionTangent, AlternateSolutionNormal, AlternateSolutionBinormal,
  AlternateSolutionOppositeTangent, AlternateSolutionOppositeNormal, AlternateSolutionOppositeBinormal, AlternateSolutionProject
}
 Specifies the alternate solution for datum axis using point on curve method only. More...
enum  ConstraintType {
  ConstraintTypeUndefined, ConstraintTypeCoincident, ConstraintTypeParallel, ConstraintTypePerpendicular,
  ConstraintTypeCenter, ConstraintTypeTangent, ConstraintTypeDistance, ConstraintTypeAngle,
  ConstraintTypeFrenet
}
 Specifies different constraint types for selected geometries. More...
enum  CurveOption { CurveOptionDistance, CurveOptionPercent }
 Specifies the distance on the curve as absolute distance or relative distance as percentage. More...
enum  CurveOrientations {
  CurveOrientationsTangent, CurveOrientationsNormal, CurveOrientationsBinormal, CurveOrientationsPerpendicularToObject,
  CurveOrientationsParallelToObject
}
 Available orientations that the user can choose when the Datum Axis type is On Curve Vector. More...
enum  DirectionOrientations { DirectionOrientationsParallelToVector, DirectionOrientationsPerpendicularToVector }
 Two available direction orientations that the user can choose when the Datum Axis type is Point and Direction. More...
enum  FixedType { FixedTypeAll, FixedTypeX, FixedTypeY, FixedTypeZ }
 Specifies the fixed type datum axis going thru only one specific axis or thru all axes. More...
enum  Types {
  TypesInferred, TypesIntersection, TypesCurveOrFaceAxis, TypesOnCurveVector,
  TypesXcAxis, TypesYcAxis, TypesZcAxis, TypesPointAndDir,
  TypesTwoPoints, TypesFixed
}
 New Datum Axis types in NX5. More...
enum  UseArcLength { UseArcLengthNoPoint, UseArcLengthFirstPoint, UseArcLengthSecondPoint, UseArcLengthAllPoints }
 Specifies points for which arclength is to be used. More...

Public Member Functions

NXOpen::Features::DatumAxisBuilder::AlternateSolution AlternateSolutionType ()
 Returns the alternate solution type.
NXOpen::GeometricUtilities::OnPathDimensionBuilderArcLength ()
 Returns the arc length.
NXOpen::SelectICurveCurve ()
 Returns the curve or edge.
NXOpen::SelectNXObjectCurveOrFace ()
 Returns the curve or face .
NXOpen::Features::DatumAxisBuilder::CurveOrientations CurveOrientation ()
 Returns the orientation of vector on a curve.
NXOpen::Features::DatumAxisBuilder::DirectionOrientations DirectionOrientation ()
 Returns the direction orientation.
void EvaluatePath (NXOpen::Section *section)
 Evaluate the path.
bool IsAssociative ()
 Returns the associativity.
bool IsAxisReversed ()
 Returns the datum axis direction.
NXOpen::SelectNXObjectObject1 ()
 Returns the first object (i.e.
NXOpen::SelectNXObjectObject2 ()
 Returns the second object (i.e.
NXOpen::SelectNXObjectListObjects ()
 Returns the objects to define Datum Axis.
NXOpen::SelectNXObjectOrientationObject ()
 Returns the orientation object.
NXOpen::PointPoint ()
 Returns the point.
NXOpen::PointPoint1 ()
 Returns the first point.
NXOpen::PointPoint2 ()
 Returns the second point.
double ResizedEndDistance ()
 Returns the resized distance for the end point.
bool ReverseDirection ()
 Returns
Created in NX4.0.0.
NXOpen::SectionSection ()
 Returns the section.
void SetAlternateSolutionType (NXOpen::Features::DatumAxisBuilder::AlternateSolution alternateSolutionType)
 Sets the alternate solution type.
void SetAssociative (bool isAssociative)
 Sets the associativity.
void SetAxisReversed (bool isAxisReversed)
 Sets the datum axis direction.
void SetCurveOrientation (NXOpen::Features::DatumAxisBuilder::CurveOrientations curveOrientation)
 Sets the orientation of vector on a curve.
void SetDirectionOrientation (NXOpen::Features::DatumAxisBuilder::DirectionOrientations directionOrientation)
 Sets the direction orientation.
void SetFixedDatumAxis (NXOpen::Features::DatumAxisBuilder::FixedType type)
 Sets type of fixed datum axis
Created in NX3.0.0.
void SetGeometryAndConstraints (NXOpen::DisplayableObject *geometry1, NXOpen::Features::DatumAxisBuilder::ConstraintType geometryConstraintType1, int constraintAttribute1, double constraintValue1, const NXString &constraint1, NXOpen::DisplayableObject *geometry2, NXOpen::Features::DatumAxisBuilder::ConstraintType geometryConstraintType2, int constraintAttribute2, double constraintValue2, const NXString &constraint2, NXOpen::Sense direction)
 Sets two different geometric objects.
void SetPoint (NXOpen::Point *point)
 Sets the point.
void SetPoint1 (NXOpen::Point *point1)
 Sets the first point.
void SetPoint2 (NXOpen::Point *point2)
 Sets the second point.
void SetPointAndDirection (NXOpen::Point *point, NXOpen::Direction *direction)
 
Created in NX3.0.0.
void SetPointOnCurve (double arcLength, const NXString &constraint, NXOpen::Features::DatumAxisBuilder::AlternateSolution alternateSolution, NXOpen::Features::DatumAxisBuilder::CurveOption option, NXOpen::ICurve *curve)
 Sets curve or edge and arc length
Created in NX3.0.0.
void SetPointOnCurve (double arcLength, const NXString &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
Created in NX3.0.0.
void SetPointOnCurve (double arcLength, const NXString &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
Created in NX3.0.0.
void SetResizedEndDistance (double resizedEndDistance)
 Sets the resized distance for the end point.
void SetReverseDirection (bool reverseDirection)
 Sets
Created in NX4.0.0.
void SetTwoPoints (NXOpen::Point *point1, NXOpen::Point *point2, NXOpen::Features::DatumAxisBuilder::UseArcLength useArcLength)
 Sets two points
Created in NX3.0.0.
void SetType (NXOpen::Features::DatumAxisBuilder::Types type)
 Sets the Datum Axis type
Created in NX5.0.0.
void SetVector (NXOpen::Direction *vector)
 Sets the vector.
NXOpen::Features::DatumAxisBuilder::Types Type ()
 Returns the Datum Axis type
Created in NX5.0.0.
NXOpen::DirectionVector ()
 Returns the vector.

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 Features::FeatureCollection::CreateDatumAxisBuilder

Created in NX3.0.0.


Member Enumeration Documentation

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

Enumerator:
AlternateSolutionUndefined 

Not defined.

AlternateSolutionTangent 

Indicates the datum axis at tangent to curve.

AlternateSolutionNormal 

Datum axis at normal to curve.

AlternateSolutionBinormal 

Datum axis at binormal to curve.

AlternateSolutionOppositeTangent 

Datum axis at opposite to tangent to curve.

AlternateSolutionOppositeNormal 

Datum axis at opposite to normal to curve.

AlternateSolutionOppositeBinormal 

Datum axis at opposite to binormal to curve.

AlternateSolutionProject 

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.

Specifies different constraint types for selected geometries.

Enumerator:
ConstraintTypeUndefined 

Not defined.

ConstraintTypeCoincident 

Coincident constraint.

ConstraintTypeParallel 

Parallel constraint.

ConstraintTypePerpendicular 

Perpendicular constraint.

ConstraintTypeCenter 

Center constraint.

ConstraintTypeTangent 

Tangent constraint.

ConstraintTypeDistance 

Distance constraint.

ConstraintTypeAngle 

Angle constraint.

ConstraintTypeFrenet 

Frenet constraint.

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

Enumerator:
CurveOptionDistance 

Absolute distance.

CurveOptionPercent 

Relative distance as percentage.

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

Enumerator:
CurveOrientationsTangent 

Orientation at tangent to curve.

CurveOrientationsNormal 

Orientation at normal to curve.

CurveOrientationsBinormal 

Orientation at binormal to curve.

CurveOrientationsPerpendicularToObject 

Orientation at perpendicular to object.

CurveOrientationsParallelToObject 

Orientation at parallel to object.

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

Enumerator:
DirectionOrientationsParallelToVector 

Orientation parallel to Direction.

DirectionOrientationsPerpendicularToVector 

Orientation perpendicular to Direction.

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

Enumerator:
FixedTypeAll 

Fixed datum axis thru all Axis.

FixedTypeX 

Fixed datum axis thru X Axis.

FixedTypeY 

Fixed datum axis thru Y Axis.

FixedTypeZ 

Fixed datum axis thru Z Axis.

New Datum Axis types in NX5.

Enumerator:
TypesInferred 

Inferred.

TypesIntersection 

Datum axis at the intersection of objects.

TypesCurveOrFaceAxis 

Datum axis at the curve or face axis.

TypesOnCurveVector 

Datum axis at vector on curve.

TypesXcAxis 

Datum axis thru X axis.

TypesYcAxis 

Datum axis thru Y axis.

TypesZcAxis 

Datum axis thru Z axis.

TypesPointAndDir 

Datum axis thru a point and parallel or perpendicular to direction.

TypesTwoPoints 

Datum axis thru two point.

TypesFixed 

Indicate the datum axis is fixed.

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:
UseArcLengthNoPoint 

All points use percentage of arclength.

UseArcLengthFirstPoint 

Only first point uses arclength.

UseArcLengthSecondPoint 

Only second point uses arclength.

UseArcLengthAllPoints 

Both points use arclength.


Member Function Documentation

Returns the alternate solution type.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesOnCurveVector


Created in NX5.0.0.

License requirements : None

Returns the arc length.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesOnCurveVector


Created in NX5.0.0.

License requirements : None

Returns the curve or edge.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesOnCurveVector


Created in NX5.0.0.

License requirements : None

Returns the curve or face .

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesCurveOrFaceAxis


Created in NX5.0.0.

License requirements : None

Returns the orientation of vector on a curve.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesOnCurveVector


Created in NX5.0.0.

License requirements : None

Returns the direction orientation.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesPointAndDir


Created in NX5.0.0.

License requirements : None

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::TypesOnCurveVector


Created in NX8.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
sectionsection

Returns the associativity.

If true, the Datum Axis is associative
Created in NX5.0.0.

License requirements : None

Returns the datum axis direction.

If true, the Datum Axis direction is reversed
Created in NX5.0.0.

License requirements : None

Returns the first object (i.e.

a planar face or datum plane). This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesIntersection


Created in NX5.0.0.

License requirements : None

Returns the second object (i.e.

a planar face or datum plane). This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesIntersection


Created in NX5.0.0.

License requirements : None

Returns the objects to define Datum Axis.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesInferred


Created in NX5.0.0.

License requirements : None

Returns the orientation object.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesOnCurveVector


Created in NX5.0.0.

License requirements : None

Returns the point.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesPointAndDir


Created in NX5.0.0.

License requirements : None

Returns the first point.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesTwoPoints


Created in NX5.0.0.

License requirements : None

Returns the second point.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesTwoPoints


Created in NX5.0.0.

License requirements : None

Returns 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 : None

Returns
Created in NX4.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Returns the section.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesOnCurveVector


Created in NX8.0.0.

License requirements : None

Sets the alternate solution type.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesOnCurveVector


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
alternateSolutionTypealternate solution type

Sets the associativity.

If true, the Datum Axis is associative
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
isAssociativeisassociative

Sets the datum axis direction.

If true, the Datum Axis direction is reversed
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
isAxisReversedisaxisreversed

Sets the orientation of vector on a curve.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesOnCurveVector


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
curveOrientationcurveorientation

Sets the direction orientation.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesPointAndDir


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
directionOrientationdirectionorientation

Sets type of fixed datum axis
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
typeIndicates fixed datum axis type
void NXOpen::Features::DatumAxisBuilder::SetGeometryAndConstraints ( NXOpen::DisplayableObject geometry1,
NXOpen::Features::DatumAxisBuilder::ConstraintType  geometryConstraintType1,
int  constraintAttribute1,
double  constraintValue1,
const NXString constraint1,
NXOpen::DisplayableObject geometry2,
NXOpen::Features::DatumAxisBuilder::ConstraintType  geometryConstraintType2,
int  constraintAttribute2,
double  constraintValue2,
const NXString constraint2,
NXOpen::Sense  direction 
)

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")

Parameters:
geometry1First geometric object
geometryConstraintType1Constraint type of first geometry
constraintAttribute1Constraint attribute value of first geometry VRH alternate_solution_only - only for point on curve
constraintValue1Constraint value parameter of first geometry
constraint1Constraint attached with first geometric object. Set to "0.0" in case value is not specified
NOTE: The full Unicode character set is not supported for this parameter.
geometry2Second geometric object
geometryConstraintType2Constraint type of second geometry
constraintAttribute2Constraint attribute value of second geometry
constraintValue2Constraint value parameter of second geometry
constraint2Constraint attached with second geometric object. Set to "0.0" in case value is not specified
NOTE: The full Unicode character set is not supported for this parameter.
directionFlag to specify datum axis direction

Sets the point.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesPointAndDir


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
pointpoint

Sets the first point.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesTwoPoints


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
point1point1

Sets the second point.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesTwoPoints


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
point2point2


Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
pointpoint
directiondirection

Sets curve or edge and arc length
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
arcLengthArc length
constraintConstraint expression. Usually same as arc_length
NOTE: The full Unicode character set is not supported for this parameter.
alternateSolutionAlternate solution
optionAbsolute distance or relative distance
curveCurve or Edge object
void NXOpen::Features::DatumAxisBuilder::SetPointOnCurve ( double  arcLength,
const NXString 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
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
arcLengthArc length
constraintConstraint expression. Usually same as arc_length
NOTE: The full Unicode character set is not supported for this parameter.
optionAbsolute distance or relative distance
curveCurve or Edge object
secondGeometrySecond geometric object
void NXOpen::Features::DatumAxisBuilder::SetPointOnCurve ( double  arcLength,
const NXString 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
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
arcLengthArc length
constraintConstraint expression. Usually same as arc_length
NOTE: The full Unicode character set is not supported for this parameter.
optionAbsolute distance or relative distance
secondGeometrySecond Geometric object
curveCurve or Edge object
void NXOpen::Features::DatumAxisBuilder::SetResizedEndDistance ( double  resizedEndDistance)

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 : solid_modeling ("SOLIDS MODELING")

Parameters:
resizedEndDistanceresizedenddistance

Sets
Created in NX4.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
reverseDirectionreverse direction

Sets two points
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
point1point1
point2point2
useArcLengthSpecify points which use arclength instead of percentage of arclength

Sets the Datum Axis type
Created in NX5.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
typetype

Sets the vector.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesPointAndDir


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
vectorvector

Returns the Datum Axis type
Created in NX5.0.0.



License requirements : None

Returns the vector.

This is used only if the Datum Axis type is Features::DatumAxisBuilder::TypesPointAndDir


Created in NX5.0.0.

License requirements : None


The documentation for this class was generated from the following file:
Copyright 2011 Siemens Product Lifecycle Management Software Inc. All Rights Reserved.