NX Open C++ Reference Guide
Public Types | Public Member Functions
NXOpen::Features::SheetMetal::GussetBuilder Class Reference

Represents a NX Sheet Metal Features::Gusset builder
To create a new instance of this class, use Features::SheetMetal::SheetmetalManager::CreateGussetBuilder
Default values. More...

Inheritance diagram for NXOpen::Features::SheetMetal::GussetBuilder:
NXOpen::Features::FeatureBuilder NXOpen::Builder NXOpen::TaggedObject NXOpen::GeometricUtilities::IComponentBuilder

List of all members.

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::SelectFaceBendFace ()
 Returns the bend face
Selects the bend face along which the gusset is placed.
NXOpen::ExpressionCornerRadius ()
 Returns the corner radius
This value is used only for the Features::SheetMetal::GussetBuilder::ShapesSquare shape.
NXOpen::ExpressionDepth ()
 Returns the depth
This value is used for the automatic profile Gussets.
NXOpen::ExpressionDieRadius ()
 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::ExpressionPlacementDistance ()
 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::ExpressionPlacementSpacing ()
 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::ExpressionPunchRadius ()
 Returns the punch radius value of the sharp edges of the top face.
NXOpen::SectionSection ()
 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::ExpressionSideAngle ()
 Returns the side angle.
NXOpen::SelectEdgeStartEdge ()
 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::ExpressionWidth ()
 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.

Detailed Description

Represents a NX Sheet Metal Features::Gusset builder
To create a new instance of this class, use Features::SheetMetal::SheetmetalManager::CreateGussetBuilder
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

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.

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.

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.

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

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")

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



Created in NX7.5.0.

License requirements : None

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

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

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

Get the placement origin and direction.


Get the point from which the placement distance will be measured and the direction along which the positive distance is defined.

Returns:
Direction along which the placement distance is measured.
Created in NX7.5.0.

License requirements : None
Parameters:
originStart point from which placement distance is measured.

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


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.


Created in NX7.5.0.

License requirements : None

Parameters:
candidateEdgesAn array of edges that are valid for selection as start edge

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

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

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

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

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

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

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:
placementCountplacementcount

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:
placementTypeplacementtype

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



Created in NX7.5.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters:
shapeshape

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



License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters:
typetype

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.


Created in NX7.5.0.

License requirements : nx_sheet_metal ("NX Sheet Metal")

Parameters:
widthSidewidthside

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



Created in NX7.5.0.

License requirements : None

Returns the side angle.

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

License requirements : None

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



Created in NX7.5.0.

License requirements : None

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



License requirements : None

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



License requirements : None

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.


Created in NX7.5.0.

License requirements : None


The documentation for this class was generated from the following file:
Copyright 2011 Siemens Product Lifecycle Management Software Inc. All Rights Reserved.