Function FeatureCut4( _
   ByVal Sd As System.Boolean, _
   ByVal Flip As System.Boolean, _
   ByVal Dir As System.Boolean, _
   ByVal T1 As System.Integer, _
   ByVal T2 As System.Integer, _
   ByVal D1 As System.Double, _
   ByVal D2 As System.Double, _
   ByVal Dchk1 As System.Boolean, _
   ByVal Dchk2 As System.Boolean, _
   ByVal Ddir1 As System.Boolean, _
   ByVal Ddir2 As System.Boolean, _
   ByVal Dang1 As System.Double, _
   ByVal Dang2 As System.Double, _
   ByVal OffsetReverse1 As System.Boolean, _
   ByVal OffsetReverse2 As System.Boolean, _
   ByVal TranslateSurface1 As System.Boolean, _
   ByVal TranslateSurface2 As System.Boolean, _
   ByVal NormalCut As System.Boolean, _
   ByVal UseFeatScope As System.Boolean, _
   ByVal UseAutoSelect As System.Boolean, _
   ByVal AssemblyFeatureScope As System.Boolean, _
   ByVal AutoSelectComponents As System.Boolean, _
   ByVal PropagateFeatureToParts As System.Boolean, _
   ByVal T0 As System.Integer, _
   ByVal StartOffset As System.Double, _
   ByVal FlipStartOffset As System.Boolean, _
   ByVal OptimizeGeometry As System.Boolean _
) As Feature

Dim instance As IFeatureManager
Dim Sd As System.Boolean
Dim Flip As System.Boolean
Dim Dir As System.Boolean
Dim T1 As System.Integer
Dim T2 As System.Integer
Dim D1 As System.Double
Dim D2 As System.Double
Dim Dchk1 As System.Boolean
Dim Dchk2 As System.Boolean
Dim Ddir1 As System.Boolean
Dim Ddir2 As System.Boolean
Dim Dang1 As System.Double
Dim Dang2 As System.Double
Dim OffsetReverse1 As System.Boolean
Dim OffsetReverse2 As System.Boolean
Dim TranslateSurface1 As System.Boolean
Dim TranslateSurface2 As System.Boolean
Dim NormalCut As System.Boolean
Dim UseFeatScope As System.Boolean
Dim UseAutoSelect As System.Boolean
Dim AssemblyFeatureScope As System.Boolean
Dim AutoSelectComponents As System.Boolean
Dim PropagateFeatureToParts As System.Boolean
Dim T0 As System.Integer
Dim StartOffset As System.Double
Dim FlipStartOffset As System.Boolean
Dim OptimizeGeometry As System.Boolean
Dim value As Feature
 
value = instance.FeatureCut4(Sd, Flip, Dir, T1, T2, D1, D2, Dchk1, Dchk2, Ddir1, Ddir2, Dang1, Dang2, OffsetReverse1, OffsetReverse2, TranslateSurface1, TranslateSurface2, NormalCut, UseFeatScope, UseAutoSelect, AssemblyFeatureScope, AutoSelectComponents, PropagateFeatureToParts, T0, StartOffset, FlipStartOffset, OptimizeGeometry)

Feature FeatureCut4( 
   System.bool Sd,
   System.bool Flip,
   System.bool Dir,
   System.int T1,
   System.int T2,
   System.double D1,
   System.double D2,
   System.bool Dchk1,
   System.bool Dchk2,
   System.bool Ddir1,
   System.bool Ddir2,
   System.double Dang1,
   System.double Dang2,
   System.bool OffsetReverse1,
   System.bool OffsetReverse2,
   System.bool TranslateSurface1,
   System.bool TranslateSurface2,
   System.bool NormalCut,
   System.bool UseFeatScope,
   System.bool UseAutoSelect,
   System.bool AssemblyFeatureScope,
   System.bool AutoSelectComponents,
   System.bool PropagateFeatureToParts,
   System.int T0,
   System.double StartOffset,
   System.bool FlipStartOffset,
   System.bool OptimizeGeometry
)

Feature^ FeatureCut4( 
&   System.bool Sd,
&   System.bool Flip,
&   System.bool Dir,
&   System.int T1,
&   System.int T2,
&   System.double D1,
&   System.double D2,
&   System.bool Dchk1,
&   System.bool Dchk2,
&   System.bool Ddir1,
&   System.bool Ddir2,
&   System.double Dang1,
&   System.double Dang2,
&   System.bool OffsetReverse1,
&   System.bool OffsetReverse2,
&   System.bool TranslateSurface1,
&   System.bool TranslateSurface2,
&   System.bool NormalCut,
&   System.bool UseFeatScope,
&   System.bool UseAutoSelect,
&   System.bool AssemblyFeatureScope,
&   System.bool AutoSelectComponents,
&   System.bool PropagateFeatureToParts,
&   System.int T0,
&   System.double StartOffset,
&   System.bool FlipStartOffset,
&   System.bool OptimizeGeometry
) 

Parameters

Sd

True for a single-ended cut, false for a doubled-ended cut

Flip

True to remove material outside of the profile of the flip side to cut, false to not

Dir

True for Direction 1 to be opposite of the default direction (see Remarks)

T1

Termination type for the first end as defined in swEndConditions_e

T2

Termination type for the second end as defined in swEndConditions_e

D1

Depth of extrusion for the first end in meters

D2

Depth of extrusion for the second end in meters

Dchk1

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

Dchk2

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

Ddir1

True for the first draft angle to be inward, false to be outward; only valid when Dchk1 is true

Ddir2

True for the second draft angle to be inward, false to be outward; only valid when Dchk2 is true

Dang1

Draft angle for the first end; only valid when Dchk1 is true

Dang2

Draft angle for the second end; only valid when Dchk2 is true

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 a 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 a direction toward the sketch

TranslateSurface1

When you choose swEndConditions_e.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 swEndConditions_e.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

NormalCut

True to create the cut normal to the sheet metal thickness, false to not (only valid for sheet metal parts; use false for non-sheet metal parts)

UseFeatScope

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

UseAutoSelect

True to automatically select all bodies or components and have the feature affect those bodies or components, false to only select the bodies or components the feature affects (see Remarks)

AssemblyFeatureScope

True if the assembly feature only affects selected components in the assembly, false if the assembly feature affects all components in the assembly

AutoSelectComponents

True to automatically select all affected components, false to use only the selected components

PropagateFeatureToParts

True to propagate the assembly feature to the components in the model that it affects, false to not

T0

Start conditions as defined in swStartConditions_e

StartOffset

If T0 is swStartConditions_e.swStartOffset, then specify an offset value

FlipStartOffset

If T0 is swStartConditions_e.swStartOffset, then true to flip the direction of cut, false to not

OptimizeGeometry

True to optimize the normal cut in a sheet metal part, false to not; only valid for sheet metal parts and when NormalCut is true

Return Value

The default direction for:

• cut operations is opposite the sketch normal.
• boss operations is along the sketch normal.

Setting the direction parameters to true reverses the default direction. For double-ended extrusions, Direction 2 is always opposite to Direction 1.

The default sketch normal is the face or plane that is perpendicular to the sketch plane. To determine the sketch normal, see IFace2::Normal and IRefPlane::Transform.

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.