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InsertNetBlend Method (IFeatureManager)

This method inserts a boundary feature or a boundary surface feature.

.NET Syntax

Visual Basic (Declaration) 
Function InsertNetBlend( _
   ByVal Type As System.Short, _
   ByVal NCurvesDir1 As System.Short, _
   ByVal NCurvesDir2 As System.Short, _
   ByVal HasCenterline As System.Boolean, _
   ByVal TessTolFactor As System.Double, _
   ByVal WantsSolid As System.Boolean, _
   ByVal MergeBody As System.Boolean, _
   ByVal FeatureScope As System.Boolean, _
   ByVal AutoSelect As System.Boolean, _
   ByVal Thin As System.Boolean, _
   ByVal Thickness1 As System.Double, _
   ByVal Thickness2 As System.Double, _
   ByVal ReverseThickness As System.Boolean, _
   ByVal ThinSolidType As System.Short, _
   ByVal UseSharedThickness As System.Boolean, _
   ByVal CapEnds As System.Boolean, _
   ByVal EndThickness As System.Double, _
   ByVal AutoFillet As System.Boolean, _
   ByVal FilletRadius As System.Double, _
   ByVal ForceNonRational As System.Boolean _
) As Feature
Visual Basic (Usage) 
Dim instance As IFeatureManager
Dim Type As System.Short
Dim NCurvesDir1 As System.Short
Dim NCurvesDir2 As System.Short
Dim HasCenterline As System.Boolean
Dim TessTolFactor As System.Double
Dim WantsSolid As System.Boolean
Dim MergeBody As System.Boolean
Dim FeatureScope As System.Boolean
Dim AutoSelect As System.Boolean
Dim Thin As System.Boolean
Dim Thickness1 As System.Double
Dim Thickness2 As System.Double
Dim ReverseThickness As System.Boolean
Dim ThinSolidType As System.Short
Dim UseSharedThickness As System.Boolean
Dim CapEnds As System.Boolean
Dim EndThickness As System.Double
Dim AutoFillet As System.Boolean
Dim FilletRadius As System.Double
Dim ForceNonRational As System.Boolean
Dim value As Feature
 
value = instance.InsertNetBlend(Type, NCurvesDir1, NCurvesDir2, HasCenterline, TessTolFactor, WantsSolid, MergeBody, FeatureScope, AutoSelect, Thin, Thickness1, Thickness2, ReverseThickness, ThinSolidType, UseSharedThickness, CapEnds, EndThickness, AutoFillet, FilletRadius, ForceNonRational)
C# 
Feature InsertNetBlend( 
   System.short Type,
   System.short NCurvesDir1,
   System.short NCurvesDir2,
   System.bool HasCenterline,
   System.double TessTolFactor,
   System.bool WantsSolid,
   System.bool MergeBody,
   System.bool FeatureScope,
   System.bool AutoSelect,
   System.bool Thin,
   System.double Thickness1,
   System.double Thickness2,
   System.bool ReverseThickness,
   System.short ThinSolidType,
   System.bool UseSharedThickness,
   System.bool CapEnds,
   System.double EndThickness,
   System.bool AutoFillet,
   System.double FilletRadius,
   System.bool ForceNonRational
)
C++/CLI 
Feature^ InsertNetBlend( 
&   System.short Type,
&   System.short NCurvesDir1,
&   System.short NCurvesDir2,
&   System.bool HasCenterline,
&   System.double TessTolFactor,
&   System.bool WantsSolid,
&   System.bool MergeBody,
&   System.bool FeatureScope,
&   System.bool AutoSelect,
&   System.bool Thin,
&   System.double Thickness1,
&   System.double Thickness2,
&   System.bool ReverseThickness,
&   System.short ThinSolidType,
&   System.bool UseSharedThickness,
&   System.bool CapEnds,
&   System.double EndThickness,
&   System.bool AutoFillet,
&   System.double FilletRadius,
&   System.bool ForceNonRational
) 

Parameters

Type
  • 0 = Base
  • 1 = Boss
  • 2 = Surface
  • 3 = Cut
NCurvesDir1
Number of curves in Direction 1
NCurvesDir2
Number of curves in Direction 2
HasCenterline
True if a centerline exists, false if not
TessTolFactor
Factor to control the number of intermediate sections used for loft with centerline; default value is 1.0; the greater the variable, the more intermediate sections created
WantsSolid

True if you want a solid body, false if you want a surface body; valid only when Type = 0, 1, or 3

MergeBody
True merges the results in a multibody part, false does not
FeatureScope
True if the feature only affects selected bodies, false if the feature affects all bodies
AutoSelect
True to automatically select all bodies and have the feature affect those bodies, false to select the bodies the feature affects
Thin
True if this feature is a thin body, false if not
Thickness1
Thickness value for the first direction
Thickness2
Thickness value for the second direction
ReverseThickness
True to reverse the thickness, false to not
ThinSolidType
Thin wall type as defined in swThinWallType_e
UseSharedThickness
True to use shared thickness, false to not
CapEnds
RUE to cap the ends, false to not
EndThickness
End cap thickness
AutoFillet
True to fillet the corners automatically, false to not
FilletRadius
Fillet radius when FilletRadius is true
ForceNonRational
True to force the resulting surface to be non-rational, false to not

Return Value

Pointer to the IFeature object

Example

Remarks

You can only use IModelDocExtension::SelectByID2 to select the entities for a boundary feature or boundary surface feature. Valid marks are:

Feature Selection marks
Boundary

Sketch curves:

  • Direction 1: 8193, 16385, 24577
  • Direction 2: 8194, 16386, 24578

Faces:

  • Direction 1: 8193, 16385, 24577
  • Direction 2: 8194, 16386, 24578

Other sketch entities (3D sketch (Unknown/SELOBJGROUP):

  • Direction 1: 12289, 24577
  • Direction 2: 16386, 28674
Boundary surface

Sketch curves:

  • Direction 1: 1
  • Direction 2: 2

 

 

See Also

Availability

SOLIDWORKS 2007 FCS, Revision Number 15.0


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