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SketchTrim Method (ISketchManager)

Trims the selected sketch entities.

.NET Syntax

Visual Basic (Declaration) 
Function SketchTrim( _
   ByVal Option As System.Integer, _
   ByVal X As System.Double, _
   ByVal Y As System.Double, _
   ByVal Z As System.Double _
) As System.Boolean
Visual Basic (Usage) 
Dim instance As ISketchManager
Dim Option As System.Integer
Dim X As System.Double
Dim Y As System.Double
Dim Z As System.Double
Dim value As System.Boolean
 
value = instance.SketchTrim(Option, X, Y, Z)
C# 
System.bool SketchTrim( 
   System.int Option,
   System.double X,
   System.double Y,
   System.double Z
)
C++/CLI 
System.bool SketchTrim( 
&   System.int Option,
&   System.double X,
&   System.double Y,
&   System.double Z
)

Parameters

Option
Sketch trim option as defined in swSketchTrimChoice_e (see Remarks)
X
x coordinate of pick location (see Remarks)
Y
y coordinate of pick location (see Remarks)
Z
z coordinate of pick location (for 3D sketch) (see Remarks)

Return Value

True if the sketch entities are trimmed, false if not

Example

Remarks

Before calling this method, you must edit a sketch and select sketch segments to trim using IModelDocExtension::SelectByID2.

Specify X, Y, and Z with:

  • non-zero doubles only when Option is specified with swSketchTrimChoice_e.swSketchTrimEntityPoint. 
  • 0.0, 0.0, and 0.0 for all other Options.
Option swSketchTrimChoice_e... Corresponds to Trim PropertyManager's... Before calling this method, you must select...
swSketchTrimClosest Trim to closest One, and only one, sketch segment to be trimmed to its closest intersection with another sketch entity.
swSketchTrimCorner Corner Two, and only two, sketch segments to extend/trim to form a corner.
swSketchTrimEntities Power trim

One or more (up to total number) sketch segments in the model, specifying their pick points. The sketch segments are trimmed to the sketch segments nearest the pick points.

When you trim sketch segments using Power trim in the user interface, you drag your cursor across sketch segments, and the point at which the cursor crosses a sketch segment is where that sketch segment is trimmed. The API simulates this functionality by requiring you to select sketch segments by pick points, which are used as references when trimming the selected sketch segments.

swSketchTrimEntityPoint Power trim One and only one sketch segment; trims to a specific point on the sketch segment. Call this method, specifying non-zero X, Y, and Z, the point at which to trim the selected sketch segment. The specified point must lie on the sketch segment.
swSketchTrimInside Trim away inside At least three sketch segments: two to create the boundary, and one or more that intersect both sketch segments in the boundary. All selected sketch segments that intersect the boundary are trimmed inside the boundary segments.
swSketchTrimOutside Trim away outside At least three sketch segments; two to create the trim boundary, and one or more that intersect both sketch segments in the boundary. All selected sketch segments that intersect the boundary are trimmed outside the boundary segments.
swSketchTrimTwoEntities Power trim Two intersecting sketch segments; trims the first selected sketch segment to the second intersecting sketch segment. Use IModelDocExtension::SelectByID2 with Mark = 0 to select two sketch segments, specifying their pick points. The order in which the sketch segments are selected determines which one is trimmed. The first selected sketch segment will be trimmed on its pick point side to the second selected sketch segment.

 See the Trim Entities topic in the SOLIDWORKS help for more information about trimming sketch entities.

 

See Also

Availability

SOLIDWORKS 2007 FCS, Revision Number 15.0


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