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SketchOffset Method (ISketchManager)

Offsets the selected sketch entities.

.NET Syntax

Visual Basic (Declaration) 
Function SketchOffset( _
   ByVal Offset As Double, _
   ByVal BothDirections As Boolean, _
   ByVal Chain As Boolean, _
   ByVal CapEnds As Boolean, _
   ByVal MakeConstruction As Boolean, _
   ByVal AddDimensions As Boolean _
) As Boolean
Visual Basic (Usage) 
Dim instance As ISketchManager
Dim Offset As Double
Dim BothDirections As Boolean
Dim Chain As Boolean
Dim CapEnds As Boolean
Dim MakeConstruction As Boolean
Dim AddDimensions As Boolean
Dim value As Boolean
 
value = instance.SketchOffset(Offset, BothDirections, Chain, CapEnds, MakeConstruction, AddDimensions)
C# 
bool SketchOffset( 
   double Offset,
   bool BothDirections,
   bool Chain,
   bool CapEnds,
   bool MakeConstruction,
   bool AddDimensions
)
C++/CLI 
bool SketchOffset( 
&   double Offset,
&   bool BothDirections,
&   bool Chain,
&   bool CapEnds,
&   bool MakeConstruction,
&   bool AddDimensions
) 

Parameters

Offset
Offset value; negative value offsets in opposite direction
BothDirections

True to offset the sketch entities in both directions, false to not

Chain

True to offset the chain of sketch entities, false if you want only the selected sketch entities offset (see Remarks)

CapEnds
True to cap the bidirectional offset with arcs, false to not
MakeConstruction

True to make the sketch entities construction geometry after offsetting, false to not

AddDimensions

True to include the offset distance in the sketch, false to not

Return Value

True if the sketch entities are offset, false if not

Remarks

Specifying True to the Chain argument offsets the selected entity and any other entities that belong to the same contour or chain (contiguous, geometric entities like edges).

 

See Also

Availability

SolidWorks 2005 FCS, Revision Number 13.0


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