Represents a NX Sheet Metal @link Features::Gusset Features::Gusset@endlink  builder
 <br> To create a new instance of this class, use @link Features::SheetMetal::SheetmetalManager::CreateGussetBuilder  Features::SheetMetal::SheetmetalManager::CreateGussetBuilder @endlink  <br>

Default values. More...

Inheritance diagram for NXOpen::Features::SheetMetal::GussetBuilder:

Public Types
enum	PlacementTypes { PlacementTypesSingle, PlacementTypesFit, PlacementTypesFill, PlacementTypesFixed }
	This enum represents the different options for placing an automatic profile Gusset. More...

enum	Shapes { ShapesSquare, ShapesRound }
	This enum represents the two different shapes for Gusset. More...

enum	Types { TypesAutomaticProfile, TypesUserDefinedProfile }
	This enum represents the two Gusset Feature types. More...

enum	WidthSides { WidthSidesSide1, WidthSidesSide2, WidthSidesSymmetric }
	This enum represents the different options for thickening the user defined profile Gusset. More...

Public Member Functions
void	AlternateSolution ()
	Cycles the available solutions when a user defined profile intersects the solid body.

NXOpen::SelectFace *	BendFace ()
	Returns the bend face Selects the bend face along which the gusset is placed.

NXOpen::Expression *	CornerRadius ()
	Returns the corner radius This value is used only for the Features::SheetMetal::GussetBuilder::ShapesSquare shape.

NXOpen::Expression *	Depth ()
	Returns the depth This value is used for the automatic profile Gussets.

NXOpen::Expression *	DieRadius ()
	Returns the die radius value of the sharp edges of the bottom face.

NXOpen::Vector3d	GetPlacementOriginAndDirection (NXOpen::Point3d *origin)
	Get the placement origin and direction.

void	GetStartEdgeCandidates (std::vector< NXOpen::Edge * > &candidateEdges)
	Get the edges on the bend face that can be selected as Start Edge.

int	PlacementCount ()
	Returns the placement count This value is used if the Features::SheetMetal::GussetBuilder::PlacementTypes is set to Features::SheetMetal::GussetBuilder::PlacementTypesFit or Features::SheetMetal::GussetBuilder::PlacementTypesFixed .

NXOpen::Expression *	PlacementDistance ()
	Returns the placement distance If the Features::SheetMetal::GussetBuilder::PlacementTypes is set to Features::SheetMetal::GussetBuilder::PlacementTypesSingle , then this option represents the location of the automatic profile Gusset from one of the ends of the selected bend face.

NXOpen::Expression *	PlacementSpacing ()
	Returns the placement spacing This value is used if the Features::SheetMetal::GussetBuilder::PlacementTypes is set to Features::SheetMetal::GussetBuilder::PlacementTypesFill or Features::SheetMetal::GussetBuilder::PlacementTypesFixed .

NXOpen::Features::SheetMetal::GussetBuilder::PlacementTypes	PlacementType ()
	Returns the placement type Specify the Gusset placement option.

NXOpen::Expression *	PunchRadius ()
	Returns the punch radius value of the sharp edges of the top face.

NXOpen::Section *	Section ()
	Returns the section This section object contains a planar set of connected curves that will be used to create a Gusset of type Features::SheetMetal::GussetBuilder::TypesUserDefinedProfile .

void	SetPlacementCount (int placementCount)
	Sets the placement count This value is used if the Features::SheetMetal::GussetBuilder::PlacementTypes is set to Features::SheetMetal::GussetBuilder::PlacementTypesFit or Features::SheetMetal::GussetBuilder::PlacementTypesFixed .

void	SetPlacementType (NXOpen::Features::SheetMetal::GussetBuilder::PlacementTypes placementType)
	Sets the placement type Specify the Gusset placement option.

void	SetShape (NXOpen::Features::SheetMetal::GussetBuilder::Shapes shape)
	Sets the shape See Features::SheetMetal::GussetBuilder::Shapes for details.

void	SetType (NXOpen::Features::SheetMetal::GussetBuilder::Types type)
	Sets the type of Gusset feature Created in NX7.5.0.

void	SetWidthSide (NXOpen::Features::SheetMetal::GussetBuilder::WidthSides widthSide)
	Sets the width side Defines the side of the profile to which material should be added or from which material should be removed to construct the feature.

NXOpen::Features::SheetMetal::GussetBuilder::Shapes	Shape ()
	Returns the shape See Features::SheetMetal::GussetBuilder::Shapes for details.

NXOpen::Expression *	SideAngle ()
	Returns the side angle.

NXOpen::SelectEdge *	StartEdge ()
	Returns the start edge Selects the edge on the bend face to determine the gusset offset direction.

NXOpen::Features::SheetMetal::GussetBuilder::Types	Type ()
	Returns the type of Gusset feature Created in NX7.5.0.

NXOpen::Expression *	Width ()
	Returns the width value for the Gusset Created in NX7.5.0.

NXOpen::Features::SheetMetal::GussetBuilder::WidthSides	WidthSide ()
	Returns the width side Defines the side of the profile to which material should be added or from which material should be removed to construct the feature.

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

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

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

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

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

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

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.

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.

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

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

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

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

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

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

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

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

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

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

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

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

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

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

Public Member Functions inherited from NXOpen::TaggedObject
tag_t	GetTag () const
	<b>Deprecated</b>:<br> Use Tag instead.

tag_t	Tag () const
	Returns the tag of this object.

Detailed Description

Represents a NX Sheet Metal @link Features::Gusset Features::Gusset@endlink  builder
 <br> To create a new instance of this class, use @link Features::SheetMetal::SheetmetalManager::CreateGussetBuilder  Features::SheetMetal::SheetmetalManager::CreateGussetBuilder @endlink  <br>

Default values.

Property

Value

CornerRadius.Value

1 (millimeters part), 0.05 (inches part)

Depth.Value

10 (millimeters part), 1 (inches part)

DieRadius.Value

2 (millimeters part), 0.1 (inches part)

PlacementCount

2

PlacementDistance.Value

10 (millimeters part), 1 (inches part)

PlacementSpacing.Value

20 (millimeters part), 2 (inches part)

PlacementType

Single

PunchRadius.Value

2 (millimeters part), 0.1 (inches part)

Shape

Square

SideAngle.Value

0

Width.Value

10 (millimeters part), 1 (inches part)

WidthSide

Side1

Created in NX7.5.0.

Member Enumeration Documentation

enum NXOpen::Features::SheetMetal::GussetBuilder::PlacementTypes

This enum represents the different options for placing an automatic profile Gusset.

Enumerator:

PlacementTypesSingle	One Gusset will be created at an offset from an edge on the selected bend face.
PlacementTypesFit	Users will specify the number of occurances of Gusset on the selected bend face and software will calculate the spacing.
PlacementTypesFill	Users will specify the spacing of Gussets on the selected bend face and software will calculate the number of occurances.
PlacementTypesFixed	Users will specify the number of occurances and the spacing for Gussets on the selected bend face.

enum NXOpen::Features::SheetMetal::GussetBuilder::Shapes

This enum represents the two different shapes for Gusset.

Enumerator:

ShapesSquare	Specifies a square shape for the Gusset.
ShapesRound	Specifies a round shape for the Gusset.

enum NXOpen::Features::SheetMetal::GussetBuilder::Types

This enum represents the two Gusset Feature types.

Enumerator:

TypesAutomaticProfile	Gusset(s) will be created between the planar faces adjacent to the selected bend face.
TypesUserDefinedProfile	Gusset will be created using a profile defined by the user.

enum NXOpen::Features::SheetMetal::GussetBuilder::WidthSides

This enum represents the different options for thickening the user defined profile Gusset.

Enumerator:

WidthSidesSide1	The Gusset will be created on the side of plane normal of the user defined profile.
WidthSidesSide2	The Gusset will be created on the opposite side of the plane normal of the user defined profile.
WidthSidesSymmetric	The Gusset will be created on both sides of the plane of the user defined profile.

Member Function Documentation

void NXOpen::Features::SheetMetal::GussetBuilder::AlternateSolution ( )

Cycles the available solutions when a user defined profile intersects the solid body.

If there is only one working solution then it will be automatically selected and this method will not do anything.
Created in NX7.5.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

NXOpen::SelectFace* NXOpen::Features::SheetMetal::GussetBuilder::BendFace ( )

Returns the bend face
Selects the bend face along which the gusset is placed.

        <br>

Created in NX7.5.0.

License requirements : None

NXOpen::Expression* NXOpen::Features::SheetMetal::GussetBuilder::CornerRadius ( )

Returns the corner radius
This value is used only for the Features::SheetMetal::GussetBuilder::ShapesSquare shape.

The value must be greater than or equal to zero.

Created in NX7.5.0.

License requirements : None

NXOpen::Expression* NXOpen::Features::SheetMetal::GussetBuilder::Depth ( )

Returns the depth
This value is used for the automatic profile Gussets.

It represents the distance from the outer bend face of the selected bends along the bisector of the planar faces adjacent to the outer bend face.

Created in NX7.5.0.

License requirements : None

NXOpen::Expression* NXOpen::Features::SheetMetal::GussetBuilder::DieRadius ( )

Returns the die radius value of the sharp edges of the bottom face.

The value must be greater than or equal to zero.
Created in NX7.5.0.

License requirements : None

NXOpen::Vector3d NXOpen::Features::SheetMetal::GussetBuilder::GetPlacementOriginAndDirection ( NXOpen::Point3d * origin )

Get the placement origin and direction.

        <br> 
           Get the point from which the placement distance will be measured and the 
           direction along which the positive distance is defined.
        <br> 
    @return  Direction along which the placement distance is measured.

Created in NX7.5.0.

License requirements : None

Parameters

origin Start point from which placement distance is measured.

void NXOpen::Features::SheetMetal::GussetBuilder::GetStartEdgeCandidates ( std::vector< NXOpen::Edge * > & candidateEdges )

Get the edges on the bend face that can be selected as Start Edge.

        <br> 
           Get the edges on the bend face that can be selected as Start Edge.
           If there is no Bend Face, then no edges will be returned.
        <br>

Created in NX7.5.0.

License requirements : None

Parameters

candidateEdges An array of edges that are valid for selection as start edge

int NXOpen::Features::SheetMetal::GussetBuilder::PlacementCount ( )

Returns the placement count
This value is used if the Features::SheetMetal::GussetBuilder::PlacementTypes is set to Features::SheetMetal::GussetBuilder::PlacementTypesFit or Features::SheetMetal::GussetBuilder::PlacementTypesFixed .

It represents the number of occurances of the automatic profile Gusset to create on the selected bend face. The count must be greater than zero for Features::SheetMetal::GussetBuilder::PlacementTypesFit and greater than one for Features::SheetMetal::GussetBuilder::PlacementTypesFixed .

Created in NX7.5.0.

License requirements : None

NXOpen::Expression* NXOpen::Features::SheetMetal::GussetBuilder::PlacementDistance ( )

Returns the placement distance
If the Features::SheetMetal::GussetBuilder::PlacementTypes is set to Features::SheetMetal::GussetBuilder::PlacementTypesSingle , then this option represents the location of the automatic profile Gusset from one of the ends of the selected bend face.

The distance is measured in a direction going from the start end to the other end. Users can specify which end of the selected bend face to use as the start.

Created in NX7.5.0.

License requirements : None

NXOpen::Expression* NXOpen::Features::SheetMetal::GussetBuilder::PlacementSpacing ( )

Returns the placement spacing
This value is used if the Features::SheetMetal::GussetBuilder::PlacementTypes is set to Features::SheetMetal::GussetBuilder::PlacementTypesFill or Features::SheetMetal::GussetBuilder::PlacementTypesFixed .

It represents the spacing between the automatic profile Gussets to create on the selected bend face.

Created in NX7.5.0.

License requirements : None

NXOpen::Features::SheetMetal::GussetBuilder::PlacementTypes NXOpen::Features::SheetMetal::GussetBuilder::PlacementType ( )

Returns the placement type
Specify the Gusset placement option.

See the description of Features::SheetMetal::GussetBuilder::PlacementTypes elements for details.

Created in NX7.5.0.

License requirements : None

NXOpen::Expression* NXOpen::Features::SheetMetal::GussetBuilder::PunchRadius ( )

Returns the punch radius value of the sharp edges of the top face.

The value must be greater than or equal to zero.
Created in NX7.5.0.

License requirements : None

NXOpen::Section* NXOpen::Features::SheetMetal::GussetBuilder::Section ( )

Returns the section
This section object contains a planar set of connected curves that will be used to create a Gusset of type Features::SheetMetal::GussetBuilder::TypesUserDefinedProfile .

This profile can be closed or open. If it is open, then the end points can touch face(s). The profile must not intersect the solid body. If an open profile does not intersect or touch any face, each end will be extended until it touches a face.

Created in NX7.5.0.

License requirements : None

void NXOpen::Features::SheetMetal::GussetBuilder::SetPlacementCount ( int placementCount )

Sets the placement count
This value is used if the Features::SheetMetal::GussetBuilder::PlacementTypes is set to Features::SheetMetal::GussetBuilder::PlacementTypesFit or Features::SheetMetal::GussetBuilder::PlacementTypesFixed .

It represents the number of occurances of the automatic profile Gusset to create on the selected bend face. The count must be greater than zero for Features::SheetMetal::GussetBuilder::PlacementTypesFit and greater than one for Features::SheetMetal::GussetBuilder::PlacementTypesFixed .

Created in NX7.5.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

placementCount placementcount

void NXOpen::Features::SheetMetal::GussetBuilder::SetPlacementType ( NXOpen::Features::SheetMetal::GussetBuilder::PlacementTypes placementType )

Sets the placement type
Specify the Gusset placement option.

See the description of Features::SheetMetal::GussetBuilder::PlacementTypes elements for details.

Created in NX7.5.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

placementType placementtype

void NXOpen::Features::SheetMetal::GussetBuilder::SetShape ( NXOpen::Features::SheetMetal::GussetBuilder::Shapes shape )

Sets the shape
See Features::SheetMetal::GussetBuilder::Shapes for details.

        <br>

Created in NX7.5.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

shape shape

void NXOpen::Features::SheetMetal::GussetBuilder::SetType ( NXOpen::Features::SheetMetal::GussetBuilder::Types type )

Sets the type of Gusset feature
Created in NX7.5.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

type type

void NXOpen::Features::SheetMetal::GussetBuilder::SetWidthSide ( NXOpen::Features::SheetMetal::GussetBuilder::WidthSides widthSide )

Sets the width side
Defines the side of the profile to which material should be added or from which material should be removed to construct the feature.

           The side option is not required when the profile is closed.
        <br>

Created in NX7.5.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters

widthSide widthside

NXOpen::Features::SheetMetal::GussetBuilder::Shapes NXOpen::Features::SheetMetal::GussetBuilder::Shape ( )

Returns the shape
See Features::SheetMetal::GussetBuilder::Shapes for details.

        <br>

Created in NX7.5.0.

License requirements : None

NXOpen::Expression* NXOpen::Features::SheetMetal::GussetBuilder::SideAngle ( )

Returns the side angle.

The value must be greater than or equal to zero.
Created in NX7.5.0.

License requirements : None

NXOpen::SelectEdge* NXOpen::Features::SheetMetal::GussetBuilder::StartEdge ( )

Returns the start edge
Selects the edge on the bend face to determine the gusset offset direction.

        <br>

Created in NX7.5.0.

License requirements : None

NXOpen::Features::SheetMetal::GussetBuilder::Types NXOpen::Features::SheetMetal::GussetBuilder::Type ( )

Returns the type of Gusset feature
Created in NX7.5.0.

License requirements : None

NXOpen::Expression* NXOpen::Features::SheetMetal::GussetBuilder::Width ( )

Returns the width value for the Gusset
Created in NX7.5.0.

License requirements : None

NXOpen::Features::SheetMetal::GussetBuilder::WidthSides NXOpen::Features::SheetMetal::GussetBuilder::WidthSide ( )

Returns the width side
Defines the side of the profile to which material should be added or from which material should be removed to construct the feature.

           The side option is not required when the profile is closed.
        <br>

Created in NX7.5.0.

License requirements : None

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

Features_SheetMetal_GussetBuilder.hxx

Public Types

Public Member Functions

Detailed Description

Member Enumeration Documentation

Member Function Documentation