NX Open C++ Reference Guide
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Represents a Flange feature builder. More...
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. | |
NXOpen::Features::SheetMetal::BendOptions * | BendOptions () |
Returns the bend options object. | |
void | DeleteSketch () |
Delete the flange sketch Created in NX6.0.0. | |
NXOpen::Edge * | Edge () |
Returns the edge on which the flange is created. | |
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. | |
NXOpen::Expression * | FirstDistance () |
Returns a distance based on WidthType . | |
NXOpen::Sketch * | GetSketch () |
Get the flange sketch. | |
NXOpen::Features::SheetMetal::FlangeBuilder::InsetTypeOptions | InsetType () |
Returns the inset type (inside, outside, bendoutside) for the flange. | |
NXOpen::Expression * | Length () |
Returns the length of the flange. | |
NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptions | LengthType () |
Returns a enum indicating the length type. | |
NXOpen::Features::SheetMetal::FlangeBuilder::MatchFaceOptions | MatchFaceOption () |
Returns the match face selection type. | |
NXOpen::Plane * | MatchPlane () |
Returns the Match Plane. | |
NXOpen::Expression * | Offset () |
Returns the offset value for the flange. | |
NXOpen::Features::SheetMetal::FlangeBuilder::OffsetTypeOptions | OffsetType () |
Returns the offset type for the flange. | |
NXOpen::Expression * | SecondDistance () |
Returns a distance based on WidthType . | |
void | SetBendAngle (const NXString &bendAngle) |
Created in NX4.0.0. | |
void | SetEdge (NXOpen::Edge *edge) |
Sets the edge on which the flange is created. | |
void | SetFirstDistance (const NXString &firstDistance) |
Created in NX4.0.0. | |
void | SetInsetType (NXOpen::Features::SheetMetal::FlangeBuilder::InsetTypeOptions insetType) |
Sets the inset type (inside, outside, bendoutside) for the flange. | |
void | SetLength (const NXString &length) |
Created in NX4.0.0. | |
void | SetLengthType (NXOpen::Features::SheetMetal::FlangeBuilder::LengthTypeOptions lengthType) |
Sets a enum indicating the length type. | |
void | SetMatchFaceOption (NXOpen::Features::SheetMetal::FlangeBuilder::MatchFaceOptions matchFaceOption) |
Sets the match face selection type. | |
void | SetMatchPlane (NXOpen::Plane *matchPlane) |
Sets the Match Plane. | |
void | SetOffset (const NXString &offset) |
Created in NX4.0.0. | |
void | SetOffsetType (NXOpen::Features::SheetMetal::FlangeBuilder::OffsetTypeOptions offsetType) |
Sets the offset type for the flange. | |
void | SetSecondDistance (const NXString &secondDistance) |
Created in NX4.0.0. | |
void | SetVertex (const NXOpen::Point3d &vertex) |
Sets the vertex on the flange edge, needed to dimension the flange width. | |
void | SetWidthType (NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptions widthType) |
Sets the width type for flange. | |
int | ValidateBuilderData () |
Verify that the builder data is valid for creating a flange. | |
NXOpen::Point3d | Vertex () |
Returns the vertex on the flange edge, needed to dimension the flange width. | |
NXOpen::Features::SheetMetal::FlangeBuilder::WidthTypeOptions | WidthType () |
Returns the width type for flange. |
Represents a Flange feature builder.
To create a new instance of this class, use Features::SheetMetal::SheetmetalManager::CreateFlangeFeatureBuilder
Created in NX4.0.0.
This enum represents the inset type for the material of the flange.
This enum indicates the two ways that the flange length can be measured.
This enum represents the width type for the flange.
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")
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")
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")
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")
Returns a distance based on WidthType .
See WidthType and 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")
Get the flange sketch.
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")
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 Features::SheetMetal::FlangeBuilder::LengthTypeOptionsInsideDimension or if the flange length is specifed from the other edge use value 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 Features::SheetMetal::FlangeBuilder::LengthTypeOptionsInsideDimension or if the flange length is specifed from the outer mold line use value Features::SheetMetal::FlangeBuilder::LengthTypeOptionsOutsideDimension or if the flange length is specifed from the bend tangent line use value 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")
Returns the Match Plane.
Created in NX8.0.0.
License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB")
Returns the offset value for the flange.
The direction of the offset is determined by the value off OffsetType .
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 distance based on WidthType .
See WidthType and 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 | ) |
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")
bendAngle | NOTE: The full Unicode character set is not supported for this parameter. |
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")
edge | The flange is created on this edge. |
void NXOpen::Features::SheetMetal::FlangeBuilder::SetFirstDistance | ( | const NXString & | 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")
firstDistance | NOTE: The full Unicode character set is not supported for this parameter. |
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")
insetType | inset type |
void NXOpen::Features::SheetMetal::FlangeBuilder::SetLength | ( | const NXString & | length | ) |
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")
length | NOTE: The full Unicode character set is not supported for this parameter. |
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 Features::SheetMetal::FlangeBuilder::LengthTypeOptionsInsideDimension or if the flange length is specifed from the other edge use value 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 Features::SheetMetal::FlangeBuilder::LengthTypeOptionsInsideDimension or if the flange length is specifed from the outer mold line use value Features::SheetMetal::FlangeBuilder::LengthTypeOptionsOutsideDimension or if the flange length is specifed from the bend tangent line use value 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")
lengthType | length type |
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")
matchPlane | matchplane |
void NXOpen::Features::SheetMetal::FlangeBuilder::SetOffset | ( | const NXString & | offset | ) |
Created in NX4.0.0.
License requirements : nx_sheet_metal ("NX Sheet Metal") OR nx_flexible_pcb ("NX Flexible PCB")
offset | The flange offset value NOTE: The full Unicode character set is not supported for this parameter. |
void NXOpen::Features::SheetMetal::FlangeBuilder::SetOffsetType | ( | NXOpen::Features::SheetMetal::FlangeBuilder::OffsetTypeOptions | offsetType | ) |
Sets the offset type for the flange.
Describes the value of the offset in Offset and SetOffset .
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")
offsetType | The flange can be offset inside or outside. |
void NXOpen::Features::SheetMetal::FlangeBuilder::SetSecondDistance | ( | const NXString & | secondDistance | ) |
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")
secondDistance | NOTE: The full Unicode character set is not supported for this parameter. |
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 WidthType is set to one of Features::SheetMetal::FlangeBuilder::WidthTypeOptionsAtEdgeEnd , Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromEdgeEnd . In case of Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromBothEnds , the start vertex of the edge is assumed to be the start point for 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")
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 Features::SheetMetal::FlangeBuilder::WidthTypeOptions . Depending on which of the values from the enum is used, none, either or both of the distance values from FirstDistance and SecondDistance may be used. Here is a description of the distances:
If the value is Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFullEdge , then both the FirstDistance and SecondDistance values are unused.
If the value is Features::SheetMetal::FlangeBuilder::WidthTypeOptionsCenterOfEdge , then both the FirstDistance and SecondDistance represent exactly half the width of the flange.
If the value is Features::SheetMetal::FlangeBuilder::WidthTypeOptionsAtEdgeEnd , then FirstDistance represents the width of the flange, starting from the end of the edge specified by the Vertex and the SecondDistance is not used.
If the value is Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromEdgeEnd , then FirstDistance represents the distance of the start point of the flange from the end of the edge specified by Vertex and SecondDistance represents the width of the flange.
If the value is Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromBothEnds , then FirstDistance represents the distance of the start point of the flange from the from the end of the edge specified by Vertex and SecondDistance represents the distance of the end point of the flange from end of the edge opposite to the end specified by Vertex .
The value 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 FirstDistance and 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")
widthType | width type |
Verify that the builder data is valid for creating a flange.
If the builder data is valid, return value is zero.
Returns the vertex on the flange edge, needed to dimension the flange width.
The vertex needs to be specified ONLY if WidthType is set to one of Features::SheetMetal::FlangeBuilder::WidthTypeOptionsAtEdgeEnd , Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromEdgeEnd . In case of Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromBothEnds , the start vertex of the edge is assumed to be the start point for 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 Features::SheetMetal::FlangeBuilder::WidthTypeOptions . Depending on which of the values from the enum is used, none, either or both of the distance values from FirstDistance and SecondDistance may be used. Here is a description of the distances:
If the value is Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFullEdge , then both the FirstDistance and SecondDistance values are unused.
If the value is Features::SheetMetal::FlangeBuilder::WidthTypeOptionsCenterOfEdge , then both the FirstDistance and SecondDistance represent exactly half the width of the flange.
If the value is Features::SheetMetal::FlangeBuilder::WidthTypeOptionsAtEdgeEnd , then FirstDistance represents the width of the flange, starting from the end of the edge specified by the Vertex and the SecondDistance is not used.
If the value is Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromEdgeEnd , then FirstDistance represents the distance of the start point of the flange from the end of the edge specified by Vertex and SecondDistance represents the width of the flange.
If the value is Features::SheetMetal::FlangeBuilder::WidthTypeOptionsFromBothEnds , then FirstDistance represents the distance of the start point of the flange from the from the end of the edge specified by Vertex and SecondDistance represents the distance of the end point of the flange from end of the edge opposite to the end specified by Vertex .
The value 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 FirstDistance and 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")