DatumPlaneBuilder Class — NXOpen Python API Reference 12.0.0 documentation

# 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
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
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
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
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`

  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”) OR insp_programming (“INSPECTION PROGRAMMING”)

## 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”) OR insp_programming (“INSPECTION PROGRAMMING”)

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

  Setter Method

  Signature `ResizeDuringUpdate`

  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”) OR insp_programming (“INSPECTION PROGRAMMING”)

# 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”) OR insp_programming (“INSPECTION PROGRAMMING”)

## 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”) OR insp_programming (“INSPECTION PROGRAMMING”)

## 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”) OR insp_programming (“INSPECTION PROGRAMMING”)

## 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

  New in version NX3.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”) OR insp_programming (“INSPECTION PROGRAMMING”)

## SetFixedDatumPlane

`DatumPlaneBuilder.``SetFixedDatumPlane`

  Sets type of fixed datum plane.

  Signature `SetFixedDatumPlane(type)`

  Parameters: | type (`NXOpen.Features.DatumPlaneBuilderFixedType`) – Indicates fixed datum plane type

  New in version NX3.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”) OR insp_programming (“INSPECTION PROGRAMMING”)

## 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
  - 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

  New in version NX3.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR cam_base (“CAM BASE”) OR geometric_tol (“GDT”) OR insp_programming (“INSPECTION PROGRAMMING”)

## 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”) OR insp_programming (“INSPECTION PROGRAMMING”)

## 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
  - 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”) OR insp_programming (“INSPECTION PROGRAMMING”)

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

  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
  - 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”) OR insp_programming (“INSPECTION PROGRAMMING”)

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

  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
  - 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”) OR insp_programming (“INSPECTION PROGRAMMING”)

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

## 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”) OR insp_programming (“INSPECTION PROGRAMMING”)

## 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”) OR insp_programming (“INSPECTION PROGRAMMING”)

## 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.