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, useNXOpen.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 @return |
CreateDimension | Creates a new empty RPODimension object @return The RPO dimensions |
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 @return The RPO dimensions |
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(referencePoint)
Parameters: referencePoint ( NXOpen.Point3d
) – Reference point for the holeNew 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(placementFace)
Parameters: placementFace ( NXOpen.ISurface
) – Placement faceNew 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(reverse)
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(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”)
- referencePoint (
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”)
- referencePoint (
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”)
- referencePoint (
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 BodyNew 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 faceNew 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.