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

Represents a Hole feature builder. More...

Inheritance diagram for NXOpen::Features::HoleFeatureBuilder:
NXOpen::Features::RPOBuilder NXOpen::Features::FeatureBuilder NXOpen::Builder NXOpen::TaggedObject NXOpen::GeometricUtilities::IComponentBuilder

List of all members.

Public Types

enum  HoleSubtype { HoleSubtypeSimple, HoleSubtypeCounterbore, HoleSubtypeCountersink }
 Represents the subtype of the hole. More...

Public Member Functions

NXOpen::ExpressionCounterboreDepth ()
 Returns the depth of the counterbore for a hole.
NXOpen::ExpressionCounterboreDiameter ()
 Returns the diameter of the counterbore for a hole.
NXOpen::ExpressionCountersinkAngle ()
 Returns the angle of the countersink for a hole.
NXOpen::ExpressionCountersinkDiameter ()
 Returns the diameter of the countersink for a hole.
void CreateHole ()
 Creates a hole body which can be positioned
Created in NX3.0.0.
NXOpen::ExpressionDepth ()
 Returns the depth of the hole.
NXOpen::ExpressionDiameter ()
 Returns the diameter of the hole.
NXOpen::BodyGetTargetBody ()
 Returns target body for the hole.
NXOpen::ISurfaceGetThruFace ()
 Returns thru face parameter for the hole.
NXOpen::Point3d HoleLocation ()
 Returns the reference point of the hole.
NXOpen::ISurfacePlacementFace ()
 Returns the placement face of the hole.
bool ReverseDirection ()
 Returns the reverse direction flag of the hole.
void SetCounterboreDepth (const NXString &depth)
 Sets the depth of the counterbore for a hole.
void SetCounterboreDiameter (const NXString &diameter)
 Sets the diameter of the counterbore for a hole.
void SetCounterboreHole (const NXOpen::Point3d &referencePoint, bool reverseDirection, NXOpen::ISurface *placementFace, const NXString &diameter, const NXString &counterboreDiameter, const NXString &counterboreDepth)
 Sets parameters for counterbore hole
Created in NX3.0.0.
void SetCountersinkAngle (const NXString &angle)
 Sets the angle of the countersink for a hole.
void SetCountersinkDiameter (const NXString &diameter)
 Sets the diameter of the countersink for a hole.
void SetCountersinkHole (const NXOpen::Point3d &referencePoint, bool reverseDirection, NXOpen::ISurface *placementFace, const NXString &diameter, const NXString &countersinkDiameter, const NXString &countersinkAngle)
 Sets parameters for countersink hole
Created in NX3.0.0.
void SetDepth (const NXString &depth)
 Sets the depth of the hole.
void SetDepthAndTipAngle (const NXString &depth, const NXString &tipAngle)
 Sets depth and tip angle parameters for the hole.
void SetDiameter (const NXString &diameter)
 Sets the diameter of the hole.
void SetHoleLocation (const NXOpen::Point3d &referencePoint)
 Sets the reference point of the hole.
void SetPlacementFace (NXOpen::ISurface *placementFace)
 Sets the placement face of the hole.
void SetReverseDirection (bool reverse)
 Sets the reverse direction flag of the hole.
void SetSimpleHole (const NXOpen::Point3d &referencePoint, bool reverseDirection, NXOpen::ISurface *placementFace, const NXString &diameter)
 Sets parameters for simple hole
Created in NX3.0.0.
void SetSubtype (NXOpen::Features::HoleFeatureBuilder::HoleSubtype subtype)
 Sets the type of hole.
void SetTargetBody (NXOpen::Body *targetBody)
 Sets target body for the hole.
void SetThruFace (NXOpen::ISurface *thruFace)
 Sets thru face parameter for the hole.
void SetTipAngle (const NXString &tipAngle)
 Sets the tip angle of the hole.
NXOpen::Features::HoleFeatureBuilder::HoleSubtype Subtype ()
 Returns the type of hole.
NXOpen::ExpressionTipAngle ()
 Returns the tip angle of the hole.

Detailed Description

Represents a Hole feature builder.

See RPOBuilder for details on positioning the hole.
To create a new instance of this class, use Features::FeatureCollection::CreateHoleFeatureBuilder

Created in NX3.0.0.


Member Enumeration Documentation

Represents the subtype of the hole.

Enumerator:
HoleSubtypeSimple 

Simple hole.

HoleSubtypeCounterbore 

Counterbore hole.

HoleSubtypeCountersink 

Countersink hole.


Member Function Documentation

Returns the depth of the counterbore for a hole.

Only used if the hole type is couterbore


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Returns the diameter of the counterbore for a hole.

Only used if the hole type is couterbore


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Returns the angle of the countersink for a hole.

Only used if the hole type is coutersink


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Returns the diameter of the countersink for a hole.

Only used if the hole type is coutersink


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Creates a hole body which can be positioned
Created in NX3.0.0.



License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Returns the depth of the hole.

If this parameter is set then the thru face is ignored.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Returns the diameter of the hole.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Returns target body for the hole.

If this parameter is set then depth and tip angle are ignored and will prompt for thru_face.

Returns:
Target Body
Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Returns thru face parameter for the hole.

If this parameter is set then depth and tip angle are ignored.

Returns:
Thru face
Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Returns the reference point of the hole.

This parameter will position the hole unless relative positioning dimensions are used


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Returns the placement face of the hole.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Returns the reverse direction flag of the hole.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Sets the depth of the counterbore for a hole.

Only used if the hole type is couterbore


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
depthcounterbore depth
NOTE: The full Unicode character set is not supported for this parameter.

Sets the diameter of the counterbore for a hole.

Only used if the hole type is couterbore


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
diameterHole diameter
NOTE: The full Unicode character set is not supported for this parameter.
void NXOpen::Features::HoleFeatureBuilder::SetCounterboreHole ( const NXOpen::Point3d referencePoint,
bool  reverseDirection,
NXOpen::ISurface placementFace,
const NXString diameter,
const NXString counterboreDiameter,
const NXString counterboreDepth 
)

Sets parameters for counterbore hole
Created in NX3.0.0.



License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
referencePointReference point for the hole
reverseDirectionReverse direction flag, applicable only if placement face is a datum plane
placementFacePlacement face
diameterHole diameter
NOTE: The full Unicode character set is not supported for this parameter.
counterboreDiameterCounterbore diameter
NOTE: The full Unicode character set is not supported for this parameter.
counterboreDepthCounterbore depth
NOTE: The full Unicode character set is not supported for this parameter.

Sets the angle of the countersink for a hole.

Only used if the hole type is coutersink


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
anglecountersink angle
NOTE: The full Unicode character set is not supported for this parameter.

Sets the diameter of the countersink for a hole.

Only used if the hole type is coutersink


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
diameterHole diameter
NOTE: The full Unicode character set is not supported for this parameter.
void NXOpen::Features::HoleFeatureBuilder::SetCountersinkHole ( const NXOpen::Point3d referencePoint,
bool  reverseDirection,
NXOpen::ISurface placementFace,
const NXString diameter,
const NXString countersinkDiameter,
const NXString countersinkAngle 
)

Sets parameters for countersink hole
Created in NX3.0.0.



License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
referencePointReference point for the hole
reverseDirectionReverse direction flag, applicable only if placement face is a datum plane
placementFacePlacement face
diameterHole diameter
NOTE: The full Unicode character set is not supported for this parameter.
countersinkDiameterCountersink diameter
NOTE: The full Unicode character set is not supported for this parameter.
countersinkAngleCountersink angle
NOTE: The full Unicode character set is not supported for this parameter.

Sets the depth of the hole.

If this parameter is set then the thru face is ignored.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
depthHole depth
NOTE: The full Unicode character set is not supported for this parameter.
void NXOpen::Features::HoleFeatureBuilder::SetDepthAndTipAngle ( const NXString depth,
const NXString tipAngle 
)

Sets depth and tip angle parameters for the hole.


Created in NX3.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
depthHole depth
NOTE: The full Unicode character set is not supported for this parameter.
tipAngleTip angle of the tool
NOTE: The full Unicode character set is not supported for this parameter.

Sets the diameter of the hole.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
diameterHole diameter
NOTE: The full Unicode character set is not supported for this parameter.

Sets the reference point of the hole.

This parameter will position the hole unless relative positioning dimensions are used


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
referencePointReference point for the hole

Sets the placement face of the hole.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
placementFacePlacement face

Sets the reverse direction flag of the hole.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
reversereverse
void NXOpen::Features::HoleFeatureBuilder::SetSimpleHole ( const NXOpen::Point3d referencePoint,
bool  reverseDirection,
NXOpen::ISurface placementFace,
const NXString diameter 
)

Sets parameters for simple hole
Created in NX3.0.0.



License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
referencePointReference point for the hole
reverseDirectionReverse direction flag, applicable only if placement face is a datum plane
placementFacePlacement face
diameterHole diameter
NOTE: The full Unicode character set is not supported for this parameter.

Sets the type of hole.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
subtypesubtype

Sets target body for the hole.

If this parameter is set then depth and tip angle are ignored and will prompt for thru_face.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
targetBodyTarget Body

Sets thru face parameter for the hole.

If this parameter is set then depth and tip angle are ignored.


Created in NX3.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
thruFaceThru face

Sets the tip angle of the hole.

If this parameter is set then the thru face is ignored.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Parameters:
tipAngleTip angle
NOTE: The full Unicode character set is not supported for this parameter.

Returns the type of hole.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")

Returns the tip angle of the hole.

If this parameter is set then the thru face is ignored.


Created in NX4.0.0.

License requirements : features_modeling ("FEATURES MODELING"), 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.