Represents a builder for a NXOpen::Features::Thicken feature. More...

Inheritance diagram for NXOpen::Features::ThickenBuilder:

Public Member Functions
bool	ApproximateOffset ()
	Returns the "approximate offset surface" or "resolve self-intersections using patches" option. More...

NXOpen::GeometricUtilities::BooleanOperation *	BooleanOperation ()
	Returns the boolean operation. More...

NXOpen::ScCollector *	FaceCollector ()
	Returns the faces to thicken. More...

NXOpen::Expression *	FirstOffset ()
	Returns the first offset. More...

NXOpen::GeometricUtilities::TwoExpressionsSectionSetList *	RegionSectionList ()
	Returns the list of SC_section The sections with corresponding expression for the Thicken feature Created in NX9.0.0. More...

NXOpen::Section *	RegionToPierce ()
	Returns the section for regions to pierce The section associated for the Thicken feature Created in NX9.0.0. More...

bool	RemoveGashes ()
	Returns the remove gashes option. More...

bool	ReverseDirection ()
	Returns the reverse direction. More...

NXOpen::Expression *	SecondOffset ()
	Returns the second offset. More...

void	SetApproximateOffset (bool approximateOffset)
	Sets the "approximate offset surface" or "resolve self-intersections using patches" option. More...

void	SetRemoveGashes (bool removeGashes)
	Sets the remove gashes option. More...

void	SetReverseDirection (bool reverseDirection)
	Sets the reverse direction. More...

void	SetTolerance (double tolerance)
	Sets the tolerance. More...

double	Tolerance ()
	Returns the tolerance. More...

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

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

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

bool	ParentFeatureInternal ()
	Returns whether or not the latest timestamped parent feature of this feature should be made internal Created in NX5.0.0. More...

bool	PatchSolutionFlag ()
	Returns the patch solution flag Created in NX8.0.1. More...

NXString	PatchSurfaceFilename ()
	Returns the patch surface filename Created in NX8.0.1. More...

void	SetParentFeatureInternal (NXOpen::Features::Feature *parentFeature)
	Set the parent features which would be internal or slaves to the feature being created or commited Created in NX6.0.0. More...

void	SetParentFeatureInternal (bool isInternal)
	Sets whether or not the latest timestamped parent feature of this feature should be made internal Created in NX5.0.0. More...

void	SetPatchSolutionFlag (bool optionValue)
	Sets the patch solution flag Created in NX8.0.1. More...

void	SetPatchSurfaceFilename (const NXString &surfaceFilename)
	Sets the patch surface filename Created in NX8.0.1. More...

void	SetPatchSurfaceFilename (const char *surfaceFilename)
	Sets the patch surface filename Created in NX8.0.1. More...

void	SetSurroundingPatchSurfaceFilename (const NXString &surroundingSurfaceFilename)
	Sets the surrounding patch surface filename Created in NX8.0.1. More...

void	SetSurroundingPatchSurfaceFilename (const char *surroundingSurfaceFilename)
	Sets the surrounding patch surface filename Created in NX8.0.1. More...

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

NXString	SurroundingPatchSurfaceFilename ()
	Returns the surrounding patch surface filename Created in NX8.0.1. More...

void	UnsetParentFeatureInternal (NXOpen::Features::Feature *parentFeature)
	Set the internal parent feature of the feature being edited to external Created in NX6.0.0. More...

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

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

std::vector< NXOpen::NXObject * >	GetCommittedObjects ()
	For builders that create more than one object, this method returns the objects that are created by commit. More...

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

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

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

Public Member Functions inherited from NXOpen::TaggedObject
tag_t	Tag () const
	Returns the tag of this object. More...

Detailed Description

Represents a builder for a NXOpen::Features::Thicken feature.

This allows creation and editing of a Thicken feature which takes a set of faces and offsets them along their normals to create a solid body which has constant thickness. Since this can not be done precisely for the supported geometry types there is a tolerance to specify the accuracy of the result. Inputs to this class can be convergent objects.
To create a new instance of this class, use NXOpen::Features::FeatureCollection::CreateThickenBuilder
Default values.

Property

Value

ApproximateOffset

True

BooleanOperation.Type

Create

FirstOffset.Value

2.5 (millimeters part), 0.1 (inches part)

RemoveGashes

False

ReverseDirection

False

SecondOffset.Value

0.0 (millimeters part), 0.0 (inches part)

Created in NX5.0.0.

Member Function Documentation

bool NXOpen::Features::ThickenBuilder::ApproximateOffset ( )

Returns the "approximate offset surface" or "resolve self-intersections using patches" option.

The option to approximate offset surfaces for thickening operation is renamed to "resolve self-intersections using patches". This option is available for editing pre-NX8 thicken features only. The value set by the user for this option is ignored for thicken features created from NX8 onwards and its value will always be set to true internally for thicken features created in NX8 and later.
Created in NX5.0.0.

License requirements : None

NXOpen::GeometricUtilities::BooleanOperation* NXOpen::Features::ThickenBuilder::BooleanOperation ( )

Returns the boolean operation.

The boolean operation associated with the Thicken feature
Created in NX5.0.0.

License requirements : None

NXOpen::ScCollector* NXOpen::Features::ThickenBuilder::FaceCollector ( )

Returns the faces to thicken.

A list of one or more faces to thicken.
Created in NX5.0.0.

License requirements : None

NXOpen::Expression* NXOpen::Features::ThickenBuilder::FirstOffset ( )

Returns the first offset.

The first offset for the Thicken feature. A positive value is applied along the normal of the face to be thickened. Negative values are applied in the opposite direction. The difference between the first and second offset must be non-zero.
Created in NX5.0.0.

License requirements : None

NXOpen::GeometricUtilities::TwoExpressionsSectionSetList* NXOpen::Features::ThickenBuilder::RegionSectionList ( )

Returns the list of SC_section The sections with corresponding expression for the Thicken feature
Created in NX9.0.0.

License requirements : None

NXOpen::Section* NXOpen::Features::ThickenBuilder::RegionToPierce ( )

Returns the section for regions to pierce The section associated for the Thicken feature
Created in NX9.0.0.

License requirements : None

bool NXOpen::Features::ThickenBuilder::RemoveGashes ( )

Returns the remove gashes option.

If the option is selected, Thicken will heal the input and attempt the operation on the healed input. If after healing the input, the Thicken operation succeeds, the Part Navigator will indicate as such with an information symbol and an entry in the Alert column.
Created in NX8.0.0.

License requirements : None

bool NXOpen::Features::ThickenBuilder::ReverseDirection ( )

Returns the reverse direction.

A flag to indicate whether the offset direction is reversed with respect to the normal of the face to be thickened.
Created in NX5.0.0.

License requirements : None

NXOpen::Expression* NXOpen::Features::ThickenBuilder::SecondOffset ( )

Returns the second offset.

the second offset for the Thicken feature.
Created in NX5.0.0.

License requirements : None

void NXOpen::Features::ThickenBuilder::SetApproximateOffset ( bool approximateOffset )

Sets the "approximate offset surface" or "resolve self-intersections using patches" option.

The option to approximate offset surfaces for thickening operation is renamed to "resolve self-intersections using patches". This option is available for editing pre-NX8 thicken features only. The value set by the user for this option is ignored for thicken features created from NX8 onwards and its value will always be set to true internally for thicken features created in NX8 and later.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

approximateOffset approximateoffset

void NXOpen::Features::ThickenBuilder::SetRemoveGashes ( bool removeGashes )

Sets the remove gashes option.

If the option is selected, Thicken will heal the input and attempt the operation on the healed input. If after healing the input, the Thicken operation succeeds, the Part Navigator will indicate as such with an information symbol and an entry in the Alert column.
Created in NX8.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

removeGashes removegashes

void NXOpen::Features::ThickenBuilder::SetReverseDirection ( bool reverseDirection )

Sets the reverse direction.

A flag to indicate whether the offset direction is reversed with respect to the normal of the face to be thickened.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

reverseDirection reversedirection

void NXOpen::Features::ThickenBuilder::SetTolerance ( double tolerance )

Sets the tolerance.

The maximum allowable distance between the true theoretical sheet and the body created to approximate it.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR cam_base ("CAM BASE") OR insp_programming ("INSPECTION PROGRAMMING")

Parameters

tolerance tolerance

double NXOpen::Features::ThickenBuilder::Tolerance ( )

Returns the tolerance.

The maximum allowable distance between the true theoretical sheet and the body created to approximate it.
Created in NX5.0.0.

License requirements : None

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

Features_ThickenBuilder.hxx

Public Member Functions

Detailed Description

Member Function Documentation