DatumPlaneBuilder Class¶
-
class
NXOpen.Features.
DatumPlaneBuilder
¶ Bases:
NXOpen.Features.DatumBuilder
Represents a datum plane feature builder.
Provides methods to create datum planes thru three points, point and direction and point on curve To create a new instance of this class, use
NXOpen.Features.FeatureCollection.CreateDatumPlaneBuilder
New in version NX3.0.0.
Properties¶
Property | Description |
---|---|
OffsetInstance | Returns or sets the offset instance plane flag |
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 |
ResizeDuringUpdate | Returns or sets the resize during update |
SurroundingPatchSurfaceFilename | Returns or sets the surrounding patch surface filename |
Tag | Returns the Tag for this object. |
Methods¶
Method | Description |
---|---|
Commit | Commits any edits that have been applied to the builder. |
CommitFeature | Commits the feature parameters and creates the feature @return |
CreateConstraint | Creates a new empty constraint object. |
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. |
GetConstraints | Gets the contraint objects that define the positioning of this datum. |
GetDatum | The datum display object this is the feature output @return |
GetFeature | Returns the feature currently being edited by this builder. |
GetObject | Returns the object currently being edited by this builder. |
GetPlane | The plane is use to create the feature @return |
HideInternalParentFeatureAfterEdit | Re-suppress an internal parent feature (a slave feature) after it has been edited. |
SetConstraints | Sets the contraint objects that define the positioning of this datum. |
SetCornerPoints | Sets corner points to builder |
SetFaceAndOffset | Sets one face object and offset |
SetFixedDatumPlane | Sets type of fixed datum plane. |
SetGeometryAndConstraints | Sets two different geometric objects. |
SetParentFeatureInternal | Set the parent features which would be internal or slaves to the feature being created or commited |
SetPointAndDirection | Sets point and direction |
SetPointOnCurve | Sets curve or edge and arc length |
SetThreePoints | Sets three different points. |
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 |
UpdateFeature | Update the feature if the feature does not exist then create it @return |
Validate | Validate whether the inputs to the component are sufficient for commit to be called. |
Enumerations¶
DatumPlaneBuilderAlternateSolution Enumeration | Specifies the alternate solution for a datum plane using point on curve method |
DatumPlaneBuilderConstraintType Enumeration | Specifies different constraint types of selected geometries |
DatumPlaneBuilderCurveOption Enumeration | Specifies the distance on the curve as absolute distance or relative distance as percentage |
DatumPlaneBuilderFixedType Enumeration | Specifies the fixed type datum plane going thru only one specific plane or thru all planes |
DatumPlaneBuilderUseArcLength Enumeration | Specifies points for which arclength is to be used. |
Property Detail¶
OffsetInstance¶
-
DatumPlaneBuilder.
OffsetInstance
¶ Returns or sets the offset instance plane flag
-------------------------------------
Getter Method
Signature
OffsetInstance()
Returns: offset instance Return type: bool New in version NX8.5.0.
License requirements: None.
-------------------------------------
Setter Method
Signature
OffsetInstance(offsetInstance)
Parameters: offsetInstance (bool) – offset instance New in version NX8.5.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
ResizeDuringUpdate¶
-
DatumPlaneBuilder.
ResizeDuringUpdate
¶ Returns or sets the resize during update
-------------------------------------
Getter Method
Signature
ResizeDuringUpdate()
Returns: resize during update Return type: bool New in version NX8.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
-------------------------------------
Setter Method
Signature
ResizeDuringUpdate(resize)
Parameters: resize (bool) – resize during update New in version NX8.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
Method Detail¶
GetDatum¶
-
DatumPlaneBuilder.
GetDatum
¶ The datum display object this is the feature output
Signature
GetDatum()
Returns: Return type: NXOpen.DatumPlane
New in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”)
GetPlane¶
-
DatumPlaneBuilder.
GetPlane
¶ The plane is use to create the feature
Signature
GetPlane()
Returns: Return type: NXOpen.Plane
New in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
SetCornerPoints¶
-
DatumPlaneBuilder.
SetCornerPoints
¶ Sets corner points to builder
Signature
SetCornerPoints(corner1, corner2, corner3, corner4)
Parameters: - corner1 (
NXOpen.Point3d
) – - corner2 (
NXOpen.Point3d
) – - corner3 (
NXOpen.Point3d
) – - corner4 (
NXOpen.Point3d
) –
New in version NX7.5.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
- corner1 (
SetFaceAndOffset¶
-
DatumPlaneBuilder.
SetFaceAndOffset
¶ Sets one face object and offset
Signature
SetFaceAndOffset(face, offsetValue, expression)
Parameters: - face (
NXOpen.Face
) – Face object - offsetValue (float) – Offset double parameter
- expression (str) – Offset string parameter NOTE: The full Unicode character set is not supported for this parameter.
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
- face (
SetFixedDatumPlane¶
-
DatumPlaneBuilder.
SetFixedDatumPlane
¶ Sets type of fixed datum plane.
Signature
SetFixedDatumPlane(type)
Parameters: type ( NXOpen.Features.DatumPlaneBuilderFixedType
) – Indicates fixed datum plane typeNew in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
SetGeometryAndConstraints¶
-
DatumPlaneBuilder.
SetGeometryAndConstraints
¶ Sets two different geometric objects.
Possible combinations are:
- If first constrain is Through Datum Axis, then the second contraint can be:
- Through Axis Through Edge
- Linear Geometry Through Face Axis Through Point Angle to Plane
- If first constrain is Through Solid Edge and Linear Geometry, then the second contraint can be:
- Through Axis Through Edge
- Linear Geometry Through Face Axis Through Point Angle to Plane
- If first constrain is Through Face Axis, then the second contraint can be:
- Through Axis Through Edge
- Linear Geometry Through Face Axis Through Point Angle to Plane
- If first constrain is Through Point, then the second contraint can be:
- Through Axis Through Edge
- Linear Geometry Parallel to Plane Perpendicular to Curve
Parallel to Surface’s Tangent Plane
- If first constrain is Angle to Plane, then the second contraint can be:
- Through Axis Through Edge
- Linear Geometry Through Face Axis
- If first constrain is Tangent to Face, then the second contraint can be:
- Through Point Angle to Plane
- 0 Deg Angle to Plane
- 90 Deg Tangent to Face
- If first constrain is Through Curve, then the second contraint can be:
- Through Point Perpendicular to View Plane
Signature
SetGeometryAndConstraints(geometry1, geometryConstraintType1, constraintAttribute1, constraintValue1, constraint1, geometry2, geometryConstraintType2, constraintAttribute2, constraintValue2, constraint2)
Parameters: - geometry1 (
NXOpen.DisplayableObject
) – First geometric object - geometryConstraintType1 (
NXOpen.Features.DatumPlaneBuilderConstraintType
) – Constraint type of first geometry - constraintAttribute1 (int) – Constraint attribute value of first geometry
- constraintValue1 (float) – Constraint value parameter of first geometry
- constraint1 (str) – Constraint attached with first geometric object. Set to “0.0” in case value is not specified NOTE: The full Unicode character set is not supported for this parameter.
- geometry2 (
NXOpen.DisplayableObject
) – Second geometric object - geometryConstraintType2 (
NXOpen.Features.DatumPlaneBuilderConstraintType
) – Constraint type of first geometry - constraintAttribute2 (int) – Constraint attribute value of second geometry
- constraintValue2 (float) – Constraint value parameter of second geometry
- constraint2 (str) – Constraint attached with second geometric object. Set to “0.0” in case value is not specified NOTE: The full Unicode character set is not supported for this parameter.
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
SetPointAndDirection¶
-
DatumPlaneBuilder.
SetPointAndDirection
¶ Sets point and direction
Signature
SetPointAndDirection(point, direction)
Parameters: - point (
NXOpen.Point
) – Point - direction (
NXOpen.Direction
) – Direction
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
- point (
SetPointOnCurve¶
-
DatumPlaneBuilder.
SetPointOnCurve
¶ Overloaded method SetPointOnCurve
SetPointOnCurve(arcLength, constraint, alternateSolution, option, curve)
SetPointOnCurve(arcLength, constraint, alternateSolution, option, curve, direction)
SetPointOnCurve(arcLength, constraint, option, curve, secondGeometry)
-------------------------------------
Sets curve or edge and arc length
Signature
SetPointOnCurve(arcLength, constraint, alternateSolution, option, curve)
Parameters: - arcLength (float) – Arc length
- constraint (str) – Constraint expression. Usually same as arc_length NOTE: The full Unicode character set is not supported for this parameter.
- alternateSolution (
NXOpen.Features.DatumPlaneBuilderAlternateSolution
) – Alternate solution - option (
NXOpen.Features.DatumPlaneBuilderCurveOption
) – Absolute distance or relative distance - curve (
NXOpen.ICurve
) – curve or edge
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
-------------------------------------
Sets curve or edge and arc length
Signature
SetPointOnCurve(arcLength, constraint, alternateSolution, option, curve, direction)
Parameters: - arcLength (float) – Arc length
- constraint (str) – Constraint expression. Usually same as arc_length NOTE: The full Unicode character set is not supported for this parameter.
- alternateSolution (
NXOpen.Features.DatumPlaneBuilderAlternateSolution
) – Alternate solution - option (
NXOpen.Features.DatumPlaneBuilderCurveOption
) – Absolute distance or relative distance - curve (
NXOpen.ICurve
) – Curve or edge - direction (
NXOpen.Direction
) – Direction
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
-------------------------------------
Sets curve or edge object and arc length with other geometry selected.
Signature
SetPointOnCurve(arcLength, constraint, option, curve, secondGeometry)
Parameters: - arcLength (float) – Arc length
- constraint (str) – Constraint expression. Usually same as arc_length NOTE: The full Unicode character set is not supported for this parameter.
- option (
NXOpen.Features.DatumPlaneBuilderCurveOption
) – Whether the absolute distance has been selected or relative - curve (
NXOpen.ICurve
) – Curve or Edge object already created - secondGeometry (
NXOpen.DisplayableObject
) – Second geometric object
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
-------------------------------------
SetThreePoints¶
-
DatumPlaneBuilder.
SetThreePoints
¶ Sets three different points.
Signature
SetThreePoints(point1, point2, point3, useArcLength)
Parameters: - point1 (
NXOpen.Point
) – First point - point2 (
NXOpen.Point
) – Second point - point3 (
NXOpen.Point
) – Third point - useArcLength (
NXOpen.Features.DatumPlaneBuilderUseArcLength
) – Specify points which use arclength instead of percentage of arclength
New in version NX3.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
- point1 (
UpdateFeature¶
-
DatumPlaneBuilder.
UpdateFeature
¶ Update the feature if the feature does not exist then create it
Signature
UpdateFeature()
Returns: Return type: NXOpen.Features.Feature
New in version NX4.0.0.
License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”)
Validate¶
-
DatumPlaneBuilder.
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.