Function InsertProtrusionBlend( _
   ByVal Closed As Boolean, _
   ByVal KeepTangency As Boolean, _
   ByVal ForceNonRational As Boolean, _
   ByVal TessToleranceFactor As Double, _
   ByVal StartMatchingType As Short, _
   ByVal EndMatchingType As Short, _
   ByVal StartTangentLength As Double, _
   ByVal EndTangentLength As Double, _
   ByVal StartTangentDir As Boolean, _
   ByVal EndTangentDir As Boolean, _
   ByVal IsThinBody As Boolean, _
   ByVal Thickness1 As Double, _
   ByVal Thickness2 As Double, _
   ByVal ThinType As Short, _
   ByVal Merge As Boolean, _
   ByVal UseFeatScope As Boolean, _
   ByVal UseAutoSelect As Boolean _
) As Feature

Dim instance As IFeatureManager
Dim Closed As Boolean
Dim KeepTangency As Boolean
Dim ForceNonRational As Boolean
Dim TessToleranceFactor As Double
Dim StartMatchingType As Short
Dim EndMatchingType As Short
Dim StartTangentLength As Double
Dim EndTangentLength As Double
Dim StartTangentDir As Boolean
Dim EndTangentDir As Boolean
Dim IsThinBody As Boolean
Dim Thickness1 As Double
Dim Thickness2 As Double
Dim ThinType As Short
Dim Merge As Boolean
Dim UseFeatScope As Boolean
Dim UseAutoSelect As Boolean
Dim value As Feature
 
value = instance.InsertProtrusionBlend(Closed, KeepTangency, ForceNonRational, TessToleranceFactor, StartMatchingType, EndMatchingType, StartTangentLength, EndTangentLength, StartTangentDir, EndTangentDir, IsThinBody, Thickness1, Thickness2, ThinType, Merge, UseFeatScope, UseAutoSelect)

Feature InsertProtrusionBlend( 
   bool Closed,
   bool KeepTangency,
   bool ForceNonRational,
   double TessToleranceFactor,
   short StartMatchingType,
   short EndMatchingType,
   double StartTangentLength,
   double EndTangentLength,
   bool StartTangentDir,
   bool EndTangentDir,
   bool IsThinBody,
   double Thickness1,
   double Thickness2,
   short ThinType,
   bool Merge,
   bool UseFeatScope,
   bool UseAutoSelect
)

Feature^ InsertProtrusionBlend( 
&   bool Closed,
&   bool KeepTangency,
&   bool ForceNonRational,
&   double TessToleranceFactor,
&   short StartMatchingType,
&   short EndMatchingType,
&   double StartTangentLength,
&   double EndTangentLength,
&   bool StartTangentDir,
&   bool EndTangentDir,
&   bool IsThinBody,
&   double Thickness1,
&   double Thickness2,
&   short ThinType,
&   bool Merge,
&   bool UseFeatScope,
&   bool UseAutoSelect
) 

Parameters

Closed

True closes the loft, false leaves the loft open; if true and you selected less that three profiles, any selected guide curves must be closed curves

KeepTangency

True maintains the tangency as seen in the section curves, false does not

If the section curves are tangent, then you have the option to specify whether the resulting faces are also tangent; when generating tangent surfaces, SolidWorks maintains planar and cylindrical surface shapes if the section curves exhibit these characteristics

ForceNonRational

True obtains smoother surfaces, false does not

NOTE: This argument corresponds to the Advanced smoothing option in the user interface. This option is available only if the loft sections have circular or elliptical arcs. The sections are approximated, and sketch arcs can be converted to splines.

TessToleranceFactor

Factor that controls the number of intermediate sections used for loft with centerline; the default value is 1.0; the greater the value, the more intermediate sections are created

StartMatchingType

Tangency type at the start profile:

• 0 = none

• 1 = tangent to the normal of the profile

• 2 = tangent to a selected vector

• 3 = tangency to all the adjacent faces sharing an edge with the start profile

• 4 = tangent to some of the selected faces sharing an edge with the start profile (not available)

EndMatchingType

Tangency type at the end profile:

• 0 = none

• 1 = tangent to the normal of the profile

• 2 = tangent to a selected vector

• 3 = tangency to all the adjacent faces sharing an edge with the start profile

• 4 = tangent to some of the selected faces sharing an edge with the start profile (not available)

StartTangentLength

Start tangent length

EndTangentLength

End tangent length

StartTangentDir

True is one direction, false is the opposite

EndTangentDir

True is one direction, false is the opposite

IsThinBody

True if this feature is a thin body, false if it is not

Thickness1

Thickness value for the first direction

Thickness2

Thickness value for the second direction

ThinType

Thin wall type:

• 0 = One direction

• 1 = One direction reverse

• 2 = Mid-plane

• 3 = Two direction

Merge

True merges the results in a multibody part, false does not

UseFeatScope

True if the feature only affects selected bodies, false if the feature affects all bodies

UseAutoSelect

True to automatically select all bodies and have the feature affect those bodies, false to select the bodies the feature affects

Return Value

Pointer to the IFeature object

Selection of guide curves and centerline is optional. However, you must select the profiles in an order consistent with the desired direction of the loft. Because a solid is being created, the section profiles must be closed.

It is best to use guide curves, especially when you select profiles in the FeatureManager design tree.

You can use any number of profiles; however, if you select only one profile, then any selected guide curves must be closed curves.

Use IModelDocExtension::SelectByID2 to select the profiles and guide curves. Set the mark for:

• profile selections to 1

• any guide curve selection to 2

• centerline selection to 4

• start tangency vector selection to 8

• start tangency faces selection to 16 (not available)

• end tangency vector selection to 32

• end tangency faces selection to 64 (not available)

NOTE: Linear edge, sketch line, axis, plane and planar faces are qualified for tangency vector sections.

When UseAutoSelect is false, the user must select the bodies that the feature will affect.