Sub FeatureExtruRefSurface( _
   ByVal Sd As Boolean, _
   ByVal Flip As Boolean, _
   ByVal Dir As Boolean, _
   ByVal T1 As Integer, _
   ByVal T2 As Integer, _
   ByVal D1 As Double, _
   ByVal D2 As Double, _
   ByVal Dchk1 As Boolean, _
   ByVal Dchk2 As Boolean, _
   ByVal Ddir1 As Boolean, _
   ByVal Ddir2 As Boolean, _
   ByVal Dang1 As Double, _
   ByVal Dang2 As Double, _
   ByVal OffsetReverse1 As Boolean, _
   ByVal OffsetReverse2 As Boolean, _
   ByVal TranslateSurface1 As Boolean, _
   ByVal TranslateSurface2 As Boolean, _
   ByVal CapEnd1 As Boolean, _
   ByVal CapEnd2 As Boolean, _
   ByVal DeleteOriginalFace As Boolean, _
   ByVal KnitResult As Boolean _
) 

Dim instance As IFeatureManager
Dim Sd As Boolean
Dim Flip As Boolean
Dim Dir As Boolean
Dim T1 As Integer
Dim T2 As Integer
Dim D1 As Double
Dim D2 As Double
Dim Dchk1 As Boolean
Dim Dchk2 As Boolean
Dim Ddir1 As Boolean
Dim Ddir2 As Boolean
Dim Dang1 As Double
Dim Dang2 As Double
Dim OffsetReverse1 As Boolean
Dim OffsetReverse2 As Boolean
Dim TranslateSurface1 As Boolean
Dim TranslateSurface2 As Boolean
Dim CapEnd1 As Boolean
Dim CapEnd2 As Boolean
Dim DeleteOriginalFace As Boolean
Dim KnitResult As Boolean
 
instance.FeatureExtruRefSurface(Sd, Flip, Dir, T1, T2, D1, D2, Dchk1, Dchk2, Ddir1, Ddir2, Dang1, Dang2, OffsetReverse1, OffsetReverse2, TranslateSurface1, TranslateSurface2, CapEnd1, CapEnd2, DeleteOriginalFace, KnitResult)

void FeatureExtruRefSurface( 
   bool Sd,
   bool Flip,
   bool Dir,
   int T1,
   int T2,
   double D1,
   double D2,
   bool Dchk1,
   bool Dchk2,
   bool Ddir1,
   bool Ddir2,
   double Dang1,
   double Dang2,
   bool OffsetReverse1,
   bool OffsetReverse2,
   bool TranslateSurface1,
   bool TranslateSurface2,
   bool CapEnd1,
   bool CapEnd2,
   bool DeleteOriginalFace,
   bool KnitResult
)

void FeatureExtruRefSurface( 
&   bool Sd,
&   bool Flip,
&   bool Dir,
&   int T1,
&   int T2,
&   double D1,
&   double D2,
&   bool Dchk1,
&   bool Dchk2,
&   bool Ddir1,
&   bool Ddir2,
&   double Dang1,
&   double Dang2,
&   bool OffsetReverse1,
&   bool OffsetReverse2,
&   bool TranslateSurface1,
&   bool TranslateSurface2,
&   bool CapEnd1,
&   bool CapEnd2,
&   bool DeleteOriginalFace,
&   bool KnitResult
) 

Parameters

Sd

True for single-ended, false for double-ended

Flip

True to flip the direction to cut, false to not

Dir

True to flip direction of the extrude, false to not

T1

Termination type for first end as defined in swEndConditions_e

T2

Termination type for second end as defined in swEndConditions_e

D1

Depth of extrusion for first end in meters

D2

Depth of extrusion for second end in meters

Dchk1

True allows draft angle in first direction, false does not allow drafting

Dchk2

True allows draft angle in second direction, false does not allow drafting

Ddir1

For first draft angle to be inward use true, for draft angle outward use false

Ddir2

For second draft angle to be inward use true, for draft angle outward use false

Dang1

Draft angle for first end

Dang2

Draft angle for second end

OffsetReverse1

If you choose to offset the first end condition from another face or plane, then true specifies the offset from the face or plane in a direction away from the sketch, and false specifies the offset in a direction toward the sketch

OffsetReverse2

If you choose to offset the second end condition from another face or plane, then true specifies the offset from the face or plane in direction away from the sketch, and false specifies the offset in a direction toward the sketch

TranslateSurface1

If you specified T1 as swEndConditions_e.swEndCondOffsetFromSurface, then true specifies that the end of the extrusion is a translation of the reference surface, and false specifies to use a true offset

TranslateSurface2

If you specified T2 as swEndConditions_e.swEndCondOffsetFromSurface, then true specifies that the end of the extrusion is a translation of the reference surface, and false specifies to use a true offset

CapEnd1

True to cap first end, false to not

CapEnd2

True to cap second end, false to not

DeleteOriginalFace

True to delete original faces, false to not (see Remarks)

KnitResult

True to knit the extrusion result, false to not (see Remarks)

Before calling this method, select the entities from which to extrude reference surfaces. Do one of the following:

• select a sketch containing one face or multiple co-planar faces
• select one face or multiple co-planar faces in the view

DeleteOriginalFace and KnitResult are ignored if the extrusion is in two directions.

KnitResult is ignored if DeleteOriginalFace is false.