pycatia.part_interfaces.shape_factory

Module initially auto generated using V5Automation files from CATIA V5 R28 on 2020-06-11 12:40:47.360445

Warning

The notes denoted “CAA V5 Visual Basic Help” are to be used as reference only. They are there as a guide as to how the visual basic / catscript functions work and thus help debugging in pycatia.

class pycatia.part_interfaces.shape_factory.ShapeFactory(com_object)

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384)

System.IUnknown
System.IDispatch
System.CATBaseUnknown
System.CATBaseDispatch
System.AnyObject
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 parameters. Other
shapes parameters may be set further on by using methods offered by the shape
itself.
add_new_add(i_body_to_add: Body) → Add

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_body_to_add (Body) –

Return type:

Add

add_new_affinity2(x_ratio: float, y_ratio: float, z_ratio: float) → AnyObject

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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.
Parameters:

  • x_ratio (float) –

  • y_ratio (float) –

  • z_ratio (float) –

Return type:

AnyObject

add_new_assemble(i_body_to_assemble: Body) → Assemble

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_body_to_assemble (Body) –

Return type:

Assemble

add_new_auto_draft(i_draft_angle: float) → AutoDraft

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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.
Parameters:

i_draft_angle (float) –

Return type:

AutoDraft

add_new_auto_fillet(i_fillet_radius: float, i_round_radius: float) → AutoFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_fillet_radius (float) –

  • i_round_radius (float) –

Return type:

AutoFillet

add_new_axis_to_axis2(i_reference: Reference, i_target: Reference) → AnyObject

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func AddNewAxisToAxis2(Reference iReference,
Reference iTarget) As AnyObject

Creates and returns an AxisToAxis transformation feature.

Parameters:

iReference
The reference axis.
iTarget
The target axis.

Returns:
The created AxisToAxis transformation feature.
Parameters:
Return type:

AnyObject

add_new_blend() → AnyObject

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func AddNewBlend() As AnyObject

Creates and returns a new Blend feature.

Returns:
The created Blend feature
Return type:

AnyObject

add_new_chamfer(i_object_to_chamfer: Reference, i_propagation: int, i_mode: int, i_orientation: int, i_length1: float, i_length2_or_angle: float) → Chamfer

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_object_to_chamfer (Reference) –

  • i_propagation (int) – enum cat_chamfer_propagation

  • i_mode (int) –

  • i_orientation (int) –

  • i_length1 (float) –

  • i_length2_or_angle (float) –

Return type:

Chamfer

add_new_circ_pattern(i_shape_to_copy: AnyObject, i_nb_of_copies_in_radial_dir: int, i_nb_of_copies_in_angular_dir: int, i_step_in_radial_dir: float, i_step_in_angular_dir: float, i_shape_to_copy_position_along_radial_dir: int, i_shape_to_copy_position_along_angular_dir: int, i_rotation_center: Reference, i_rotation_axis: Reference, i_is_reversed_rotation_axis: bool, i_rotation_angle: float, i_is_radius_aligned: bool) → CircPattern

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_shape_to_copy (AnyObject) –

  • i_nb_of_copies_in_radial_dir (int) –

  • i_nb_of_copies_in_angular_dir (int) –

  • i_step_in_radial_dir (float) –

  • i_step_in_angular_dir (float) –

  • i_shape_to_copy_position_along_radial_dir (int) –

  • i_shape_to_copy_position_along_angular_dir (int) –

  • i_rotation_center (Reference) –

  • i_rotation_axis (Reference) –

  • i_is_reversed_rotation_axis (bool) –

  • i_rotation_angle (float) –

  • i_is_radius_aligned (bool) –

Return type:

CircPattern

add_new_circ_patternof_list(i_shape_to_copy: AnyObject, i_nb_of_copies_in_radial_dir: int, i_nb_of_copies_in_angular_dir: int, i_step_in_radial_dir: float, i_step_in_angular_dir: float, i_shape_to_copy_position_along_radial_dir: int, i_shape_to_copy_position_along_angular_dir: int, i_rotation_center: Reference, i_rotation_axis: Reference, i_is_reversed_rotation_axis: bool, i_rotation_angle: float, i_is_radius_aligned: bool) → CircPattern

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_shape_to_copy (AnyObject) –

  • i_nb_of_copies_in_radial_dir (int) –

  • i_nb_of_copies_in_angular_dir (int) –

  • i_step_in_radial_dir (float) –

  • i_step_in_angular_dir (float) –

  • i_shape_to_copy_position_along_radial_dir (int) –

  • i_shape_to_copy_position_along_angular_dir (int) –

  • i_rotation_center (Reference) –

  • i_rotation_axis (Reference) –

  • i_is_reversed_rotation_axis (bool) –

  • i_rotation_angle (float) –

  • i_is_radius_aligned (bool) –

Return type:

CircPattern

add_new_close_surface(i_close_element: Reference) → CloseSurface

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_close_element (Reference) –

Return type:

CloseSurface

add_new_defeaturing() → Defeaturing

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func AddNewDefeaturing() As Defeaturing

Creates and returns a new defeaturing operation within the current
container.

Returns:
The created defeaturing operation
Return type:

Defeaturing

add_new_draft(i_face_to_draft: Reference, i_neutral: Reference, i_neutral_mode: int, i_parting: Reference, i_dir_x: float, i_dir_y: float, i_dir_z: float, i_mode: int, i_angle: float, i_multiselection_mode: int) → Draft

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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 Boundary object is supported:
PlanarFace.
iNeutralMode
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 Boundary object is supported:
PlanarFace.
iDirX,iDirY,iDirZ
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
Parameters:

  • i_face_to_draft (Reference) –

  • i_neutral (Reference) –

  • i_neutral_mode (int) – enum cat_draft_neutral_propagation_mode

  • i_parting (Reference) –

  • i_dir_x (float) –

  • i_dir_y (float) –

  • i_dir_z (float) –

  • i_mode (int) – enum cat_draft_mode

  • i_angle (float) –

  • i_multiselection_mode (int) – enum cat_draft_multiselection_mode

Return type:

Draft

add_new_edge_fillet_with_constant_radius(i_edge_to_fillet: Reference, i_propag_mode: int, i_radius: float) → ConstRadEdgeFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_edge_to_fillet (Reference) –

  • i_propag_mode (int) – enum cat_fillet_edge_propagation

  • i_radius (float) –

Return type:

ConstRadEdgeFillet

add_new_edge_fillet_with_varying_radius(i_edge_to_fillet: Reference, i_propag_mode: int, i_variation_mode: int, i_default_radius: float) → VarRadEdgeFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_edge_to_fillet (Reference) –

  • i_propag_mode (int) – enum cat_fillet_edge_propagation

  • i_variation_mode (int) – enum cat_fillet_variation

  • i_default_radius (float) –

Return type:

VarRadEdgeFillet

add_new_face_fillet(i_f1: Reference, i_f2: Reference, i_radius: float) → FaceFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:
Return type:

FaceFillet

add_new_groove(i_sketch: Sketch) → Groove

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_sketch (Sketch) –

Return type:

Groove

add_new_groove_from_ref(i_profile_elt: Reference) → Groove

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_profile_elt (Reference) –

Return type:

Groove

add_new_gsd_circ_pattern(i_shape_to_copy: AnyObject, i_nb_of_copies_in_radial_dir: int, i_nb_of_copies_in_angular_dir: int, i_step_in_radial_dir: float, i_step_in_angular_dir: float, i_shape_to_copy_position_along_radial_dir: int, i_shape_to_copy_position_along_angular_dir: int, i_rotation_center: Reference, i_rotation_axis: Reference, i_is_reversed_rotation_axis: bool, i_rotation_angle: float, i_is_radius_aligned: bool, i_complete_crown: bool, i_type: float) → CircPattern

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_shape_to_copy (AnyObject) –

  • i_nb_of_copies_in_radial_dir (int) –

  • i_nb_of_copies_in_angular_dir (int) –

  • i_step_in_radial_dir (float) –

  • i_step_in_angular_dir (float) –

  • i_shape_to_copy_position_along_radial_dir (int) –

  • i_shape_to_copy_position_along_angular_dir (int) –

  • i_rotation_center (Reference) –

  • i_rotation_axis (Reference) –

  • i_is_reversed_rotation_axis (bool) –

  • i_rotation_angle (float) –

  • i_is_radius_aligned (bool) –

  • i_complete_crown (bool) –

  • i_type (float) –

Return type:

CircPattern

add_new_gsd_rect_pattern(i_shape_to_copy: AnyObject, i_nb_of_copies_in_dir1: int, i_nb_of_copies_in_dir2: int, i_step_in_dir1: float, i_step_in_dir2: float, i_shape_to_copy_position_along_dir1: int, i_shape_to_copy_position_along_dir2: int, i_dir1: Reference, i_dir2: Reference, i_is_reversed_dir1: bool, i_is_reversed_dir2: bool, i_rotation_angle: float, i_type: float) → RectPattern

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_shape_to_copy (AnyObject) –

  • i_nb_of_copies_in_dir1 (int) –

  • i_nb_of_copies_in_dir2 (int) –

  • i_step_in_dir1 (float) –

  • i_step_in_dir2 (float) –

  • i_shape_to_copy_position_along_dir1 (int) –

  • i_shape_to_copy_position_along_dir2 (int) –

  • i_dir1 (Reference) –

  • i_dir2 (Reference) –

  • i_is_reversed_dir1 (bool) –

  • i_is_reversed_dir2 (bool) –

  • i_rotation_angle (float) –

  • i_type (float) –

Return type:

RectPattern

add_new_hole(i_support: Reference, i_depth: float) → Hole

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_support (Reference) –

  • i_depth (float) –

Return type:

Hole

add_new_hole_from_point(i_x: float, i_y: float, i_z: float, i_support: Reference, i_depth: float) → Hole

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_x (float) –

  • i_y (float) –

  • i_z (float) –

  • i_support (Reference) –

  • i_depth (float) –

Return type:

Hole

add_new_hole_from_ref_point(i_origin: Reference, i_support: Reference, i_depth: float) → Hole

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:
Return type:

Hole

add_new_hole_from_sketch(i_sketch: Sketch, i_depth: float) → Hole

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_sketch (Sketch) –

  • i_depth (float) –

Return type:

Hole

add_new_hole_with2_constraints(i_x: float, i_y: float, i_z: float, i_edge1: Reference, i_edge2: Reference, i_support: Reference, i_depth: float) → Hole

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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 Boundary object is supported: Face.
iDepth
The hole depth.
Returns:
The created hole
Parameters:

  • i_x (float) –

  • i_y (float) –

  • i_z (float) –

  • i_edge1 (Reference) –

  • i_edge2 (Reference) –

  • i_support (Reference) –

  • i_depth (float) –

Return type:

Hole

add_new_hole_with_constraint(i_x: float, i_y: float, i_z: float, i_edge: Reference, i_support: Reference, i_depth: float) → Hole

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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 Boundary object is supported: Face.
iDepth
The hole depth.
Returns:
The created hole
Parameters:

  • i_x (float) –

  • i_y (float) –

  • i_z (float) –

  • i_edge (Reference) –

  • i_support (Reference) –

  • i_depth (float) –

Return type:

Hole

add_new_intersect(i_body_to_intersect: Body) → Intersect

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_body_to_intersect (Body) –

Return type:

Intersect

add_new_loft() → AnyObject

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func AddNewLoft() As AnyObject

Creates and returns a new Loft feature.

Returns:
The created Loft feature
Return type:

AnyObject

add_new_mirror(i_mirroring_element: Reference) → Mirror

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_mirroring_element (Reference) –

Return type:

Mirror

add_new_pad(i_sketch: Sketch, i_height: float) → Pad

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_sketch (Sketch) –

  • i_height (float) –

Return type:

Pad

add_new_pad_from_ref(i_profile_elt: Reference, i_height: float) → Pad

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_profile_elt (Reference) –

  • i_height (float) –

Return type:

Pad

add_new_pocket(i_sketch: Sketch, i_height: float) → Pocket

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_sketch (Sketch) –

  • i_height (float) –

Return type:

Pocket

add_new_pocket_from_ref(i_profile_elt: Reference, i_height: float) → Pocket

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_profile_elt (Reference) –

  • i_height (float) –

Return type:

Pocket

add_new_rect_pattern(i_shape_to_copy: AnyObject, i_nb_of_copies_in_dir1: int, i_nb_of_copies_in_dir2: int, i_step_in_dir1: float, i_step_in_dir2: float, i_shape_to_copy_position_along_dir1: int, i_shape_to_copy_position_along_dir2: int, i_dir1: Reference, i_dir2: Reference, i_is_reversed_dir1: bool, i_is_reversed_dir2: bool, i_rotation_angle: float) → RectPattern

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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 Boundary objects are supported: PlanarFace,
RectilinearTriDimFeatEdge, RectilinearBiDimFeatEdge.
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
Parameters:

  • i_shape_to_copy (AnyObject) –

  • i_nb_of_copies_in_dir1 (int) –

  • i_nb_of_copies_in_dir2 (int) –

  • i_step_in_dir1 (float) –

  • i_step_in_dir2 (float) –

  • i_shape_to_copy_position_along_dir1 (int) –

  • i_shape_to_copy_position_along_dir2 (int) –

  • i_dir1 (Reference) –

  • i_dir2 (Reference) –

  • i_is_reversed_dir1 (bool) –

  • i_is_reversed_dir2 (bool) –

  • i_rotation_angle (float) –

Return type:

RectPattern

add_new_rect_patternof_list(i_shape_to_copy: AnyObject, i_nb_of_copies_in_dir1: int, i_nb_of_copies_in_dir2: int, i_step_in_dir1: float, i_step_in_dir2: float, i_shape_to_copy_position_along_dir1: int, i_shape_to_copy_position_along_dir2: int, i_dir1: Reference, i_dir2: Reference, i_is_reversed_dir1: bool, i_is_reversed_dir2: bool, i_rotation_angle: float) → RectPattern

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_shape_to_copy (AnyObject) –

  • i_nb_of_copies_in_dir1 (int) –

  • i_nb_of_copies_in_dir2 (int) –

  • i_step_in_dir1 (float) –

  • i_step_in_dir2 (float) –

  • i_shape_to_copy_position_along_dir1 (int) –

  • i_shape_to_copy_position_along_dir2 (int) –

  • i_dir1 (Reference) –

  • i_dir2 (Reference) –

  • i_is_reversed_dir1 (bool) –

  • i_is_reversed_dir2 (bool) –

  • i_rotation_angle (float) –

Return type:

RectPattern

add_new_remove(i_body_to_remove: Body) → Remove

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_body_to_remove (Body) –

Return type:

Remove

add_new_remove_face(i_keep_faces: Reference, i_remove_faces: Reference) → RemoveFace

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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.
Parameters:
Return type:

RemoveFace

add_new_removed_blend() → AnyObject

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func AddNewRemovedBlend() As AnyObject

Creates and returns a new Removed Blend feature.

Returns:
The created Removed Blend feature
Return type:

AnyObject

add_new_removed_loft() → AnyObject

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func AddNewRemovedLoft() As AnyObject

Creates and returns a new Removed Loft feature.

Returns:
The created Removed Loft feature
Return type:

AnyObject

add_new_replace_face(i_split_plane: Reference, i_remove_face: Reference, i_splitting_side: int) → ReplaceFace

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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.
Parameters:

  • i_split_plane (Reference) –

  • i_remove_face (Reference) –

  • i_splitting_side (int) – enum cat_split_side

Return type:

ReplaceFace

add_new_rib(i_sketch: Sketch, i_center_curve: Sketch) → Rib

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:
Return type:

Rib

add_new_rib_from_ref(i_profile: Reference, i_center_curve: Reference) → Rib

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:
Return type:

Rib

add_new_rotate2(i_axis: Reference, i_angle: float) → AnyObject

Note

Microsoft Visual Basic Object Browser
Function AddNewRotate2(iAxis As Reference, iAngle As Double) As AnyObject
Member of PARTITF.ShapeFactory
Parameters:
Return type:

AnyObject

add_new_scaling(i_scaling_reference: Reference, i_factor: float) → Scaling

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_scaling_reference (Reference) –

  • i_factor (float) –

Return type:

Scaling

add_new_sew_surface(i_sewing_element: Reference, i_sewing_side: int) → SewSurface

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_sewing_element (Reference) –

  • i_sewing_side (int) – enum cat_split_side

Return type:

SewSurface

add_new_shaft(i_sketch: Sketch) → Shaft

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_sketch (Sketch) –

Return type:

Shaft

add_new_shaft_from_ref(i_profile_elt: Reference) → Shaft

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_profile_elt (Reference) –

Return type:

Shaft

add_new_shell(i_face_to_remove: Reference, i_internal_thickness: float, i_external_thickness: float) → Shell

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_face_to_remove (Reference) –

  • i_internal_thickness (float) –

  • i_external_thickness (float) –

Return type:

Shell

add_new_slot(i_sketch: Sketch, i_center_curve: Sketch) → Slot

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:
Return type:

Slot

add_new_slot_from_ref(i_profile: Reference, i_center_curve: Reference) → Slot

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:
Return type:

Slot

add_new_solid_combine(i_profile_elt_first: Reference, i_profile_elt_second: Reference) → SolidCombine

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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.
Parameters:
Return type:

SolidCombine

add_new_solid_edge_fillet_with_constant_radius(i_edge_to_fillet: Reference, i_propag_mode: int, i_radius: float) → ConstRadEdgeFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_edge_to_fillet (Reference) –

  • i_propag_mode (int) – enum cat_fillet_edge_propagation

  • i_radius (float) –

Return type:

ConstRadEdgeFillet

add_new_solid_edge_fillet_with_varying_radius(i_edge_to_fillet: Reference, i_propag_mode: int, i_variation_mode: int, i_default_radius: float) → VarRadEdgeFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_edge_to_fillet (Reference) –

  • i_propag_mode (int) – enum cat_fillet_edge_propagation

  • i_variation_mode (int) – enum cat_fillet_variation

  • i_default_radius (float) –

Return type:

VarRadEdgeFillet

add_new_solid_face_fillet(i_f1: Reference, i_f2: Reference, i_radius: float) → FaceFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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 Boundary object is supported: Face.
iRadius
The fillet radius
Returns:
The created face-to-face fillet
Parameters:
Return type:

FaceFillet

add_new_solid_tritangent_fillet(i_f1: Reference, i_f2: Reference, i_removed_face: Reference) → TritangentFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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 Boundary object is supported: Face.
iRemovedFace
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 Boundary object is supported: Face
Returns:
The created tritangent fillet
Parameters:
Return type:

TritangentFillet

add_new_split(i_splitting_element: Reference, i_split_side: int) → Split

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_splitting_element (Reference) –

  • i_split_side (int) – enum cat_split_side

Return type:

Split

add_new_stiffener(i_sketch: Sketch) → Stiffener

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_sketch (Sketch) –

Return type:

Stiffener

add_new_stiffener_from_ref(i_profile_elt: Reference) → Stiffener

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_profile_elt (Reference) –

Return type:

Stiffener

add_new_surface_edge_fillet_with_constant_radius(i_edge_to_fillet: Reference, i_propag_mode: int, i_radius: float) → ConstRadEdgeFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_edge_to_fillet (Reference) –

  • i_propag_mode (int) – enum cat_fillet_edge_propagation

  • i_radius (float) –

Return type:

ConstRadEdgeFillet

add_new_surface_edge_fillet_with_varying_radius(i_edge_to_fillet: Reference, i_propag_mode: int, i_variation_mode: int, i_default_radius: float) → VarRadEdgeFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_edge_to_fillet (Reference) –

  • i_propag_mode (int) – enum cat_fillet_edge_propagation

  • i_variation_mode (int) – enum cat_fillet_variation

  • i_default_radius (float) –

Return type:

VarRadEdgeFillet

add_new_surface_face_fillet(i_f1: Reference, i_f2: Reference, i_radius: float) → FaceFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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 Boundary object is supported: Face.
iRadius
The fillet radius
Returns:
The created face-to-face fillet
Parameters:
Return type:

FaceFillet

add_new_surface_tritangent_fillet(i_f1: Reference, i_f2: Reference, i_removed_face: Reference) → TritangentFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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 Boundary object is supported: Face.
iRemovedFace
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 Boundary object is supported: Face
Returns:
The created tritangent fillet
Parameters:
Return type:

TritangentFillet

add_new_surfacic_auto_fillet(i_fillet_radius: float) → AutoFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_fillet_radius (float) –

Return type:

AutoFillet

add_new_surfacic_circ_pattern(i_shape_to_copy: AnyObject, i_nb_of_copies_in_radial_dir: int, i_nb_of_copies_in_angular_dir: int, i_step_in_radial_dir: float, i_step_in_angular_dir: float, i_shape_to_copy_position_along_radial_dir: int, i_shape_to_copy_position_along_angular_dir: int, i_rotation_center: Reference, i_rotation_axis: Reference, i_is_reversed_rotation_axis: bool, i_rotation_angle: float, i_is_radius_aligned: bool, i_complete_crown: bool) → CircPattern

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
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).
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
Parameters:

  • i_shape_to_copy (AnyObject) –

  • i_nb_of_copies_in_radial_dir (int) –

  • i_nb_of_copies_in_angular_dir (int) –

  • i_step_in_radial_dir (float) –

  • i_step_in_angular_dir (float) –

  • i_shape_to_copy_position_along_radial_dir (int) –

  • i_shape_to_copy_position_along_angular_dir (int) –

  • i_rotation_center (Reference) –

  • i_rotation_axis (Reference) –

  • i_is_reversed_rotation_axis (bool) –

  • i_rotation_angle (float) –

  • i_is_radius_aligned (bool) –

  • i_complete_crown (bool) –

Return type:

CircPattern

add_new_surfacic_rect_pattern(i_shape_to_copy: AnyObject, i_nb_of_copies_in_dir1: int, i_nb_of_copies_in_dir2: int, i_step_in_dir1: float, i_step_in_dir2: float, i_shape_to_copy_position_along_dir1: int, i_shape_to_copy_position_along_dir2: int, i_dir1: Reference, i_dir2: Reference, i_is_reversed_dir1: bool, i_is_reversed_dir2: bool, i_rotation_angle: float) → RectPattern

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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 Boundary objects are supported: PlanarFace,
RectilinearTriDimFeatEdge, RectilinearBiDimFeatEdge.
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
Parameters:

  • i_shape_to_copy (AnyObject) –

  • i_nb_of_copies_in_dir1 (int) –

  • i_nb_of_copies_in_dir2 (int) –

  • i_step_in_dir1 (float) –

  • i_step_in_dir2 (float) –

  • i_shape_to_copy_position_along_dir1 (int) –

  • i_shape_to_copy_position_along_dir2 (int) –

  • i_dir1 (Reference) –

  • i_dir2 (Reference) –

  • i_is_reversed_dir1 (bool) –

  • i_is_reversed_dir2 (bool) –

  • i_rotation_angle (float) –

Return type:

RectPattern

add_new_surfacic_sew_surface(i_type: int, i_support_surface: Reference, i_sewing_element: Reference, i_sewing_side: int) → SewSurface

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func AddNewSurfacicSewSurface(long iType,
Reference iSupportSurface,
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
iSupportSurface
The surfacic 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
Parameters:

  • i_type (int) –

  • i_support_surface (Reference) –

  • i_sewing_element (Reference) –

  • i_sewing_side (int) – enum cat_split_side

Return type:

SewSurface

add_new_surfacic_user_pattern(i_shape_to_copy: AnyObject, i_nb_of_copies: int) → UserPattern

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_shape_to_copy (AnyObject) –

  • i_nb_of_copies (int) –

Return type:

UserPattern

add_new_symmetry_2(i_reference: Reference) → HybridShapeSymmetry

Note

CAA V5 Visual Basic Help - Manually created. (2022-10-10)
o Func AddNewSymmetry2(Reference iReference) As HybridShapeSymmetry

Creates a new Symmetry within the current body.

Parameters:

iReference
Point, line or reference plane.
Sub-element(s) supported (see Boundary object): see PlanarFace, Edge
and Vertex.
oSymmetry
Created symmetry.
Parameters:

i_reference (Reference) –

Return type:

HybridShapeSymmetry

add_new_thick_surface(i_offset_element: Reference, i_isens_offset: int, i_top_offset: float, i_bot_offset: float) → ThickSurface

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_offset_element (Reference) –

  • i_isens_offset (int) –

  • i_top_offset (float) –

  • i_bot_offset (float) –

Return type:

ThickSurface

add_new_thickness(i_face_to_thicken: Reference, i_offset: float) → Thickness

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_face_to_thicken (Reference) –

  • i_offset (float) –

Return type:

Thickness

add_new_thread_with_out_ref() → Thread

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func AddNewThreadWithOutRef() As Thread

Creates and returns a new thread ap within the current
body.

Returns:
The created Thread
Return type:

Thread

add_new_thread_with_ref(i_lateral_face: Reference, i_limit_face: Reference) → Thread

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
o Func AddNewThreadWithRef(Reference iLateralFace,
Reference iLimitFace) As Thread

Creates and returns a new thread ap within the current
body.

Parameters:

iLateralFace
The Face defining the support of thread ap
The following

Boundary object is supported: Face.
iLimitFacee
The Face defining the origin of the thread.
The following Boundary object is supported:
PlanarFace.
Returns:
The created Thread
Parameters:
Return type:

Thread

add_new_translate2(i_distance: float) → Translate

Note

Microsoft Visual Basic Object Browser
Function AddNewTranslate2(iDistance As Double) As AnyObject
Member of PARTITF.ShapeFactory
Parameters:

i_distance (float) –

Return type:

AnyObject

add_new_trim(i_body_to_trim: Body) → Trim

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_body_to_trim (Body) –

Return type:

Trim

add_new_tritangent_fillet(i_f1: Reference, i_f2: Reference, i_removed_face: Reference) → TritangentFillet

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:
Return type:

TritangentFillet

add_new_user_pattern(i_shape_to_copy: AnyObject, i_nb_of_copies: int) → UserPattern

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_shape_to_copy (AnyObject) –

  • i_nb_of_copies (int) –

Return type:

UserPattern

add_new_user_patternof_list(i_shape_to_copy: AnyObject, i_nb_of_copies: int) → UserPattern

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_shape_to_copy (AnyObject) –

  • i_nb_of_copies (int) –

Return type:

UserPattern

add_new_volume_add(i_body1: Reference, i_body2: Reference, i_type: float) → Add

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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.
Parameters:
Return type:

Add

add_new_volume_close_surface(i_close_element: Reference) → CloseSurface

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

i_close_element (Reference) –

Return type:

CloseSurface

add_new_volume_intersect(i_body1: Reference, i_body2: Reference, i_type: float) → Intersect

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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.
Parameters:
Return type:

Intersect

add_new_volume_remove(i_body1: Reference, i_body2: Reference, i_type: float) → Remove

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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.
Parameters:
Return type:

Remove

add_new_volume_sew_surface(i_type: int, i_support_volume: Reference, i_sewing_element: Reference, i_sewing_side: int) → SewSurface

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_type (int) –

  • i_support_volume (Reference) –

  • i_sewing_element (Reference) –

  • i_sewing_side (int) – enum cat_split_side

Return type:

SewSurface

add_new_volume_shell(i_face_to_remove: Reference, i_internal_thickness: float, i_external_thickness: float, i_volume_support: Reference) → Shell

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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.
Parameters:

  • i_face_to_remove (Reference) –

  • i_internal_thickness (float) –

  • i_external_thickness (float) –

  • i_volume_support (Reference) –

Return type:

Shell

add_new_volume_thick_surface(i_offset_element: Reference, i_isens_offset: int, i_top_offset: float, i_bot_offset: float) → ThickSurface

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_offset_element (Reference) –

  • i_isens_offset (int) –

  • i_top_offset (float) –

  • i_bot_offset (float) –

Return type:

ThickSurface

add_new_volume_thickness(i_face_to_thicken: Reference, i_offset: float, i_type: int, i_volume_support: Reference) → Thickness

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:

  • i_face_to_thicken (Reference) –

  • i_offset (float) –

  • i_type (int) –

  • i_volume_support (Reference) –

Return type:

Thickness

add_new_volume_trim(i_support_volume: Reference, i_cutting_volume: Reference) → Trim

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
Parameters:
Return type:

Trim

add_new_volumic_draft(i_face_to_draft: Reference, i_neutral: Reference, i_neutral_mode: int, i_parting: Reference, i_dir_x: float, i_dir_y: float, i_dir_z: float, i_mode: int, i_angle: float, i_multiselection_mode: int, i_type: int, i_volume_support: Reference) → Draft

Note

CAA V5 Visual Basic Help (2020-07-06 14:02:20.222384))
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
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 Boundary object is supported:
PlanarFace.
iNeutralMode
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 Boundary object is supported:
PlanarFace.
iDirX,iDirY,iDirZ
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
Parameters:

  • i_face_to_draft (Reference) –

  • i_neutral (Reference) –

  • i_neutral_mode (int) – enum cat_draft_neutral_propagation_mode

  • i_parting (Reference) –

  • i_dir_x (float) –

  • i_dir_y (float) –

  • i_dir_z (float) –

  • i_mode (int) – enum cat_draft_mode

  • i_angle (float) –

  • i_multiselection_mode (int) – enum cat_draft_multiselection_mode

  • i_type (int) –

  • i_volume_support (Reference) –

Return type:

Draft