ChamferBuilder Class — NXOpen Python API Reference 12.0.0 documentation

# ChamferBuilder Class

class `NXOpen.Features.``ChamferBuilder`

  Bases: `NXOpen.Features.FeatureBuilder`

  Represents the chamfer builder data.

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

  New in version NX4.0.0.

# Properties

Property | Description
--- | ---
AllInstances | Returns or sets the chamfer all instance status
Angle | Returns or sets the chamfer angle (expression).
AngleExp | Returns the angle expression object of chamfer.
FirstOffset | Returns or sets the first offset distance (expression).
FirstOffsetExp | Returns the first offset expression object of chamfer.
Method | Returns or sets the offset method.
Option | Returns or sets the chamfer parameter option.
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
ReverseOffsets | Returns or sets the offset reverse status
SecondOffset | Returns or sets the second offset distance (expression).
SecondOffsetExp | Returns the second offset expression object of chamfer.
SmartCollector | Returns or sets the smart collector
SurroundingPatchSurfaceFilename | Returns or sets the surrounding patch surface filename
Tag | Returns the Tag for this object.
Tolerance | Returns or sets the tolerance used for creating chamfer

# Methods

Method | Description
--- | ---
Commit | Commits any edits that have been applied to the builder.
CommitFeature | Commits the feature parameters and creates the feature
CreatePreview | Creates the chamfer preview body
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.

# Enumerations

ChamferBuilderChamferOption Enumeration | This enum represents the chamfer parameter options
ChamferBuilderOffsetMethod Enumeration | This enum represents the offset method options

# Property Detail

## AllInstances

`ChamferBuilder.``AllInstances`

  Returns or sets the chamfer all instance status

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

  Getter Method

  Signature `AllInstances`

  Returns: | Chamfer all_instances flag
  Return type: | bool

  New in version NX4.0.0.

  License requirements: None.

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

  Setter Method

  Signature `AllInstances`

  Parameters: | allInstances (bool) –

  New in version NX4.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

## Angle

`ChamferBuilder.``Angle`

  Returns or sets the chamfer angle (expression).

  Please do not use this property to access/modify the `Features.ChamferBuilder.AngleExp()`. This might be removed from KF bindings in NX 9.

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

  Getter Method

  Signature `Angle`

  Returns: | Chamfer angle
  Return type: | str

  New in version NX4.0.0.

  License requirements: None.

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

  Setter Method

  Signature `Angle`

  Parameters: | angleExpression (str) –

  New in version NX4.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

## AngleExp

`ChamferBuilder.``AngleExp`

  Returns the angle expression object of chamfer.

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

  Getter Method

  Signature `AngleExp`

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

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

## FirstOffset

`ChamferBuilder.``FirstOffset`

  Returns or sets the first offset distance (expression).

  Please do not use this property to access/modify the `Features.ChamferBuilder.FirstOffsetExp()`. This might be removed from KF bindings in NX 9.

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

  Getter Method

  Signature `FirstOffset`

  Returns: | Chamfer first offset
  Return type: | str

  New in version NX4.0.0.

  License requirements: None.

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

  Setter Method

  Signature `FirstOffset`

  Parameters: | offsetExpression (str) –

  New in version NX4.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

## FirstOffsetExp

`ChamferBuilder.``FirstOffsetExp`

  Returns the first offset expression object of chamfer.

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

  Getter Method

  Signature `FirstOffsetExp`

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

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

## Method

`ChamferBuilder.``Method`

  Returns or sets the offset method.

  `Features.ChamferBuilderOffsetMethod.EdgesAlongFaces` `Features.ChamferBuilderOffsetMethod.FacesAndTrim`

  The EdgesAlongFaces method is the normal chamfer in which the chamfer boundary is determined by offsetting the input edges along its adjacent faces. The FacesAndTrim method is the free-form chamfer in which the chamfer boundary is determined by offsetting the adjacent faces of the input edges, using the chamfer parameters in either case.

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

  Getter Method

  Signature `Method`

  Returns: | Offset method option
  Return type: | `NXOpen.Features.ChamferBuilderOffsetMethod`

  New in version NX4.0.0.

  License requirements: None.

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

  Setter Method

  Signature `Method`

  Parameters: | method (`NXOpen.Features.ChamferBuilderOffsetMethod`) –

  New in version NX4.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

## Option

`ChamferBuilder.``Option`

  Returns or sets the chamfer parameter option.

  `Features.ChamferBuilderChamferOption.SymmetricOffsets` `Features.ChamferBuilderChamferOption.TwoOffsets` `Features.ChamferBuilderChamferOption.OffsetAndAngle`

  Each of these options correspond to a chamfer defined by two equal offset distances, two unequal offset distances, an offset distance and angle respectively.

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

  Getter Method

  Signature `Option`

  Returns: | Chamfer parameter option
  Return type: | `NXOpen.Features.ChamferBuilderChamferOption`

  New in version NX4.0.0.

  License requirements: None.

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

  Setter Method

  Signature `Option`

  Parameters: | opt (`NXOpen.Features.ChamferBuilderChamferOption`) –

  New in version NX4.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

## ReverseOffsets

`ChamferBuilder.``ReverseOffsets`

  Returns or sets the offset reverse status

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

  Getter Method

  Signature `ReverseOffsets`

  Returns: | Chamfer reverse flag
  Return type: | bool

  New in version NX4.0.0.

  License requirements: None.

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

  Setter Method

  Signature `ReverseOffsets`

  Parameters: | reverse (bool) –

  New in version NX4.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

## SecondOffset

`ChamferBuilder.``SecondOffset`

  Returns or sets the second offset distance (expression).

  Please do not use this property to access/modify the `Features.ChamferBuilder.SecondOffsetExp()`. This might be removed from KF bindings in NX 9.

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

  Getter Method

  Signature `SecondOffset`

  Returns: | Chamfer second offset
  Return type: | str

  New in version NX4.0.0.

  License requirements: None.

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

  Setter Method

  Signature `SecondOffset`

  Parameters: | offsetExpression (str) –

  New in version NX4.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

## SecondOffsetExp

`ChamferBuilder.``SecondOffsetExp`

  Returns the second offset expression object of chamfer.

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

  Getter Method

  Signature `SecondOffsetExp`

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

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

## SmartCollector

`ChamferBuilder.``SmartCollector`

  Returns or sets the smart collector

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

  Getter Method

  Signature `SmartCollector`

  Returns: | Smart collector tag
  Return type: | `NXOpen.ScCollector`

  New in version NX4.0.0.

  License requirements: None.

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

  Setter Method

  Signature `SmartCollector`

  Parameters: | sc (`NXOpen.ScCollector`) –

  New in version NX4.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

## Tolerance

`ChamferBuilder.``Tolerance`

  Returns or sets the tolerance used for creating chamfer

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

  Getter Method

  Signature `Tolerance`

  Returns: |
  Return type: | float

  New in version NX6.0.0.

  License requirements: None.

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

  Setter Method

  Signature `Tolerance`

  Parameters: | tolerance (float) –

  New in version NX6.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

# Method Detail

## CreatePreview

`ChamferBuilder.``CreatePreview`

  Creates the chamfer preview body

  Signature `CreatePreview()`

  Returns: | Parasolid body
  Return type: | int

  New in version NX4.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”)

## Validate

`ChamferBuilder.``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.