NX Open C++ Reference Guide
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Represents a NX Sheet Metal Features::Gusset builder
To create a new instance of this class, use Features::SheetMetal::SheetmetalManager::CreateGussetBuilder
Default values.
More...
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. |
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.
This enum represents the different options for placing an automatic profile Gusset.
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 different options for thickening the user defined profile Gusset.
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. |
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
NXOpen::Vector3d NXOpen::Features::SheetMetal::GussetBuilder::GetPlacementOriginAndDirection | ( | NXOpen::Point3d * | origin | ) |
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.
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.
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
candidateEdges | An 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
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
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
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")
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")
placementType | placementtype |
void NXOpen::Features::SheetMetal::GussetBuilder::SetShape | ( | NXOpen::Features::SheetMetal::GussetBuilder::Shapes | shape | ) |
Sets the shape
See Features::SheetMetal::GussetBuilder::Shapes for details.
Created in NX7.5.0.
License requirements : nx_sheet_metal ("NX Sheet Metal")
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")
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.
Created in NX7.5.0.
License requirements : nx_sheet_metal ("NX Sheet Metal")
widthSide | widthside |
NXOpen::Features::SheetMetal::GussetBuilder::Shapes NXOpen::Features::SheetMetal::GussetBuilder::Shape | ( | ) |
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
NXOpen::Features::SheetMetal::GussetBuilder::Types NXOpen::Features::SheetMetal::GussetBuilder::Type | ( | ) |
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
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.
Created in NX7.5.0.
License requirements : None