FlangeBuilder Class

class NXOpen.Features.SheetMetal.FlangeBuilder

Bases: NXOpen.Features.SheetMetal.SheetmetalBaseBuilder

Represents a Flange feature builder.

To create a new instance of this class, use NXOpen.Features.SheetMetal.SheetmetalManager.CreateFlangeFeatureBuilder()

New in version NX4.0.0.

Properties

Property	Description
BendAngle	Returns the bend angle for flange.
BendOptions	Returns the bend options object.
Edge	Returns or sets the edge on which the flange is created.
FirstDistance	Returns a distance based on NXOpen.Features.SheetMetal.FlangeBuilder.WidthType().
InsetType	Returns or sets the inset type (inside, outside, bendoutside) for the flange.
Length	Returns the length of the flange.
LengthType	Returns or sets a enum indicating the length type.
MatchFaceOption	Returns or sets the match face selection type.
MatchPlane	Returns or sets the Match Plane.
Offset	Returns the offset value for the flange.
OffsetType	Returns or sets the offset type for the flange.
ParentFeatureInternal	Returns or sets whether or not the latest timestamped parent feature of this feature should be made internal
PatchSolutionFlag	Returns or sets the patch solution flag
PatchSurfaceFilename	Returns or sets the patch surface filename
SecondDistance	Returns a distance based on NXOpen.Features.SheetMetal.FlangeBuilder.WidthType().
SurroundingPatchSurfaceFilename	Returns or sets the surrounding patch surface filename
Tag	Returns the Tag for this object.
Vertex	Returns or sets the vertex on the flange edge, needed to dimension the flange width.
WidthType	Returns or sets the width type for flange.

Methods

Method	Description
Commit	Commits any edits that have been applied to the builder.
CommitFeature	Commits the feature parameters and creates the feature
DeleteSketch	Delete the flange sketch
Destroy	Deletes the builder, and cleans up any objects created by the builder.
EditSketch	Edit the sketch base on a new edge you need to call SetEdge to set a new edge
GetApplicationContext	Get the application context.
GetCommittedObjects	For builders that create more than one object, this method returns the objects that are created by commit.
GetFeature	Returns the feature currently being edited by this builder.
GetObject	Returns the object currently being edited by this builder.
GetSketch	Get the flange sketch
HideInternalParentFeatureAfterEdit	Re-suppress an internal parent feature (a slave feature) after it has been edited.
SetApplicationContext	Set the application context.
SetBendAngle
SetFirstDistance
SetLength
SetOffset
SetParentFeatureInternal	Set the parent features which would be internal or slaves to the feature being created or commited
SetSecondDistance
ShowInternalParentFeatureForEdit	Unsuppress an internal parent feature (a slave feature) so it can be edited.
ShowResults	Updates the model to reflect the result of an edit to the model for all builders that support showing results.
UnsetParentFeatureInternal	Set the internal parent feature of the feature being edited to external
Validate	Validate whether the inputs to the component are sufficient for commit to be called.
ValidateBuilderData	Verify that the builder data is valid for creating a flange.

Enumerations

FlangeBuilderInsetTypeOptions Enumeration	This enum represents the inset type for the material of the flange.
FlangeBuilderLengthTypeOptions Enumeration	This enum indicates the two ways that the flange length can be measured.
FlangeBuilderMatchFaceOptions Enumeration	This enum represents the match face option for the flange.
FlangeBuilderOffsetTypeOptions Enumeration	This enum represents the offset type for the flange.
FlangeBuilderWidthTypeOptions Enumeration	This enum represents the width type for the flange.

Property Detail

BendAngle

FlangeBuilder.BendAngle

Returns the bend angle for flange.

It should be set in degrees (??????).

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Getter Method

Signature BendAngle

Returns: Return type:NXOpen.Expression

New in version 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”)

BendOptions

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.

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Getter Method

Signature BendOptions

Returns: Return type:NXOpen.Features.SheetMetal.BendOptions

New in version 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

FlangeBuilder.Edge

Returns or sets the edge on which the flange is created.

The edge should be linear and it should not be a thickness edge.

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Getter Method

Signature Edge

Returns:The flange is created on this edge. Return type:NXOpen.Edge

New in version 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”)

-------------------------------------

Setter Method

Signature Edge

Parameters:edge (NXOpen.Edge) – The flange is created on this edge.

New in version 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

FlangeBuilder.FirstDistance

Returns a distance based on NXOpen.Features.SheetMetal.FlangeBuilder.WidthType().

See NXOpen.Features.SheetMetal.FlangeBuilder.WidthType`() for a detailed desctiption of what this distance stands for.

-------------------------------------

Getter Method

Signature FirstDistance

Returns: Return type:NXOpen.Expression

New in version 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

FlangeBuilder.InsetType

Returns or sets the inset type (inside, outside, bendoutside) for the flange.

-------------------------------------

Getter Method

Signature InsetType

Returns: Return type:NXOpen.Features.SheetMetal.FlangeBuilderInsetTypeOptions

New in version 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”)

-------------------------------------

Setter Method

Signature InsetType

Parameters:insetType (NXOpen.Features.SheetMetal.FlangeBuilderInsetTypeOptions) –

New in version 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

FlangeBuilder.Length

Returns the length of the flange.

-------------------------------------

Getter Method

Signature Length

Returns: Return type:NXOpen.Expression

New in version 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

FlangeBuilder.LengthType

Returns or 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 NXOpen.Features.SheetMetal.FlangeBuilderLengthTypeOptions.InsideDimension or if the flange length is specifed from the other edge use value NXOpen.Features.SheetMetal.FlangeBuilderLengthTypeOptions.OutsideDimension.

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 NXOpen.Features.SheetMetal.FlangeBuilderLengthTypeOptions.InsideDimension or if the flange length is specifed from the outer mold line use value NXOpen.Features.SheetMetal.FlangeBuilderLengthTypeOptions.OutsideDimension.

-------------------------------------

Getter Method

Signature LengthType

Returns: Return type:NXOpen.Features.SheetMetal.FlangeBuilderLengthTypeOptions

New in version 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”)

-------------------------------------

Setter Method

Signature LengthType

Parameters:lengthType (NXOpen.Features.SheetMetal.FlangeBuilderLengthTypeOptions) –

New in version 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”)

MatchFaceOption

FlangeBuilder.MatchFaceOption

Returns or sets the match face selection type.

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

-------------------------------------

Getter Method

Signature MatchFaceOption

Returns: Return type:NXOpen.Features.SheetMetal.FlangeBuilderMatchFaceOptions

New in version NX8.0.0.

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

-------------------------------------

Setter Method

Signature MatchFaceOption

Parameters:matchFaceOption (NXOpen.Features.SheetMetal.FlangeBuilderMatchFaceOptions) –

New in version NX8.0.0.

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

MatchPlane

FlangeBuilder.MatchPlane

Returns or sets the Match Plane.

-------------------------------------

Getter Method

Signature MatchPlane

Returns: Return type:NXOpen.Plane

New in version NX8.0.0.

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

-------------------------------------

Setter Method

Signature MatchPlane

Parameters:matchPlane (NXOpen.Plane) –

New in version NX8.0.0.

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

Offset

FlangeBuilder.Offset

Returns the offset value for the flange.

-------------------------------------

Getter Method

Signature Offset

Returns:The flange offset value Return type:NXOpen.Expression

New in version 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

FlangeBuilder.OffsetType

Returns or sets the offset type for the flange.

-------------------------------------

Getter Method

Signature OffsetType

Returns:The flange can be offset inside or outside. Return type:NXOpen.Features.SheetMetal.FlangeBuilderOffsetTypeOptions

New in version 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”)

-------------------------------------

Setter Method

Signature OffsetType

Parameters:offsetType (NXOpen.Features.SheetMetal.FlangeBuilderOffsetTypeOptions) – The flange can be offset inside or outside.

New in version 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

FlangeBuilder.SecondDistance

Returns a distance based on NXOpen.Features.SheetMetal.FlangeBuilder.WidthType().

See NXOpen.Features.SheetMetal.FlangeBuilder.WidthType`() for a detailed desctiption of what this distance stands for.

-------------------------------------

Getter Method

Signature SecondDistance

Returns: Return type:NXOpen.Expression

New in version 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

FlangeBuilder.Vertex

Returns or sets the vertex on the flange edge, needed to dimension the flange width.

The vertex needs to be specified ONLY if NXOpen.Features.SheetMetal.FlangeBuilder.WidthType() is set to one of NXOpen.Features.SheetMetal.FlangeBuilderWidthTypeOptions.AtEdgeEnd, NXOpen.Features.SheetMetal.FlangeBuilderWidthTypeOptions.FromEdgeEnd. In case of NXOpen.Features.SheetMetal.FlangeBuilderWidthTypeOptions.FromBothEnds, the start vertex of the edge is assumed to be the start point for NXOpen.Features.SheetMetal.FlangeBuilder.FirstDistance().

-------------------------------------

Getter Method

Signature Vertex

Returns:A vertex on the flange edge. Return type:NXOpen.Point3d

New in version 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”)

-------------------------------------

Setter Method

Signature Vertex

Parameters:vertex (NXOpen.Point3d) – A vertex on the flange edge.

New in version 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

FlangeBuilder.WidthType

Returns or sets the width type for flange.

Use one of the values from NXOpen.Features.SheetMetal.FlangeBuilderWidthTypeOptions. Depending on which of the values from the enum is used, none, either or both of the distance values from NXOpen.Features.SheetMetal.FlangeBuilder.FirstDistance() and NXOpen.Features.SheetMetal.FlangeBuilder.SecondDistance() may be used. Here is a description of the distances:

If the value is NXOpen.Features.SheetMetal.FlangeBuilderWidthTypeOptions.FullEdge, then both the FirstDistance() and NXOpen.Features.SheetMetal.FlangeBuilder.SecondDistance() values are unused.

If the value is NXOpen.Features.SheetMetal.FlangeBuilderWidthTypeOptions.CenterOfEdge, then both the NXOpen.Features.SheetMetal.FlangeBuilder.FirstDistance() and NXOpen.Features.SheetMetal.FlangeBuilder.SecondDistance() represent exactly half the width of the flange.

If the value is NXOpen.Features.SheetMetal.FlangeBuilderWidthTypeOptions.AtEdgeEnd, then NXOpen.Features.SheetMetal.FlangeBuilder.FirstDistance() represents the width of the flange, starting from the end of the edge specified by the NXOpen.Features.SheetMetal.FlangeBuilder.Vertex() and the NXOpen.Features.SheetMetal.FlangeBuilder.SecondDistance() is not used.

If the value is NXOpen.Features.SheetMetal.FlangeBuilderWidthTypeOptions.FromEdgeEnd, then NXOpen.Features.SheetMetal.FlangeBuilder.FirstDistance() represents the distance of the start point of the flange from the end of the edge specified by NXOpen.Features.SheetMetal.FlangeBuilder.Vertex() and NXOpen.Features.SheetMetal.FlangeBuilder.SecondDistance() represents the width of the flange.

If the value is NXOpen.Features.SheetMetal.FlangeBuilderWidthTypeOptions.FromBothEnds, then NXOpen.Features.SheetMetal.FlangeBuilder.FirstDistance() represents the distance of the start point of the flange from the from the end of the edge specified by NXOpen.Features.SheetMetal.FlangeBuilder.Vertex() and NXOpen.Features.SheetMetal.FlangeBuilder.SecondDistance() represents the distance of the end point of the flange from end of the edge opposite to the end specified by NXOpen.Features.SheetMetal.FlangeBuilder.Vertex().

The value NXOpen.Features.SheetMetal.FlangeBuilderWidthTypeOptions.Custom, 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 NXOpen.Features.SheetMetal.FlangeBuilder.FirstDistance() and NXOpen.Features.SheetMetal.FlangeBuilder.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.

-------------------------------------

Getter Method

Signature WidthType

Returns: Return type:NXOpen.Features.SheetMetal.FlangeBuilderWidthTypeOptions

New in version 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”)

-------------------------------------

Setter Method

Signature WidthType

Parameters:widthType (NXOpen.Features.SheetMetal.FlangeBuilderWidthTypeOptions) –

New in version 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”)

Method Detail

DeleteSketch

FlangeBuilder.DeleteSketch

Delete the flange sketch

Signature DeleteSketch()

New in version 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”)

EditSketch

FlangeBuilder.EditSketch

Edit the sketch base on a new edge you need to call SetEdge to set a new edge

Signature EditSketch()

New in version 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”)

GetSketch

FlangeBuilder.GetSketch

Get the flange sketch

Signature GetSketch()

Returns: Return type:NXOpen.Sketch

New in version 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”)

SetBendAngle

FlangeBuilder.SetBendAngle

Signature SetBendAngle(bendAngle)

Parameters:bendAngle (str) –

New in version NX4.0.0.

Deprecated since version NX10.0.0: Use NXOpen.Expression.RightHandSide() on the NXOpen.Expression object returned from NXOpen.Features.SheetMetal.FlangeBuilder.BendAngle() instead.

License requirements: nx_sheet_metal (“NX Sheet Metal”) OR nx_flexible_pcb (“NX Flexible PCB”) OR nx_ship_detail (“Ship Detail Design”)

SetFirstDistance

FlangeBuilder.SetFirstDistance

Signature SetFirstDistance(firstDistance)

Parameters:firstDistance (str) –

New in version NX4.0.0.

Deprecated since version NX10.0.0: Use NXOpen.Expression.RightHandSide() on the NXOpen.Expression object returned from NXOpen.Features.SheetMetal.FlangeBuilder.FirstDistance() instead.

License requirements: nx_sheet_metal (“NX Sheet Metal”) OR nx_flexible_pcb (“NX Flexible PCB”) OR nx_ship_detail (“Ship Detail Design”)

SetLength

FlangeBuilder.SetLength

Signature SetLength(length)

Parameters:length (str) –

New in version NX4.0.0.

Deprecated since version NX10.0.0: Use NXOpen.Expression.RightHandSide() on the NXOpen.Expression object returned from NXOpen.Features.SheetMetal.FlangeBuilder.Length() instead.

License requirements: nx_sheet_metal (“NX Sheet Metal”) OR nx_flexible_pcb (“NX Flexible PCB”) OR nx_ship_detail (“Ship Detail Design”)

SetOffset

FlangeBuilder.SetOffset

Signature SetOffset(offset)

Parameters:offset (str) – The flange offset value

New in version NX4.0.0.

Deprecated since version NX10.0.0: Use NXOpen.Expression.RightHandSide() on the NXOpen.Expression object returned from NXOpen.Features.SheetMetal.FlangeBuilder.Offset() instead.

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

SetSecondDistance

FlangeBuilder.SetSecondDistance

Signature SetSecondDistance(secondDistance)

Parameters:secondDistance (str) –

New in version NX4.0.0.

Deprecated since version NX10.0.0: Use NXOpen.Expression.RightHandSide() on the NXOpen.Expression object returned from NXOpen.Features.SheetMetal.FlangeBuilder.SecondDistance() instead.

License requirements: nx_sheet_metal (“NX Sheet Metal”) OR nx_flexible_pcb (“NX Flexible PCB”) OR nx_ship_detail (“Ship Detail Design”)

Validate

FlangeBuilder.Validate

Validate whether the inputs to the component are sufficient for commit to be called.

If the component is not in a state to commit then an exception is thrown. For example, if the component requires you to set some property, this method will throw an exception if you haven’t set it. This method throws a not-yet-implemented NXException for some components.

Signature Validate()

Returns:Was self validation successful Return type:bool

New in version NX3.0.1.

License requirements: None.

ValidateBuilderData

FlangeBuilder.ValidateBuilderData

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

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

Signature ValidateBuilderData()

Returns:A value of zero is returned if the data in the builder is valid. Return type:int

New in version 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”)