SketchCollection Class — NXOpen Python API Reference 12.0.0 documentation

# SketchCollection Class

class `NXOpen.``SketchCollection`

  Bases: `object`

  Represents a collection of sketches

  To obtain an instance of this class, refer to `NXOpen.Part`

  New in version NX3.0.0.

# Methods

Method | Description
--- | ---
CreateAngularDimensionBuilder | Creates a `NXOpen.SketchAngularDimensionBuilder`
CreateAutoConstrainBuilder | Creates a `NXOpen.SketchAutoConstrainBuilder`
CreateAutoDimensionBuilder | Creates a `NXOpen.SketchAutoDimensionBuilder`
CreateConstraintBuilder | Creates a `NXOpen.SketchConstraintBuilder`
CreateConvertToFromReferenceBuilder | Creates a `NXOpen.ConvertToFromReferenceBuilder`
CreateCornerBuilder | Creates a `NXOpen.SketchCornerBuilder`
CreateDimensionBuilder | Creates a `NXOpen.SketchDimensionBuilder`
CreateEditDefiningSectionBuilder | Creates a `NXOpen.SketchEditDefiningSectionBuilder`
CreateInferredConstraintsBuilder | Creates a `NXOpen.InferredConstraintsBuilder`
CreateIntersectionCurveBuilder | Creates the builder for intersection curve
CreateIntersectionPointBuilder | Creates the builder for intersection point
CreateLinearDimensionBuilder | Creates a `NXOpen.SketchLinearDimensionBuilder`
CreateMakeSymmetricBuilder | Creates a `NXOpen.SketchMakeSymmetricBuilder`
CreateNewSketchInPlaceBuilder | Creates a `NXOpen.SketchInPlaceBuilder`
CreateProjectBuilder | Creates a `NXOpen.SketchProjectBuilder`
CreateQuickExtendBuilder | Creates a `NXOpen.SketchQuickExtendBuilder`
CreateQuickTrimBuilder | Creates a `NXOpen.SketchQuickTrimBuilder`
CreateRadialDimensionBuilder | Creates a `NXOpen.SketchRadialDimensionBuilder`
CreateRapidDimensionBuilder | Creates a `NXOpen.SketchRapidDimensionBuilder`
CreateSketch | Creates a sketch
CreateSketchAlongPathBuilder | Creates a `NXOpen.SketchAlongPathBuilder`
CreateSketchAssociativeTrimBuilder | Creates a `NXOpen.SketchAssociativeTrimBuilder`
CreateSketchChamferBuilder | Creates a `NXOpen.SketchChamferBuilder`
CreateSketchConicBuilder | Creates a `NXOpen.SketchConicBuilder`
CreateSketchEllipseBuilder | Creates a `NXOpen.SketchEllipseBuilder`
CreateSketchInDraftingBuilder | Creates a `NXOpen.SketchInDraftingBuilder`
CreateSketchInPlaceBuilder2 | Creates a `NXOpen.SketchInPlaceBuilder`
CreateSketchMirrorPatternBuilder | Creates a `NXOpen.SketchMirrorPatternBuilder`
CreateSketchOffsetBuilder | Creates a `NXOpen.SketchOffsetBuilder`.
CreateSketchPasteBuilder | Creates a `NXOpen.SketchPasteBuilder`
CreateSketchPatternBuilder | Creates a `NXOpen.SketchPatternBuilder`
CreateSketchPolygonBuilder | Creates a `NXOpen.SketchPolygonBuilder`
FindObject | Finds the `NXOpen.Sketch` with the given name.
GetOwningSketch | Returns the sketch that owns the specified geometry

# Method Detail

## CreateAngularDimensionBuilder

`SketchCollection.``CreateAngularDimensionBuilder`

  Creates a `NXOpen.SketchAngularDimensionBuilder`

  Signature `CreateAngularDimensionBuilder(angularDimension)`

  Parameters: | angularDimension – the angular dimension to be edited, if None.

  then create an angular dimension :type angularDimension: `NXOpen.Annotations.AngularDimension` :returns: the angular dimension builder :rtype: `NXOpen.SketchAngularDimensionBuilder`

  New in version NX9.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR geometric_tol (“GDT”)

## CreateAutoConstrainBuilder

`SketchCollection.``CreateAutoConstrainBuilder`

  Creates a `NXOpen.SketchAutoConstrainBuilder`

  Signature `CreateAutoConstrainBuilder()`

  Returns: | Sketch Auto-Constrain Builder object
  Return type: | `NXOpen.SketchAutoConstrainBuilder`

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateAutoDimensionBuilder

`SketchCollection.``CreateAutoDimensionBuilder`

  Creates a `NXOpen.SketchAutoDimensionBuilder`

  Signature `CreateAutoDimensionBuilder()`

  Returns: | Sketch Auto-Dimension Builder object
  Return type: | `NXOpen.SketchAutoDimensionBuilder`

  New in version NX7.5.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateConstraintBuilder

`SketchCollection.``CreateConstraintBuilder`

  Creates a `NXOpen.SketchConstraintBuilder`

  Signature `CreateConstraintBuilder()`

  Returns: |
  Return type: | `NXOpen.SketchConstraintBuilder`

  New in version NX8.5.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateConvertToFromReferenceBuilder

`SketchCollection.``CreateConvertToFromReferenceBuilder`

  Creates a `NXOpen.ConvertToFromReferenceBuilder`

  Signature `CreateConvertToFromReferenceBuilder()`

  Returns: | Sketch ConvertToFromReferenceBuilder object
  Return type: | `NXOpen.ConvertToFromReferenceBuilder`

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateCornerBuilder

`SketchCollection.``CreateCornerBuilder`

  Creates a `NXOpen.SketchCornerBuilder`

  Signature `CreateCornerBuilder()`

  Returns: | CornerBuilder object
  Return type: | `NXOpen.SketchCornerBuilder`

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateDimensionBuilder

`SketchCollection.``CreateDimensionBuilder`

  Creates a `NXOpen.SketchDimensionBuilder`

  Signature `CreateDimensionBuilder(constraint)`

  Parameters: | constraint (`NXOpen.SketchDimensionalConstraint`) – The sketch dimensional constraint to be edited.
  Returns: | DimensionBuilder object
  Return type: | `NXOpen.SketchDimensionBuilder`

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateEditDefiningSectionBuilder

`SketchCollection.``CreateEditDefiningSectionBuilder`

  Creates a `NXOpen.SketchEditDefiningSectionBuilder`

  Signature `CreateEditDefiningSectionBuilder()`

  Returns: | Edit Defining Section Builder object
  Return type: | `NXOpen.SketchEditDefiningSectionBuilder`

  New in version NX7.5.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR geometric_tol (“GDT”)

## CreateInferredConstraintsBuilder

`SketchCollection.``CreateInferredConstraintsBuilder`

  Creates a `NXOpen.InferredConstraintsBuilder`

  Signature `CreateInferredConstraintsBuilder()`

  Returns: | InferredConstraintsBuilder object
  Return type: | `NXOpen.InferredConstraintsBuilder`

  New in version NX5.0.0.

  License requirements: None.

## CreateIntersectionCurveBuilder

`SketchCollection.``CreateIntersectionCurveBuilder`

  Creates the builder for intersection curve

  Signature `CreateIntersectionCurveBuilder(operation)`

  Parameters: | operation (`NXOpen.SketchIntersectionCurve`) –
  Returns: |
  Return type: | `NXOpen.SketchIntersectionCurveBuilder`

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateIntersectionPointBuilder

`SketchCollection.``CreateIntersectionPointBuilder`

  Creates the builder for intersection point

  Signature `CreateIntersectionPointBuilder(operation)`

  Parameters: | operation (`NXOpen.SketchIntersectionPoint`) –
  Returns: |
  Return type: | `NXOpen.SketchIntersectionPointBuilder`

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateLinearDimensionBuilder

`SketchCollection.``CreateLinearDimensionBuilder`

  Creates a `NXOpen.SketchLinearDimensionBuilder`

  Signature `CreateLinearDimensionBuilder(linearDimension)`

  Parameters: | linearDimension (`NXOpen.Annotations.Dimension`) – the linear dimension to be edited, if None, then create a linear dimension
  Returns: | the linear dimension builder
  Return type: | `NXOpen.SketchLinearDimensionBuilder`

  New in version NX9.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR geometric_tol (“GDT”)

## CreateMakeSymmetricBuilder

`SketchCollection.``CreateMakeSymmetricBuilder`

  Creates a `NXOpen.SketchMakeSymmetricBuilder`

  Signature `CreateMakeSymmetricBuilder()`

  Returns: | MakeSymmetricBuilder object
  Return type: | `NXOpen.SketchMakeSymmetricBuilder`

  New in version NX7.5.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateNewSketchInPlaceBuilder

`SketchCollection.``CreateNewSketchInPlaceBuilder`

  Creates a `NXOpen.SketchInPlaceBuilder`

  Signature `CreateNewSketchInPlaceBuilder(operation)`

  Parameters: | operation (`NXOpen.Sketch`) – The `NXOpen.Sketch` to reattach or None to create a new one
  Returns: | SketchInPlaceBuilder object
  Return type: | `NXOpen.SketchInPlaceBuilder`

  New in version NX7.5.0.

  Deprecated since version NX11.0.0: Use `NXOpen.SketchCollection.CreateSketchInPlaceBuilder2()` instead.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateProjectBuilder

`SketchCollection.``CreateProjectBuilder`

  Creates a `NXOpen.SketchProjectBuilder`

  Signature `CreateProjectBuilder(operation)`

  Parameters: | operation (`NXOpen.Features.Feature`) – The feature for the `NXOpen.SketchProjectBuilder` to be edited, if None then create a new one
  Returns: | ProjectBuilder object
  Return type: | `NXOpen.SketchProjectBuilder`

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateQuickExtendBuilder

`SketchCollection.``CreateQuickExtendBuilder`

  Creates a `NXOpen.SketchQuickExtendBuilder`

  Signature `CreateQuickExtendBuilder()`

  Returns: | Sketch Quick-Extend Builder object
  Return type: | `NXOpen.SketchQuickExtendBuilder`

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateQuickTrimBuilder

`SketchCollection.``CreateQuickTrimBuilder`

  Creates a `NXOpen.SketchQuickTrimBuilder`

  Signature `CreateQuickTrimBuilder()`

  Returns: | Sketch QuickTrim Builder object
  Return type: | `NXOpen.SketchQuickTrimBuilder`

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateRadialDimensionBuilder

`SketchCollection.``CreateRadialDimensionBuilder`

  Creates a `NXOpen.SketchRadialDimensionBuilder`

  Signature `CreateRadialDimensionBuilder(radialDimension)`

  Parameters: | radialDimension (`NXOpen.Annotations.Dimension`) – the radial dimension to be edited, if None, then create a radial dimension
  Returns: | the radial dimension builder
  Return type: | `NXOpen.SketchRadialDimensionBuilder`

  New in version NX9.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR geometric_tol (“GDT”)

## CreateRapidDimensionBuilder

`SketchCollection.``CreateRapidDimensionBuilder`

  Creates a `NXOpen.SketchRapidDimensionBuilder`

  Signature `CreateRapidDimensionBuilder()`

  Returns: | the rapid dimension builder
  Return type: | `NXOpen.SketchRapidDimensionBuilder`

  New in version NX9.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR geometric_tol (“GDT”)

## CreateSketch

`SketchCollection.``CreateSketch`

  Overloaded method CreateSketch

  - `CreateSketch(name, attachmentPlane, referenceAxis, referenceDirection, referenceAxisOrientation, referenceAxisSense, normalOrientation)`
  - `CreateSketch(name, attachmentPlane, referenceAxis, referenceDirection, referenceAxisOrientation, referenceAxisSense, normalOrientation, view)`

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

  Creates a sketch

  Signature `CreateSketch(name, attachmentPlane, referenceAxis, referenceDirection, referenceAxisOrientation, referenceAxisSense, normalOrientation)`

  Parameters:

  - name (str) – Name of the sketch. The name will be converted to upper case. If this is an empty string or None, a name will be provided by the system.
  - attachmentPlane (`NXOpen.ISurface`) – A face or datum plane that the sketch will be attached to. Must be planar.
  - referenceAxis (`NXOpen.IReferenceAxis`) – Can be a datum axis, edge, datum plane, face, or NXOpen.IReferenceAxis.NULL. If it is an edge, the edge must be a line segment. If it is a face, the face must be a plane. If NXOpen.IReferenceAxis.NULL, the reference_direction is used instead
  - referenceDirection (`NXOpen.Vector3d`) – If reference_axis is None, this parameter sets the reference direction of the sketch. In this case, this parameter must not be (0,0,0). If reference_axis is not None and this parameter is not (0,0,0), this parameter determines whether the reference direction should be in the same direction as reference_axis or in the opposite direction. If this parameter is (0,0,0), this parameter is not used.
  - referenceAxisOrientation (`NXOpen.AxisOrientation`) – indicates whether the reference axis is horizontal or vertical
  - referenceAxisSense (`NXOpen.Sense`) – Ignored unless reference_direction is (0,0,0) and reference_axis is an edge or datum axis. This parameter indicates whether the reference axis should be in the same direction as reference_axis or in the opposite direction
  - normalOrientation (`NXOpen.PlaneNormalOrientation`) – whether the sketch’s Z-axis should be outward or inward

  Returns: | the new sketch
  Return type: | `NXOpen.Sketch`

  New in version NX3.0.0.

  Deprecated since version NX7.5.3: Use `NXOpen.SketchInPlaceBuilder` instead.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”)

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

  Creates a sketch. This function takes in an argument for the view to create the sketch in a drafting member view.

  Signature `CreateSketch(name, attachmentPlane, referenceAxis, referenceDirection, referenceAxisOrientation, referenceAxisSense, normalOrientation, view)`

  Parameters:

  - name (str) – Name of the sketch. The name will be converted to upper case. If this is an empty string or None, a name will be provided by the system.
  - attachmentPlane (`NXOpen.ISurface`) – A face or datum plane that the sketch will be attached to. Must be planar.
  - referenceAxis (`NXOpen.IReferenceAxis`) – Can be a datum axis, edge, datum plane, face, or NXOpen.IReferenceAxis.NULL. If it is an edge, the edge must be a line segment. If it is a face, the face must be a plane. If NXOpen.IReferenceAxis.NULL, the reference_direction is used instead
  - referenceDirection (`NXOpen.Vector3d`) – If reference_axis is None, this parameter sets the reference direction of the sketch. In this case, this parameter must not be (0,0,0). If reference_axis is not None and this parameter is not (0,0,0), this parameter determines whether the reference direction should be in the same direction as reference_axis or in the opposite direction. If this parameter is (0,0,0), this parameter is not used.
  - referenceAxisOrientation (`NXOpen.AxisOrientation`) – indicates whether the reference axis is horizontal or vertical
  - referenceAxisSense (`NXOpen.Sense`) – Ignored unless reference_direction is (0,0,0) and reference_axis is an edge or datum axis. This parameter indicates whether the reference axis should be in the same direction as reference_axis or in the opposite direction
  - normalOrientation (`NXOpen.PlaneNormalOrientation`) – whether the sketch’s Z-axis should be outward or inward
  - view (`NXOpen.NXObject`) – View of the drafting view in which the sketch needsto be created

  Returns: | the new sketch
  Return type: | `NXOpen.Sketch`

  New in version NX4.0.0.

  Deprecated since version NX7.5.3: Use `NXOpen.SketchInDraftingBuilder` instead.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”)

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

## CreateSketchAlongPathBuilder

`SketchCollection.``CreateSketchAlongPathBuilder`

  Creates a `NXOpen.SketchAlongPathBuilder`

  Signature `CreateSketchAlongPathBuilder(operation)`

  Parameters: | operation (`NXOpen.Sketch`) – The `NXOpen.Sketch` to reattach or None to create a new one
  Returns: | SketchAlongPathBuilder object
  Return type: | `NXOpen.SketchAlongPathBuilder`

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateSketchAssociativeTrimBuilder

`SketchCollection.``CreateSketchAssociativeTrimBuilder`

  Creates a `NXOpen.SketchAssociativeTrimBuilder`

  Signature `CreateSketchAssociativeTrimBuilder(trimCon)`

  Parameters: | trimCon (`NXOpen.SketchAssociativeTrim`) – Trim constraint
  Returns: |
  Return type: | `NXOpen.SketchAssociativeTrimBuilder`

  New in version NX6.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateSketchChamferBuilder

`SketchCollection.``CreateSketchChamferBuilder`

  Creates a `NXOpen.SketchChamferBuilder`

  Signature `CreateSketchChamferBuilder()`

  Returns: | Sketch Chamfer Builder object
  Return type: | `NXOpen.SketchChamferBuilder`

  New in version NX7.5.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateSketchConicBuilder

`SketchCollection.``CreateSketchConicBuilder`

  Creates a `NXOpen.SketchConicBuilder`

  Signature `CreateSketchConicBuilder(conic)`

  Parameters: | conic (`NXOpen.NXObject`) – The conic to be edited.
  Returns: | SketchConicBuilder object
  Return type: | `NXOpen.SketchConicBuilder`

  New in version NX6.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateSketchEllipseBuilder

`SketchCollection.``CreateSketchEllipseBuilder`

  Creates a `NXOpen.SketchEllipseBuilder`

  Signature `CreateSketchEllipseBuilder(ellipse)`

  Parameters: | ellipse (`NXOpen.NXObject`) – The ellipse to be edited.
  Returns: | SketchEllipseBuilder object
  Return type: | `NXOpen.SketchEllipseBuilder`

  New in version NX6.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateSketchInDraftingBuilder

`SketchCollection.``CreateSketchInDraftingBuilder`

  Creates a `NXOpen.SketchInDraftingBuilder`

  Signature `CreateSketchInDraftingBuilder()`

  Returns: | SketchInDraftingBuilder object
  Return type: | `NXOpen.SketchInDraftingBuilder`

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”)

## CreateSketchInPlaceBuilder2

`SketchCollection.``CreateSketchInPlaceBuilder2`

  Creates a `NXOpen.SketchInPlaceBuilder`

  Signature `CreateSketchInPlaceBuilder2(operation)`

  Parameters: | operation (`NXOpen.Sketch`) – The `NXOpen.Sketch` to reattach or None to create a new one
  Returns: | SketchInPlaceBuilder object
  Return type: | `NXOpen.SketchInPlaceBuilder`

  New in version NX11.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateSketchMirrorPatternBuilder

`SketchCollection.``CreateSketchMirrorPatternBuilder`

  Creates a `NXOpen.SketchMirrorPatternBuilder`

  Signature `CreateSketchMirrorPatternBuilder(con)`

  Parameters: | con (`NXOpen.SketchPattern`) – Pattern constraint
  Returns: |
  Return type: | `NXOpen.SketchMirrorPatternBuilder`

  New in version NX7.5.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateSketchOffsetBuilder

`SketchCollection.``CreateSketchOffsetBuilder`

  Creates a `NXOpen.SketchOffsetBuilder`.

  This command only supports creation of up to 200 output curves. That means number of curves in input section multiplied by the number of copies must be less than or equal to 200.

  Signature `CreateSketchOffsetBuilder(offCon)`

  Parameters: | offCon (`NXOpen.SketchOffset`) – Offset constraint
  Returns: |
  Return type: | `NXOpen.SketchOffsetBuilder`

  New in version NX5.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateSketchPasteBuilder

`SketchCollection.``CreateSketchPasteBuilder`

  Creates a `NXOpen.SketchPasteBuilder`

  Signature `CreateSketchPasteBuilder(sketches)`

  Parameters: | sketches (list of `NXOpen.Sketch`) – `NXOpen.Sketch` to be copy/paste
  Returns: |
  Return type: | `NXOpen.SketchPasteBuilder`

  New in version NX7.5.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateSketchPatternBuilder

`SketchCollection.``CreateSketchPatternBuilder`

  Creates a `NXOpen.SketchPatternBuilder`

  Signature `CreateSketchPatternBuilder(con)`

  Parameters: | con (`NXOpen.SketchPattern`) – Pattern constraint
  Returns: |
  Return type: | `NXOpen.SketchPatternBuilder`

  New in version NX7.5.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”) OR geometric_tol (“GDT”)

## CreateSketchPolygonBuilder

`SketchCollection.``CreateSketchPolygonBuilder`

  Creates a `NXOpen.SketchPolygonBuilder`

  Signature `CreateSketchPolygonBuilder(polygonconstraint)`

  Parameters: | polygonconstraint – The polygon constraint.

  The only acceptable value here is None. :type polygonconstraint: `NXOpen.SketchPolygon` :returns: SketchPolygonBuilder object :rtype: `NXOpen.SketchPolygonBuilder`

  New in version NX7.5.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR geometric_tol (“GDT”)

## FindObject

`SketchCollection.``FindObject`

  Finds the `NXOpen.Sketch` with the given name.

  An exception will be thrown if no object can be found with the given name.

  Signature `FindObject(name)`

  Parameters: | name (str) – The name of the `NXOpen.Sketch`
  Returns: | Sketch with this name
  Return type: | `NXOpen.Sketch`

  New in version NX3.0.0.

  License requirements: None.

## GetOwningSketch

`SketchCollection.``GetOwningSketch`

  Returns the sketch that owns the specified geometry

  Signature `GetOwningSketch(geometry)`

  Parameters: | geometry (`NXOpen.SmartObject`) –
  Returns: | The sketch that owns the geometry
  Return type: | `NXOpen.Sketch`

  New in version NX4.0.0.

  License requirements: solid_modeling (“SOLIDS MODELING”) OR drafting (“DRAFTING”)