FlatSolidBuilder Class — NXOpen Python API Reference 12.0.0 documentation

# FlatSolidBuilder Class

class `NXOpen.Features.SheetMetal.``FlatSolidBuilder`

  Bases: `NXOpen.Features.SheetMetal.SheetmetalBaseBuilder`

  Represents a Flat As Solid feature builder.

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

  Default values.

  Property | Value
  --- | ---
  Associative | true
  InnerCornerTreatment.TreatmentType | None
  InnerCornerTreatment.UseGlobal | 1
  InnerCornerTreatment.Value.Value | 0 (millimeters part), 0 (inches part)
  TransformComponents | None
  TransformRestrictionAreas | 0

  New in version NX4.0.0.

# Properties

Property | Description
--- | ---
AddedGeometry | Returns the added geometry selection
Associative | Returns or sets the setting which decides whether the flattened solid will be associative to parent body.
FixAtTimestamp | Returns or sets the setting decides whether the flattened solid will be fixed at timestamp.
InnerCornerTreatment | Returns the inner corner treatment corner object
Orientation | Returns or sets the option which decides if the flattened solid will be transformed to Absolute CSYS.
OrientationCsys | Returns or sets the orientation csys ** This is applicable to flat solid features created (or renewed) in NX12 and later release.
OuterCornerTreatment | Returns the outer corner treatment corner object
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
ReferenceVertex | Returns or sets the end of the edge where the tangent will define the x axis for flat as solid.
StationaryFace | Returns the stationary face selection
SurroundingPatchSurfaceFilename | Returns or sets the surrounding patch surface filename
Tag | Returns the Tag for this object.
TransformComponents | Returns or sets the setting indicating how to represent transformed components in flat solid.
TransformRestrictionAreas | Returns or sets the setting indicating whether to transform restriction areas in flat solid.
TransformToAbsoluteCsys | Returns or sets the flag which decides if the flattened solid will be transformed to Absolute CSYS.
XAxisEdge | Returns the x axis edge selection

# Methods

Method | Description
--- | ---
Commit | Commits any edits that have been applied to the builder.
CommitFeature | Commits the feature parameters and creates the feature
Destroy | Deletes the builder, and cleans up any objects created by the builder.
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.
HideInternalParentFeatureAfterEdit | Re-suppress an internal parent feature (a slave feature) after it has been edited.
SetApplicationContext | Set the application context.
SetParentFeatureInternal | Set the parent features which would be internal or slaves to the feature being created or commited
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 | Validate the builder data

# Enumerations

FlatSolidBuilderOrientationType Enumeration | The enum defines how to orient flat solid body.
FlatSolidBuilderTransformComponentsOption Enumeration | The enum defines how to represent PCB components on flat solid.

# Property Detail

## AddedGeometry

`FlatSolidBuilder.``AddedGeometry`

  Returns the added geometry selection

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

  Getter Method

  Signature `AddedGeometry`

  Returns: |
  Return type: | `NXOpen.Section`

  New in version NX6.0.0.

  License requirements: None.

## Associative

`FlatSolidBuilder.``Associative`

  Returns or sets the setting which decides whether the flattened solid will be associative to parent body.

  ** This is applicable to flat solid features created in NX12 and later release. ** Cannot change during feature edit if the feature was created as non associative.

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

  Getter Method

  Signature `Associative`

  Returns: | True = Feature is associative, False = Feature is not associative.
  Return type: | bool

  New in version NX12.0.0.

  License requirements: None.

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

  Setter Method

  Signature `Associative`

  Parameters: | associative (bool) – True = Feature is associative, False = Feature is not associative.

  New in version NX12.0.0.

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

## FixAtTimestamp

`FlatSolidBuilder.``FixAtTimestamp`

  Returns or sets the setting decides whether the flattened solid will be fixed at timestamp.

  ** This is applicable to flat solid features created in NX12 and later release. ** Cannot change during feature edit if the feature was created as fixed at timestamp.

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

  Getter Method

  Signature `FixAtTimestamp`

  Returns: | True = Fix at Timestamp, False = Do not Fix at Timestamp.
  Return type: | bool

  New in version NX12.0.0.

  License requirements: None.

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

  Setter Method

  Signature `FixAtTimestamp`

  Parameters: | fixAtTimestamp (bool) – True = Fix at Timestamp, False = Do not Fix at Timestamp.

  New in version NX12.0.0.

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

## InnerCornerTreatment

`FlatSolidBuilder.``InnerCornerTreatment`

  Returns the inner corner treatment corner object

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

  Getter Method

  Signature `InnerCornerTreatment`

  Returns: |
  Return type: | `NXOpen.Features.SheetMetal.CornerTreatmentBuilder`

  New in version NX6.0.0.

  License requirements: None.

## Orientation

`FlatSolidBuilder.``Orientation`

  Returns or sets the option which decides if the flattened solid will be transformed to Absolute CSYS.

  This is applicable to flat solid / flat pattern features created (or renewed) to NX12 and later release.

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

  Getter Method

  Signature `Orientation`

  Returns: |
  Return type: | `NXOpen.Features.SheetMetal.FlatSolidBuilderOrientationType`

  New in version NX12.0.0.

  License requirements: None.

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

  Setter Method

  Signature `Orientation`

  Parameters: | orientation (`NXOpen.Features.SheetMetal.FlatSolidBuilderOrientationType`) –

  New in version NX12.0.0.

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

## OrientationCsys

`FlatSolidBuilder.``OrientationCsys`

  Returns or sets the orientation csys ** This is applicable to flat solid features created (or renewed) in NX12 and later release.

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

  Getter Method

  Signature `OrientationCsys`

  Returns: |
  Return type: | `NXOpen.CoordinateSystem`

  New in version NX12.0.0.

  License requirements: None.

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

  Setter Method

  Signature `OrientationCsys`

  Parameters: | csys (`NXOpen.CoordinateSystem`) –

  New in version NX12.0.0.

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

## OuterCornerTreatment

`FlatSolidBuilder.``OuterCornerTreatment`

  Returns the outer corner treatment corner object

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

  Getter Method

  Signature `OuterCornerTreatment`

  Returns: |
  Return type: | `NXOpen.Features.SheetMetal.CornerTreatmentBuilder`

  New in version NX6.0.0.

  License requirements: None.

## ReferenceVertex

`FlatSolidBuilder.``ReferenceVertex`

  Returns or sets the end of the edge where the tangent will define the x axis for flat as solid.

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

  Getter Method

  Signature `ReferenceVertex`

  Returns: | One of the end points of the reference 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”)

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

  Setter Method

  Signature `ReferenceVertex`

  Parameters: | vertex (`NXOpen.Point3d`) – One of the end points of the reference edge.

  New in version NX4.0.0.

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

## StationaryFace

`FlatSolidBuilder.``StationaryFace`

  Returns the stationary face selection

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

  Getter Method

  Signature `StationaryFace`

  Returns: |
  Return type: | `NXOpen.SelectFace`

  New in version NX6.0.0.

  License requirements: None.

## TransformComponents

`FlatSolidBuilder.``TransformComponents`

  Returns or sets the setting indicating how to represent transformed components in flat solid.

  Only applies to the Flexible Printed Circuit Design application and will have no effect in Sheet Metal.

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

  Getter Method

  Signature `TransformComponents`

  Returns: |
  Return type: | `NXOpen.Features.SheetMetal.FlatSolidBuilderTransformComponentsOption`

  New in version NX10.0.0.

  License requirements: None.

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

  Setter Method

  Signature `TransformComponents`

  Parameters: | transformComponents (`NXOpen.Features.SheetMetal.FlatSolidBuilderTransformComponentsOption`) –

  New in version NX10.0.0.

  License requirements: nx_flexible_pcb (“NX Flexible PCB”)

## TransformRestrictionAreas

`FlatSolidBuilder.``TransformRestrictionAreas`

  Returns or sets the setting indicating whether to transform restriction areas in flat solid.

  Only applies to the Flexible Printed Circuit Design application and will have no effect in Sheet Metal.

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

  Getter Method

  Signature `TransformRestrictionAreas`

  Returns: |
  Return type: | bool

  New in version NX10.0.0.

  License requirements: None.

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

  Setter Method

  Signature `TransformRestrictionAreas`

  Parameters: | transformRestrictionAreas (bool) –

  New in version NX10.0.0.

  License requirements: nx_flexible_pcb (“NX Flexible PCB”)

## TransformToAbsoluteCsys

`FlatSolidBuilder.``TransformToAbsoluteCsys`

  Returns or sets the flag which decides if the flattened solid will be transformed to Absolute CSYS.

  This is applicable to flat solid / flat pattern features created before NX12 release and not yet renewed. The API can not be deprecated because it is required to edit features created before NX12 release. But user should modify automation programs written before NX12 and replace use this option with the orientation option, before using the program to create new features in NX12 or later.

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

  Getter Method

  Signature `TransformToAbsoluteCsys`

  Returns: | True = Transform to ABS, False = Do not transform to ABS.
  Return type: | bool

  New in version NX4.0.0.

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

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

  Setter Method

  Signature `TransformToAbsoluteCsys`

  Parameters: | transformFlag (bool) – True = Transform to ABS, False = Do not transform to ABS.

  New in version NX4.0.0.

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

## XAxisEdge

`FlatSolidBuilder.``XAxisEdge`

  Returns the x axis edge selection

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

  Getter Method

  Signature `XAxisEdge`

  Returns: |
  Return type: | `NXOpen.SelectEdge`

  New in version NX6.0.0.

  License requirements: None.

# Method Detail

## Validate

`FlatSolidBuilder.``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

`FlatSolidBuilder.``ValidateBuilderData`

  Validate the builder data

  Signature `ValidateBuilderData()`

  Returns: | 0 Means no errors.
  Return type: | int

  New in version NX4.0.0.

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