Hide Table of Contents
InsertProtrusionBlend Method (IFeatureManager)

Obsolete. Superseded by IFeatureManager::InsertProtrusionBlend2.

.NET Syntax

Visual Basic (Declaration) 
Function InsertProtrusionBlend( _
   ByVal Closed As System.Boolean, _
   ByVal KeepTangency As System.Boolean, _
   ByVal ForceNonRational As System.Boolean, _
   ByVal TessToleranceFactor As System.Double, _
   ByVal StartMatchingType As System.Short, _
   ByVal EndMatchingType As System.Short, _
   ByVal StartTangentLength As System.Double, _
   ByVal EndTangentLength As System.Double, _
   ByVal StartTangentDir As System.Boolean, _
   ByVal EndTangentDir As System.Boolean, _
   ByVal IsThinBody As System.Boolean, _
   ByVal Thickness1 As System.Double, _
   ByVal Thickness2 As System.Double, _
   ByVal ThinType As System.Short, _
   ByVal Merge As System.Boolean, _
   ByVal UseFeatScope As System.Boolean, _
   ByVal UseAutoSelect As System.Boolean _
) As Feature
Visual Basic (Usage) 
Dim instance As IFeatureManager
Dim Closed As System.Boolean
Dim KeepTangency As System.Boolean
Dim ForceNonRational As System.Boolean
Dim TessToleranceFactor As System.Double
Dim StartMatchingType As System.Short
Dim EndMatchingType As System.Short
Dim StartTangentLength As System.Double
Dim EndTangentLength As System.Double
Dim StartTangentDir As System.Boolean
Dim EndTangentDir As System.Boolean
Dim IsThinBody As System.Boolean
Dim Thickness1 As System.Double
Dim Thickness2 As System.Double
Dim ThinType As System.Short
Dim Merge As System.Boolean
Dim UseFeatScope As System.Boolean
Dim UseAutoSelect As System.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)
C# 
Feature InsertProtrusionBlend( 
   System.bool Closed,
   System.bool KeepTangency,
   System.bool ForceNonRational,
   System.double TessToleranceFactor,
   System.short StartMatchingType,
   System.short EndMatchingType,
   System.double StartTangentLength,
   System.double EndTangentLength,
   System.bool StartTangentDir,
   System.bool EndTangentDir,
   System.bool IsThinBody,
   System.double Thickness1,
   System.double Thickness2,
   System.short ThinType,
   System.bool Merge,
   System.bool UseFeatScope,
   System.bool UseAutoSelect
)
C++/CLI 
Feature^ InsertProtrusionBlend( 
&   System.bool Closed,
&   System.bool KeepTangency,
&   System.bool ForceNonRational,
&   System.double TessToleranceFactor,
&   System.short StartMatchingType,
&   System.short EndMatchingType,
&   System.double StartTangentLength,
&   System.double EndTangentLength,
&   System.bool StartTangentDir,
&   System.bool EndTangentDir,
&   System.bool IsThinBody,
&   System.double Thickness1,
&   System.double Thickness2,
&   System.short ThinType,
&   System.bool Merge,
&   System.bool UseFeatScope,
&   System.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

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

Remarks

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.

 

See Also

Availability

SOLIDWORKS 2003 FCS, Revision Number 11.0


Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   InsertProtrusionBlend Method (IFeatureManager)
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:



x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: API Help (English only) 2017 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.