Represents a Flange feature builder. More...

Inheritance diagram for NXOpen.Features.SheetMetal.FlangeBuilder:

Public Types
enum	InsetTypeOptions { MaterialInside, MaterialOutside, BendOutside }
	This enum represents the inset type for the material of the flange. More...

enum	LengthTypeOptions { InsideDimension, OutsideDimension, WebDimension }
	This enum indicates the two ways that the flange length can be measured. More...

enum	MatchFaceOptions { None, UntilSelected }
	This enum represents the match face option for the flange. More...

enum	OffsetTypeOptions { Inside, Outside }
	This enum represents the offset type for the flange. More...

enum	WidthTypeOptions { FullEdge, CenterOfEdge, AtEdgeEnd, FromEdgeEnd, FromBothEnds, Custom }
	This enum represents the width type for the flange. More...

Public Member Functions
unsafe void	DeleteSketch ()
	Delete the flange sketch More...

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

unsafe NXOpen.Sketch	GetSketch ()
	Get the flange sketch More...

unsafe void	SetBendAngle (string bendAngle)
	More...

unsafe void	SetFirstDistance (string firstDistance)
	More...

unsafe void	SetLength (string length)
	More...

unsafe void	SetOffset (string offset)
	More...

unsafe void	SetSecondDistance (string secondDistance)
	More...

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

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

unsafe void	SetApplicationContext (NXOpen.Features.SheetMetal.ApplicationContext appContext)
	Set the application context. More...

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

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

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

unsafe void	SetParentFeatureInternal (NXOpen.Features.Feature parentFeature)
	Set the parent features which would be internal or slaves to the feature being created or commited More...

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

unsafe void	UnsetParentFeatureInternal (NXOpen.Features.Feature parentFeature)
	Set the internal parent feature of the feature being edited to external More...

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

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

unsafe NXOpen.NXObject[]	GetCommittedObjects ()
	For builders that create more than one object, this method returns the objects that are created by commit. More...

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

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

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

Public Member Functions inherited from NXOpen.TaggedObject
void	PrintTestData (String variableName)
	<exclude> More...

void	PrintTestData (String variableName, int lineNumber)
	<exclude> More...

override string	ToString ()
	Returns a String that represents the current Object. More...

Public Member Functions inherited from NXOpen.Utilities.NXRemotableObject
IMessageCtrl	AsyncProcessMessage (IMessage msg, IMessageSink replySink)
	Asynchronously processes the given message. More...

IMessage	SyncProcessMessage (IMessage msg)
	Synchronously processes the given message. More...

Properties
unsafe NXOpen.Expression	BendAngle `[get]`
	Returns the bend angle for flange. More...

unsafe NXOpen.Features.SheetMetal.BendOptions	BendOptions `[get]`
	Returns the bend options object. More...

unsafe NXOpen.Edge	Edge `[get, set]`
	Returns or sets the edge on which the flange is created. More...

unsafe NXOpen.Expression	FirstDistance `[get]`
	Returns a distance based on NXOpen.Features.SheetMetal.FlangeBuilder.WidthType . More...

unsafe NXOpen.Features.SheetMetal.FlangeBuilder.InsetTypeOptions	InsetType `[get, set]`
	Returns or sets the inset type (inside, outside, bendoutside) for the flange. More...

unsafe NXOpen.Expression	Length `[get]`
	Returns the length of the flange. More...

unsafe NXOpen.Features.SheetMetal.FlangeBuilder.LengthTypeOptions	LengthType `[get, set]`
	Returns or sets a enum indicating the length type. More...

unsafe NXOpen.Features.SheetMetal.FlangeBuilder.MatchFaceOptions	MatchFaceOption `[get, set]`
	Returns or sets the match face selection type. More...

unsafe NXOpen.Plane	MatchPlane `[get, set]`
	Returns or sets the Match Plane. More...

unsafe NXOpen.Expression	Offset `[get]`
	Returns the offset value for the flange. More...

unsafe NXOpen.Features.SheetMetal.FlangeBuilder.OffsetTypeOptions	OffsetType `[get, set]`
	Returns or sets the offset type for the flange. More...

unsafe NXOpen.Expression	SecondDistance `[get]`
	Returns a distance based on NXOpen.Features.SheetMetal.FlangeBuilder.WidthType . More...

unsafe NXOpen.Point3d	Vertex `[get, set]`
	Returns or sets the vertex on the flange edge, needed to dimension the flange width. More...

unsafe NXOpen.Features.SheetMetal.FlangeBuilder.WidthTypeOptions	WidthType `[get, set]`
	Returns or sets the width type for flange. More...

Additional Inherited Members
Protected Member Functions inherited from NXOpen.TaggedObject
new void	initialize ()
	<exclude> 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
MaterialInside	The flange is flush with the thickness face on the inside
MaterialOutside	The flange is flush with the thickness face on the outside
BendOutside	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
InsideDimension	The flange length is dimensioned to the Inner Mold line.
OutsideDimension	The flange length is dimensioned to the Outer Mold Line.
WebDimension	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
None	The flange is placed on the selected edge
UntilSelected	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
Inside	The flange is offset to the inside of the face
Outside	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
FullEdge	The flange spans the entire edge.
CenterOfEdge	The flange is centered on the edge.
AtEdgeEnd	The flange starts from the specified end of the edge.
FromEdgeEnd	The flange starts at a specified distance from an end of the edge.
FromBothEnds	The flange starts and ends at specified distances from the ends of the edge.
Custom	The flange sketch has been edited after creation and may or may not conform to any of the above.

Member Function Documentation

unsafe void NXOpen.Features.SheetMetal.FlangeBuilder.DeleteSketch ( )

inline

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")

unsafe void NXOpen.Features.SheetMetal.FlangeBuilder.EditSketch ( )

inline

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")

unsafe NXOpen.Sketch NXOpen.Features.SheetMetal.FlangeBuilder.GetSketch ( )

inline

Get 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")

Returns

unsafe void NXOpen.Features.SheetMetal.FlangeBuilder.SetBendAngle ( string bendAngle )

inline

Created in NX4.0.0

Deprecated in NX10.0.0. Use NXOpen.Expression.RightHandSide on the NXOpen.Expression object returned from NXOpen.Features.SheetMetal.FlangeBuilder.BendAngle instead.

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

Parameters

bendAngle

unsafe void NXOpen.Features.SheetMetal.FlangeBuilder.SetFirstDistance ( string firstDistance )

inline

Created in NX4.0.0

Deprecated in NX10.0.0. Use NXOpen.Expression.RightHandSide on the NXOpen.Expression object returned from NXOpen.Features.SheetMetal.FlangeBuilder.FirstDistance instead.

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

Parameters

firstDistance

unsafe void NXOpen.Features.SheetMetal.FlangeBuilder.SetLength ( string length )

inline

Created in NX4.0.0

Deprecated in NX10.0.0. Use NXOpen.Expression.RightHandSide on the NXOpen.Expression object returned from NXOpen.Features.SheetMetal.FlangeBuilder.Length instead.

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

Parameters

length

unsafe void NXOpen.Features.SheetMetal.FlangeBuilder.SetOffset ( string offset )

inline

Created in NX4.0.0

Deprecated in NX10.0.0. Use NXOpen.Expression.RightHandSide on the NXOpen.Expression object returned from NXOpen.Features.SheetMetal.FlangeBuilder.Offset instead.

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

Parameters

offset The flange offset value

unsafe void NXOpen.Features.SheetMetal.FlangeBuilder.SetSecondDistance ( string secondDistance )

inline

Created in NX4.0.0

Deprecated in NX10.0.0. Use NXOpen.Expression.RightHandSide on the NXOpen.Expression object returned from NXOpen.Features.SheetMetal.FlangeBuilder.SecondDistance instead.

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

Parameters

secondDistance

unsafe int NXOpen.Features.SheetMetal.FlangeBuilder.ValidateBuilderData ( )

inline

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

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

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")

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

Property Documentation

unsafe NXOpen.Expression NXOpen.Features.SheetMetal.FlangeBuilder.BendAngle

get

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")

unsafe NXOpen.Features.SheetMetal.BendOptions NXOpen.Features.SheetMetal.FlangeBuilder.BendOptions

get

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")

unsafe NXOpen.Edge NXOpen.Features.SheetMetal.FlangeBuilder.Edge

getset

Returns or 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 to get this property: nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

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

unsafe NXOpen.Expression NXOpen.Features.SheetMetal.FlangeBuilder.FirstDistance

get

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

See NXOpen.Features.SheetMetal.FlangeBuilder.WidthType 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")

unsafe NXOpen.Features.SheetMetal.FlangeBuilder.InsetTypeOptions NXOpen.Features.SheetMetal.FlangeBuilder.InsetType

getset

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

Created in NX4.0.0

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

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

unsafe NXOpen.Expression NXOpen.Features.SheetMetal.FlangeBuilder.Length

get

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")

unsafe NXOpen.Features.SheetMetal.FlangeBuilder.LengthTypeOptions NXOpen.Features.SheetMetal.FlangeBuilder.LengthType

getset

Returns or 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.LengthTypeOptions.InsideDimension or if the flange length is specifed from the other edge use value NXOpen.Features.SheetMetal.FlangeBuilder.LengthTypeOptions.OutsideDimension .

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.LengthTypeOptions.InsideDimension or if the flange length is specifed from the outer mold line use value NXOpen.Features.SheetMetal.FlangeBuilder.LengthTypeOptions.OutsideDimension or if the flange length is specifed from the bend tangent line use value NXOpen.Features.SheetMetal.FlangeBuilder.LengthTypeOptions.WebDimension .

Created in NX4.0.0

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

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

unsafe NXOpen.Features.SheetMetal.FlangeBuilder.MatchFaceOptions NXOpen.Features.SheetMetal.FlangeBuilder.MatchFaceOption

getset

Returns or 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 to get this property: nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB")

License requirements to set this property: nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB")

unsafe NXOpen.Plane NXOpen.Features.SheetMetal.FlangeBuilder.MatchPlane

getset

Returns or sets the Match Plane.

Created in NX8.0.0

License requirements to get this property: nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB")

License requirements to set this property: nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB")

unsafe NXOpen.Expression NXOpen.Features.SheetMetal.FlangeBuilder.Offset

get

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")

unsafe NXOpen.Features.SheetMetal.FlangeBuilder.OffsetTypeOptions NXOpen.Features.SheetMetal.FlangeBuilder.OffsetType

getset

Returns or sets the offset type for the flange.

Created in NX4.0.0

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

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

unsafe NXOpen.Expression NXOpen.Features.SheetMetal.FlangeBuilder.SecondDistance

get

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

See NXOpen.Features.SheetMetal.FlangeBuilder.WidthType 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")

unsafe NXOpen.Point3d NXOpen.Features.SheetMetal.FlangeBuilder.Vertex

getset

Returns or 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.WidthTypeOptions.AtEdgeEnd , NXOpen.Features.SheetMetal.FlangeBuilder.WidthTypeOptions.FromEdgeEnd . In case of NXOpen.Features.SheetMetal.FlangeBuilder.WidthTypeOptions.FromBothEnds , 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 to get this property: nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

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

unsafe NXOpen.Features.SheetMetal.FlangeBuilder.WidthTypeOptions NXOpen.Features.SheetMetal.FlangeBuilder.WidthType

getset

Returns or 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.WidthTypeOptions.FullEdge , then both the FirstDistance and NXOpen.Features.SheetMetal.FlangeBuilder.SecondDistance values are unused.

If the value is NXOpen.Features.SheetMetal.FlangeBuilder.WidthTypeOptions.CenterOfEdge , 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.WidthTypeOptions.AtEdgeEnd , 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.WidthTypeOptions.FromEdgeEnd , 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.WidthTypeOptions.FromBothEnds , 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.WidthTypeOptions.Custom , 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 to get this property: nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB") OR nx_ship_detail ("Ship Detail Design")

License requirements to set this property: 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.cs

Public Types

Public Member Functions

Properties

Additional Inherited Members

Detailed Description

Member Enumeration Documentation

Member Function Documentation

Property Documentation