Function FeatureExtrusionThin2( _
   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 Merge As Boolean, _
   ByVal Thk1 As Double, _
   ByVal Thk2 As Double, _
   ByVal EndThk As Double, _
   ByVal RevThinDir As Integer, _
   ByVal CapEnds As Integer, _
   ByVal AddBends As Boolean, _
   ByVal BendRad As Double, _
   ByVal UseFeatScope As Boolean, _
   ByVal UseAutoSelect As Boolean, _
   ByVal T0 As Integer, _
   ByVal StartOffset As Double, _
   ByVal FlipStartOffset As Boolean _
) As Feature

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 Merge As Boolean
Dim Thk1 As Double
Dim Thk2 As Double
Dim EndThk As Double
Dim RevThinDir As Integer
Dim CapEnds As Integer
Dim AddBends As Boolean
Dim BendRad As Double
Dim UseFeatScope As Boolean
Dim UseAutoSelect As Boolean
Dim T0 As Integer
Dim StartOffset As Double
Dim FlipStartOffset As Boolean
Dim value As Feature
 
value = instance.FeatureExtrusionThin2(Sd, Flip, Dir, T1, T2, D1, D2, Dchk1, Dchk2, Ddir1, Ddir2, Dang1, Dang2, OffsetReverse1, OffsetReverse2, TranslateSurface1, TranslateSurface2, Merge, Thk1, Thk2, EndThk, RevThinDir, CapEnds, AddBends, BendRad, UseFeatScope, UseAutoSelect, T0, StartOffset, FlipStartOffset)

Feature FeatureExtrusionThin2( 
   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 Merge,
   double Thk1,
   double Thk2,
   double EndThk,
   int RevThinDir,
   int CapEnds,
   bool AddBends,
   double BendRad,
   bool UseFeatScope,
   bool UseAutoSelect,
   int T0,
   double StartOffset,
   bool FlipStartOffset
)

Feature^ FeatureExtrusionThin2( 
&   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 Merge,
&   double Thk1,
&   double Thk2,
&   double EndThk,
&   int RevThinDir,
&   int CapEnds,
&   bool AddBends,
&   double BendRad,
&   bool UseFeatScope,
&   bool UseAutoSelect,
&   int T0,
&   double StartOffset,
&   bool FlipStartOffset
) 

Parameters

Sd

True for single ended, false for double ended

Flip

Not used

Dir

Reverse direction; True if you want Direction1 to be opposite the default direction (see Remarks)

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

True for first draft angle to be inward, false to be outward

Ddir2

True for second draft angle to be inward, false to be outward

Dang1

First draft angle

Dang2

Second draft angle

OffsetReverse1

If you chose to offset the first end condition from another face or plane, then True specifies offset in direction away from the sketch, false specifies offset from the face or plane in direction toward the sketch

OffsetReverse2

If you chose to offset the second end condition from another face or plane, then True specifies offset in direction away from the sketch, false specifies offset from the face or plane in direction toward the sketch

TranslateSurface1

When you choose swEndcondOffsetFromSurface as the termination type for the first end, then True specifies that the end of the extrusion is a translation of the reference surface, false specifies to use a true offset

TranslateSurface2

When you choose swEndcondOffsetFromSurface as the termination type for the second end, then True specifies that the end of the extrusion is a translation of the reference surface, false specifies to use a true offset

Merge

True to merge the resultant base or boss body into an existing body, false to create a distinct solid body

Thk1

Wall thickness 1 (Mid-plane type uses (Thk1)/2 for each direction)

Thk2

Wall thickness 2 (Only used when RevThinType =3 )

EndThk

End cap thickness (Only used when CapEnds = 1)

RevThinDir

Thin feature type:

• 0 = One direction

• 1 = One direction reverse

• 2 = Mid-plane

• 3 = Two direction

CapEnds

Cap the ends:

• 0 = no cap

• 1 = cap (base features only)

AddBends

True to add auto bends (open profile base features only), false to not

BendRad

Fillet radii if AddBends = True

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 (see Remarks)

T0

Start condition as defined in swStartConditions_e

StartOffset

If T0 set to swStartOffset, then specify offset value

FlipStartOffset

If T0 set to swStartOffset, then True to flip the direction or false to not

Return Value

Pointer to the IFeature object

The default direction for cut operations is opposite the sketch normal. The default direction for boss operations is along the sketch normal. Setting the Dir argument to True reverses the default direction. For double-ended extrusions, Direction 2 is always opposite of Direction 1.

The default sketch normal is the same as the face or plane normal where the sketch was placed. To determine this normal vector, see IFace2::Normal and IRefPlane::Transform, respectively.

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

When using cut or cavity features that result in multiple bodies, you cannot select to keep all of the resulting bodies or one or more selected bodies.