Represents a collection of sketches More...
Protected Member Functions | |
| override int | EnumerateMoveNext (ref Tag currentTag, byte[] state) |
| Advances the enumerator to the next element of the collection. More... | |
Properties | |
| Tag | Tag [get] |
| Returns the tag of this object. More... | |
Detailed Description
Represents a collection of sketches
To obtain an instance of this class, refer to NXOpen.Part
Created in NX3.0.0
Member Function Documentation
| unsafe NXOpen.SketchAngularDimensionBuilder NXOpen.SketchCollection.CreateAngularDimensionBuilder | ( | NXOpen.Annotations.AngularDimension | angularDimension | ) |
Creates a NXOpen.SketchAngularDimensionBuilder
Created in NX9.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")
- Parameters
-
angularDimension the angular dimension to be edited, if a null reference (Nothing in Visual Basic). then create an angular dimension
- Returns
- the angular dimension builder
| unsafe NXOpen.SketchAutoConstrainBuilder NXOpen.SketchCollection.CreateAutoConstrainBuilder | ( | ) |
Creates a NXOpen.SketchAutoConstrainBuilder
Created in NX5.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Returns
- Sketch Auto-Constrain Builder object
| unsafe NXOpen.SketchAutoDimensionBuilder NXOpen.SketchCollection.CreateAutoDimensionBuilder | ( | ) |
Creates a NXOpen.SketchAutoDimensionBuilder
Created in NX7.5.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Returns
- Sketch Auto-Dimension Builder object
| unsafe NXOpen.SketchConstraintBuilder NXOpen.SketchCollection.CreateConstraintBuilder | ( | ) |
Creates a NXOpen.SketchConstraintBuilder
Created in NX8.5.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Returns
| unsafe NXOpen.ConvertToFromReferenceBuilder NXOpen.SketchCollection.CreateConvertToFromReferenceBuilder | ( | ) |
Creates a NXOpen.ConvertToFromReferenceBuilder
Created in NX5.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Returns
- Sketch ConvertToFromReferenceBuilder object
| unsafe NXOpen.SketchCornerBuilder NXOpen.SketchCollection.CreateCornerBuilder | ( | ) |
Creates a NXOpen.SketchCornerBuilder
Created in NX5.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Returns
- CornerBuilder object
| unsafe NXOpen.SketchDimensionBuilder NXOpen.SketchCollection.CreateDimensionBuilder | ( | NXOpen.SketchDimensionalConstraint | constraint | ) |
Creates a NXOpen.SketchDimensionBuilder
Created in NX5.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
constraint The sketch dimensional constraint to be edited.
- Returns
- DimensionBuilder object
| unsafe NXOpen.SketchEditDefiningSectionBuilder NXOpen.SketchCollection.CreateEditDefiningSectionBuilder | ( | ) |
Creates a NXOpen.SketchEditDefiningSectionBuilder
Created in NX7.5.0
License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")
- Returns
- Edit Defining Section Builder object
| unsafe NXOpen.InferredConstraintsBuilder NXOpen.SketchCollection.CreateInferredConstraintsBuilder | ( | ) |
Creates a NXOpen.InferredConstraintsBuilder
Created in NX5.0.0
License requirements: None.
- Returns
- InferredConstraintsBuilder object
| unsafe NXOpen.SketchIntersectionCurveBuilder NXOpen.SketchCollection.CreateIntersectionCurveBuilder | ( | NXOpen.SketchIntersectionCurve | operation | ) |
Creates the builder for intersection curve
Created in NX5.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
operation
- Returns
| unsafe NXOpen.SketchIntersectionPointBuilder NXOpen.SketchCollection.CreateIntersectionPointBuilder | ( | NXOpen.SketchIntersectionPoint | operation | ) |
Creates the builder for intersection point
Created in NX5.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
operation
- Returns
| unsafe NXOpen.SketchLinearDimensionBuilder NXOpen.SketchCollection.CreateLinearDimensionBuilder | ( | NXOpen.Annotations.Dimension | linearDimension | ) |
Creates a NXOpen.SketchLinearDimensionBuilder
Created in NX9.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")
- Parameters
-
linearDimension the linear dimension to be edited, if a null reference (Nothing in Visual Basic), then create a linear dimension
- Returns
- the linear dimension builder
| unsafe NXOpen.SketchMakeSymmetricBuilder NXOpen.SketchCollection.CreateMakeSymmetricBuilder | ( | ) |
Creates a NXOpen.SketchMakeSymmetricBuilder
Created in NX7.5.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Returns
- MakeSymmetricBuilder object
| unsafe NXOpen.SketchInPlaceBuilder NXOpen.SketchCollection.CreateNewSketchInPlaceBuilder | ( | NXOpen.Sketch | operation | ) |
Creates a NXOpen.SketchInPlaceBuilder
Created in NX7.5.0
Deprecated in NX11.0.0. Use NXOpen.SketchCollection.CreateSketchInPlaceBuilder2 instead.
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
operation The NXOpen.Sketch to reattach or a null reference (Nothing in Visual Basic) to create a new one
- Returns
- SketchInPlaceBuilder object
| unsafe NXOpen.SketchProjectBuilder NXOpen.SketchCollection.CreateProjectBuilder | ( | NXOpen.Features.Feature | operation | ) |
Creates a NXOpen.SketchProjectBuilder
Created in NX5.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
operation The feature for the NXOpen.SketchProjectBuilder to be edited, if a null reference (Nothing in Visual Basic) then create a new one
- Returns
- ProjectBuilder object
| unsafe NXOpen.SketchQuickExtendBuilder NXOpen.SketchCollection.CreateQuickExtendBuilder | ( | ) |
Creates a NXOpen.SketchQuickExtendBuilder
Created in NX5.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Returns
- Sketch Quick-Extend Builder object
| unsafe NXOpen.SketchQuickTrimBuilder NXOpen.SketchCollection.CreateQuickTrimBuilder | ( | ) |
Creates a NXOpen.SketchQuickTrimBuilder
Created in NX5.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Returns
- Sketch QuickTrim Builder object
| unsafe NXOpen.SketchRadialDimensionBuilder NXOpen.SketchCollection.CreateRadialDimensionBuilder | ( | NXOpen.Annotations.Dimension | radialDimension | ) |
Creates a NXOpen.SketchRadialDimensionBuilder
Created in NX9.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")
- Parameters
-
radialDimension the radial dimension to be edited, if a null reference (Nothing in Visual Basic), then create a radial dimension
- Returns
- the radial dimension builder
| unsafe NXOpen.SketchRapidDimensionBuilder NXOpen.SketchCollection.CreateRapidDimensionBuilder | ( | ) |
Creates a NXOpen.SketchRapidDimensionBuilder
Created in NX9.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")
- Returns
- the rapid dimension builder
| unsafe NXOpen.Sketch NXOpen.SketchCollection.CreateSketch | ( | string | name, |
| NXOpen.ISurface | attachmentPlane, | ||
| NXOpen.IReferenceAxis | referenceAxis, | ||
| NXOpen.Vector3d | referenceDirection, | ||
| NXOpen.AxisOrientation | referenceAxisOrientation, | ||
| NXOpen.Sense | referenceAxisSense, | ||
| NXOpen.PlaneNormalOrientation | normalOrientation | ||
| ) |
Creates a sketch
Created in NX3.0.0
Deprecated in NX7.5.3. Use NXOpen.SketchInPlaceBuilder instead.
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING")
- Parameters
-
name Name of the sketch. The name will be converted to upper case. If this is an empty string or a null reference (Nothing in Visual Basic), a name will be provided by the system. attachmentPlane A face or datum plane that the sketch will be attached to. Must be planar. referenceAxis Can be a datum axis, edge, datum plane, face, or a null reference (Nothing in Visual Basic). If it is an edge, the edge must be a line segment. If it is a face, the face must be a plane. If a null reference (Nothing in Visual Basic), the reference_direction is used instead referenceDirection If reference_axis is a null reference (Nothing in Visual Basic), 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 a null reference (Nothing in Visual Basic) 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 indicates whether the reference axis is horizontal or vertical referenceAxisSense 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 whether the sketch's Z-axis should be outward or inward
- Returns
- the new sketch
| unsafe NXOpen.Sketch NXOpen.SketchCollection.CreateSketch | ( | string | name, |
| NXOpen.ISurface | attachmentPlane, | ||
| NXOpen.IReferenceAxis | referenceAxis, | ||
| NXOpen.Vector3d | referenceDirection, | ||
| NXOpen.AxisOrientation | referenceAxisOrientation, | ||
| NXOpen.Sense | referenceAxisSense, | ||
| NXOpen.PlaneNormalOrientation | normalOrientation, | ||
| NXOpen.NXObject | view | ||
| ) |
Creates a sketch.
This function takes in an argument for the view to create the sketch in a drafting member view.
Created in NX4.0.0
Deprecated in NX7.5.3. Use NXOpen.SketchInDraftingBuilder instead.
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING")
- Parameters
-
name Name of the sketch. The name will be converted to upper case. If this is an empty string or a null reference (Nothing in Visual Basic), a name will be provided by the system. attachmentPlane A face or datum plane that the sketch will be attached to. Must be planar. referenceAxis Can be a datum axis, edge, datum plane, face, or a null reference (Nothing in Visual Basic). If it is an edge, the edge must be a line segment. If it is a face, the face must be a plane. If a null reference (Nothing in Visual Basic), the reference_direction is used instead referenceDirection If reference_axis is a null reference (Nothing in Visual Basic), 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 a null reference (Nothing in Visual Basic) 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 indicates whether the reference axis is horizontal or vertical referenceAxisSense 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 whether the sketch's Z-axis should be outward or inward view View of the drafting view in which the sketch needsto be created
- Returns
- the new sketch
| unsafe NXOpen.SketchAlongPathBuilder NXOpen.SketchCollection.CreateSketchAlongPathBuilder | ( | NXOpen.Sketch | operation | ) |
Creates a NXOpen.SketchAlongPathBuilder
Created in NX5.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
operation The NXOpen.Sketch to reattach or a null reference (Nothing in Visual Basic) to create a new one
- Returns
- SketchAlongPathBuilder object
| unsafe NXOpen.SketchAssociativeTrimBuilder NXOpen.SketchCollection.CreateSketchAssociativeTrimBuilder | ( | NXOpen.SketchAssociativeTrim | trimCon | ) |
Creates a NXOpen.SketchAssociativeTrimBuilder
Created in NX6.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
trimCon Trim constraint
- Returns
| unsafe NXOpen.SketchChamferBuilder NXOpen.SketchCollection.CreateSketchChamferBuilder | ( | ) |
Creates a NXOpen.SketchChamferBuilder
Created in NX7.5.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Returns
- Sketch Chamfer Builder object
| unsafe NXOpen.SketchConicBuilder NXOpen.SketchCollection.CreateSketchConicBuilder | ( | NXOpen.NXObject | conic | ) |
Creates a NXOpen.SketchConicBuilder
Created in NX6.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
conic The conic to be edited.
- Returns
- SketchConicBuilder object
| unsafe NXOpen.SketchEllipseBuilder NXOpen.SketchCollection.CreateSketchEllipseBuilder | ( | NXOpen.NXObject | ellipse | ) |
Creates a NXOpen.SketchEllipseBuilder
Created in NX6.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
ellipse The ellipse to be edited.
- Returns
- SketchEllipseBuilder object
| unsafe NXOpen.SketchInDraftingBuilder NXOpen.SketchCollection.CreateSketchInDraftingBuilder | ( | ) |
Creates a NXOpen.SketchInDraftingBuilder
Created in NX5.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING")
- Returns
- SketchInDraftingBuilder object
| unsafe NXOpen.SketchInPlaceBuilder NXOpen.SketchCollection.CreateSketchInPlaceBuilder2 | ( | NXOpen.Sketch | operation | ) |
Creates a NXOpen.SketchInPlaceBuilder
Created in NX11.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
operation The NXOpen.Sketch to reattach or a null reference (Nothing in Visual Basic) to create a new one
- Returns
- SketchInPlaceBuilder object
| unsafe NXOpen.SketchMirrorPatternBuilder NXOpen.SketchCollection.CreateSketchMirrorPatternBuilder | ( | NXOpen.SketchPattern | con | ) |
Creates a NXOpen.SketchMirrorPatternBuilder
Created in NX7.5.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
con Pattern constraint
- Returns
| unsafe NXOpen.SketchOffsetBuilder NXOpen.SketchCollection.CreateSketchOffsetBuilder | ( | NXOpen.SketchOffset | offCon | ) |
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.
Created in NX5.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
offCon Offset constraint
- Returns
| unsafe NXOpen.SketchPasteBuilder NXOpen.SketchCollection.CreateSketchPasteBuilder | ( | NXOpen.Sketch[] | sketches | ) |
Creates a NXOpen.SketchPasteBuilder
Created in NX7.5.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
sketches NXOpen.Sketch to be copy/paste
- Returns
| unsafe NXOpen.SketchPatternBuilder NXOpen.SketchCollection.CreateSketchPatternBuilder | ( | NXOpen.SketchPattern | con | ) |
Creates a NXOpen.SketchPatternBuilder
Created in NX7.5.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING") OR geometric_tol ("GDT")
- Parameters
-
con Pattern constraint
- Returns
| unsafe NXOpen.SketchPolygonBuilder NXOpen.SketchCollection.CreateSketchPolygonBuilder | ( | NXOpen.SketchPolygon | polygonconstraint | ) |
Creates a NXOpen.SketchPolygonBuilder
Created in NX7.5.0
License requirements: solid_modeling ("SOLIDS MODELING") OR geometric_tol ("GDT")
- Parameters
-
polygonconstraint The polygon constraint. The only acceptable value here is a null reference (Nothing in Visual Basic).
- Returns
- SketchPolygonBuilder object
|
protected |
Advances the enumerator to the next element of the collection.
| unsafe NXOpen.Sketch NXOpen.SketchCollection.FindObject | ( | string | name | ) |
Finds the NXOpen.Sketch with the given name.
An exception will be thrown if no object can be found with the given name.
Created in NX3.0.0
License requirements: None.
- Parameters
-
name The name of the NXOpen.Sketch
- Returns
- Sketch with this name
| unsafe NXOpen.Sketch NXOpen.SketchCollection.GetOwningSketch | ( | NXOpen.SmartObject | geometry | ) |
Returns the sketch that owns the specified geometry
Created in NX4.0.0
License requirements: solid_modeling ("SOLIDS MODELING") OR drafting ("DRAFTING")
- Parameters
-
geometry
- Returns
- The sketch that owns the geometry
| NXOpen.Sketch [] NXOpen.SketchCollection.ToArray | ( | ) |
Returns an array of NXOpen.Sketch objects.
Property Documentation
|
get |
Returns the tag of this object.
The documentation for this class was generated from the following file:
- dotnet_pool/SketchCollection.cs