Function CreateLoftBody2( _
   ByVal PModDoc As ModelDoc2, _
   ByVal Profile As Object, _
   ByVal GuideCurve As Object, _
   ByVal CenterLine As Object, _
   ByVal IsThinBody As Boolean, _
   ByVal ThinType As Integer, _
   ByVal Thickness1 As Double, _
   ByVal Thickness2 As Double, _
   ByVal FeatureScope As Boolean, _
   ByVal IsBlendClosed As Boolean, _
   ByVal KeepTangency As Boolean, _
   ByVal ForceNonRational As Boolean, _
   ByVal IsSolidBody As Boolean, _
   ByVal TessTolFactor As Double, _
   ByVal StartTangentLength As Double, _
   ByVal EndTangentLength As Double, _
   ByVal StartTangentDir As Boolean, _
   ByVal EndTangentDir As Boolean, _
   ByVal StartMatchingType As Integer, _
   ByVal EndMatchingType As Integer, _
   ByVal Merge As Boolean _
) As Body2

Dim instance As IModeler
Dim PModDoc As ModelDoc2
Dim Profile As Object
Dim GuideCurve As Object
Dim CenterLine As Object
Dim IsThinBody As Boolean
Dim ThinType As Integer
Dim Thickness1 As Double
Dim Thickness2 As Double
Dim FeatureScope As Boolean
Dim IsBlendClosed As Boolean
Dim KeepTangency As Boolean
Dim ForceNonRational As Boolean
Dim IsSolidBody As Boolean
Dim TessTolFactor As Double
Dim StartTangentLength As Double
Dim EndTangentLength As Double
Dim StartTangentDir As Boolean
Dim EndTangentDir As Boolean
Dim StartMatchingType As Integer
Dim EndMatchingType As Integer
Dim Merge As Boolean
Dim value As Body2
 
value = instance.CreateLoftBody2(PModDoc, Profile, GuideCurve, CenterLine, IsThinBody, ThinType, Thickness1, Thickness2, FeatureScope, IsBlendClosed, KeepTangency, ForceNonRational, IsSolidBody, TessTolFactor, StartTangentLength, EndTangentLength, StartTangentDir, EndTangentDir, StartMatchingType, EndMatchingType, Merge)

Body2 CreateLoftBody2( 
   ModelDoc2 PModDoc,
   object Profile,
   object GuideCurve,
   object CenterLine,
   bool IsThinBody,
   int ThinType,
   double Thickness1,
   double Thickness2,
   bool FeatureScope,
   bool IsBlendClosed,
   bool KeepTangency,
   bool ForceNonRational,
   bool IsSolidBody,
   double TessTolFactor,
   double StartTangentLength,
   double EndTangentLength,
   bool StartTangentDir,
   bool EndTangentDir,
   int StartMatchingType,
   int EndMatchingType,
   bool Merge
)

Body2^ CreateLoftBody2( 
&   ModelDoc2^ PModDoc,
&   Object^ Profile,
&   Object^ GuideCurve,
&   Object^ CenterLine,
&   bool IsThinBody,
&   int ThinType,
&   double Thickness1,
&   double Thickness2,
&   bool FeatureScope,
&   bool IsBlendClosed,
&   bool KeepTangency,
&   bool ForceNonRational,
&   bool IsSolidBody,
&   double TessTolFactor,
&   double StartTangentLength,
&   double EndTangentLength,
&   bool StartTangentDir,
&   bool EndTangentDir,
&   int StartMatchingType,
&   int EndMatchingType,
&   bool Merge
) 

Parameters

PModDoc

Model document in which to create the loft body

Profile

Array of sketches representing the profiles of the loft body

GuideCurve

Array of sketches representing the guide curves of the loft body

CenterLine

Sketch representing a centerline of the loft body

IsThinBody

True if the loft body is to be a thin body, false if not

ThinType

• 0 = One direction

• 1 = One direction reverse

• 2 = Midplane

• 3 = Two direction

Thickness1

Value for thickness for first direction if a thin body

Thickness2

Value for thickness for second direction if a thin body

FeatureScope

True if the loft body only affects selected bodies, false if the loft body affects all bodies

IsBlendClosed

True for a closed loft, false for an open loft; if true and you selected less that three profiles, then any selected guide curves must be closed curves

KeepTangency

If the section curves are tangent, then you have the option to specify whether the resulting faces are also tangent; specify true to maintain the tangency as seen in the section curves, false to not

NOTE: When generating tangent surfaces, SolidWorks maintains planar and cylindrical surface shapes if the section curves exhibit these characteristics.

ForceNonRational

True to force the resulting surface to be non-rational, false to not

IsSolidBody

True to return a solid loft body, false to return a surface loft body

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

StartTangentLength

Start tangent length

EndTangentLength

End tangent length

StartTangentDir

True is one direction, false is the opposite direction

EndTangentDir

True is one direction, false is the opposite direction

StartMatchingType

Tangency type at the start profile:

• 0 = none

• 1 = tangent to the normal of the profile

• 2 = tangent to the selected vector

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

EndMatchingType

Tangency type as the end profile:

• 0 = none

• 1 = tangent to the normal of the profile

• 2 = tangent to the selected vector

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

Merge

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

Return Value

Specifying guide curves and a centerline are optional. It is best to use guide curves, especially when you select profiles in the FeatureManager design tree.

You must specify the profiles in an order consistent with the desired direction of the loft. If creating a solid loft body, then the profiles must be closed. You can use any number of profiles. However, if you specify only one profile, then any specified guide curves must be closed curves.

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