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

Represents a datum plane feature builder. More...

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

List of all members.

Public Types

enum  AlternateSolution {
  AlternateSolutionTangent, AlternateSolutionNormal, AlternateSolutionBinormal, AlternateSolutionOppositeTangent,
  AlternateSolutionOppositeNormal, AlternateSolutionOppositeBinormal, AlternateSolutionProject, AlternateSolutionProjectView
}
 Specifies the alternate solution for a datum plane using point on curve method. More...
enum  ConstraintType {
  ConstraintTypeUndefined, ConstraintTypeCoincident, ConstraintTypeParallel, ConstraintTypePerpendicular,
  ConstraintTypeCenter, ConstraintTypeTangent, ConstraintTypeDistance, ConstraintTypeAngle,
  ConstraintTypeFrenet
}
 Specifies different constraint types of selected geometries. More...
enum  CurveOption { CurveOptionDistance, CurveOptionPercent }
 Specifies the distance on the curve as absolute distance or relative distance as percentage. More...
enum  FixedType { FixedTypeAll, FixedTypeXy, FixedTypeYz, FixedTypeZx }
 Specifies the fixed type datum plane going thru only one specific plane or thru all planes. More...
enum  UseArcLength {
  UseArcLengthNoPoint, UseArcLengthFirstPoint, UseArcLengthSecondPoint, UseArcLengthThirdPoint,
  UseArcLengthFirstAndSecondPoint, UseArcLengthFirstAndThirdPoint, UseArcLengthSecondAndThirdPoint, UseArcLengthAllPoints
}
 Specifies points for which arclength is to be used. More...

Public Member Functions

NXOpen::DatumPlaneGetDatum ()
 The datum display object this is the feature output.
NXOpen::PlaneGetPlane ()
 The plane is use to create the feature.
bool ResizeDuringUpdate ()
 Returns the resize during update
Created in NX8.0.0.
void SetCornerPoints (const NXOpen::Point3d &corner1, const NXOpen::Point3d &corner2, const NXOpen::Point3d &corner3, const NXOpen::Point3d &corner4)
 Sets corner points to builder
Created in NX7.5.0.
void SetFaceAndOffset (NXOpen::Face *face, double offsetValue, const NXString &expression)
 Sets one face object and offset
Created in NX3.0.0.
void SetFixedDatumPlane (NXOpen::Features::DatumPlaneBuilder::FixedType type)
 Sets type of fixed datum plane.
void SetGeometryAndConstraints (NXOpen::DisplayableObject *geometry1, NXOpen::Features::DatumPlaneBuilder::ConstraintType geometryConstraintType1, int constraintAttribute1, double constraintValue1, const NXString &constraint1, NXOpen::DisplayableObject *geometry2, NXOpen::Features::DatumPlaneBuilder::ConstraintType geometryConstraintType2, int constraintAttribute2, double constraintValue2, const NXString &constraint2)
 Sets two different geometric objects.
void SetPointAndDirection (NXOpen::Point *point, NXOpen::Direction *direction)
 Sets point and direction
Created in NX3.0.0.
void SetPointOnCurve (double arcLength, const NXString &constraint, NXOpen::Features::DatumPlaneBuilder::AlternateSolution alternateSolution, NXOpen::Features::DatumPlaneBuilder::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::DatumPlaneBuilder::AlternateSolution alternateSolution, NXOpen::Features::DatumPlaneBuilder::CurveOption option, NXOpen::ICurve *curve, NXOpen::Direction *direction)
 Sets curve or edge and arc length
Created in NX3.0.0.
void SetPointOnCurve (double arcLength, const NXString &constraint, NXOpen::Features::DatumPlaneBuilder::CurveOption option, NXOpen::ICurve *curve, NXOpen::DisplayableObject *secondGeometry)
 Sets curve or edge object and arc length with other geometry selected.
void SetResizeDuringUpdate (bool resize)
 Sets the resize during update
Created in NX8.0.0.
void SetThreePoints (NXOpen::Point *point1, NXOpen::Point *point2, NXOpen::Point *point3, NXOpen::Features::DatumPlaneBuilder::UseArcLength useArcLength)
 Sets three different points.
NXOpen::Features::FeatureUpdateFeature ()
 Update the feature if the feature does not exist then create it.

Detailed Description

Represents a datum plane feature builder.

Provides methods to create datum planes thru three points, point and direction and point on curve
To create a new instance of this class, use Features::FeatureCollection::CreateDatumPlaneBuilder

Created in NX3.0.0.


Member Enumeration Documentation

Specifies the alternate solution for a datum plane using point on curve method.

Enumerator:
AlternateSolutionTangent 

Indicates the datum plane as tangent to curve.

AlternateSolutionNormal 

Datum plane at normal to curve.

AlternateSolutionBinormal 

Datum plane at binormal to curve.

AlternateSolutionOppositeTangent 

Datum plane at opposite to tangent to curve.

AlternateSolutionOppositeNormal 

Datum plane at opposite to normal to curve.

AlternateSolutionOppositeBinormal 

Datum plane 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.

AlternateSolutionProjectView 

Datum plane direction is calculated during creation based on the view plane.

The datum plane normal is projected onto the view plane during creation time. The datum plane normal is maintained constant thereafter

Specifies different constraint types of 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.

Specifies the fixed type datum plane going thru only one specific plane or thru all planes.

Enumerator:
FixedTypeAll 

Fixed datum plane thru all planes.

FixedTypeXy 

Fixed datum plane thru XY plane.

FixedTypeYz 

Fixed datum plane thru YZ plane.

FixedTypeZx 

Fixed datum plane thru ZX plane.

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 plane using thru three points method.

Enumerator:
UseArcLengthNoPoint 

All points use percentage of arclength.

UseArcLengthFirstPoint 

Only first point uses arclength.

UseArcLengthSecondPoint 

Only second point uses arclength.

UseArcLengthThirdPoint 

Only third point uses arclength.

UseArcLengthFirstAndSecondPoint 

Only first and second point use arclength.

UseArcLengthFirstAndThirdPoint 

Only first and third point use arclength.

UseArcLengthSecondAndThirdPoint 

Only second and third point use arclength.

UseArcLengthAllPoints 

All points use arclength.


Member Function Documentation

The datum display object this is the feature output.

Returns:

Created in NX4.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

The plane is use to create the feature.

Returns:

Created in NX4.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Returns the resize during update
Created in NX8.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

void NXOpen::Features::DatumPlaneBuilder::SetCornerPoints ( const NXOpen::Point3d corner1,
const NXOpen::Point3d corner2,
const NXOpen::Point3d corner3,
const NXOpen::Point3d corner4 
)

Sets corner points to builder
Created in NX7.5.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
corner1corner1
corner2corner2
corner3corner3
corner4corner4
void NXOpen::Features::DatumPlaneBuilder::SetFaceAndOffset ( NXOpen::Face face,
double  offsetValue,
const NXString expression 
)

Sets one face object and offset
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
faceFace object
offsetValueOffset double parameter
expressionOffset string parameter
NOTE: The full Unicode character set is not supported for this parameter.

Sets type of fixed datum plane.


Created in NX3.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

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

Sets two different geometric objects.

Possible combinations are:


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
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 first 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.

Sets point and direction
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

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
directionDirection
void NXOpen::Features::DatumPlaneBuilder::SetPointOnCurve ( double  arcLength,
const NXString constraint,
NXOpen::Features::DatumPlaneBuilder::CurveOption  option,
NXOpen::ICurve curve,
NXOpen::DisplayableObject secondGeometry 
)

Sets curve or edge object and arc length with other geometry selected.


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.
optionWhether the absolute distance has been selected or relative
curveCurve or Edge object already created
secondGeometrySecond geometric object

Sets the resize during update
Created in NX8.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
resizeresize during update

Sets three different points.


Created in NX3.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
point1First point
point2Second point
point3Third point
useArcLengthSpecify points which use arclength instead of percentage of arclength

Update the feature if the feature does not exist then create it.

Returns:

Created in NX4.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

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