HoleFeatureBuilder Class

class NXOpen.Features.HoleFeatureBuilder

Bases: NXOpen.Features.RPOBuilder

Represents a Hole feature builder.

See NXOpen.Features.RPOBuilder for details on positioning the hole. To create a new instance of this class, use NXOpen.Features.FeatureCollection.CreateHoleFeatureBuilder()

New in version NX3.0.0.

Properties

Property Description
CounterboreDepth Returns the depth of the counterbore for a hole.
CounterboreDiameter Returns the diameter of the counterbore for a hole.
CountersinkAngle Returns the angle of the countersink for a hole.
CountersinkDiameter Returns the diameter of the countersink for a hole.
Depth Returns the depth of the hole.
Diameter Returns the diameter of the hole.
HoleLocation Returns or sets the reference point of the hole.
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
PlacementFace Returns or sets the placement face of the hole.
ReverseDirection Returns or sets the reverse direction flag of the hole.
Subtype Returns or sets the type of hole
SurroundingPatchSurfaceFilename Returns or sets the surrounding patch surface filename
Tag Returns the Tag for this object.
TipAngle Returns the tip angle of the hole.

Methods

Method Description
ApplyDimensions Transforms the feature by applying the positioning dimensions
Commit Commits any edits that have been applied to the builder.
CommitFeature Commits the feature parameters and creates the feature
CreateDimension Creates a new empty RPODimension object
CreateHole Creates a hole body which can be positioned
CreatePositioningDimension Creates a positioning dimension.
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.
GetReferenceDirection Query/Set a horizontal or vertical reference for the feature.
GetRpoDimensions Gets the list of RPO dimemsions
GetTargetBody Returns target body for the hole.
GetThruFace Returns thru face parameter for the hole.
HideInternalParentFeatureAfterEdit Re-suppress an internal parent feature (a slave feature) after it has been edited.
HidePositioningDimensions Hides display of all the positioning dimensions
SetCounterboreDepth Sets the depth of the counterbore for a hole.
SetCounterboreDiameter Sets the diameter of the counterbore for a hole.
SetCounterboreHole Sets parameters for counterbore hole
SetCountersinkAngle Sets the angle of the countersink for a hole.
SetCountersinkDiameter Sets the diameter of the countersink for a hole.
SetCountersinkHole Sets parameters for countersink hole
SetDepth Sets the depth of the hole.
SetDepthAndTipAngle Sets depth and tip angle parameters for the hole.
SetDiameter Sets the diameter of the hole.
SetExpression Sets the expression value in order to constrain the target and tool entities which are set using NXOpen.Features.RPOBuilder.SetTargetAndTool().
SetParentFeatureInternal Set the parent features which would be internal or slaves to the feature being created or commited
SetReferenceDirection Sets a horizontal or vertical reference for the feature.
SetRpoDimensions Sets the list of RPO dimemsions
SetSimpleHole Sets parameters for simple hole
SetTargetAndTool Sets the target and tool entities.
SetTargetBody Sets target body for the hole.
SetThruFace Sets thru face parameter for the hole.
SetTipAngle Sets the tip angle of the hole.
ShowInternalParentFeatureForEdit Unsuppress an internal parent feature (a slave feature) so it can be edited.
ShowPositioningDimensions Displays all the positioning dimensions
ShowResults Updates the model to reflect the result of an edit to the model for all builders that support showing results.
UndoLastDimension Undo the last positioning dimension
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

HoleFeatureBuilderHoleSubtype Enumeration Represents the subtype of the hole

Property Detail

CounterboreDepth

HoleFeatureBuilder.CounterboreDepth

Returns the depth of the counterbore for a hole.

Only used if the hole type is couterbore

-------------------------------------

Getter Method

Signature CounterboreDepth

Returns:counterbore depth
Return type:NXOpen.Expression

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CounterboreDiameter

HoleFeatureBuilder.CounterboreDiameter

Returns the diameter of the counterbore for a hole.

Only used if the hole type is couterbore

-------------------------------------

Getter Method

Signature CounterboreDiameter

Returns:counterbore diameter
Return type:NXOpen.Expression

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CountersinkAngle

HoleFeatureBuilder.CountersinkAngle

Returns the angle of the countersink for a hole.

Only used if the hole type is coutersink

-------------------------------------

Getter Method

Signature CountersinkAngle

Returns:countersink angle
Return type:NXOpen.Expression

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

CountersinkDiameter

HoleFeatureBuilder.CountersinkDiameter

Returns the diameter of the countersink for a hole.

Only used if the hole type is coutersink

-------------------------------------

Getter Method

Signature CountersinkDiameter

Returns:countersink diameter
Return type:NXOpen.Expression

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

Depth

HoleFeatureBuilder.Depth

Returns the depth of the hole.

If this parameter is set then the thru face is ignored.

-------------------------------------

Getter Method

Signature Depth

Returns:Hole depth
Return type:NXOpen.Expression

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

Diameter

HoleFeatureBuilder.Diameter

Returns the diameter of the hole.

-------------------------------------

Getter Method

Signature Diameter

Returns:Hole diameter
Return type:NXOpen.Expression

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

HoleLocation

HoleFeatureBuilder.HoleLocation

Returns or sets the reference point of the hole.

This parameter will position the hole unless relative positioning dimensions are used

-------------------------------------

Getter Method

Signature HoleLocation

Returns:Reference point for the hole
Return type:NXOpen.Point3d

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

-------------------------------------

Setter Method

Signature HoleLocation

Parameters:referencePoint (NXOpen.Point3d) – Reference point for the hole

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

PlacementFace

HoleFeatureBuilder.PlacementFace

Returns or sets the placement face of the hole.

-------------------------------------

Getter Method

Signature PlacementFace

Returns:Placement face
Return type:NXOpen.ISurface

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

-------------------------------------

Setter Method

Signature PlacementFace

Parameters:placementFace (NXOpen.ISurface) – Placement face

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

ReverseDirection

HoleFeatureBuilder.ReverseDirection

Returns or sets the reverse direction flag of the hole.

-------------------------------------

Getter Method

Signature ReverseDirection

Returns:
Return type:bool

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

-------------------------------------

Setter Method

Signature ReverseDirection

Parameters:reverse (bool) –

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

Subtype

HoleFeatureBuilder.Subtype

Returns or sets the type of hole

-------------------------------------

Getter Method

Signature Subtype

Returns:
Return type:NXOpen.Features.HoleFeatureBuilderHoleSubtype

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

-------------------------------------

Setter Method

Signature Subtype

Parameters:subtype (NXOpen.Features.HoleFeatureBuilderHoleSubtype) –

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

TipAngle

HoleFeatureBuilder.TipAngle

Returns the tip angle of the hole.

If this parameter is set then the thru face is ignored.

-------------------------------------

Getter Method

Signature TipAngle

Returns:Tip angle
Return type:NXOpen.Expression

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

Method Detail

CreateHole

HoleFeatureBuilder.CreateHole

Creates a hole body which can be positioned

Signature CreateHole()

New in version NX3.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

GetTargetBody

HoleFeatureBuilder.GetTargetBody

Returns target body for the hole.

If this parameter is set then depth and tip angle are ignored and will prompt for thru_face.

Signature GetTargetBody()

Returns:Target Body
Return type:NXOpen.Body

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

GetThruFace

HoleFeatureBuilder.GetThruFace

Returns thru face parameter for the hole.

If this parameter is set then depth and tip angle are ignored.

Signature GetThruFace()

Returns:Thru face
Return type:NXOpen.ISurface

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetCounterboreDepth

HoleFeatureBuilder.SetCounterboreDepth

Sets the depth of the counterbore for a hole.

Only used if the hole type is couterbore

Signature SetCounterboreDepth(depth)

Parameters:depth (str) – counterbore depth

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetCounterboreDiameter

HoleFeatureBuilder.SetCounterboreDiameter

Sets the diameter of the counterbore for a hole.

Only used if the hole type is couterbore

Signature SetCounterboreDiameter(diameter)

Parameters:diameter (str) – Hole diameter

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetCounterboreHole

HoleFeatureBuilder.SetCounterboreHole

Sets parameters for counterbore hole

Signature SetCounterboreHole(referencePoint, reverseDirection, placementFace, diameter, counterboreDiameter, counterboreDepth)

Parameters:
  • referencePoint (NXOpen.Point3d) – Reference point for the hole
  • reverseDirection (bool) – Reverse direction flag, applicable only if placement face is a datum plane
  • placementFace (NXOpen.ISurface) – Placement face
  • diameter (str) – Hole diameter
  • counterboreDiameter (str) – Counterbore diameter
  • counterboreDepth (str) – Counterbore depth

New in version NX3.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetCountersinkAngle

HoleFeatureBuilder.SetCountersinkAngle

Sets the angle of the countersink for a hole.

Only used if the hole type is coutersink

Signature SetCountersinkAngle(angle)

Parameters:angle (str) – countersink angle

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetCountersinkDiameter

HoleFeatureBuilder.SetCountersinkDiameter

Sets the diameter of the countersink for a hole.

Only used if the hole type is coutersink

Signature SetCountersinkDiameter(diameter)

Parameters:diameter (str) – Hole diameter

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetCountersinkHole

HoleFeatureBuilder.SetCountersinkHole

Sets parameters for countersink hole

Signature SetCountersinkHole(referencePoint, reverseDirection, placementFace, diameter, countersinkDiameter, countersinkAngle)

Parameters:
  • referencePoint (NXOpen.Point3d) – Reference point for the hole
  • reverseDirection (bool) – Reverse direction flag, applicable only if placement face is a datum plane
  • placementFace (NXOpen.ISurface) – Placement face
  • diameter (str) – Hole diameter
  • countersinkDiameter (str) – Countersink diameter
  • countersinkAngle (str) – Countersink angle

New in version NX3.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetDepth

HoleFeatureBuilder.SetDepth

Sets the depth of the hole.

If this parameter is set then the thru face is ignored.

Signature SetDepth(depth)

Parameters:depth (str) – Hole depth

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetDepthAndTipAngle

HoleFeatureBuilder.SetDepthAndTipAngle

Sets depth and tip angle parameters for the hole.

Signature SetDepthAndTipAngle(depth, tipAngle)

Parameters:
  • depth (str) – Hole depth
  • tipAngle (str) – Tip angle of the tool

New in version NX3.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetDiameter

HoleFeatureBuilder.SetDiameter

Sets the diameter of the hole.

Signature SetDiameter(diameter)

Parameters:diameter (str) – Hole diameter

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetSimpleHole

HoleFeatureBuilder.SetSimpleHole

Sets parameters for simple hole

Signature SetSimpleHole(referencePoint, reverseDirection, placementFace, diameter)

Parameters:
  • referencePoint (NXOpen.Point3d) – Reference point for the hole
  • reverseDirection (bool) – Reverse direction flag, applicable only if placement face is a datum plane
  • placementFace (NXOpen.ISurface) – Placement face
  • diameter (str) – Hole diameter

New in version NX3.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetTargetBody

HoleFeatureBuilder.SetTargetBody

Sets target body for the hole.

If this parameter is set then depth and tip angle are ignored and will prompt for thru_face.

Signature SetTargetBody(targetBody)

Parameters:targetBody (NXOpen.Body) – Target Body

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetThruFace

HoleFeatureBuilder.SetThruFace

Sets thru face parameter for the hole.

If this parameter is set then depth and tip angle are ignored.

Signature SetThruFace(thruFace)

Parameters:thruFace (NXOpen.ISurface) – Thru face

New in version NX3.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

SetTipAngle

HoleFeatureBuilder.SetTipAngle

Sets the tip angle of the hole.

If this parameter is set then the thru face is ignored.

Signature SetTipAngle(tipAngle)

Parameters:tipAngle (str) – Tip angle

New in version NX4.0.0.

License requirements: features_modeling (“FEATURES MODELING”), solid_modeling (“SOLIDS MODELING”)

Validate

HoleFeatureBuilder.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.