Represents a NXOpen::SketchOffsetBuilder
To create a new instance of this class, use NXOpen::SketchCollection::CreateSketchOffsetBuilder
Default values. More...

Inheritance diagram for NXOpen::SketchOffsetBuilder:

Public Member Functions
void	BreakChain (NXOpen::NXObject object1, NXOpen::NXObject object2, const NXOpen::Point3d &helpPt)
	This function breaks the base chain and all the associated offsets at a given location Created in NX5.0.0. More...

NXOpen::SketchOffset::CapType	CapType ()
	Returns the type of the cap needed at the corners Created in NX5.0.0. More...

bool	ConvertToReference ()
	Returns the flag to indicate if the input curves needs to converted to reference Created in NX5.0.0. More...

bool	CreateDimension ()
	Returns the flag to create offset with a dimension or a dimensionless offset Created in NX5.0.0. More...

NXOpen::Section *	CreateSection ()
	The function creates a new empty section object and adds it to the builder. More...

int	Degree ()
	Returns the degree for approximating offset spline Created in NX5.0.0. More...

NXOpen::Expression *	Distance ()
	Returns the offset distance expression Created in NX5.0.0. More...

void	EvaluateOffset ()
	This function will solve the offset constraint to update it based on the new data set in the builder Created in NX8.5.0. More...

std::vector< NXOpen::NXObject * >	GetOutputCurvesOfOffset ()
	This function gets all output curves of an offset. More...

std::vector< NXOpen::Section * >	GetSections ()
	This function gets all sections of an offset during create/edit. More...

bool	IsSymmetric ()
	Returns the flag to indicate if the offset needs to be symmetric or not Created in NX5.0.0. More...

void	MergeChains (NXOpen::NXObject object1, NXOpen::NXObject object2, const NXOpen::Point3d &helpPt)
	This function merges the two chains. More...

int	NumberOfCopies ()
	Returns the number of offset copies Created in NX5.0.0. More...

void	RemoveSection (NXOpen::Section *section)
	The function removes the given section from the builder Created in NX5.0.0. More...

void	ReverseOffsetDirectionOfChain (NXOpen::NXObject *objectInChain)
	This function reverses the offset direction of the chain containing the input geometry Created in NX5.0.0. More...

void	SetCapType (NXOpen::SketchOffset::CapType capType)
	Sets the type of the cap needed at the corners Created in NX5.0.0. More...

void	SetConvertToReference (bool reference)
	Sets the flag to indicate if the input curves needs to converted to reference Created in NX5.0.0. More...

void	SetCreateDimension (bool createDim)
	Sets the flag to create offset with a dimension or a dimensionless offset Created in NX5.0.0. More...

void	SetDegree (int degree)
	Sets the degree for approximating offset spline Created in NX5.0.0. More...

void	SetEndConstraint (NXOpen::NXObject *objectInChain, int inx, bool isStartEnd, bool constraint)
	This function removes end constraint from the given offset Created in NX5.0.0. More...

void	SetNumberOfCopies (int copies)
	Sets the number of offset copies Created in NX5.0.0. More...

void	SetSymmetric (bool symmetric)
	Sets the flag to indicate if the offset needs to be symmetric or not Created in NX5.0.0. More...

void	SetTolerance (double tolerance)
	Sets the tolerance for approximating offset spline Created in NX5.0.0. More...

double	Tolerance ()
	Returns the tolerance for approximating offset spline Created in NX5.0.0. More...

void	UpdateLoopsAndCopies ()
	This function will update the offset after curves are selected. More...

void	UpdateSolverDistance ()
	This function will update the distance in the sketch solver using the new data set in the builder Created in NX11.0.0. 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::SketchOffsetBuilder
To create a new instance of this class, use NXOpen::SketchCollection::CreateSketchOffsetBuilder
Default values.

Property

Value

CapType

Extension

ConvertToReference

False

CreateDimension

True

Degree

3

Distance.Value

5.0 (millimeters part), 2.0 (inches part)

IsSymmetric

False

NumberOfCopies

1

Created in NX5.0.0.

Member Function Documentation

void NXOpen::SketchOffsetBuilder::BreakChain	(	NXOpen::NXObject *	object1,
		NXOpen::NXObject *	object2,
		const NXOpen::Point3d &	helpPt
	)

This function breaks the base chain and all the associated offsets at a given location
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

object1	An object in chain to break
object2	Adjacent object to the previous one
helpPt	Help point for multiple intersections

NXOpen::SketchOffset::CapType NXOpen::SketchOffsetBuilder::CapType ( )

Returns the type of the cap needed at the corners
Created in NX5.0.0.

License requirements : None

bool NXOpen::SketchOffsetBuilder::ConvertToReference ( )

Returns the flag to indicate if the input curves needs to converted to reference
Created in NX5.0.0.

License requirements : None

bool NXOpen::SketchOffsetBuilder::CreateDimension ( )

Returns the flag to create offset with a dimension or a dimensionless offset
Created in NX5.0.0.

License requirements : None

NXOpen::Section* NXOpen::SketchOffsetBuilder::CreateSection ( )

The function creates a new empty section object and adds it to the builder.

Returns: New section object
Created in NX5.0.0.

License requirements : None

int NXOpen::SketchOffsetBuilder::Degree ( )

Returns the degree for approximating offset spline
Created in NX5.0.0.

License requirements : None

NXOpen::Expression* NXOpen::SketchOffsetBuilder::Distance ( )

Returns the offset distance expression
Created in NX5.0.0.

License requirements : None

void NXOpen::SketchOffsetBuilder::EvaluateOffset ( )

This function will solve the offset constraint to update it based on the new data set in the builder
Created in NX8.5.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

std::vector<NXOpen::NXObject *> NXOpen::SketchOffsetBuilder::GetOutputCurvesOfOffset ( )

This function gets all output curves of an offset.

Returns: All the curves associated with constraint
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

std::vector<NXOpen::Section *> NXOpen::SketchOffsetBuilder::GetSections ( )

This function gets all sections of an offset during create/edit.

Returns: All the sections associated with the builder
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

bool NXOpen::SketchOffsetBuilder::IsSymmetric ( )

Returns the flag to indicate if the offset needs to be symmetric or not
Created in NX5.0.0.

License requirements : None

void NXOpen::SketchOffsetBuilder::MergeChains	(	NXOpen::NXObject *	object1,
		NXOpen::NXObject *	object2,
		const NXOpen::Point3d &	helpPt
	)

This function merges the two chains.

The last geom of first chain and first geom of next chain are taken as input.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

object1	Last geom of first chain
object2	First geom of next chain
helpPt	Help point for multiple intersections

int NXOpen::SketchOffsetBuilder::NumberOfCopies ( )

Returns the number of offset copies
Created in NX5.0.0.

License requirements : None

void NXOpen::SketchOffsetBuilder::RemoveSection ( NXOpen::Section * section )

The function removes the given section from the builder
Created in NX5.0.0.

License requirements : None

Parameters

section Section obj to remove

void NXOpen::SketchOffsetBuilder::ReverseOffsetDirectionOfChain ( NXOpen::NXObject * objectInChain )

This function reverses the offset direction of the chain containing the input geometry
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

objectInChain An object in chain to reverse

void NXOpen::SketchOffsetBuilder::SetCapType ( NXOpen::SketchOffset::CapType capType )

Sets the type of the cap needed at the corners
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

capType captype

void NXOpen::SketchOffsetBuilder::SetConvertToReference ( bool reference )

Sets the flag to indicate if the input curves needs to converted to reference
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

reference reference

void NXOpen::SketchOffsetBuilder::SetCreateDimension ( bool createDim )

Sets the flag to create offset with a dimension or a dimensionless offset
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

createDim createdim

void NXOpen::SketchOffsetBuilder::SetDegree ( int degree )

Sets the degree for approximating offset spline
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

degree degree

void NXOpen::SketchOffsetBuilder::SetEndConstraint	(	NXOpen::NXObject *	objectInChain,
		int	inx,
		bool	isStartEnd,
		bool	constraint
	)

This function removes end constraint from the given offset
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

objectInChain	An object in the base chain
inx	Index of the constraint - starts from 0
isStartEnd	TRUE, if we want to remove the start end con
constraint	TRUE to add the con, false to remove

void NXOpen::SketchOffsetBuilder::SetNumberOfCopies ( int copies )

Sets the number of offset copies
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

copies copies

void NXOpen::SketchOffsetBuilder::SetSymmetric ( bool symmetric )

Sets the flag to indicate if the offset needs to be symmetric or not
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

symmetric symmetric

void NXOpen::SketchOffsetBuilder::SetTolerance ( double tolerance )

Sets the tolerance for approximating offset spline
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

Parameters

tolerance tolerance

double NXOpen::SketchOffsetBuilder::Tolerance ( )

Returns the tolerance for approximating offset spline
Created in NX5.0.0.

License requirements : None

void NXOpen::SketchOffsetBuilder::UpdateLoopsAndCopies ( )

This function will update the offset after curves are selected.

If the input section is updated to add/remove curves, this function must be called to update the offset constraint. This function will keep the offset constraint synchronised with the edits done to input section.
Created in NX8.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

void NXOpen::SketchOffsetBuilder::UpdateSolverDistance ( )

This function will update the distance in the sketch solver using the new data set in the builder
Created in NX11.0.0.

License requirements : solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")

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

SketchOffsetBuilder.hxx

Public Member Functions

Detailed Description

Member Function Documentation