FlangeBuilder Class — NXOpen Python API Reference 12.0.0 documentation

# 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 (??????).

  `-------------------------------------`

  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.

  `-------------------------------------`

  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.

  `-------------------------------------`

  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”)