Represents a Flange feature builder. More...

Inheritance diagram for NXOpen::Features::SheetMetal::FlangeBuilder:

Public Types
enum	InsetTypeOptions { InsetTypeOptionsMaterialInside, InsetTypeOptionsMaterialOutside, InsetTypeOptionsBendOutside }
	This enum represents the inset type for the material of the flange. More...

enum	LengthTypeOptions { LengthTypeOptionsInsideDimension, LengthTypeOptionsOutsideDimension, LengthTypeOptionsWebDimension }
	This enum indicates the two ways that the flange length can be measured. More...

enum	MatchFaceOptions { MatchFaceOptionsNone, MatchFaceOptionsUntilSelected }
	This enum represents the match face option for the flange. More...

enum	OffsetTypeOptions { OffsetTypeOptionsInside, OffsetTypeOptionsOutside }
	This enum represents the offset type for the flange. More...

enum	WidthTypeOptions { WidthTypeOptionsFullEdge, WidthTypeOptionsCenterOfEdge, WidthTypeOptionsAtEdgeEnd, WidthTypeOptionsFromEdgeEnd, WidthTypeOptionsFromBothEnds, WidthTypeOptionsCustom }
	This enum represents the width type for the flange. More...

Public Member Functions
NXOpen::Expression *	BendAngle ()
	Returns the bend angle for flange. More...

NXOpen::Features::SheetMetal::BendOptions *	BendOptions ()
	Returns the bend options object. More...

void	DeleteSketch ()
	Delete the flange sketch Created in NX6.0.0. More...

NXOpen::Edge *	Edge ()
	Returns the edge on which the flange is created. More...

void	EditSketch ()
	Edit the sketch base on a new edge you need to call SetEdge to set a new edge Created in NX6.0.0. More...

NXOpen::Expression *	FirstDistance ()
	Returns a distance based on NXOpen::Features::SheetMetal::FlangeBuilder::WidthType . More...

NXOpen::Sketch *	GetSketch ()
	Get the flange sketch. More...

NXOpen::Features::SheetMetal::FlangeBuilder::InsetTypeOptions	InsetType ()
	Returns the inset type (inside, outside, bendoutside) for the flange. More...

NXOpen::Expression *	Length ()
	Returns the length of the flange. More...

NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptions	LengthType ()
	Returns a enum indicating the length type. More...

NXOpen::Features::SheetMetal::FlangeBuilder::MatchFaceOptions	MatchFaceOption ()
	Returns the match face selection type. More...

NXOpen::Plane *	MatchPlane ()
	Returns the Match Plane. More...

NXOpen::Expression *	Offset ()
	Returns the offset value for the flange. More...

NXOpen::Features::SheetMetal::FlangeBuilder::OffsetTypeOptions	OffsetType ()
	Returns the offset type for the flange. More...

NXOpen::Expression *	SecondDistance ()
	Returns a distance based on NXOpen::Features::SheetMetal::FlangeBuilder::WidthType . More...

void	SetBendAngle (const NXString &bendAngle)
	More...

void	SetBendAngle (const char *bendAngle)
	More...

void	SetEdge (NXOpen::Edge *edge)
	Sets the edge on which the flange is created. More...

void	SetFirstDistance (const NXString &firstDistance)
	More...

void	SetFirstDistance (const char *firstDistance)
	More...

void	SetInsetType (NXOpen::Features::SheetMetal::FlangeBuilder::InsetTypeOptions insetType)
	Sets the inset type (inside, outside, bendoutside) for the flange. More...

void	SetLength (const NXString &length)
	More...

void	SetLength (const char *length)
	More...

void	SetLengthType (NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptions lengthType)
	Sets a enum indicating the length type. More...

void	SetMatchFaceOption (NXOpen::Features::SheetMetal::FlangeBuilder::MatchFaceOptions matchFaceOption)
	Sets the match face selection type. More...

void	SetMatchPlane (NXOpen::Plane *matchPlane)
	Sets the Match Plane. More...

void	SetOffset (const NXString &offset)
	More...

void	SetOffset (const char *offset)
	More...

void	SetOffsetType (NXOpen::Features::SheetMetal::FlangeBuilder::OffsetTypeOptions offsetType)
	Sets the offset type for the flange. More...

void	SetSecondDistance (const NXString &secondDistance)
	More...

void	SetSecondDistance (const char *secondDistance)
	More...

void	SetVertex (const NXOpen::Point3d &vertex)
	Sets the vertex on the flange edge, needed to dimension the flange width. More...

void	SetWidthType (NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptions widthType)
	Sets the width type for flange. More...

int	ValidateBuilderData ()
	Verify that the builder data is valid for creating a flange. More...

NXOpen::Point3d	Vertex ()
	Returns the vertex on the flange edge, needed to dimension the flange width. More...

NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptions	WidthType ()
	Returns the width type for flange. More...

Public Member Functions inherited from NXOpen::Features::SheetMetal::SheetmetalBaseBuilder
NXOpen::Features::SheetMetal::ApplicationContext	GetApplicationContext ()
	Get the application context. More...

void	SetApplicationContext (NXOpen::Features::SheetMetal::ApplicationContext appContext)
	Set the application context. 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 Flange feature builder.

To create a new instance of this class, use NXOpen::Features::SheetMetal::SheetmetalManager::CreateFlangeFeatureBuilder

Created in NX4.0.0.

Member Enumeration Documentation

enum NXOpen::Features::SheetMetal::FlangeBuilder::InsetTypeOptions

This enum represents the inset type for the material of the flange.

Enumerator
InsetTypeOptionsMaterialInside	The flange is flush with the thickness face on the inside.
InsetTypeOptionsMaterialOutside	The flange is flush with the thickness face on the outside.
InsetTypeOptionsBendOutside	The bend and flange are outside the thickness face.

enum NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptions

This enum indicates the two ways that the flange length can be measured.

Enumerator
LengthTypeOptionsInsideDimension	The flange length is dimensioned to the Inner Mold line.
LengthTypeOptionsOutsideDimension	The flange length is dimensioned to the Outer Mold Line.
LengthTypeOptionsWebDimension	The flange length is dimensioned to the Bend Tangent Line.

enum NXOpen::Features::SheetMetal::FlangeBuilder::MatchFaceOptions

This enum represents the match face option for the flange.

Enumerator
MatchFaceOptionsNone	The flange is placed on the selected edge.
MatchFaceOptionsUntilSelected	The flange face is extended until the selected plane.

enum NXOpen::Features::SheetMetal::FlangeBuilder::OffsetTypeOptions

This enum represents the offset type for the flange.

Enumerator
OffsetTypeOptionsInside	The flange is offset to the inside of the face.
OffsetTypeOptionsOutside	The flange is offset to the outside of the face.

enum NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptions

This enum represents the width type for the flange.

Enumerator
WidthTypeOptionsFullEdge	The flange spans the entire edge.
WidthTypeOptionsCenterOfEdge	The flange is centered on the edge.
WidthTypeOptionsAtEdgeEnd	The flange starts from the specified end of the edge.
WidthTypeOptionsFromEdgeEnd	The flange starts at a specified distance from an end of the edge.
WidthTypeOptionsFromBothEnds	The flange starts and ends at specified distances from the ends of the edge.
WidthTypeOptionsCustom	The flange sketch has been edited after creation and may or may not conform to any of the above.

Member Function Documentation

NXOpen::Expression* NXOpen::Features::SheetMetal::FlangeBuilder::BendAngle ( )

Returns the bend angle for flange.

It should be set in degrees (??????).
Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

NXOpen::Features::SheetMetal::BendOptions* NXOpen::Features::SheetMetal::FlangeBuilder::BendOptions ( )

Returns the bend options object.

The bend options object stores additional parameters for the bend, such as bend radius, bend relief width and depth, corner relief type etc.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

void NXOpen::Features::SheetMetal::FlangeBuilder::DeleteSketch ( )

Delete the flange sketch
Created in NX6.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

NXOpen::Edge* NXOpen::Features::SheetMetal::FlangeBuilder::Edge ( )

Returns the edge on which the flange is created.

The edge should be linear and it should not be a thickness edge.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

void NXOpen::Features::SheetMetal::FlangeBuilder::EditSketch ( )

Edit the sketch base on a new edge you need to call SetEdge to set a new edge
Created in NX6.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

NXOpen::Expression* NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance ( )

Returns a distance based on NXOpen::Features::SheetMetal::FlangeBuilder::WidthType .

See NXOpen::Features::SheetMetal::FlangeBuilder::WidthType and NXOpen::Features::SheetMetal::FlangeBuilder::SetWidthType for a detailed desctiption of what this distance stands for.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

NXOpen::Sketch* NXOpen::Features::SheetMetal::FlangeBuilder::GetSketch ( )

Get the flange sketch.

Returns: Created in NX6.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

NXOpen::Features::SheetMetal::FlangeBuilder::InsetTypeOptions NXOpen::Features::SheetMetal::FlangeBuilder::InsetType ( )

Returns the inset type (inside, outside, bendoutside) for the flange.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

NXOpen::Expression* NXOpen::Features::SheetMetal::FlangeBuilder::Length ( )

Returns the length of the flange.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptions NXOpen::Features::SheetMetal::FlangeBuilder::LengthType ( )

Returns a enum indicating the length type.

For Features created in NX8 and above: The way length is measured for the flange. It can either be measure from the inside edge or the outside edge.
Flange length can be specified starting from the selected edge or from the corresponding edge on the other face (other linear edge on the other side of the thickness face). If the length is specified from the selected edge use value NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptionsInsideDimension or if the flange length is specifed from the other edge use value NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptionsOutsideDimension .

For Features created in NX8 and above: Flange length can be measure from the Inner Mold Line, Outer Mold Line or Bend Tangent Line.
Inner Mold Line: Intersection of inner tab face and inner flange web face Outer Mold Line: Intersection of outer tab face and outer flange web face Bend Tangent Line: common edge between flange web face and bend face.

Flange length can be specified starting from the inner mold line or outer mold line or bend tangent line. If the length is specified from the inner mold line use value NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptionsInsideDimension or if the flange length is specifed from the outer mold line use value NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptionsOutsideDimension or if the flange length is specifed from the bend tangent line use value NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptionsWebDimension .

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

NXOpen::Features::SheetMetal::FlangeBuilder::MatchFaceOptions NXOpen::Features::SheetMetal::FlangeBuilder::MatchFaceOption ( )

Returns the match face selection type.

None for Regular Flange. Until Selected for Match To Face type Flange .

Created in NX8.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB")

NXOpen::Plane* NXOpen::Features::SheetMetal::FlangeBuilder::MatchPlane ( )

Returns the Match Plane.

Created in NX8.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB")

NXOpen::Expression* NXOpen::Features::SheetMetal::FlangeBuilder::Offset ( )

Returns the offset value for the flange.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

NXOpen::Features::SheetMetal::FlangeBuilder::OffsetTypeOptions NXOpen::Features::SheetMetal::FlangeBuilder::OffsetType ( )

Returns the offset type for the flange.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

NXOpen::Expression* NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance ( )

Returns a distance based on NXOpen::Features::SheetMetal::FlangeBuilder::WidthType .

See NXOpen::Features::SheetMetal::FlangeBuilder::WidthType and NXOpen::Features::SheetMetal::FlangeBuilder::SetWidthType for a detailed desctiption of what this distance stands for.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

void NXOpen::Features::SheetMetal::FlangeBuilder::SetBendAngle ( const NXString & bendAngle )

Deprecated:: Deprecated in NX10.0.0.

Use NXOpen::Expression::SetRightHandSide on the NXOpen::Expression object returned from NXOpen::Features::SheetMetal::FlangeBuilder::BendAngle instead.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

bendAngle bend angle

void NXOpen::Features::SheetMetal::FlangeBuilder::SetBendAngle ( const char * bendAngle )

Deprecated:: Deprecated in NX10.0.0.

Use NXOpen::Expression::SetRightHandSide on the NXOpen::Expression object returned from NXOpen::Features::SheetMetal::FlangeBuilder::BendAngle instead.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

bendAngle bend angle

void NXOpen::Features::SheetMetal::FlangeBuilder::SetEdge ( NXOpen::Edge * edge )

Sets the edge on which the flange is created.

The edge should be linear and it should not be a thickness edge.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

edge	The flange is created on this edge.

void NXOpen::Features::SheetMetal::FlangeBuilder::SetFirstDistance ( const NXString & firstDistance )

Deprecated:: Deprecated in NX10.0.0.

Use NXOpen::Expression::SetRightHandSide on the NXOpen::Expression object returned from NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance instead.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

firstDistance first distance

void NXOpen::Features::SheetMetal::FlangeBuilder::SetFirstDistance ( const char * firstDistance )

Deprecated:: Deprecated in NX10.0.0.

Use NXOpen::Expression::SetRightHandSide on the NXOpen::Expression object returned from NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance instead.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

firstDistance first distance

void NXOpen::Features::SheetMetal::FlangeBuilder::SetInsetType ( NXOpen::Features::SheetMetal::FlangeBuilder::InsetTypeOptions insetType )

Sets the inset type (inside, outside, bendoutside) for the flange.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

insetType inset type

void NXOpen::Features::SheetMetal::FlangeBuilder::SetLength ( const NXString & length )

Deprecated:: Deprecated in NX10.0.0.

Use NXOpen::Expression::SetRightHandSide on the NXOpen::Expression object returned from NXOpen::Features::SheetMetal::FlangeBuilder::Length instead.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

length length

void NXOpen::Features::SheetMetal::FlangeBuilder::SetLength ( const char * length )

Deprecated:: Deprecated in NX10.0.0.

Use NXOpen::Expression::SetRightHandSide on the NXOpen::Expression object returned from NXOpen::Features::SheetMetal::FlangeBuilder::Length instead.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

length length

void NXOpen::Features::SheetMetal::FlangeBuilder::SetLengthType ( NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptions lengthType )

Sets a enum indicating the length type.

For Features created in NX8 and above: The way length is measured for the flange. It can either be measure from the inside edge or the outside edge.
Flange length can be specified starting from the selected edge or from the corresponding edge on the other face (other linear edge on the other side of the thickness face). If the length is specified from the selected edge use value NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptionsInsideDimension or if the flange length is specifed from the other edge use value NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptionsOutsideDimension .

For Features created in NX8 and above: Flange length can be measure from the Inner Mold Line, Outer Mold Line or Bend Tangent Line.
Inner Mold Line: Intersection of inner tab face and inner flange web face Outer Mold Line: Intersection of outer tab face and outer flange web face Bend Tangent Line: common edge between flange web face and bend face.

Flange length can be specified starting from the inner mold line or outer mold line or bend tangent line. If the length is specified from the inner mold line use value NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptionsInsideDimension or if the flange length is specifed from the outer mold line use value NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptionsOutsideDimension or if the flange length is specifed from the bend tangent line use value NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptionsWebDimension .

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

lengthType length type

void NXOpen::Features::SheetMetal::FlangeBuilder::SetMatchFaceOption ( NXOpen::Features::SheetMetal::FlangeBuilder::MatchFaceOptions matchFaceOption )

Sets the match face selection type.

None for Regular Flange. Until Selected for Match To Face type Flange .

Created in NX8.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB")

Parameters

matchFaceOption matchfaceoption

void NXOpen::Features::SheetMetal::FlangeBuilder::SetMatchPlane ( NXOpen::Plane * matchPlane )

Sets the Match Plane.

Created in NX8.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB")

Parameters

matchPlane matchplane

void NXOpen::Features::SheetMetal::FlangeBuilder::SetOffset ( const NXString & offset )

Deprecated:: Deprecated in NX10.0.0.

Use NXOpen::Expression::SetRightHandSide on the NXOpen::Expression object returned from NXOpen::Features::SheetMetal::FlangeBuilder::Offset instead.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB")

Parameters

offset The flange offset value

void NXOpen::Features::SheetMetal::FlangeBuilder::SetOffset ( const char * offset )

Deprecated:: Deprecated in NX10.0.0.

Use NXOpen::Expression::SetRightHandSide on the NXOpen::Expression object returned from NXOpen::Features::SheetMetal::FlangeBuilder::Offset instead.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB")

Parameters

offset The flange offset value

void NXOpen::Features::SheetMetal::FlangeBuilder::SetOffsetType ( NXOpen::Features::SheetMetal::FlangeBuilder::OffsetTypeOptions offsetType )

Sets the offset type for the flange.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

offsetType The flange can be offset inside or outside.

void NXOpen::Features::SheetMetal::FlangeBuilder::SetSecondDistance ( const NXString & secondDistance )

Deprecated:: Deprecated in NX10.0.0.

Use NXOpen::Expression::SetRightHandSide on the NXOpen::Expression object returned from NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance instead.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

secondDistance second distance

void NXOpen::Features::SheetMetal::FlangeBuilder::SetSecondDistance ( const char * secondDistance )

Deprecated:: Deprecated in NX10.0.0.

Use NXOpen::Expression::SetRightHandSide on the NXOpen::Expression object returned from NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance instead.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

secondDistance second distance

void NXOpen::Features::SheetMetal::FlangeBuilder::SetVertex ( const NXOpen::Point3d & vertex )

Sets the vertex on the flange edge, needed to dimension the flange width.

The vertex needs to be specified ONLY if NXOpen::Features::SheetMetal::FlangeBuilder::WidthType is set to one of NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsAtEdgeEnd , NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromEdgeEnd . In case of NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromBothEnds , the start vertex of the edge is assumed to be the start point for NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance .

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

vertex A vertex on the flange edge.

void NXOpen::Features::SheetMetal::FlangeBuilder::SetWidthType ( NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptions widthType )

Sets the width type for flange.

Use one of the values from NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptions . Depending on which of the values from the enum is used, none, either or both of the distance values from NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance and NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance may be used. Here is a description of the distances:

If the value is NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFullEdge , then both the FirstDistance and NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance values are unused.

If the value is NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsCenterOfEdge , then both the NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance and NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance represent exactly half the width of the flange.

If the value is NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsAtEdgeEnd , then NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance represents the width of the flange, starting from the end of the edge specified by the NXOpen::Features::SheetMetal::FlangeBuilder::Vertex and the NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance is not used.

If the value is NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromEdgeEnd , then NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance represents the distance of the start point of the flange from the end of the edge specified by NXOpen::Features::SheetMetal::FlangeBuilder::Vertex and NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance represents the width of the flange.

If the value is NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromBothEnds , then NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance represents the distance of the start point of the flange from the from the end of the edge specified by NXOpen::Features::SheetMetal::FlangeBuilder::Vertex and NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance represents the distance of the end point of the flange from end of the edge opposite to the end specified by NXOpen::Features::SheetMetal::FlangeBuilder::Vertex .

The value NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsCustom , cannot be set by the user. It is set internally if the sketch for the flange has been edited after creation. In this case, the expressions NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance and NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance may or may not retain their original meaning when the flange was first created, so the user should not rely on these any more to mean anything specific.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

Parameters

widthType width type

int NXOpen::Features::SheetMetal::FlangeBuilder::ValidateBuilderData ( )

Verify that the builder data is valid for creating a flange.

If the builder data is valid, return value is zero.

Returns: A value of zero is returned if the data in the builder is valid.
Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

NXOpen::Point3d NXOpen::Features::SheetMetal::FlangeBuilder::Vertex ( )

Returns the vertex on the flange edge, needed to dimension the flange width.

The vertex needs to be specified ONLY if NXOpen::Features::SheetMetal::FlangeBuilder::WidthType is set to one of NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsAtEdgeEnd , NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromEdgeEnd . In case of NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromBothEnds , the start vertex of the edge is assumed to be the start point for NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance .

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptions NXOpen::Features::SheetMetal::FlangeBuilder::WidthType ( )

Returns the width type for flange.

Use one of the values from NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptions . Depending on which of the values from the enum is used, none, either or both of the distance values from NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance and NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance may be used. Here is a description of the distances:

If the value is NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFullEdge , then both the FirstDistance and NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance values are unused.

If the value is NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsCenterOfEdge , then both the NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance and NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance represent exactly half the width of the flange.

If the value is NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsAtEdgeEnd , then NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance represents the width of the flange, starting from the end of the edge specified by the NXOpen::Features::SheetMetal::FlangeBuilder::Vertex and the NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance is not used.

If the value is NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromEdgeEnd , then NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance represents the distance of the start point of the flange from the end of the edge specified by NXOpen::Features::SheetMetal::FlangeBuilder::Vertex and NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance represents the width of the flange.

If the value is NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromBothEnds , then NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance represents the distance of the start point of the flange from the from the end of the edge specified by NXOpen::Features::SheetMetal::FlangeBuilder::Vertex and NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance represents the distance of the end point of the flange from end of the edge opposite to the end specified by NXOpen::Features::SheetMetal::FlangeBuilder::Vertex .

The value NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptionsCustom , cannot be set by the user. It is set internally if the sketch for the flange has been edited after creation. In this case, the expressions NXOpen::Features::SheetMetal::FlangeBuilder::FirstDistance and NXOpen::Features::SheetMetal::FlangeBuilder::SecondDistance may or may not retain their original meaning when the flange was first created, so the user should not rely on these any more to mean anything specific.

Created in NX4.0.0.

License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

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

Features_SheetMetal_FlangeBuilder.hxx

Public Types

Public Member Functions

Detailed Description

Member Enumeration Documentation

Member Function Documentation