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

Represents a Flange feature builder. More...

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

List of all members.

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::ExpressionBendAngle ()
 Returns the bend angle for flange.
NXOpen::Features::SheetMetal::BendOptionsBendOptions ()
 Returns the bend options object.
void DeleteSketch ()
 Delete the flange sketch
Created in NX6.0.0.
NXOpen::EdgeEdge ()
 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::ExpressionFirstDistance ()
 Returns a distance based on WidthType .
NXOpen::SketchGetSketch ()
 Get the flange sketch.
NXOpen::Features::SheetMetal::FlangeBuilder::InsetTypeOptions InsetType ()
 Returns the inset type (inside, outside, bendoutside) for the flange.
NXOpen::ExpressionLength ()
 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::PlaneMatchPlane ()
 Returns the Match Plane.
NXOpen::ExpressionOffset ()
 Returns the offset value for the flange.
NXOpen::Features::SheetMetal::FlangeBuilder::OffsetTypeOptions OffsetType ()
 Returns the offset type for the flange.
NXOpen::ExpressionSecondDistance ()
 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.

Detailed Description

Represents a Flange feature builder.


To create a new instance of this class, use Features::SheetMetal::SheetmetalManager::CreateFlangeFeatureBuilder

Created in NX4.0.0.


Member Enumeration Documentation

This enum represents the inset type for the material of the flange.

Enumerator:
InsetTypeOptionsMaterialInside 

The flange is flush with the thickness face on the inside.

InsetTypeOptionsMaterialOutside 

The flange is flush with the thickness face on the outside.

InsetTypeOptionsBendOutside 

The bend and flange are outside the thickness face.

This enum indicates the two ways that the flange length can be measured.

Enumerator:
LengthTypeOptionsInsideDimension 

The flange length is dimensioned to the Inner Mold line.

LengthTypeOptionsOutsideDimension 

The flange length is dimensioned to the Outer Mold Line.

LengthTypeOptionsWebDimension 

The flange length is dimensioned to the Bend Tangent Line.

This enum represents the match face option for the flange.

Enumerator:
MatchFaceOptionsNone 

The flange is placed on the selected edge.

MatchFaceOptionsUntilSelected 

The flange face is extended until the selected plane.

This enum represents the offset type for the flange.

Enumerator:
OffsetTypeOptionsInside 

The flange is offset to the inside of the face.

OffsetTypeOptionsOutside 

The flange is offset to the outside of the face.

This enum represents the width type for the flange.

Enumerator:
WidthTypeOptionsFullEdge 

The flange spans the entire edge.

WidthTypeOptionsCenterOfEdge 

The flange is centered on the edge.

WidthTypeOptionsAtEdgeEnd 

The flange starts from the specified end of the edge.

WidthTypeOptionsFromEdgeEnd 

The flange starts at a specified distance from an end of the edge.

WidthTypeOptionsFromBothEnds 

The flange starts and ends at specified distances from the ends of the edge.

WidthTypeOptionsCustom 

The flange sketch has been edited after creation and may or may not conform to any of the above.


Member Function Documentation

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")

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.

Returns:

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 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")

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 face selection type.


None for Regular Flange. Until Selected for Match To Face type Flange .


Created in NX8.0.0.

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

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 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")

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")


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")

Parameters:
bendAngle
NOTE: The full Unicode character set is not supported for this parameter.

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")

Parameters:
edgeThe flange is created on this 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")

Parameters:
firstDistance
NOTE: The full Unicode character set is not supported for this parameter.

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")

Parameters:
insetTypeinset type


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")

Parameters:
length
NOTE: The full Unicode character set is not supported for this parameter.

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")

Parameters:
lengthTypelength type

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

Parameters:
matchFaceOptionmatchfaceoption

Sets the Match Plane.


Created in NX8.0.0.

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

Parameters:
matchPlanematchplane


Created in NX4.0.0.



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

Parameters:
offsetThe flange offset value
NOTE: The full Unicode character set is not supported for this parameter.

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")

Parameters:
offsetTypeThe flange can be offset inside or outside.


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")

Parameters:
secondDistance
NOTE: The full Unicode character set is not supported for this parameter.

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")

Parameters:
vertexA vertex on the flange edge.

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")

Parameters:
widthTypewidth type

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


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

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

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")


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