ThickenBuilder Class — NXOpen Python API Reference 12.0.0 documentation

# ThickenBuilder Class

class `NXOpen.Features.``ThickenBuilder`

  Bases: `NXOpen.Features.FeatureBuilder`

  Represents a builder for a `NXOpen.Features.Thicken` feature.

  This allows creation and editing of a Thicken feature which takes a set of faces and offsets them along their normals to create a solid body which has constant thickness. Since this can not be done precisely for the supported geometry types there is a tolerance to specify the accuracy of the result. Inputs to this class can be convergent objects.

  To create a new instance of this class, use `NXOpen.Features.FeatureCollection.CreateThickenBuilder()`

  Default values.

  Property | Value
  --- | ---
  ApproximateOffset | True
  BooleanOperation.Type | Create
  FirstOffset.Value | 2.5 (millimeters part), 0.1 (inches part)
  RemoveGashes | False
  ReverseDirection | False
  SecondOffset.Value | 0.0 (millimeters part), 0.0 (inches part)

  New in version NX5.0.0.

# Properties

Property | Description
--- | ---
ApproximateOffset | Returns or sets the approximate offset surface or resolve self-intersections using patches option.
BooleanOperation | Returns the boolean operation.
FaceCollector | Returns the faces to thicken.
FirstOffset | Returns the first offset.
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
RegionSectionList | Returns the list of SC_section The sections with corresponding expression for the Thicken feature
RegionToPierce | Returns the section for regions to pierce The section associated for the Thicken feature
RemoveGashes | Returns or sets the remove gashes option.
ReverseDirection | Returns or sets the reverse direction.
SecondOffset | Returns the second offset.
SurroundingPatchSurfaceFilename | Returns or sets the surrounding patch surface filename
Tag | Returns the Tag for this object.
Tolerance | Returns or sets the tolerance.

# 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.
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.
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.

# Property Detail

## ApproximateOffset

`ThickenBuilder.``ApproximateOffset`

  Returns or sets the “approximate offset surface” or “resolve self-intersections using patches” option.

  The option to approximate offset surfaces for thickening operation is renamed to “resolve self-intersections using patches”. This option is available for editing pre-NX8 thicken features only. The value set by the user for this option is ignored for thicken features created from NX8 onwards and its value will always be set to true internally for thicken features created in NX8 and later.

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

  Getter Method

  Signature `ApproximateOffset`

  Returns: |
  Return type: | bool

  New in version NX5.0.0.

  License requirements: None.

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

  Setter Method

  Signature `ApproximateOffset`

  Parameters: | approximateOffset (bool) –

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

## BooleanOperation

`ThickenBuilder.``BooleanOperation`

  Returns the boolean operation.

  The boolean operation associated with the Thicken feature

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

  Getter Method

  Signature `BooleanOperation`

  Returns: |
  Return type: | `NXOpen.GeometricUtilities.BooleanOperation`

  New in version NX5.0.0.

  License requirements: None.

## FaceCollector

`ThickenBuilder.``FaceCollector`

  Returns the faces to thicken.

  A list of one or more faces to thicken.

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

  Getter Method

  Signature `FaceCollector`

  Returns: | Smart collector for faces to thicken
  Return type: | `NXOpen.ScCollector`

  New in version NX5.0.0.

  License requirements: None.

## FirstOffset

`ThickenBuilder.``FirstOffset`

  Returns the first offset.

  The first offset for the Thicken feature. A positive value is applied along the normal of the face to be thickened. Negative values are applied in the opposite direction. The difference between the first and second offset must be non-zero.

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

  Getter Method

  Signature `FirstOffset`

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

  New in version NX5.0.0.

  License requirements: None.

## RegionSectionList

`ThickenBuilder.``RegionSectionList`

  Returns the list of SC_section The sections with corresponding expression for the Thicken feature

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

  Getter Method

  Signature `RegionSectionList`

  Returns: | Region Section set
  Return type: | `NXOpen.GeometricUtilities.TwoExpressionsSectionSetList`

  New in version NX9.0.0.

  License requirements: None.

## RegionToPierce

`ThickenBuilder.``RegionToPierce`

  Returns the section for regions to pierce The section associated for the Thicken feature

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

  Getter Method

  Signature `RegionToPierce`

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

  New in version NX9.0.0.

  License requirements: None.

## RemoveGashes

`ThickenBuilder.``RemoveGashes`

  Returns or sets the remove gashes option.

  If the option is selected, Thicken will heal the input and attempt the operation on the healed input. If after healing the input, the Thicken operation succeeds, the Part Navigator will indicate as such with an information symbol and an entry in the Alert column.

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

  Getter Method

  Signature `RemoveGashes`

  Returns: |
  Return type: | bool

  New in version NX8.0.0.

  License requirements: None.

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

  Setter Method

  Signature `RemoveGashes`

  Parameters: | removeGashes (bool) –

  New in version NX8.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

## ReverseDirection

`ThickenBuilder.``ReverseDirection`

  Returns or sets the reverse direction.

  A flag to indicate whether the offset direction is reversed with respect to the normal of the face to be thickened.

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

  Getter Method

  Signature `ReverseDirection`

  Returns: |
  Return type: | bool

  New in version NX5.0.0.

  License requirements: None.

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

  Setter Method

  Signature `ReverseDirection`

  Parameters: | reverseDirection (bool) –

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

## SecondOffset

`ThickenBuilder.``SecondOffset`

  Returns the second offset.

  the second offset for the Thicken feature.

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

  Getter Method

  Signature `SecondOffset`

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

  New in version NX5.0.0.

  License requirements: None.

## Tolerance

`ThickenBuilder.``Tolerance`

  Returns or sets the tolerance.

  The maximum allowable distance between the true theoretical sheet and the body created to approximate it.

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

  Getter Method

  Signature `Tolerance`

  Returns: |
  Return type: | float

  New in version NX5.0.0.

  License requirements: None.

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

  Setter Method

  Signature `Tolerance`

  Parameters: | tolerance (float) –

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR insp_programming (“INSPECTION PROGRAMMING”)

# Method Detail

## Validate

`ThickenBuilder.``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.