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ShapeFactory (Object)

MecModInterfaces.Factory

ShapeFactory

Represents the factory for shapes to create all kinds of shapes that may be needed for part design.

The Shapefactory mission is to build from scratch shapes that will be used within the design process of parts. Those shapes have a strong mechanical built-in knowledge, such as chamfer or hole, and in most cases apply contextually to the part being designed. When created, they become part of the definition of whichever body or shape that is current at that time. After they are created, they become in turn the current body or shape. In most cases, shapes are created from a factory with a minimum number of parametersr. Other shapes parameters may be set further on by using methods offered by the shape itself.

AddNewAdd: Creates and returns a new add operation within the current body.
AddNewAffinity2: Creates and returns a Affinity feature.
AddNewAssemble: Creates and returns a new assembly operation within the current body.
AddNewAutoDraft: Creates and returns a new solid autodraft.
AddNewAutoFillet: Creates and returns a new solid autofillet.
AddNewAxisToAxis2: Creates and returns an AxisToAxis transformation feature.
AddNewBlend: Creates and returns a new Blend feature.
AddNewChamfer: Creates and returns a new chamfer within the current body.
AddNewCircPattern: Creates and returns a new circular pattern within the current body.
AddNewCircPatternofList: V5R8 Only: Creates and returns a new circular pattern within the current body using a list of shapes.
AddNewCloseSurface: Creates and returns a new CloseSurface feature.
AddNewDraft: Creates and returns a new draft within the current body.
AddNewEdgeFilletWithConstantRadius
AddNewEdgeFilletWithVaryingRadius
AddNewFaceFillet
AddNewGSDCircPattern
AddNewGSDRectPattern
AddNewGrooveFromRef: Creates and returns a new groove within the current body.
AddNewGroove: Creates and returns a new groove within the current body.
AddNewHoleFromPoint: Creates and returns a new hole within the current shape.
AddNewHoleFromRefPoint: Creates and returns a new hole within the current shape.
AddNewHoleFromSketch: Creates and returns a new hole within the current shape.
AddNewHoleWith2Constraints: Creates and returns a new hole within the current shape.
AddNewHoleWithConstraint: Creates and returns a new hole within the current shape.
AddNewHole: Creates and returns a new hole within the current shape.
AddNewIntersect: Creates and returns a new intersect operation within the current body.
AddNewLoft: Creates and returns a new Loft feature.
AddNewMirror: Creates and returns a new mirror within the current body.
AddNewPadFromRef: Creates and returns a new pad within the current body.
AddNewPad: Creates and returns a new pad within the current body.
AddNewPocketFromRef: Creates and returns a new pocket within the current shape.
AddNewPocket: Creates and returns a new pocket within the current shape.
AddNewRectPattern: Creates and returns a new rectangular pattern within the current body.
AddNewRectPatternofList: V5R8 Only: Creates and returns a new rectangular pattern within the current body using a list of shapes.
AddNewRemoveFace: Creates and returns a new RemoveFace feature.
AddNewRemove: Creates and returns a new remove operation within the current body.
AddNewRemovedBlend: Creates and returns a new Removed Blend feature.
AddNewRemovedLoft: Creates and returns a new Removed Loft feature.
AddNewReplaceFace: Creates and returns a new Align/ ReplaceFace feature.
AddNewRibFromRef: Creates and returns a new rib within the current body.
AddNewRib: Creates and returns a new rib within the current body.
AddNewScaling: Creates and returns a new scaling within the current body.
AddNewSewSurface: Creates and returns a new sewing operation within the current body.
AddNewShaftFromRef: Creates and returns a new shaft within the current body.
AddNewShaft: Creates and returns a new shaft within the current body.
AddNewShell: Creates and returns a new shell within the current body.
AddNewSlotFromRef: Creates and returns a new slot within the current shape.
AddNewSlot: Creates and returns a new slot within the current shape.
AddNewSolidCombine: Creates and returns a new SolidCombine feature.
AddNewSolidEdgeFilletWithConstantRadius: Creates and returns a new solid edge fillet with a constant radius.
AddNewSolidEdgeFilletWithVaryingRadius: Creates and returns a new solid edge fillet with a varying radius.
AddNewSolidFaceFillet: Creates and returns a new solid face-to-face fillet.
AddNewSolidTritangentFillet: Creates and returns a new solid tritangent fillet within the current body.
AddNewSplit: Creates and returns a new split operation within the current body.
AddNewStiffenerFromRef: Creates and returns a new stiffener within the current body.
AddNewStiffener: Creates and returns a new stiffener within the current body.
AddNewSurfaceEdgeFilletWithConstantRadius: Creates and returns a new surface edge fillet with a constant radius.
AddNewSurfaceEdgeFilletWithVaryingRadius: Creates and returns a new surface edge fillet with a varying radius.
AddNewSurfaceFaceFillet: Creates and returns a new surface face-to-face fillet.
AddNewSurfaceTritangentFillet: Creates and returns a new surface tritangent fillet within the current body.
AddNewSurfacicAutoFillet: Creates and returns a new Surfacic autofillet.
AddNewSurfacicCircPattern: Creates and returns a new gsd circular pattern within the current body.
AddNewSurfacicRectPattern: Creates and returns a new GSD rectangular pattern within the current body.
AddNewSurfacicUserPattern: Creates and returns a new GSD user pattern within the current body.
AddNewThickSurface: Creates and returns a new ThickSurface feature.
AddNewThickness: Creates and returns a new thickness within the current body.
AddNewThreadWithOutRef: Creates and returns a new thread\tap within the current body.
AddNewThreadWithRef: Creates and returns a new thread\tap within the current body.
AddNewTrim: Creates and returns a new Trim operation within the current body.
AddNewTritangentFillet
AddNewUserPattern: Creates and returns a new user pattern within the current body.
AddNewUserPatternofList: V5R8 Only: Creates and returns a new user pattern within the current body using a list of shapes.
AddNewVolumeAdd: Creates and returns a Volumic Add feature.
AddNewVolumeCloseSurface: Creates and returns a new VolumeCloseSurface feature.
AddNewVolumeIntersect: Creates and returns a Volumic Intersect feature.
AddNewVolumeRemove: Creates and returns a Volumic Remove feature.
AddNewVolumeSewSurface: Creates and returns a new volume sewing operation within the current OGS/GS.
AddNewVolumeShell: Creates and returns a Volumic Shell feature.
AddNewVolumeThickSurface: Creates and returns a new VolumeThickSurface feature.
AddNewVolumeThickness: Creates and returns a volume new thickness within the current GS or OGS.
AddNewVolumeTrim: Creates and returns a new Volume Trim operation within the GS/OGS.
AddNewVolumicDraft: Creates and returns a new volume draft within the current body.

Methods

o Func AddNewAdd( Body iBodyToAdd) As Add

Creates and returns a new add operation within the current body.

Parameters:

iBodyToAdd: The body to add to the current body

Returns:

The created add operation

o Func AddNewAffinity2(	double	`XRatio`,
	double	`YRatio`,
	double	`ZRatio`) As AnyObject

Creates and returns a Affinity feature.

Parameters:

XRatio: Value for the XRatio.
YRatio: Value for the YRatio.
ZRatio: Value for the ZRatio.

Returns:

the created Affinity feature.

o Func AddNewAssemble( Body iBodyToAssemble) As Assemble

Creates and returns a new assembly operation within the current body.

Parameters:

iBodyToAssemble: The body to assemble with the current body

Returns:

The created assembly operation

o Func AddNewAutoDraft( double iDraftAngle) As AutoDraft

Creates and returns a new solid autodraft.
Use this method to create autodraft by providing draft angle.

Parameters:

iDraftAngle: The draft angle.

Returns:

The created autodraft.

o Func AddNewAutoFillet(	double	`iFilletRadius`,
	double	`iRoundRadius`) As AutoFillet

Creates and returns a new solid autofillet.
Use this method to create autofillet by providing fillet and round radius values.

Parameters:

iFilletRadius: The fillet radius
iRoundRadius: The round radius

Returns:

The created autofillet

o Func AddNewAxisToAxis2(	Reference	`iReference`,
	Reference	`iTarget`) As AnyObject

Creates and returns an AxisToAxis transformation feature.

Parameters:

iReference: The refrence axis.
iTarget: The target axis.

Returns:

The created AxisToAxis transformation feature.

o Func AddNewBlend(

) As AnyObject

Creates and returns a new Blend feature.

Returns:: The created Blend feature

o Func AddNewChamfer(	Reference	`iObjectToChamfer`,
	CatChamferPropagation	`iPropagation`,
	CatChamferMode	`iMode`,
	CatChamferOrientation	`iOrientation`,
	double	`iLength1`,
	double	`iLength2OrAngle`) As Chamfer

Creates and returns a new chamfer within the current body.

Parameters:

iObjectToChamfer: The first edge or face to chamfer
The following

Boundary object is supported: TriDimFeatEdge.

iPropagation

Controls if and how the chamfering operation should propagate beyond the first chamfer element iObjectToChamfer, when it is an edge

iMode

Controls if the chamfer is defined by two lengthes, or by an angle and a length
The value of this argument changes the way the arguments iLength1 and iLength2OrAngle should be interpreted.

iOrientation

Defines the relative meaning of arguments iLength1 and iLength2OrAngle when defining a chamfer by two lengthes

iLength1

The first value for chamfer dimensioning. It represents the chamfer first length if the chamfer is defined by two lengthes, or the chamfer length if the chamfer is defined by a length and an angle.

iLength2OrAngle

The second value for chamfer dimensioning. It represents the chamfer second length if the chamfer is defined by two lengthes, or the chamfer angle if the chamfer is defined by a length and an angle.

Returns:

The created chamfer

o Func AddNewCircPattern(	AnyObject	`iShapeToCopy`,
	long	`iNbOfCopiesInRadialDir`,
	long	`iNbOfCopiesInAngularDir`,
	double	`iStepInRadialDir`,
	double	`iStepInAngularDir`,
	long	`iShapeToCopyPositionAlongRadialDir`,
	long	`iShapeToCopyPositionAlongAngularDir`,
	Reference	`iRotationCenter`,
	Reference	`iRotationAxis`,
	boolean	`iIsReversedRotationAxis`,
	double	`iRotationAngle`,
	boolean	`iIsRadiusAligned`) As CircPattern

Creates and returns a new circular pattern within the current body.

Parameters:

iShapeToCopy: The shape to be copied by the circular pattern
iNbOfInstancesInRadialDir: The number of times iShapeToCopy will be copied along pattern radial direction
iNbOfInstancesInAngularDir: The number of times iShapeToCopy will be copied along pattern angular direction
iStepInRadialDir: The distance that will separate two consecutive copies in the pattern along its radial direction
iStepInAngularDir: The angle that will separate two consecutive copies in the pattern along its angular direction
iShapeToCopyPositionAlongRadialDir: Specifies the position of the original shape iShapeToCopy among its copies along the radial direction
iShapeToCopyPositionAlongAngularDir: Specifies the position of the original shape iShapeToCopy among its copies along the angular direction
iRotationCenter: The point or vertex that specifies the pattern center of rotation
iRotationAxis: The line or linear edge that specifies the axis around which instances will be rotated relative to each other
The following

Boundary objects are supported: PlanarFace , CylindricalFace , RectilinearTriDimFeatEdge and RectilinearBiDimFeatEdge.

iIsReversedRotationAxis

The boolean flag indicating wether the natural orientation of iRotationAxis should be used to orient the pattern operation. A value of true indicates that iItemToDuplicate are copied in the direction of the natural orientation of iRotationAxis.

iRotationAngle

The angle applied to the direction iRotationAxis prior to applying the pattern. The original shape iShapeToCopy is used as the rotation center. Nevertheless, the copied shapes themselves are not rotated. This allows the definition of a circular pattern relatively to existing geometry, but not necessarily parallel to it.

iIsRadiusAligned

The boolean flag that specifies whether the instances of iItemToDuplicate copied by the pattern should be kept parallel to each other (True) or if they should be aligned with the radial direction they lie upon (False).

Returns:

The created circular pattern

o Func AddNewCircPatternofList(	AnyObject	`iShapeToCopy`,
	long	`iNbOfCopiesInRadialDir`,
	long	`iNbOfCopiesInAngularDir`,
	double	`iStepInRadialDir`,
	double	`iStepInAngularDir`,
	long	`iShapeToCopyPositionAlongRadialDir`,
	long	`iShapeToCopyPositionAlongAngularDir`,
	Reference	`iRotationCenter`,
	Reference	`iRotationAxis`,
	boolean	`iIsReversedRotationAxis`,
	double	`iRotationAngle`,
	boolean	`iIsRadiusAligned`) As CircPattern

V5R8 Only: Creates and returns a new circular pattern within the current body using a list of shapes.

Parameters:

iShapeToCopy: The shape to be copied by the circular pattern. Others shapes will be add by put_ItemToCopy with CATIAPattern interface
iNbOfInstancesInRadialDir: The number of times iShapeToCopy will be copied along pattern radial direction
iNbOfInstancesInAngularDir: The number of times iShapeToCopy will be copied along pattern angular direction
iStepInRadialDir: The distance that will separate two consecutive copies in the pattern along its radial direction
iStepInAngularDir: The angle that will separate two consecutive copies in the pattern along its angular direction
iShapeToCopyPositionAlongRadialDir: Specifies the position of the original shape iShapeToCopy among its copies along the radial direction
iShapeToCopyPositionAlongAngularDir: Specifies the position of the original shape iShapeToCopy among its copies along the angular direction
iRotationCenter: The point or vertex that specifies the pattern center of rotation
iRotationAxis: The line or linear edge that specifies the axis around which instances will be rotated relative to each other
iIsReversedRotationAxis: The boolean flag indicating wether the natural orientation of iRotationAxis should be used to orient the pattern operation. A value of true indicates that iItemToDuplicate are copied in the direction of the natural orientation of iRotationAxis.
iRotationAngle: The angle applied to the direction iRotationAxis prior to applying the pattern. The original shape iShapeToCopy is used as the rotation center. Nevertheless, the copied shapes themselves are not rotated. This allows the definition of a circular pattern relatively to existing geometry, but not necessarily parallel to it.
iIsRadiusAligned: The boolean flag that specifies whether the instances of iItemToDuplicate copied by the pattern should be kept parallel to each other (True) or if they should be aligned with the radial direction they lie upon (False).

Returns:

The created circular pattern

o Func AddNewCloseSurface( Reference iCloseElement) As CloseSurface

Creates and returns a new CloseSurface feature.

Parameters:

iCloseElement: The skin that will be closed and add with the current body

Returns:

The created CloseSurface feature

o Func AddNewDraft(	Reference	`iFaceToDraft`,
	Reference	`iNeutral`,
	CatDraftNeutralPropagationMode	`iNeutralMode`,
	Reference	`iParting`,
	double	`iDirX`,
	double	`iDirY`,
	double	`iDirZ`,
	CatDraftMode	`iMode`,
	double	`iAngle`,
	CatDraftMultiselectionMode	`iMultiselectionMode`) As Draft

Creates and returns a new draft within the current body.
The draft needs a reference face on the body. This face will remain unchanged in the draft operation, while faces adjacent to it and specified for drafting will be rotated by the draft angle.

Parameters:

iFaceToDraft: The first face to draft in the body. This face should be adjacent to the iFaceToDraft face. If several faces are to be drafted, only the first one is specified here, the others being inferred by propagating the draft operation onto faces adjacent to this first face. This is controlled by the iNeutralMode argument.
The following

Boundary object is supported: Face.

iNeutral

The reference face for the draft. The draft needs a reference face on the body, that will remain unchanged in the draft operation, while faces adjacent to it and specified for drafting will be rotated according to the draft angle iAngle.
The following

iNeutralMode

BoundaryPlanarFace Controls if and how the drafting operation should be propagated beyond the first face to draft iFaceToDraft to other adjacent faces.

iParting

The draft parting plane, face or surface. It specifies the element within the body to draft that represents the bottom of the mold. This element can be located either somewhere in the middle of the body or be one of its boundary faces. When located in the middle of the body, it crosses the faces to draft, and as a result, those faces are drafted with a positive angle on one side of the parting surface, and with a negative angle on the other side.
The following

iDirX,iDirY,iDirZ

BoundaryPlanarFace The X, Y, and Z components of the absolute vector representing the drafting direction (i.e. the mold extraction direction).

iMode

The draft connecting mode to its reference face iFaceToDraft

iAngle

The draft angle

iMultiselectionMode.

The elements to be drafted can be selected explicitly or can implicitly selected as neighbors of the neutral face

Returns:

The created draft

o Func AddNewEdgeFilletWithConstantRadius(	Reference	`iEdgeToFillet`,
	CatFilletEdgePropagation	`iPropagMode`,
	double	`iRadius`) As ConstRadEdgeFillet

Deprecated:: V5R14 #AddNewEdgeFilletWithConstantRadius use AddNewSolidEdgeFilletWithConstantRadius or AddNewSurfaceEdgeFilletWithConstantRadius depending on the type of fillet you want to create

o Func AddNewEdgeFilletWithVaryingRadius(	Reference	`iEdgeToFillet`,
	CatFilletEdgePropagation	`iPropagMode`,
	CatFilletVariation	`iVariationMode`,
	double	`iDefaultRadius`) As VarRadEdgeFillet

Deprecated:: V5R14 #AddNewEdgeFilletWithVaryingRadius use AddNewSolidEdgeFilletWithVaryingRadius or AddNewSurfaceEdgeFilletWithVaryingRadius depending on the type of fillet you want to create

o Func AddNewFaceFillet(	Reference	`iF1`,
	Reference	`iF2`,
	double	`iRadius`) As FaceFillet

Deprecated:: V5R14 #AddNewFaceFillet use AddNewSolidFaceFillet or AddNewSurfaceFaceFillet depending on the type of fillet you want to create

o Func AddNewGSDCircPattern(	AnyObject	`iShapeToCopy`,
	long	`iNbOfCopiesInRadialDir`,
	long	`iNbOfCopiesInAngularDir`,
	double	`iStepInRadialDir`,
	double	`iStepInAngularDir`,
	long	`iShapeToCopyPositionAlongRadialDir`,
	long	`iShapeToCopyPositionAlongAngularDir`,
	Reference	`iRotationCenter`,
	Reference	`iRotationAxis`,
	boolean	`iIsReversedRotationAxis`,
	double	`iRotationAngle`,
	boolean	`iIsRadiusAligned`,
	boolean	`iCompleteCrown`,
	double	`iType`) As CircPattern

Deprecated:: V5R15 #AddNewSurfacicCircPattern

o Func AddNewGSDRectPattern(	AnyObject	`iShapeToCopy`,
	long	`iNbOfCopiesInDir1`,
	long	`iNbOfCopiesInDir2`,
	double	`iStepInDir1`,
	double	`iStepInDir2`,
	long	`iShapeToCopyPositionAlongDir1`,
	long	`iShapeToCopyPositionAlongDir2`,
	Reference	`iDir1`,
	Reference	`iDir2`,
	boolean	`iIsReversedDir1`,
	boolean	`iIsReversedDir2`,
	double	`iRotationAngle`,
	double	`iType`) As RectPattern

Deprecated:: V5R15 #AddNewSurfacicRectPattern

o Func AddNewGrooveFromRef( Reference iProfileElt) As Groove

Creates and returns a new groove within the current body.

Parameters:

iProfileElt: The reference on the element defining the groove base

Returns:

The created groove

o Func AddNewGroove( Sketch iSketch) As Groove

Creates and returns a new groove within the current body.
The Revolution, as a supertype for grooves, provides starting and ending angles for the groove definition.

Parameters:

iSketch: The sketch defining the groove section. The sketch must contain a contour and an axis that will be used to rotate the contour in the space, thus defining the groove. The contour has to penetrate in 3D space the current shape.

Returns:

The created groove

o Func AddNewHoleFromPoint(	double	`iX`,
	double	`iY`,
	double	`iZ`,
	Reference	`iSupport`,
	double	`iDepth`) As Hole

Creates and returns a new hole within the current shape.
Actual hole shape is defined by editing hole properties after its creation.

Parameters:

iX: Origin point x absolute coordinate
iY: Origin point y absolute coordinate
iZ: Origin point z absolute coordinate
Sets the origin point which the hole is anchored to.
If mandatory, the entry point will be projected onto a tangent plane.
iSupport: The support defining the hole reference plane.
The following

Boundary object is supported: Face.

iDepth

The hole depth.

Returns:

The created hole

o Func AddNewHoleFromRefPoint(	Reference	`iOrigin`,
	Reference	`iSupport`,
	double	`iDepth`) As Hole

Creates and returns a new hole within the current shape.
Actual hole shape is defined by editing hole properties after its creation.

Parameters:

iOrigin: The origin point which the hole is anchored to.
iSupport: The support defining the hole reference plane.
The following

Boundary object is supported: Face.

iDepth

The hole depth.

Returns:

The created hole

o Func AddNewHoleFromSketch(	Sketch	`iSketch`,
	double	`iDepth`) As Hole

Creates and returns a new hole within the current shape.
Actual hole shape is defined by editing hole properties after its creation.

Parameters:

iSketch: The sketch defining the hole reference plane and anchor point.
This sketch must contain a single point that defines the hole axis: the hole axis in 3D passes through that point and is normal to the sketch plane.
iDepth: The hole depth.

Returns:

The created hole

o Func AddNewHoleWith2Constraints(	double	`iX`,
	double	`iY`,
	double	`iZ`,
	Reference	`iEdge1`,
	Reference	`iEdge2`,
	Reference	`iSupport`,
	double	`iDepth`) As Hole

Creates and returns a new hole within the current shape.
Actual hole shape is defined by editing hole properties after its creation.

Parameters:

iX: Origin point x absolute coordinate
iY: Origin point y absolute coordinate
iZ: Origin point z absolute coordinate
Sets the origin point which the hole is anchored to.
If mandatory, the entry point will be projected onto a tangent plane.
iEdge: The edge which the hole is constrained to.
The origin of the hole will have a length constraint with each edge.
The following

Boundary object is supported: TriDimFeatEdge.

iSupport

The support defining the hole reference plane.
The following

iDepth

BoundaryFace The hole depth.

Returns:

The created hole

o Func AddNewHoleWithConstraint(	double	`iX`,
	double	`iY`,
	double	`iZ`,
	Reference	`iEdge`,
	Reference	`iSupport`,
	double	`iDepth`) As Hole

Creates and returns a new hole within the current shape.
Actual hole shape is defined by editing hole properties after its creation.

Parameters:

iX: Origin point x absolute coordinate
iY: Origin point y absolute coordinate
iZ: Origin point z absolute coordinate
Sets the origin point which the hole is anchored to.
If mandatory, the entry point will be projected onto a tangent plane.
iEdge: The edge which the hole is constrained to.
If edge is circular, the origin of the hole will be concentric to the edge (iX, iY, iZ will be overridden). if not, the origin of the hole will have a length constraint with the edge.
The following

Boundary object is supported: TriDimFeatEdge.

iSupport

The support defining the hole reference plane.
The following

iDepth

BoundaryFace The hole depth.

Returns:

The created hole

o Func AddNewHole(	Reference	`iSupport`,
	double	`iDepth`) As Hole

Creates and returns a new hole within the current shape.
Actual hole shape is defined by editing hole properties after its creation.

Parameters:

iSupport: The support defining the hole reference plane.
Anchor point is located at the barycenter of the support. The hole axis in 3D passes through that point and is normal to the plane.
The following

Boundary object is supported: Face.

iDepth

The hole depth.

Returns:

The created hole

o Func AddNewIntersect( Body iBodyToIntersect) As Intersect

Creates and returns a new intersect operation within the current body.

Parameters:

iBodyToIntersect: The body to intersect with the current body

Returns:

The created intersect operation

o Func AddNewLoft(

) As AnyObject

Creates and returns a new Loft feature.

Returns:: The created Loft feature

o Func AddNewMirror( Reference iMirroringElement) As Mirror

Creates and returns a new mirror within the current body.
A mirror allows for transforming existing shapes by a symmetry with respect to an existing plane.

Parameters:

iMirroringElement: The plane used by the mirror as the symmetry plane.
The following

Boundary object is supported: PlanarFace.

Returns:

The created mirror

o Func AddNewPadFromRef(	Reference	`iProfileElt`,
	double	`iHeight`) As Pad

Creates and returns a new pad within the current body.

Parameters:

iProfileElt: The reference on the element defining the pad base
iHeight: The pad height

Returns:

The created pad

o Func AddNewPad(	Sketch	`iSketch`,
	double	`iHeight`) As Pad

Creates and returns a new pad within the current body.

Parameters:

iSketch: The sketch defining the pad base
iHeight: The pad height

Returns:

The created pad

o Func AddNewPocketFromRef(	Reference	`iProfileElt`,
	double	`iHeight`) As Pocket

Creates and returns a new pocket within the current shape.

Parameters:

iProfileElt: The reference on the element defining the pocket base
iDepth: The pocket depth

Returns:

The created pocket

o Func AddNewPocket(	Sketch	`iSketch`,
	double	`iHeight`) As Pocket

Creates and returns a new pocket within the current shape.

Parameters:

iSketch: The sketch defining the pocket base
iDepth: The pocket depth

Returns:

The created pocket

o Func AddNewRectPattern(	AnyObject	`iShapeToCopy`,
	long	`iNbOfCopiesInDir1`,
	long	`iNbOfCopiesInDir2`,
	double	`iStepInDir1`,
	double	`iStepInDir2`,
	long	`iShapeToCopyPositionAlongDir1`,
	long	`iShapeToCopyPositionAlongDir2`,
	Reference	`iDir1`,
	Reference	`iDir2`,
	boolean	`iIsReversedDir1`,
	boolean	`iIsReversedDir2`,
	double	`iRotationAngle`) As RectPattern

Creates and returns a new rectangular pattern within the current body.

Parameters:

iShapeToCopy: The shape to be copied by the rectangular pattern
iNbOfCopiesInDir1: The number of times iShapeToCopy will be copied along the pattern first direction
iNbOfCopiesInDir2: The number of times iShapeToCopy will be copied along the pattern second direction
iStepInDir1: The distance that will separate two consecutive copies in the pattern along its first direction
iStepInDir2: The distance that will separate two consecutive copies in the pattern along its second direction
iShapeToCopyPositionAlongDir1: Specifies the position of the original shape iShapeToCopy among its copies along iDir1
iShapeToCopyPositionAlongDir2: Specifies the position of the original shape iShapeToCopy among its copies along iDir2
iDir1: The line or linear edge that specifies the pattern first repartition direction
The following

Boundary objects are supported: PlanarFace, RectilinearTriDimFeatEdge, RectilinearBiDimFeatEdge.

iDir2

The line or linear edge that specifies the pattern second repartition direction
The following

iIsReversedDir1

BoundaryPlanarFaceRectilinearTriDimFeatEdgeRectilinearBiDimFeatEdge The boolean flag indicating whether the natural orientation of iDir1 should be used to orient the pattern operation. True indicates that iShapeToCopy is copied in the direction of the natural orientation of iDir1.

iIsReversedDir2

The boolean flag indicating whether the natural orientation of iDir2 should be used to orient the pattern operation. True indicates that iShapeToCopy is copied in the direction of the natural orientation of iDir2.

iRotationAngle

The angle applied to both directions iDir1 and iDir2 prior to applying the pattern. The original shape iShapeToCopy is used as the rotation center. Nevertheless, the copied shapes themselves are not rotated. This allows the definition of a rectangular pattern relatively to existing geometry, but not necessarily parallel to it.

Returns:

The created rectangular pattern

o Func AddNewRectPatternofList(	AnyObject	`iShapeToCopy`,
	long	`iNbOfCopiesInDir1`,
	long	`iNbOfCopiesInDir2`,
	double	`iStepInDir1`,
	double	`iStepInDir2`,
	long	`iShapeToCopyPositionAlongDir1`,
	long	`iShapeToCopyPositionAlongDir2`,
	Reference	`iDir1`,
	Reference	`iDir2`,
	boolean	`iIsReversedDir1`,
	boolean	`iIsReversedDir2`,
	double	`iRotationAngle`) As RectPattern

V5R8 Only: Creates and returns a new rectangular pattern within the current body using a list of shapes.

Parameters:

iShapeToCopy: The shape to be copied by the rectangular pattern Others shapes will be add by put_ItemToCopy with CATIAPattern interface
iNbOfCopiesInDir1: The number of times iShapeToCopy will be copied along the pattern first direction
iNbOfCopiesInDir2: The number of times iShapeToCopy will be copied along the pattern second direction
iStepInDir1: The distance that will separate two consecutive copies in the pattern along its first direction
iStepInDir2: The distance that will separate two consecutive copies in the pattern along its second direction
iShapeToCopyPositionAlongDir1: Specifies the position of the original shape iShapeToCopy among its copies along iDir1
iShapeToCopyPositionAlongDir2: Specifies the position of the original shape iShapeToCopy among its copies along iDir2
iDir1: The line or linear edge that specifies the pattern first repartition direction
iDir2: The line or linear edge that specifies the pattern second repartition direction
iIsReversedDir1: The boolean flag indicating whether the natural orientation of iDir1 should be used to orient the pattern operation. True indicates that iShapeToCopy is copied in the direction of the natural orientation of iDir1.
iIsReversedDir2: The boolean flag indicating whether the natural orientation of iDir2 should be used to orient the pattern operation. True indicates that iShapeToCopy is copied in the direction of the natural orientation of iDir2.
iRotationAngle: The angle applied to both directions iDir1 and iDir2 prior to applying the pattern. The original shape iShapeToCopy is used as the rotation center. Nevertheless, the copied shapes themselves are not rotated. This allows the definition of a rectangular pattern relatively to existing geometry, but not necessarily parallel to it.

Returns:

The created rectangular pattern

o Func AddNewRemoveFace(	Reference	`iKeepFaces`,
	Reference	`iRemoveFaces`) As RemoveFace

Creates and returns a new RemoveFace feature.

Parameters:

iKeepFaces: The reference of the face to Keep.
iRemoveFaces: The reference of the face to Remove.

Returns:

The created RemoveFace feature.

o Func AddNewRemove( Body iBodyToRemove) As Remove

Creates and returns a new remove operation within the current body.

Parameters:

iBodyToRemove: The body to remove from the current body

Returns:

The created remove operation

o Func AddNewRemovedBlend(

) As AnyObject

Creates and returns a new Removed Blend feature.

Returns:: The created Removed Blend feature

o Func AddNewRemovedLoft(

) As AnyObject

Creates and returns a new Removed Loft feature.

Returns:: The created Removed Loft feature

o Func AddNewReplaceFace(	Reference	`iSplitPlane`,
	Reference	`iRemoveFace`,
	CatSplitSide	`iSplittingSide`) As ReplaceFace

Creates and returns a new Align/ ReplaceFace feature.

Parameters:

iSplitPlane: The reference of the element defining the Splitting Plane.
iRemoveFace: The reference of the Face to Remove.
iSplittingSide: The specification for which side of the current body should be Align

Returns:

The created Align/ ReplaceFace feature.

o Func AddNewRibFromRef(	Reference	`iProfile`,
	Reference	`iCenterCurve`) As Rib

Creates and returns a new rib within the current body.

Parameters:

iProfile: The Profile defining the rib section
iCenterCurve: The curve that defines the rib center curve.
The following

Boundary object is supported: TriDimFeatEdge.

Returns:

The created rib

o Func AddNewRib(	Sketch	`iSketch`,
	Sketch	`iCenterCurve`) As Rib

Creates and returns a new rib within the current body.

Parameters:

iSketch: The sketch defining the rib section
iCenterCurve: The sketched curve that defines the rib center curve. It must cross the section definition sketch iSketch within the inner part of its contour.

Returns:

The created rib

o Func AddNewScaling(	Reference	`iScalingReference`,
	double	`iFactor`) As Scaling

Creates and returns a new scaling within the current body.

Parameters:

iScalingReference: The point, plane or face of the current body that will remain fixed during the scaling process: even if the face itself shrinks or expands during the scaling, its supporting plane will remain unchanged after the scaling.
The following

Boundary objects are supported: PlanarFace and Vertex.

iFactor

The scaling factor

Returns:

The created scaling

o Func AddNewSewSurface(	Reference	`iSewingElement`,
	CatSplitSide	`iSewingSide`) As SewSurface

Creates and returns a new sewing operation within the current body.

Parameters:

iSewingElement: The face or skin or surface that will be sewn on the current body
iSewingSide: The specification for which side of the current body should be kept at the end of the sewing operation

Returns:

The created sewing operation

o Func AddNewShaftFromRef( Reference iProfileElt) As Shaft

Creates and returns a new shaft within the current body.

Parameters:

iProfileElt: The reference on the element defining the shaft base

Returns:

The created shaft

o Func AddNewShaft( Sketch iSketch) As Shaft

Creates and returns a new shaft within the current body.
The Revolution, as a supertype for shafts, provides starting and ending angles for the shaft definition.

Parameters:

iSketch

The sketch defining the shaft section.

If the shaft applies to the current body, then the sketch must contain a contour and an axis that will be used to rotate the contour in the space, thus defining the shaft.
If the shaft is the first shape defined, there is not current body to apply to. In such a case, the sketch must contain a curve whose end points are linked by an axis. By rotating the curve in the space around the axis, the shaft operation will define a revolution shape. This also works if the sketch contains a closed contour and an axis outside of this contour: in that case a revolution shape will be created, for example a torus.

Returns:

The created shaft

o Func AddNewShell(	Reference	`iFaceToRemove`,
	double	`iInternalThickness`,
	double	`iExternalThickness`) As Shell

Creates and returns a new shell within the current body.

Parameters:

iFaceToRemove: The first face to be removed in the shell process.
The following

Boundary object is supported: Face.

iInternalThickness

The thickness of material to be added on the internal side of all the faces during the shell process, except for those to be removed

iExternaThickness

The thickness of material to be added on the external side of all the faces during the shell process, except for those to be removed

Returns:

The created shell

o Func AddNewSlotFromRef(	Reference	`iProfile`,
	Reference	`iCenterCurve`) As Slot

Creates and returns a new slot within the current shape.

Parameters:

iProfile: The sketch defining the slot section
iCenterCurve: The curve that defines the slot center curve.
The following

Boundary object is supported: TriDimFeatEdge.

Returns:

The created slot

o Func AddNewSlot(	Sketch	`iSketch`,
	Sketch	`iCenterCurve`) As Slot

Creates and returns a new slot within the current shape.

Parameters:

iSketch: The sketch defining the slot section
iCenterCurve: The sketched curve that defines the slot center curve. It must cross the section definition sketch iSketch within the inner part of its contour.

Returns:

The created slot

o Func AddNewSolidCombine(	Reference	`iProfileEltFirst`,
	Reference	`iProfileEltSecond`) As SolidCombine

Creates and returns a new SolidCombine feature.

Parameters:

iProfileEltFirst: The reference of the element defining the profile for first component.
iProfileEltSecond: The reference of the element defining the profile for second component.

Returns:

The created SolidCombine feature.

o Func AddNewSolidEdgeFilletWithConstantRadius(	Reference	`iEdgeToFillet`,
	CatFilletEdgePropagation	`iPropagMode`,
	double	`iRadius`) As ConstRadEdgeFillet

Creates and returns a new solid edge fillet with a constant radius. within the current body.

Parameters:

iEdgeToFillet: The edge that will be filleted first
The following

Boundary object is supported: TriDimFeatEdge.

iPropagMode

Controls whether other edges found adjacent to the first one should also be filleted in the same operation

iRadius

The fillet radius

Returns:

The created edge fillet

o Func AddNewSolidEdgeFilletWithVaryingRadius(	Reference	`iEdgeToFillet`,
	CatFilletEdgePropagation	`iPropagMode`,
	CatFilletVariation	`iVariationMode`,
	double	`iDefaultRadius`) As VarRadEdgeFillet

Creates and returns a new solid edge fillet with a varying radius. within the current body.

Parameters:

iEdgeToFillet: The edge that will be filleted first
The following

Boundary object is supported: TriDimFeatEdge.

iPropagMode

Controls whether other edges found adjacent to the first one should also be filleted in the same operation

iVariationMode

Controls the law of evolution for the fillet radius between specified control points, such as edges extremities

iDefaultRadius

The fillet default radius, that will apply when no other radius can be inferred from the iVariationMode parameter

Returns:

The created edge fillet

o Func AddNewSolidFaceFillet(	Reference	`iF1`,
	Reference	`iF2`,
	double	`iRadius`) As FaceFillet

Creates and returns a new solid face-to-face fillet.
Use this method to created face-to-face fillets with varying fillet radii, by editing fillet attributes driving its radius after its creation.

Parameters:

iF1: The first face that will support the fillet
The following

Boundary object is supported: Face.

iF2

The second face that will support the fillet
The following

iRadius

BoundaryFace The fillet radius

Returns:

The created face-to-face fillet

o Func AddNewSolidTritangentFillet(	Reference	`iF1`,
	Reference	`iF2`,
	Reference	`iRemovedFace`) As TritangentFillet

Creates and returns a new solid tritangent fillet within the current body.
This kind of fillet begins with tangency on a first face iF1, gets tangent to a second one iRemovedFace and ends with tangency to a third one iF2. During the process the second face iRemovedFace is removed.

Parameters:

iF1: The starting face for the fillet
The following

Boundary object is supported: Face.

iF2

The ending face for the fillet
The following

iRemovedFace

BoundaryFace The face used as an intermediate tangent support for the fillet during its course from iF1 to iF2. This face will be removed at the end of the filleting operation.
The following

Returns:

BoundaryFace The created tritangent fillet

o Func AddNewSplit(	Reference	`iSplittingElement`,
	CatSplitSide	`iSplitSide`) As Split

Creates and returns a new split operation within the current body.

Parameters:

iSplittingElement: The face or plane that will split the current body
The following

Boundary object is supported: Face.

iSplitSide

The specification for which side of the current body should be kept at the end of the split operation

Returns:

The created split operation

o Func AddNewStiffenerFromRef( Reference iProfileElt) As Stiffener

Creates and returns a new stiffener within the current body.

Parameters:

iProfileElt: The reference on the element defining the stiffener profile

Returns:

The created stiffener

o Func AddNewStiffener( Sketch iSketch) As Stiffener

Creates and returns a new stiffener within the current body.
A stiffener is made up of a sketch used as the stiffener profile, that is extruded (offset) and that fills the nearest shape.

Parameters:

iSketch: The sketch defining the stiffener border. It must contain a line or a curve that does not cross in 3D space the face(s) to stiffen.

Returns:

The created stiffener

o Func AddNewSurfaceEdgeFilletWithConstantRadius(	Reference	`iEdgeToFillet`,
	CatFilletEdgePropagation	`iPropagMode`,
	double	`iRadius`) As ConstRadEdgeFillet

Creates and returns a new surface edge fillet with a constant radius. within the current body.

Parameters:

iEdgeToFillet: The edge that will be filleted first
The following

Boundary object is supported: TriDimFeatEdge.

iPropagMode

Controls whether other edges found adjacent to the first one should also be filleted in the same operation

iRadius

The fillet radius

Returns:

The created edge fillet

o Func AddNewSurfaceEdgeFilletWithVaryingRadius(	Reference	`iEdgeToFillet`,
	CatFilletEdgePropagation	`iPropagMode`,
	CatFilletVariation	`iVariationMode`,
	double	`iDefaultRadius`) As VarRadEdgeFillet

Creates and returns a new surface edge fillet with a varying radius. within the current body.

Parameters:

iEdgeToFillet: The edge that will be filleted first
The following

Boundary object is supported: TriDimFeatEdge.

iPropagMode

Controls whether other edges found adjacent to the first one should also be filleted in the same operation

iVariationMode

Controls the law of evolution for the fillet radius between specified control points, such as edges extremities

iDefaultRadius

The fillet default radius, that will apply when no other radius can be inferred from the iVariationMode parameter

Returns:

The created edge fillet

o Func AddNewSurfaceFaceFillet(	Reference	`iF1`,
	Reference	`iF2`,
	double	`iRadius`) As FaceFillet

Creates and returns a new surface face-to-face fillet.
Use this method to created face-to-face fillets with varying fillet radii, by editing fillet attributes driving its radius after its creation.

Parameters:

iF1: The first face that will support the fillet
The following

Boundary object is supported: Face.

iF2

The second face that will support the fillet
The following

iRadius

BoundaryFace The fillet radius

Returns:

The created face-to-face fillet

o Func AddNewSurfaceTritangentFillet(	Reference	`iF1`,
	Reference	`iF2`,
	Reference	`iRemovedFace`) As TritangentFillet

Creates and returns a new surface tritangent fillet within the current body.
This kind of fillet begins with tangency on a first face iF1, gets tangent to a second one iRemovedFace and ends with tangency to a third one iF2. During the process the second face iRemovedFace is removed.

Parameters:

iF1: The starting face for the fillet
The following

Boundary object is supported: Face.

iF2

The ending face for the fillet
The following

iRemovedFace

BoundaryFace The face used as an intermediate tangent support for the fillet during its course from iF1 to iF2. This face will be removed at the end of the filleting operation.
The following

Returns:

BoundaryFace The created tritangent fillet

o Func AddNewSurfacicAutoFillet( double iFilletRadius) As AutoFillet

Creates and returns a new Surfacic autofillet.
Use this method to create autofillet by providing fillet radius value.

Parameters:

iFilletRadius: The fillet radius

Returns:

The created autofillet

o Func AddNewSurfacicCircPattern(	AnyObject	`iShapeToCopy`,
	long	`iNbOfCopiesInRadialDir`,
	long	`iNbOfCopiesInAngularDir`,
	double	`iStepInRadialDir`,
	double	`iStepInAngularDir`,
	long	`iShapeToCopyPositionAlongRadialDir`,
	long	`iShapeToCopyPositionAlongAngularDir`,
	Reference	`iRotationCenter`,
	Reference	`iRotationAxis`,
	boolean	`iIsReversedRotationAxis`,
	double	`iRotationAngle`,
	boolean	`iIsRadiusAligned`,
	boolean	`iCompleteCrown`) As CircPattern

Creates and returns a new gsd circular pattern within the current body.

Parameters:

iShapeToCopy: The shape to be copied by the circular pattern
iNbOfInstancesInRadialDir: The number of times iShapeToCopy will be copied along pattern radial direction
iNbOfInstancesInAngularDir: The number of times iShapeToCopy will be copied along pattern angular direction
iStepInRadialDir: The distance that will separate two consecutive copies in the pattern along its radial direction
iStepInAngularDir: The angle that will separate two consecutive copies in the pattern along its angular direction
iShapeToCopyPositionAlongRadialDir: Specifies the position of the original shape iShapeToCopy among its copies along the radial direction
iShapeToCopyPositionAlongAngularDir: Specifies the position of the original shape iShapeToCopy among its copies along the angular direction
iRotationCenter: The point or vertex that specifies the pattern center of rotation
iRotationAxis: The line or linear edge that specifies the axis around which instances will be rotated relative to each other
The following

Boundary objects are supported: PlanarFace , CylindricalFace , RectilinearTriDimFeatEdge and RectilinearBiDimFeatEdge.

iIsReversedRotationAxis

iRotationAngle

iIsRadiusAligned

iCompleteCrown

The boolean flag specifies the mode of angular distribution. True indicates that the angular step will be equal to 360 degrees iNba.

Returns:

The created circular pattern

o Func AddNewSurfacicRectPattern(	AnyObject	`iShapeToCopy`,
	long	`iNbOfCopiesInDir1`,
	long	`iNbOfCopiesInDir2`,
	double	`iStepInDir1`,
	double	`iStepInDir2`,
	long	`iShapeToCopyPositionAlongDir1`,
	long	`iShapeToCopyPositionAlongDir2`,
	Reference	`iDir1`,
	Reference	`iDir2`,
	boolean	`iIsReversedDir1`,
	boolean	`iIsReversedDir2`,
	double	`iRotationAngle`) As RectPattern

Creates and returns a new GSD rectangular pattern within the current body.

Parameters:

iShapeToCopy: The shape to be copied by the rectangular pattern
iNbOfCopiesInDir1: The number of times iShapeToCopy will be copied along the pattern first direction
iNbOfCopiesInDir2: The number of times iShapeToCopy will be copied along the pattern second direction
iStepInDir1: The distance that will separate two consecutive copies in the pattern along its first direction
iStepInDir2: The distance that will separate two consecutive copies in the pattern along its second direction
iShapeToCopyPositionAlongDir1: Specifies the position of the original shape iShapeToCopy among its copies along iDir1
iShapeToCopyPositionAlongDir2: Specifies the position of the original shape iShapeToCopy among its copies along iDir2
iDir1: The line or linear edge that specifies the pattern first repartition direction
The following

Boundary objects are supported: PlanarFace, RectilinearTriDimFeatEdge, RectilinearBiDimFeatEdge.

iDir2

The line or linear edge that specifies the pattern second repartition direction
The following

iIsReversedDir1

iIsReversedDir2

iRotationAngle

Returns:

The created rectangular pattern

o Func AddNewSurfacicUserPattern(	AnyObject	`iShapeToCopy`,
	long	`iNbOfCopies`) As UserPattern

Creates and returns a new GSD user pattern within the current body.

Parameters:

iShapeToCopy: The shape to be copied by the user pattern
iNbOfCopies: The number of times iShapeToCopy will be copied

Returns:

The created user pattern

o Func AddNewThickSurface(	Reference	`iOffsetElement`,
	long	`iIsensOffset`,
	double	`iTopOffset`,
	double	`iBotOffset`) As ThickSurface

Creates and returns a new ThickSurface feature.

Parameters:

iOffsetElement: The skin that will be thicken and added with the current body
iIsensOffset: The direction of the offset in regard to the direction of the normal
iTopOffset: The Offset between the iOffsetElement and the upper skin of the resulting feature
iBotOffset: The Offset between the iOffsetElement and the lower skin of the resulting feature

Returns:

The created ThickSurface feature

o Func AddNewThickness(	Reference	`iFaceToThicken`,
	double	`iOffset`) As Thickness

Creates and returns a new thickness within the current body.

Parameters:

iFaceToThicken: The first face to thicken in the thickening process.
New faces to thicken can be added to the thickness afterwards by using methods offered by the created thickness
The following

Boundary object is supported: Face.

iOffset

The thickness of material to be added on the external side of the face iFaceToThicken during the thickening process

Returns:

The created thickness

o Func AddNewThreadWithOutRef(

) As Thread

Creates and returns a new thread\tap within the current body.

Returns:: The created Thread

o Func AddNewThreadWithRef(	Reference	`iLateralFace`,
	Reference	`iLimitFace`) As Thread

Creates and returns a new thread\tap within the current body.

Parameters:

iLateralFace: The Face defining the support of thread\tap
The following

Boundary object is supported: Face.

iLimitFacee

The Face defining the origin of the thread.
The following

Returns:

BoundaryPlanarFace The created Thread

o Func AddNewTrim( Body iBodyToTrim) As Trim

Creates and returns a new Trim operation within the current body.

Parameters:

iBodyToTrim: The body to Trim with current body.

Returns:

The created Trim operation

o Func AddNewTritangentFillet(	Reference	`iF1`,
	Reference	`iF2`,
	Reference	`iRemovedFace`) As TritangentFillet

Deprecated:: V5R14 #AddNewTritangentFillet use AddNewSolidTritangentFillet or AddNewSurfaceTritangentFillet depending on the type of fillet you want to create

o Func AddNewUserPattern(	AnyObject	`iShapeToCopy`,
	long	`iNbOfCopies`) As UserPattern

Creates and returns a new user pattern within the current body.

Parameters:

iShapeToCopy: The shape to be copied by the user pattern
iNbOfCopies: The number of times iShapeToCopy will be copied

Returns:

The created user pattern

o Func AddNewUserPatternofList(	AnyObject	`iShapeToCopy`,
	long	`iNbOfCopies`) As UserPattern

V5R8 Only: Creates and returns a new user pattern within the current body using a list of shapes.

Parameters:

iShapeToCopy: The shape to be copied by the user pattern Others shapes will be add by put_ItemToCopy with CATIAPattern interface
iNbOfCopies: The number of times iShapeToCopy will be copied

Returns:

The created user pattern

o Func AddNewVolumeAdd(	Reference	`iBody1`,
	Reference	`iBody2`,
	double	`iType`) As Add

Creates and returns a Volumic Add feature.

Parameters:

iBody1: The volume or body to be modified.
iBody2: The volume or body to be operated.
iType: iType = 0 if Part Design, = 4 if GSD.

Returns:

The created Volumic Add feature.

o Func AddNewVolumeCloseSurface( Reference iCloseElement) As CloseSurface

Creates and returns a new VolumeCloseSurface feature.

Parameters:

iCloseElement: The skin that will be closed and add with the current body

Returns:

The created CloseSurface feature

o Func AddNewVolumeIntersect(	Reference	`iBody1`,
	Reference	`iBody2`,
	double	`iType`) As Intersect

Creates and returns a Volumic Intersect feature.

Parameters:

iBody1: The volume or body to be modified.
iBody2: The volume or body to be operated.
iType: iType = 0 if Part Design, = 4 if GSD.

Returns:

The created Volumic Intersect feature.

o Func AddNewVolumeRemove(	Reference	`iBody1`,
	Reference	`iBody2`,
	double	`iType`) As Remove

Creates and returns a Volumic Remove feature.

Parameters:

iBody1: The volume or body to be modified.
iBody2: The volume or body to be operated.
iType: iType = 0 if Part Design, = 4 if GSD.

Returns:

The created Volumic Remove feature.

o Func AddNewVolumeSewSurface(	long	`iType`,
	Reference	`iSupportVolume`,
	Reference	`iSewingElement`,
	CatSplitSide	`iSewingSide`) As SewSurface

Creates and returns a new volume sewing operation within the current OGS/GS.

Parameters:

iType: Parameter to determine the sewing type. For Volume sewing Type = 4
iSupportVolume: The volume support on which sew operation will be performed
iSewingElement: The face or skin or surface that will be sewn on the current volume support
iSewingSide: The specification for which side of the current volume should be kept at the end of the sewing operation

Returns:

The created sewing operation

o Func AddNewVolumeShell(	Reference	`iFaceToRemove`,
	double	`iInternalThickness`,
	double	`iExternalThickness`,
	Reference	`iVolumeSupport`) As Shell

Creates and returns a Volumic Shell feature.

Parameters:

iFacesToRemove: The Faces of the Volume
iFacesToThicken: The Faces of the Volume
iInternalThickness: The thickness of material to be added on the internal side of all the faces during the shell process, except for those to be removed
iExternaThickness: The thickness of material to be added on the external side of all the faces during the shell process, except for those to be removed
iVolumeSupport: The Volume related the faces to remove and faces to thicken

Returns:

The created Volumic Shell.

o Func AddNewVolumeThickSurface(	Reference	`iOffsetElement`,
	long	`iIsensOffset`,
	double	`iTopOffset`,
	double	`iBotOffset`) As ThickSurface

Creates and returns a new VolumeThickSurface feature.

Parameters:

iOffsetElement: The skin that will be thicken and added with the current OGS/GS
iIsensOffset: The direction of the offset in regard to the direction of the normal
iTopOffset: The Offset between the iOffsetElement and the upper skin of the resulting feature
iBotOffset: The Offset between the iOffsetElement and the lower skin of the resulting feature

Returns:

The created ThickSurface feature

o Func AddNewVolumeThickness(	Reference	`iFaceToThicken`,
	double	`iOffset`,
	long	`iType`,
	Reference	`iVolumeSupport`) As Thickness

Creates and returns a volume new thickness within the current GS or OGS.

Parameters:

iFaceToThicken: The first face to thicken in the thickening process.
New faces to thicken can be added to the thickness afterwards by using methods offered by the created thickness
The following

Boundary object is supported: Face.

iOffset

The thickness of material to be added on the external side of the face iFaceToThicken during the thickening process

iType

The mode of thickness creation (4=Volume)

iVolumeSupport

The support volume for volumic draft

Returns:

The created thickness

o Func AddNewVolumeTrim(	Reference	`iSupportVolume`,
	Reference	`iCuttingVolume`) As Trim

Creates and returns a new Volume Trim operation within the GS/OGS.

Parameters:

iSupportVolume: The Support Volume
iCutttingVolume: The trimming Volume

Returns:

The created Trim operation

o Func AddNewVolumicDraft(	Reference	`iFaceToDraft`,
	Reference	`iNeutral`,
	CatDraftNeutralPropagationMode	`iNeutralMode`,
	Reference	`iParting`,
	double	`iDirX`,
	double	`iDirY`,
	double	`iDirZ`,
	CatDraftMode	`iMode`,
	double	`iAngle`,
	CatDraftMultiselectionMode	`iMultiselectionMode`,
	long	`iType`,
	Reference	`iVolumeSupport`) As Draft

Creates and returns a new volume draft within the current body.
The draft needs a reference face on the body. This face will remain unchanged in the draft operation, while faces adjacent to it and specified for drafting will be rotated by the draft angle.

Parameters:

iFaceToDraft: The first face to draft in the body. This face should be adjacent to the iFaceToDraft face. If several faces are to be drafted, only the first one is specified here, the others being inferred by propagating the draft operation onto faces adjacent to this first face. This is controlled by the iNeutralMode argument.
The following

Boundary object is supported: Face.

iNeutral

iNeutralMode

BoundaryPlanarFace Controls if and how the drafting operation should be propagated beyond the first face to draft iFaceToDraft to other adjacent faces.

iParting

iDirX,iDirY,iDirZ

BoundaryPlanarFace The X, Y, and Z components of the absolute vector representing the drafting direction (i.e. the mold extraction direction).

iMode

The draft connecting mode to its reference face iFaceToDraft

iAngle

The draft angle

iMultiselectionMode.

The elements to be drafted can be selected explicitly or can implicitly selected as neighbors of the neutral face

iType

The mode of draft creation (4=Volume)

iVolumeSupport

The support volume for volumic draft

Returns:

The created draft

ShapeFactory (Object)

Method Index

Methods