Represents a Draft Feature Builder that creates or edits a draft (Old name Taper) feature. More...

Inheritance diagram for NXOpen.Features.DraftBuilder:

Public Types
enum	DraftReferencesMethods { StationaryFace, PartingFace, StationaryAndPartingFace }
	Describes the different Draft Methods in Draft References More...

enum	Method { Isocline, TrueDraft }
	Describes the Draft type as true draft or isocline draft. More...

enum	Type { Face, Edge, Tangent, PartingEdge }
	Describes the different Draft types More...

Public Member Functions
unsafe void	SetVariableAngleOption ()
	Sets the Variable Angle option More...

Public Member Functions inherited from NXOpen.Features.FeatureBuilder
unsafe NXOpen.Features.Feature	CommitFeature ()
	Commits the feature parameters and creates the feature More...

unsafe NXOpen.Features.Feature	GetFeature ()
	Returns the feature currently being edited by this builder. More...

unsafe void	HideInternalParentFeatureAfterEdit (NXOpen.Features.Feature parentFeature)
	Re-suppress an internal parent feature (a slave feature) after it has been edited. More...

unsafe void	SetParentFeatureInternal (NXOpen.Features.Feature parentFeature)
	Set the parent features which would be internal or slaves to the feature being created or commited More...

unsafe void	ShowInternalParentFeatureForEdit (NXOpen.Features.Feature parentFeature)
	Unsuppress an internal parent feature (a slave feature) so it can be edited. More...

unsafe void	UnsetParentFeatureInternal (NXOpen.Features.Feature parentFeature)
	Set the internal parent feature of the feature being edited to external More...

Public Member Functions inherited from NXOpen.Builder
unsafe NXOpen.NXObject	Commit ()
	Commits any edits that have been applied to the builder. More...

unsafe void	Destroy ()
	Deletes the builder, and cleans up any objects created by the builder. More...

unsafe NXOpen.NXObject[]	GetCommittedObjects ()
	For builders that create more than one object, this method returns the objects that are created by commit. More...

unsafe NXOpen.NXObject	GetObject ()
	Returns the object currently being edited by this builder. More...

unsafe void	ShowResults ()
	Updates the model to reflect the result of an edit to the model for all builders that support showing results. More...

unsafe bool	Validate ()
	Validate whether the inputs to the component are sufficient for commit to be called. More...

Public Member Functions inherited from NXOpen.TaggedObject
void	PrintTestData (String variableName)
	<exclude> More...

void	PrintTestData (String variableName, int lineNumber)
	<exclude> More...

override string	ToString ()
	Returns a String that represents the current Object. More...

Public Member Functions inherited from NXOpen.Utilities.NXRemotableObject
IMessageCtrl	AsyncProcessMessage (IMessage msg, IMessageSink replySink)
	Asynchronously processes the given message. More...

IMessage	SyncProcessMessage (IMessage msg)
	Synchronously processes the given message. More...

Properties
unsafe double	AngleTolerance `[get, set]`
	Returns or sets the angle tolerance in [rad/deg] More...

unsafe NXOpen.Direction	Direction `[get, set]`
	Returns or sets the smart direction for draft More...

unsafe double	DistanceTolerance `[get, set]`
	Returns or sets the distance tolerance in [in/mm] More...

unsafe bool	DraftAllInstances `[get, set]`
	Returns or sets the option "Draft all instances" [true/false] More...

unsafe bool	DraftBothSides `[get, set]`
	Returns or sets whether to draft on both sides of the reference More...

unsafe NXOpen.Features.DraftBuilder.Method	DraftIsoclineOrTruedraft `[get, set]`
	Returns or sets the Draft method More...

unsafe NXOpen.Features.DraftBuilder.DraftReferencesMethods	DraftReferencesMethod `[get, set]`
	Returns or sets the draft references method More...

unsafe NXOpen.ExpressionCollectorSetList	EdgeSetAngleExpressionList `[get]`
	Returns the list of draft edges SC Collectors and corresponding draft angles. More...

unsafe NXOpen.ExpressionCollectorSetList	FaceSetAngleExpressionList `[get]`
	Returns the list of draft faces SC Collectors and corresponding draft angles. More...

unsafe NXOpen.ScCollector	PartingReference `[get]`
	Returns the parting reference as SC Collector containing only faces or only one datum plane or only one point. More...

unsafe NXOpen.NXObject	StationaryEntity `[get, set]`
	Returns or sets the stationary entity for draft. More...

unsafe NXOpen.ScCollector	StationaryPartingReference `[get]`
	Returns the stationary parting reference as SC Collector containing only faces or only one datum plane or only one point Note that DraftBuilder. More...

unsafe NXOpen.ScCollector	StationaryReference `[get]`
	Returns the stationary reference as SC Collector containing only faces or only one datum plane or only one point More...

unsafe bool	SymmetricAngle `[get, set]`
	Returns or sets whether draft angles on both sides of the parting reference are symmetric More...

unsafe NXOpen.GeometricUtilities.TwoExpressionsCollectorSetList	TwoDimensionFaceSetsData `[get]`
	Returns the list of draft faces SC Collectors and corresponding draft angles above and below the parting reference. More...

unsafe NXOpen.Features.DraftBuilder.Type	TypeOfDraft `[get, set]`
	Returns or sets the Draft type More...

unsafe NXOpen.GeometricUtilities.DraftVariableAngleData	VariableAngleData `[get]`
	Returns the Data object for Variable Angle Draft More...

Properties inherited from NXOpen.Features.FeatureBuilder
unsafe bool	ParentFeatureInternal `[get, set]`
	Returns or sets whether or not the latest timestamped parent feature of this feature should be made internal More...

unsafe bool	PatchSolutionFlag `[get, set]`
	Returns or sets the patch solution flag More...

unsafe string	PatchSurfaceFilename `[get, set]`
	Returns or sets the patch surface filename More...

unsafe string	SurroundingPatchSurfaceFilename `[get, set]`
	Returns or sets the surrounding patch surface filename More...

Additional Inherited Members
Protected Member Functions inherited from NXOpen.TaggedObject
new void	initialize ()
	<exclude> More...

Detailed Description

Represents a Draft Feature Builder that creates or edits a draft (Old name Taper) feature.

This class provides methods to set and get various Draft feature parameters and input entities.

Following are default values and options.

Direction Z direction

Draft method Features.DraftBuilder.Method.Isocline

Draft All instances true

Angle tolerance 0.002/0.1 [rad/deg]

Distance tolerance 0.004/0.1 [in/mm]

To create a new instance of this class, use NXOpen.Features.FeatureCollection.CreateDraftBuilder

Created in NX4.0.0

Member Enumeration Documentation

enum NXOpen.Features.DraftBuilder.DraftReferencesMethods

Describes the different Draft Methods in Draft References

Enumerator
StationaryFace	Draft from stationary face.
PartingFace	Draft from stationary parting face.
StationaryAndPartingFace	Draft from stationary face to parting face.

enum NXOpen.Features.DraftBuilder.Method

Describes the Draft type as true draft or isocline draft.

Enumerator

Isocline

Indicates use of isocline algorithm to create draft.

Default value.

TrueDraft

Indicates use of true draft algorithm to create draft.

enum NXOpen.Features.DraftBuilder.Type

Describes the different Draft types

Enumerator
Face	Face Draft type
Edge	From Edges type
Tangent	Tangent Draft type
PartingEdge	Draft with Parting Edges type

Member Function Documentation

unsafe void NXOpen.Features.DraftBuilder.SetVariableAngleOption ( )

inline

Sets the Variable Angle option

Created in NX4.0.0

License requirements: solid_modeling ("SOLIDS MODELING")

Property Documentation

unsafe double NXOpen.Features.DraftBuilder.AngleTolerance

getset

Returns or sets the angle tolerance in [rad/deg]

Created in NX4.0.0

License requirements to get this property: solid_modeling ("SOLIDS MODELING")

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.Direction NXOpen.Features.DraftBuilder.Direction

getset

Returns or sets the smart direction for draft

Created in NX4.0.0

License requirements to get this property: solid_modeling ("SOLIDS MODELING")

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe double NXOpen.Features.DraftBuilder.DistanceTolerance

getset

Returns or sets the distance tolerance in [in/mm]

Created in NX4.0.0

License requirements to get this property: solid_modeling ("SOLIDS MODELING")

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe bool NXOpen.Features.DraftBuilder.DraftAllInstances

getset

Returns or sets the option "Draft all instances" [true/false]

Created in NX4.0.0

License requirements to get this property: solid_modeling ("SOLIDS MODELING")

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe bool NXOpen.Features.DraftBuilder.DraftBothSides

getset

Returns or sets whether to draft on both sides of the reference

Created in NX8.5.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.Features.DraftBuilder.Method NXOpen.Features.DraftBuilder.DraftIsoclineOrTruedraft

getset

Returns or sets the Draft method

Created in NX4.0.0

License requirements to get this property: solid_modeling ("SOLIDS MODELING")

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.Features.DraftBuilder.DraftReferencesMethods NXOpen.Features.DraftBuilder.DraftReferencesMethod

getset

Returns or sets the draft references method

Created in NX8.5.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.ExpressionCollectorSetList NXOpen.Features.DraftBuilder.EdgeSetAngleExpressionList

get

Returns the list of draft edges SC Collectors and corresponding draft angles.

Created in NX5.0.0

License requirements: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.ExpressionCollectorSetList NXOpen.Features.DraftBuilder.FaceSetAngleExpressionList

get

Returns the list of draft faces SC Collectors and corresponding draft angles.

If the Draft is From Plane or Surface, use Features.DraftBuilder.TwoDimensionFaceSetsData instead.

Created in NX5.0.0

License requirements: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.ScCollector NXOpen.Features.DraftBuilder.PartingReference

get

Returns the parting reference as SC Collector containing only faces or only one datum plane or only one point.

Note that DraftBuilder.StationaryPartingReference and DraftBuilder.PartingReference refer to the same collector.

Created in NX9.0.0

License requirements: None.

unsafe NXOpen.NXObject NXOpen.Features.DraftBuilder.StationaryEntity

getset

Returns or sets the stationary entity for draft.

Created in NX4.0.0

Deprecated in NX8.5.0. Use Features.DraftBuilder.StationaryReference instead. Note that this API cannot be used together with the new API.

License requirements to get this property: solid_modeling ("SOLIDS MODELING")

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.ScCollector NXOpen.Features.DraftBuilder.StationaryPartingReference

get

Returns the stationary parting reference as SC Collector containing only faces or only one datum plane or only one point Note that DraftBuilder.

StationaryPartingReference and DraftBuilder.PartingReference refer to the same collector.

Created in NX8.5.0

License requirements: None.

unsafe NXOpen.ScCollector NXOpen.Features.DraftBuilder.StationaryReference

get

Returns the stationary reference as SC Collector containing only faces or only one datum plane or only one point

Created in NX8.5.0

License requirements: None.

unsafe bool NXOpen.Features.DraftBuilder.SymmetricAngle

getset

Returns or sets whether draft angles on both sides of the parting reference are symmetric

Created in NX8.5.0

License requirements to get this property: None.

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.GeometricUtilities.TwoExpressionsCollectorSetList NXOpen.Features.DraftBuilder.TwoDimensionFaceSetsData

get

Returns the list of draft faces SC Collectors and corresponding draft angles above and below the parting reference.

Created in NX8.5.0

License requirements: None.

unsafe NXOpen.Features.DraftBuilder.Type NXOpen.Features.DraftBuilder.TypeOfDraft

getset

Returns or sets the Draft type

Created in NX5.0.0

License requirements to get this property: solid_modeling ("SOLIDS MODELING")

License requirements to set this property: solid_modeling ("SOLIDS MODELING")

unsafe NXOpen.GeometricUtilities.DraftVariableAngleData NXOpen.Features.DraftBuilder.VariableAngleData

get

Returns the Data object for Variable Angle Draft

Created in NX4.0.0

License requirements: solid_modeling ("SOLIDS MODELING")

The documentation for this class was generated from the following file:

Features_DraftBuilder.cs

Public Types

Public Member Functions

Properties

Additional Inherited Members

Detailed Description

Member Enumeration Documentation

Member Function Documentation

Property Documentation