NXOpen::Features::SweptBuilder Class Reference

Represents a NXOpen::Features::Swept builder
To create a new instance of this class, use NXOpen::Features::FeatureCollection::CreateSweptBuilder
Default values. More...

Inheritance diagram for NXOpen::Features::SweptBuilder:

Public Types
enum	InterpolationOptions { InterpolationOptionsLinear, InterpolationOptionsCubic, InterpolationOptionsBlend }
	This enum represents the Interpolation option. More...
enum	SectionLocationTypes { SectionLocationTypesAnywhereAlongGuides, SectionLocationTypesEndsOfGuides }
	This enum represents the Section Location option. More...

Public Member Functions
NXOpen::GeometricUtilities::AlignmentMethodBuilder *	AlignmentMethod ()
	Returns the alignment method. More...
NXOpen::GeometricUtilities::FeatureOptions *	BodyPreference ()
	Returns the body type options Created in NX7.5.0. More...
double	G0Tolerance ()
	Returns the G0 (Position) tolerance. More...
double	G1Tolerance ()
	Returns the G1 (Tangent) tolerance. More...
NXOpen::SectionList *	GuideList ()
	Returns the list of guides. More...
NXOpen::GeometricUtilities::Rebuild *	GuideRebuildData ()
	Returns the guide rebuild data Created in NX5.0.0. More...
NXOpen::Features::SweptBuilder::InterpolationOptions	InterpolationOption ()
	Returns the interpolation option. More...
NXOpen::GeometricUtilities::OrientationMethodBuilder *	OrientationMethod ()
	Returns the orientation method. More...
bool	PreserveGuideShapeOption ()
	Returns the preserve guide shape option. More...
bool	PreserveShapeOption ()
	Returns the preserve shape option. More...
NXOpen::GeometricUtilities::ScalingMethodBuilder *	ScalingMethod ()
	Returns the scaling method. More...
NXOpen::SectionList *	SectionList ()
	Returns the list of sections. More...
NXOpen::Features::SweptBuilder::SectionLocationTypes	SectionLocation ()
	Returns the section location option. More...
NXOpen::GeometricUtilities::Rebuild *	SectionRebuildData ()
	Returns the section rebuild data Created in NX5.0.0. More...
void	SetG0Tolerance (double g0Tolerance)
	Sets the G0 (Position) tolerance. More...
void	SetG1Tolerance (double g1Tolerance)
	Sets the G1 (Tangent) tolerance. More...
void	SetInterpolationOption (NXOpen::Features::SweptBuilder::InterpolationOptions interpolationOption)
	Sets the interpolation option. More...
void	SetPreserveGuideShapeOption (bool preserveGuideShapeOption)
	Sets the preserve guide shape option. More...
void	SetPreserveShapeOption (bool preserveShapeOption)
	Sets the preserve shape option. More...
void	SetSectionLocation (NXOpen::Features::SweptBuilder::SectionLocationTypes sectionLocation)
	Sets the section location option. More...
NXOpen::Section *	Spine ()
	Returns the spine (optional). 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 NXOpen::Features::Swept builder
To create a new instance of this class, use NXOpen::Features::FeatureCollection::CreateSweptBuilder
Default values.

Property	Value
AlignmentMethod.AlignType	Parameter
GuideRebuildData.Degree	3
GuideRebuildData.RebuildType	None
OrientationMethod.AngularLaw.EndValue.Value	0 (millimeters part), 0 (inches part)
OrientationMethod.AngularLaw.Function	ft
OrientationMethod.AngularLaw.LawType	Constant
OrientationMethod.AngularLaw.Parameter	t
OrientationMethod.AngularLaw.StartValue.Value	0 (millimeters part), 0 (inches part)
OrientationMethod.AngularLaw.Value.Value	0 (millimeters part), 0 (inches part)
OrientationMethod.OrientationOption	Fixed
PreserveGuideShapeOption	False
PreserveShapeOption	True
ScalingMethod.AreaLaw.EndValue.Value	1.0 (millimeters part), 1.0 (inches part)
ScalingMethod.AreaLaw.StartValue.Value	1.0 (millimeters part), 1.0 (inches part)
ScalingMethod.AreaLaw.Value.Value	1.0 (millimeters part), 1.0 (inches part)
ScalingMethod.BlendingFunctionType	Linear
ScalingMethod.EndBlendScaleFactor	1.0
ScalingMethod.PerimeterLaw.EndValue.Value	1.0 (millimeters part), 1.0 (inches part)
ScalingMethod.PerimeterLaw.StartValue.Value	1.0 (millimeters part), 1.0 (inches part)
ScalingMethod.PerimeterLaw.Value.Value	1.0 (millimeters part), 1.0 (inches part)
ScalingMethod.ScaleFactor	1.0
ScalingMethod.ScalingOption	Constant
ScalingMethod.StartBlendScaleFactor	1.0
SectionRebuildData.Degree	3
SectionRebuildData.RebuildType	None

Created in NX5.0.0.

Member Enumeration Documentation

enum NXOpen::Features::SweptBuilder::InterpolationOptions

This enum represents the Interpolation option.

For 2 or more sections, this option specifies the method by which to interpolate between them, either Linear or Cubic.

Enumerator
InterpolationOptionsLinear	Linear.
InterpolationOptionsCubic	Cubic.
InterpolationOptionsBlend	Blend.

enum NXOpen::Features::SweptBuilder::SectionLocationTypes

This enum represents the Section Location option.

If a single section located at the middle of a guide string is specified, Anywhere Along Guides option sweeps in both directions.

Enumerator
SectionLocationTypesAnywhereAlongGuides	Anywhere along Guides.
SectionLocationTypesEndsOfGuides	Ends of Guides.

Member Function Documentation

NXOpen::GeometricUtilities::AlignmentMethodBuilder* NXOpen::Features::SweptBuilder::AlignmentMethod

(

)

Returns the alignment method.

The Alignment Method Builder sub-object, governs the alignment of the input sections along the guides. Alignment by Points is available only if more than 1 input sections are selected. Refer to GeometricUtilities.AlignmentMethodBuilder documentation.
Created in NX5.0.0.

License requirements : None

NXOpen::GeometricUtilities::FeatureOptions* NXOpen::Features::SweptBuilder::BodyPreference

(

)

Returns the body type options
Created in NX7.5.0.

License requirements : None

double NXOpen::Features::SweptBuilder::G0Tolerance

(

)

Returns the G0 (Position) tolerance.

Created in NX5.0.0.

License requirements : None

double NXOpen::Features::SweptBuilder::G1Tolerance

(

)

Returns the G1 (Tangent) tolerance.

Created in NX5.0.0.

License requirements : None

NXOpen::SectionList* NXOpen::Features::SweptBuilder::GuideList

(

)

Returns the list of guides.

At least 1 but no more than 3 guides are required.
Created in NX5.0.0.

License requirements : None

NXOpen::GeometricUtilities::Rebuild* NXOpen::Features::SweptBuilder::GuideRebuildData

(

)

Returns the guide rebuild data
Created in NX5.0.0.

License requirements : None

NXOpen::Features::SweptBuilder::InterpolationOptions NXOpen::Features::SweptBuilder::InterpolationOption

(

)

Returns the interpolation option.

This option governs the method by which to interpolate between sections, if the section list contains more than 1 section.
Created in NX5.0.0.

License requirements : None

NXOpen::GeometricUtilities::OrientationMethodBuilder* NXOpen::Features::SweptBuilder::OrientationMethod

(

)

Returns the orientation method.

The Orientation Method Builder sub-object, governs the orientation of the input sections, if the guide list contains a single guide. Refer to GeometricUtilities.OrientationMethodBuilder documentation.
Created in NX5.0.0.

License requirements : None

bool NXOpen::Features::SweptBuilder::PreserveGuideShapeOption

(

)

Returns the preserve guide shape option.

Created in NX8.5.0.

License requirements : None

bool NXOpen::Features::SweptBuilder::PreserveShapeOption

(

)

Returns the preserve shape option.

Created in NX5.0.0.

License requirements : None

NXOpen::GeometricUtilities::ScalingMethodBuilder* NXOpen::Features::SweptBuilder::ScalingMethod

(

)

Returns the scaling method.

The Scaling Method Builder sub-object, governs the size / scale of the input sections along a guide, if a single guide is selected. Refer to GeometricUtilities.ScalingMethodBuilder documentation.
Created in NX5.0.0.

License requirements : None

NXOpen::SectionList* NXOpen::Features::SweptBuilder::SectionList

(

)

Returns the list of sections.

At least 1 section is required.
Created in NX5.0.0.

License requirements : None

NXOpen::Features::SweptBuilder::SectionLocationTypes NXOpen::Features::SweptBuilder::SectionLocation

(

)

Returns the section location option.

This option governs the location of the input section with respect to the guides. The section location option is ignored if the section list contains more than 1 section.
Created in NX5.0.0.

License requirements : None

NXOpen::GeometricUtilities::Rebuild* NXOpen::Features::SweptBuilder::SectionRebuildData

(

)

Returns the section rebuild data
Created in NX5.0.0.

License requirements : None

void NXOpen::Features::SweptBuilder::SetG0Tolerance

(

double

g0Tolerance

)

Sets the G0 (Position) tolerance.

Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

g0Tolerance

g0tolerance

void NXOpen::Features::SweptBuilder::SetG1Tolerance

(

double

g1Tolerance

)

Sets the G1 (Tangent) tolerance.

Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

g1Tolerance

g1tolerance

void NXOpen::Features::SweptBuilder::SetInterpolationOption

(

NXOpen::Features::SweptBuilder::InterpolationOptions

interpolationOption

)

Sets the interpolation option.

This option governs the method by which to interpolate between sections, if the section list contains more than 1 section.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

interpolationOption

interpolationoption

void NXOpen::Features::SweptBuilder::SetPreserveGuideShapeOption

(

bool

preserveGuideShapeOption

)

Sets the preserve guide shape option.

Created in NX8.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

preserveGuideShapeOption

preserveguideshapeoption

void NXOpen::Features::SweptBuilder::SetPreserveShapeOption

(

bool

preserveShapeOption

)

Sets the preserve shape option.

Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

preserveShapeOption

preserveshapeoption

void NXOpen::Features::SweptBuilder::SetSectionLocation

(

NXOpen::Features::SweptBuilder::SectionLocationTypes

sectionLocation

)

Sets the section location option.

This option governs the location of the input section with respect to the guides. The section location option is ignored if the section list contains more than 1 section.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters

sectionLocation

sectionlocation

NXOpen::Section* NXOpen::Features::SweptBuilder::Spine

(

)

Returns the spine (optional).

For more than 1 guide, an optional spine curve can be input to gain further control of the orientation of the section string. The spine curve cannot contain more than 1 loop.
Created in NX5.0.0.

License requirements : None

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

• Features_SweptBuilder.hxx