pycatia.hybrid_shape_interfaces.hybrid_shape_factory

Module initially auto generated using V5Automation files from CATIA V5 R28 on 2020-07-06 14:02:20.222384

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.hybrid_shape_interfaces.hybrid_shape_factory.HybridShapeFactory(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

HybridShapeFactory

Interface to create all kinds of HybridShape objects that may be needed in

wireframe and surface design.

Note:

This interface concern GSD/GSO/DL1 feature creation via VB

Use of the creation methods requires to have granted license configuration for

feature creation

i.e:

- Bump, Develop,WrapCurve,WrapSurface require GSO license.

- Unfold, Develop require DL1 license.

- Other require GSD license.

Note2:

For all methods creating datums AddNew*Datum,

the object passed as parameter to create the datum has to be in the current

container.

Otherwise, an error occurs.

add_new_3d_corner(i_element1: Reference, i_element2: Reference, i_direction: HybridShapeDirection, i_radius: float, i_orientation1: int, i_orientation2: int, i_trim: bool) → HybridShapeCorner

Note

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

o Func AddNew3DCorner(Reference iElement1,

Reference iElement2,

HybridShapeDirection iDirection,

double iRadius,

long iOrientation1,

long iOrientation2,

boolean iTrim) As HybridShapeCorner

Creates a new 3D Corner within the current body.

Create a 3D corner curve between a point and a curve or 2 curves along a

direction.

Parameters:

iElement1

First reference curve.

iElement2

Second reference curve.

iDirection

Direction.

iRadius

Radius of the corner.

iOrientation1

Manage the corner center position. Value can be 1 or -1

iOrientation2

Manage the corner center position. Value can be 1 or -1

iTrim

Value can be FALSE or TRUE

if TRUE the 2 curves are trimed and asembled with the corner.

oCorner

Created corner.

Parameters:

• i_element1 (Reference) –

• i_element2 (Reference) –

• i_direction (HybridShapeDirection) –

• i_radius (float) –

• i_orientation1 (int) –

• i_orientation2 (int) –

• i_trim (bool) –

Return type:

HybridShapeCorner

add_new_3d_curve_offset(i_curve_to_offset: Reference, i_direction: HybridShapeDirection, i_offset: float, i_corner_radius: float, i_corner_tension: float) → HybridShape3DCurveOffset

Note

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

o Func AddNew3DCurveOffset(Reference iCurveToOffset,

HybridShapeDirection iDirection,

double iOffset,

double iCornerRadius,

double iCornerTension) As HybridShape3DCurveOffset

Creates a 3D Curve Offset.

Parameters:

iCurve

The curve to offset

iDirection

Offset pulling direction.

iOffsetValue

Offset Value.

iCornerRadius

Radius of the 3D corners.

iCornerTension

Tension of the 3D corners.

Returns:

CATIGSM3DCurveOffset_var created 3DCurveOffset.

Parameters:

• i_curve_to_offset (Reference) –

• i_direction (HybridShapeDirection) –

• i_offset (float) –

• i_corner_radius (float) –

• i_corner_tension (float) –

Return type:

HybridShape3DCurveOffset

add_new_affinity(i_element: Reference, i_x_ratio: float, i_y_ratio: float, i_z_ratio: float) → HybridShapeAffinity

Note

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

o Func AddNewAffinity(Reference iElement,

double iXRatio,

double iYRatio,

double iZRatio) As HybridShapeAffinity

Creates a new Affinity within the current body.

Parameters:

iElement

point, curve, surface or solid.

Sub-element(s) supported (see

Boundary object): see Face, TriDimFeatEdge, BiDimFeatEdge and Vertex.

iXRatio

Ratio of affinity in iX direction.

iYRatio

Ratio of affinity in iY direction.

iZRatio

Ratio of affinity in iZ direction.

oAffinity

Created affinity

Parameters:

• i_element (Reference) –

• i_x_ratio (float) –

• i_y_ratio (float) –

• i_z_ratio (float) –

Return type:

HybridShapeAffinity

add_new_axis_line(i_element: Reference) → HybridShapeAxisLine

Note

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

o Func AddNewAxisLine(Reference iElement) As

HybridShapeAxisLine

Creates a new AxisLine within the current body.

Parameters:

iElement

Circle, Ellipse, Oblong, Sphere, Revolution surface. Axis is

computed for this element

oAxisLine

Created axis line

Parameters:

i_element (Reference) –

Return type:

HybridShapeAxisLine

add_new_axis_to_axis(i_object: Reference, i_reference_axis: Reference, i_target_axis: Reference) → HybridShapeAxisToAxis

Note

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

o Func AddNewAxisToAxis(Reference iObject,

Reference iReferenceAxis,

Reference iTargetAxis) As HybridShapeAxisToAxis

Creates a new axis to axis transformation within the current

body.

Parameters:

iObject

Point, curve, surface or solid to transform.

iReferenceAxis

reference axis system

iTargetAxis

target axis system

oAxisToAxis

Created axis to axis transformation.

Parameters:

• i_object (Reference) –

• i_reference_axis (Reference) –

• i_target_axis (Reference) –

Return type:

HybridShapeAxisToAxis

add_new_blend() → HybridShapeBlend

Note

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

o Func AddNewBlend() As HybridShapeBlend

Creates a new blend surface within the current body.

Parameters:

oBlend

The Blend object if succeded

Return type:

HybridShapeBlend

add_new_boundary(i_initial_element: Reference, i_support: Reference, i_typede_propagation: int) → HybridShapeBoundary

Note

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

o Func AddNewBoundary(Reference iInitialElement,

Reference iSupport,

long iTypedePropagation) As HybridShapeBoundary

Creates a new Boundary within the current body.

Parameters:

iInitialElement

the element used to initialise the propagation around the

surface

Sub-element(s) supported (see

Boundary object): see BiDimFeatEdge.

iSupport

the surface used to compute the boundary around it

Sub-element(s) supported (see Boundary object): see

Face.

iTypedePropagation

Propagation type the values are: 0 for Boundary for all edges 1 for

Boundary propagation for edges on connexe point 2 for Boundary propagation for

edges tangent at point breaks 3 for Boundary not propagation from the current

edge

oBoundary

The computed element

Parameters:

• i_initial_element (Reference) –

• i_support (Reference) –

• i_typede_propagation (int) –

Return type:

HybridShapeBoundary

add_new_boundary_of_surface(surface: Reference) → HybridShapeBoundary

Note

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

o Func AddNewBoundaryOfSurface(Reference Surface) As

HybridShapeBoundary

Creates a Boundary within the current body.

Parameters:

iSurface

the feature on which all the boundaries will be computed

oBoundary

the whole boundary of the Surface given in first

parameter

Parameters:

surface (Reference) –

Return type:

HybridShapeBoundary

add_new_bump(i_body_to_bump: Reference) → HybridShapeBump

Note

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

o Func AddNewBump(Reference iBodyToBump) As HybridShapeBump

Creates a new Bump within the current body.

Note: require GSO license.

Parameters:

:

iBodyToBump Body to deform witn a Bump

:

oBump Bump result

Parameters:

i_body_to_bump (Reference) –

Return type:

HybridShapeBump

add_new_circle2_points_rad(i_point1: Reference, i_point2: Reference, i_support: Reference, i_geodesic: bool, i_radius: float, i_ori: int) → HybridShapeCircle2PointsRad

Note

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

o Func AddNewCircle2PointsRad(Reference iPoint1,

Reference iPoint2,

Reference iSupport,

boolean iGeodesic,

double iRadius,

long iOri) As HybridShapeCircle2PointsRad

Creates a new Circle passing through 2 points with a radius within the

current body.

Parameters:

iPoint1

first passing point.

Sub-element(s) supported (see

Boundary object): see Vertex.

iPoint2

second passing point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iSupport

support surface.

Sub-element(s) supported (see Boundary object): see

Face.

iGeodesic

Puts the circle on the surface.

iRadius

Value specified is considered as radius. To use this value as diameter,

set DiameterMode using SetDiameterMode method

iOri

circle orientation. Defines the side where circle is computed using the

normal direction of line between the 2 passing points.

oCircle

The Circle object if succeeded

Parameters:

• i_point1 (Reference) –

• i_point2 (Reference) –

• i_support (Reference) –

• i_geodesic (bool) –

• i_radius (float) –

• i_ori (int) –

Return type:

HybridShapeCircle2PointsRad

add_new_circle3_points(i_point1: Reference, i_point2: Reference, i_point3: Reference) → HybridShapeCircle3Points

Note

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

o Func AddNewCircle3Points(Reference iPoint1,

Reference iPoint2,

Reference iPoint3) As HybridShapeCircle3Points

Creates a new circle passing through 3 points within the current

body.

Parameters:

iPoint1

first passing point.

Sub-element(s) supported (see

Boundary object): see Vertex.

iPoint2

second passing point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iPoint3

third passing point.

Sub-element(s) supported (see Boundary object): see

Vertex.

oCircle

Created circle

Parameters:

• i_point1 (Reference) –

• i_point2 (Reference) –

• i_point3 (Reference) –

Return type:

HybridShapeCircle3Points

add_new_circle_bitangent_point(i_curve1: Reference, i_curve2: Reference, i_point: Reference, i_support: Reference, i_ori1: int, i_ori2: int) → HybridShapeCircleBitangentPoint

Note

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

o Func AddNewCircleBitangentPoint(Reference iCurve1,

Reference iCurve2,

Reference iPoint,

Reference iSupport,

long iOri1,

long iOri2) As HybridShapeCircleBitangentPoint

Creates a new circle tangent to 2 curves and passing through one point

within the current body.

Parameters:

iCurve1

first curve to which the circle will be tangent.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iCurve2

second curve to which the circle will be tangent.

Sub-element(s) supported (see Boundary object): see TriDimFeatEdge and

BiDimFeatEdge.

iPoint

passing point. This point must lie on second curve.

Sub-element(s) supported (see Boundary object): see

Vertex.

iSupport

support surface.

Sub-element(s) supported (see Boundary object): see

Face.

iOri1

first curve orientation for circle computation.

iOri2

second curve orientation for circle computation.

oCircle

Created circle

Parameters:

• i_curve1 (Reference) –

• i_curve2 (Reference) –

• i_point (Reference) –

• i_support (Reference) –

• i_ori1 (int) –

• i_ori2 (int) –

Return type:

HybridShapeCircleBitangentPoint

add_new_circle_bitangent_radius(i_curve1: Reference, i_curve2: Reference, i_support: Reference, i_radius: float, i_ori1: int, i_ori2: int) → HybridShapeCircleBitangentRadius

Note

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

o Func AddNewCircleBitangentRadius(Reference iCurve1,

Reference iCurve2,

Reference iSupport,

double iRadius,

long iOri1,

long iOri2) As HybridShapeCircleBitangentRadius

Creates a new circle tangent to 2 curves and with a radius within the

current body.

Parameters:

iCurve1

first curve to which the circle will be tangent.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iCurve2

second curve to which the circle will be tangent.

Sub-element(s) supported (see Boundary object): see TriDimFeatEdge and

BiDimFeatEdge.

iSupport

support surface.

Sub-element(s) supported (see Boundary object): see

Face.

iRadius

Value specified is considered as radius. To use this value as diameter,

set DiameterMode using SetDiameterMode method

iOri1

first curve orientation for circle computation.

iOri2

second curve orientation for circle computation.

oCircle

Created circle

Parameters:

• i_curve1 (Reference) –

• i_curve2 (Reference) –

• i_support (Reference) –

• i_radius (float) –

• i_ori1 (int) –

• i_ori2 (int) –

Return type:

HybridShapeCircleBitangentRadius

add_new_circle_center_axis(i_axis: Reference, i_point: Reference, i_value: float, i_projection: bool) → HybridShapeCircleCenterAxis

Note

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

o Func AddNewCircleCenterAxis(Reference iAxis,

Reference iPoint,

double iValue,

boolean iProjection) As HybridShapeCircleCenterAxis

Creates a circle from point and axis.

Parameters:

iAxis

Axis of plane in which circle is lying

iPoint

Point used for center computation. It will be the center if ProjectionMode is False.

If ProjectionMode = True, this point will be projected on to axis/line

iValue

Value specified is considered as radius. To use this value as

diameter, set DiameterMode property

iProjection

Sets Projection Mode. ProjectionMode = TRUE implies point will be projected on to

axis/line, ProjectionMode = FALSE implies that point will be center of the circle.

oCircle

Created circle

Parameters:

• i_axis (Reference) –

• i_point (Reference) –

• i_value (float) –

• i_projection (bool) –

Return type:

HybridShapeCircleCenterAxis

add_new_circle_center_axis_with_angles(i_axis: Reference, i_point: Reference, i_value: float, i_projection: bool, i_start_angle: float, i_end_angle: float) → HybridShapeCircleCenterAxis

Note

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

o Func AddNewCircleCenterAxisWithAngles(Reference iAxis,

Reference iPoint,

double iValue,

boolean iProjection,

double iStartAngle,

double iEndAngle) As HybridShapeCircleCenterAxis

Creates a circle from point and axis.

Parameters:

iAxis

Axis of plane in which circle is lying

Sub-element(s) supported (see

Boundary object):

iPoint

Point used for center computation. It will be the center if ProjectionMode is False.

If ProjectionMode = True, this point will be projected on to axis/line

Sub-element(s) supported (see Boundary object):

iValue

Value specified is considered as radius. To use this value as diameter,

set DiameterMode property

iProjection

Sets Projection Mode. ProjectionMode = TRUE implies point will be projected on to axis/line,

ProjectionMode = FALSE implies that point will be center of the circle.

iStartAngle

start angle

iEndAngle

end angle

oCircle

Created circle

Parameters:

• i_axis (Reference) –

• i_point (Reference) –

• i_value (float) –

• i_projection (bool) –

• i_start_angle (float) –

• i_end_angle (float) –

Return type:

HybridShapeCircleCenterAxis

add_new_circle_center_tangent(i_center_elem: Reference, i_tangent_curve: Reference, i_support: Reference, i_radius: float) → HybridShapeCircleCenterTangent

Note

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

o Func AddNewCircleCenterTangent(Reference iCenterElem,

Reference iTangentCurve,

Reference iSupport,

double iRadius) As HybridShapeCircleCenterTangent

Creates a new circle with given center element and tangent

curve.

Parameters:

iCenterElem

Can be either curve or point.

iTangentCurve

Curve to which the circle will be tangent.

iSupport

support surface or plane.

iRadius

circle radius, valid only if center element is curve. Value

specified is considered as radius. To use this value as diameter, set

DiameterMode using SetDiameterMode method

oCircle

Created circle

Parameters:

• i_center_elem (Reference) –

• i_tangent_curve (Reference) –

• i_support (Reference) –

• i_radius (float) –

Return type:

HybridShapeCircleCenterTangent

add_new_circle_ctr_pt(i_center: Reference, i_crossing_point: Reference, i_support: Reference, i_geodesic: bool) → HybridShapeCircleCtrPt

Note

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

o Func AddNewCircleCtrPt(Reference iCenter,

Reference iCrossingPoint,

Reference iSupport,

boolean iGeodesic) As HybridShapeCircleCtrPt

Creates a new whole circle defined by its center, a passing point within

the current body.

Parameters:

iCenter

circle center.

Sub-element(s) supported (see

Boundary object): see Vertex.

iCrossingPoint

passing point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iSupport

support surface.

Sub-element(s) supported (see Boundary object): see

Face.

iGeodesic

Puts the circle on the surface.

oCircle

CreatedCircle

Parameters:

• i_center (Reference) –

• i_crossing_point (Reference) –

• i_support (Reference) –

• i_geodesic (bool) –

Return type:

HybridShapeCircleCtrPt

add_new_circle_ctr_pt_with_angles(i_center: Reference, i_crossing_point: Reference, i_support: Reference, i_geodesic: bool, i_start_angle: float, i_end_angle: float) → HybridShapeCircleCtrPt

Note

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

o Func AddNewCircleCtrPtWithAngles(Reference iCenter,

Reference iCrossingPoint,

Reference iSupport,

boolean iGeodesic,

double iStartAngle,

double iEndAngle) As HybridShapeCircleCtrPt

Creates a new circle defined by its center, a passing point and angles

within the current body.

Parameters:

iCenter

circle center.

Sub-element(s) supported (see

Boundary object): see Vertex.

iCrossingPoint

passing point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iSupport

support surface.

Sub-element(s) supported (see Boundary object): see

Face.

iGeodesic

Puts the circle on the surface.

iStartAngle

start angle

iEndAngle

end angle

oCircle

Created circle

Parameters:

• i_center (Reference) –

• i_crossing_point (Reference) –

• i_support (Reference) –

• i_geodesic (bool) –

• i_start_angle (float) –

• i_end_angle (float) –

Return type:

HybridShapeCircleCtrPt

add_new_circle_ctr_rad(i_center: Reference, i_support: Reference, i_geodesic: bool, i_radius: float) → HybridShapeCircleCtrRad

Note

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

o Func AddNewCircleCtrRad(Reference iCenter,

Reference iSupport,

boolean iGeodesic,

double iRadius) As HybridShapeCircleCtrRad

Creates a new whole circle defined by its center and a radius within the

current body.

Parameters:

iCenter

circle center.

Sub-element(s) supported (see

Boundary object): see Vertex.

iSupport

support surface.

Sub-element(s) supported (see Boundary object): see

Face.

iGeodesic

Puts the circle on the surface.

iRadius

Value specified is considered as radius. To use this value as diameter,

set DiameterMode using SetDiameterMode method

oCircle

Created circle

Parameters:

• i_center (Reference) –

• i_support (Reference) –

• i_geodesic (bool) –

• i_radius (float) –

Return type:

HybridShapeCircleCtrRad

add_new_circle_ctr_rad_with_angles(i_center: Reference, i_support: Reference, i_geodesic: bool, i_radius: float, i_start_angle: float, i_end_angle: float) → HybridShapeCircleCtrRad

Note

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

o Func AddNewCircleCtrRadWithAngles(Reference iCenter,

Reference iSupport,

boolean iGeodesic,

double iRadius,

double iStartAngle,

double iEndAngle) As HybridShapeCircleCtrRad

Creates a new circle defined by its center, a radius and angles within the

current body.

Parameters:

iCenter

circle center.

Sub-element(s) supported (see

Boundary object): see Vertex.

iSupport

support surface.

Sub-element(s) supported (see Boundary object): see

Face.

iGeodesic

Puts the circle on the surface.

iRadius

Value specified is considered as radius. To use this value as diameter,

set DiameterMode using SetDiameterMode method

iStartAngle

start angle

iEndAngle

end angle

oCircle

Created circle

Parameters:

• i_center (Reference) –

• i_support (Reference) –

• i_geodesic (bool) –

• i_radius (float) –

• i_start_angle (float) –

• i_end_angle (float) –

Return type:

HybridShapeCircleCtrRad

add_new_circle_datum(i_object: Reference) → HybridShapeCircleExplicit

Note

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o Func AddNewCircleDatum(Reference iObject) As

HybridShapeCircleExplicit

Creates a new datum of circle within the current body.

Parameters:

iObject

The object whose topological body will be duplicated and put into

created datum

oCircle

Created datum Note2: the object passed as parameter to create the

datum has to be in the current container. Otherwise, an error

occurs.

Parameters:

i_object (Reference) –

Return type:

HybridShapeCircleExplicit

add_new_circle_tritangent(i_curve1: Reference, i_curve2: Reference, i_curve3: Reference, i_support: Reference, i_ori1: int, i_ori2: int, i_ori3: int) → HybridShapeCircleTritangent

Note

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

o Func AddNewCircleTritangent(Reference iCurve1,

Reference iCurve2,

Reference iCurve3,

Reference iSupport,

long iOri1,

long iOri2,

long iOri3) As HybridShapeCircleTritangent

Creates a new tritangent circle within the current body.

Parameters:

iCurve1

first curve to which the circle will be tangent.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iCurve2

second curve to which the circle will be tangent.

Sub-element(s) supported (see Boundary object): see TriDimFeatEdge and

BiDimFeatEdge.

iCurve3

third curve to which the circle will be tangent.

Sub-element(s) supported (see Boundary object): see TriDimFeatEdge and

BiDimFeatEdge.

iSupport

support surface.

Sub-element(s) supported (see Boundary object): see

Face.

iOri1

first curve orientation for circle computation.

iOri2

second curve orientation for circle computation.

iOri3

third curve orientation for circle computation.

oCircle

Created circle

Parameters:

• i_curve1 (Reference) –

• i_curve2 (Reference) –

• i_curve3 (Reference) –

• i_support (Reference) –

• i_ori1 (int) –

• i_ori2 (int) –

• i_ori3 (int) –

Return type:

HybridShapeCircleTritangent

add_new_combine(i_first_curve: Reference, i_second_curve: Reference, i_nearest_solutions: int) → HybridShapeCombine

Note

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

o Func AddNewCombine(Reference iFirstCurve,

Reference iSecondCurve,

long iNearestSolutions) As HybridShapeCombine

Creates a new Combine within the current body. By default, the combine

direction is the normal of each curve. If you want to change see

CATIAHybridShapeCombine interfaces.

Parameters:

iFirstCurve

First curve to combine

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iSecondCurve

Second curve to combine

Sub-element(s) supported (see Boundary object): see TriDimFeatEdge and

BiDimFeatEdge.

iNearestSolution

If more than one solution, to choose the nearest solution of the first

curve

oCombine

The combine object if succeded

Parameters:

• i_first_curve (Reference) –

• i_second_curve (Reference) –

• i_nearest_solutions (int) –

Return type:

HybridShapeCombine

add_new_conic(i_support: Reference, i_starting_point: Reference, i_end_point: Reference) → HybridShapeConic

Note

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

o Func AddNewConic(Reference iSupport,

Reference iStartingPoint,

Reference iEndPoint) As HybridShapeConic

Creates a new conic within the current body.

Parameters:

iSupport

The conic support (always a plane).

Sub-element(s) supported (see

Boundary object): see PlanarFace.

iStartingPoint

Starting Point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iEndPoint

End Point

Sub-element(s) supported (see Boundary object): see

Vertex.

oConic

The Conic object if succeded

Parameters:

• i_support (Reference) –

• i_starting_point (Reference) –

• i_end_point (Reference) –

Return type:

HybridShapeConic

add_new_conical_reflect_line_with_type(i_support: Reference, i_origin: Reference, i_angle: float, i_orientation_support: int, i_type: int) → HybridShapeReflectLine

Note

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o Func AddNewConicalReflectLineWithType(Reference iSupport,

Reference iOrigin,

double iAngle,

long iOrientationSupport,

long iType) As HybridShapeReflectLine

Creates a new conical ReflectLine within the current body.

Create a conical reflectline curve on a support surface from an origin

point with an angle.

Parameters:

iSupport

Support surface.

iOrigin

Origin point.

iAngle

Angle of the reflectline.

iOrientationSupport

Manage the angle used to compute the reflectline. Value can be 1 or

-1

iType

Manage the type used to compute the reflectline. Value can be 0 or

1 Returns or sets whether the reflectline curve is or should be created with

the normal to the support or the tangent plane to the

support.

Role: The TypeSolution indicates whether the created reflectline

curve is compute with the angle between the normale to the support and the

direction or with the angle between the tangent plane to the support and the

direction..

Legal values: 0 for the normal and 1 for the tangent plane.

oReflectLine

Created conical reflectline.

Parameters:

• i_support (Reference) –

• i_origin (Reference) –

• i_angle (float) –

• i_orientation_support (int) –

• i_type (int) –

Return type:

HybridShapeReflectLine

add_new_connect(i_curve1: Reference, i_point1: Reference, i_orient1: int, i_continuity1: int, i_tension1: float, i_curve2: Reference, i_point2: Reference, i_orient2: int, i_continuity2: int, i_tension2: float, trim: bool) → HybridShapeConnect

Note

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

o Func AddNewConnect(Reference iCurve1,

Reference iPoint1,

long iOrient1,

long iContinuity1,

double iTension1,

Reference iCurve2,

Reference iPoint2,

long iOrient2,

long iContinuity2,

double iTension2,

boolean Trim) As HybridShapeConnect

Creates a new Connect within the current body.

Parameters:

iCurve1

First curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iPoint1

First point (lying on the first curve)

Sub-element(s) supported (see Boundary object): see

Vertex.

iOrient1

Orientation on the first curve

iContinuity1

Continuity on first curve

iTension1

Tension on first curve

iCurve2

Second curve.

Sub-element(s) supported (see Boundary object): see TriDimFeatEdge and

BiDimFeatEdge.

iPoint2

Second point (lying on the second curve)

Sub-element(s) supported (see Boundary object): see

Vertex.

iOrient2

Orientation on the second curve

iContinuity2

Continuity on second curve

iTension2

Tension on second curve

iTrim

Trim the two curves with the connect

oConnect

The connect object

Parameters:

• i_curve1 (Reference) –

• i_point1 (Reference) –

• i_orient1 (int) –

• i_continuity1 (int) –

• i_tension1 (float) –

• i_curve2 (Reference) –

• i_point2 (Reference) –

• i_orient2 (int) –

• i_continuity2 (int) –

• i_tension2 (float) –

• trim (bool) –

Return type:

HybridShapeConnect

add_new_corner(i_element1: Reference, i_element2: Reference, i_support: Reference, i_radius: float, i_orientation1: int, i_orientation2: int, i_trim: bool) → HybridShapeCorner

Note

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

o Func AddNewCorner(Reference iElement1,

Reference iElement2,

Reference iSupport,

double iRadius,

long iOrientation1,

long iOrientation2,

boolean iTrim) As HybridShapeCorner

Creates a new Corner within the current body.

Create a corner curve between a point and a curve or 2 curves on a support

surface.

Parameters:

iElement1

First reference curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge, BiDimFeatEdge and Vertex.

iElement2

Second reference curve.

Sub-element(s) supported (see Boundary object): see TriDimFeatEdge,

BiDimFeatEdge and Vertex.

iSupport

Support surface.

Sub-element(s) supported (see Boundary object): see

Face.

iRadius

Radius of the corner.

iOrientation1

Manage the corner center position. Value can be 1 or -1

iOrientation2

Manage the corner center position. Value can be 1 or -1

iTrim

Value can be FALSE or TRUE

if TRUE the 2 curves are trimed and asembled with the corner.

oCorner

Created corner.

Parameters:

• i_element1 (Reference) –

• i_element2 (Reference) –

• i_support (Reference) –

• i_radius (float) –

• i_orientation1 (int) –

• i_orientation2 (int) –

• i_trim (bool) –

Return type:

HybridShapeCorner

add_new_curve_datum(i_object: Reference) → HybridShapeCurveExplicit

Note

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

o Func AddNewCurveDatum(Reference iObject) As

HybridShapeCurveExplicit

Creates a new datum of curve within the current body.

Parameters:

iObject

The object whose topological body will be duplicated and put into

created datum

oCurve

Created curve Note2: the object passed as parameter to create the

datum has to be in the current container. Otherwise, an error

occurs.

Parameters:

i_object (Reference) –

Return type:

HybridShapeCurveExplicit

add_new_curve_par(curve: Reference, support: Reference, distance: float, invert_direction: bool, geodesic: bool) → HybridShapeCurvePar

Note

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

o Func AddNewCurvePar(Reference Curve,

Reference Support,

double Distance,

boolean InvertDirection,

boolean Geodesic) As HybridShapeCurvePar

Creates a new CurvePar within the current body.

Parameters:

iCurve

Reference curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iSupport

Support on which the curve is lying on

Sub-element(s) supported (see Boundary object): see

Face.

iDistance

Distance value

iInvertDirection

Orientation

iGeodesic

Geodesic mode

oCurvePar

Parallel curve

Parameters:

• curve (Reference) –

• support (Reference) –

• distance (float) –

• invert_direction (bool) –

• geodesic (bool) –

Return type:

HybridShapeCurvePar

add_new_curve_smooth(ip_ia_curve: Reference) → HybridShapeCurveSmooth

Note

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

o Func AddNewCurveSmooth(Reference ipIACurve) As

HybridShapeCurveSmooth

Creates a new CurveSmooth within the current body.

Parameters:

iCurve

Reference curve to be smoothened

oCurveSmooth

Smoothened curve

Parameters:

ip_ia_curve (Reference) –

Return type:

HybridShapeCurveSmooth

add_new_cylinder(i_center: Reference, i_radius: float, i_first_length: float, i_second_length: float, i_direction: HybridShapeDirection) → HybridShapeCylinder

Note

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

o Func AddNewCylinder(Reference iCenter,

double iRadius,

double iFirstLength,

double iSecondLength,

HybridShapeDirection iDirection) As HybridShapeCylinder

Creates a new Cylinder within the current body.

Parameters:

iCenter

Center of the Cylinder - Can be Point or Vertex.

Sub-element(s) supported (see

Vertex object):

iRadius

Radius of Cylinder.

iFirstLength

Length of Cylinder in the given direction.

iSecondLength

Length of Cylinder in the opposite direction.

iDirection

Direction of extrusion for Cylinder.

oCylinderObject

Created CylinderObjct.

Parameters:

• i_center (Reference) –

• i_radius (float) –

• i_first_length (float) –

• i_second_length (float) –

• i_direction (HybridShapeDirection) –

Return type:

HybridShapeCylinder

add_new_datums(i_elem: Reference) → tuple

Note

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o Func AddNewDatums(Reference iElem) As CATSafeArrayVariant

Creates datums from a multi-domain result feature, one datum is created by

object domain.

Note; Available only for a shape design feature as input ( not for datum

feature ).

Parameters:

iElem

Reference element

oArrayOfDatum

List of datum objects , one datum is created per

omain

Level of availability = V5R14

Example:

This example converts a hybrid shape object in as much as

datums that the original hybrid shape features contains of

domain

Dim HShape

Set reference = part.CreateReferenceFromObject(hybridShapeObject)

‘ Convert to Datums

HShape = hybridShapeFactory.AddNewDatums reference

Num =UBound(HShape)

For i = 0 to Num

hybridBody1.AppendHybridShape HShape (i)

Next

part.InWorkObject = HShape(num)

part.Update

‘ Delete original feature

hybridShapeFactory.DeleteObjectForDatum

reference

Parameters:

i_elem (Reference) –

Return type:

tuple

add_new_develop(i_mode: int, i_to_develop: Reference, i_support: Reference) → HybridShapeDevelop

Note

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

o Func AddNewDevelop(long iMode,

Reference iToDevelop,

Reference iSupport) As HybridShapeDevelop

Creates a new Develop within the current body.

Note: require either DL1 or GSO license.

Parameters:

iMode

Develop method.

iToDevelop

Wire to be developed.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iSupport

Revolution support surface.

Sub-element(s) supported (see Boundary object): see

Face.

oExt

Created developed wire.

Parameters:

• i_mode (int) –

• i_to_develop (Reference) –

• i_support (Reference) –

Return type:

HybridShapeDevelop

add_new_direction(i_element: Reference) → HybridShapeDirection

Note

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

o Func AddNewDirection(Reference iElement) As

HybridShapeDirection

Creates a new direction specified by an element within the current

body.

Parameters:

iElement

Line or plane specifying the direction. In case of plane, the plane

normal vector is the direction

Sub-element(s) supported (see

Boundary object): see RectilinearTriDimFeatEdge,

RectilinearBiDimFeatEdge and RectilinearMonoDimFeatEdge.

oDirection

Created direction.

Parameters:

i_element (Reference) –

Return type:

HybridShapeDirection

add_new_direction_by_coord(i_x: float, i_y: float, i_z: float) → HybridShapeDirection

Note

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

o Func AddNewDirectionByCoord(double iX,

double iY,

double iZ) As HybridShapeDirection

Creates a new Direction specifed by coordinates within the current

body.

Parameters:

iX

X component

iY

Y component

iZ

Z component

oDirection

Created direction

Parameters:

• i_x (float) –

• i_y (float) –

• i_z (float) –

Return type:

HybridShapeDirection

add_new_empty_rotate() → HybridShapeRotate

Note

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o Func AddNewEmptyRotate() As HybridShapeRotate

Creates a new empty Rotate within the current body.

Return type:

HybridShapeRotate

add_new_empty_translate() → HybridShapeTranslate

Note

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o Func AddNewEmptyTranslate() As HybridShapeTranslate

Creates a new empty Translate within the current body.

Return type:

HybridShapeTranslate

add_new_extract(element: Reference) → HybridShapeExtract

Note

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

o Func AddNewExtract(Reference Element) As

HybridShapeExtract

Creates a new Extract within the current body.

Parameters:

iElement

Initial element used to start the extraction

Sub-element(s) supported (see

Boundary object): see Boundary.

oExt

The extracted object

Parameters:

element (Reference) –

Return type:

HybridShapeExtract

add_new_extract_multi(element: Reference) → HybridShapeExtractMulti

Note

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

o Func AddNewExtractMulti(Reference Element) As

HybridShapeExtractMulti

Creates a new Multiple Extract within the current body.

Parameters:

iElement

Initial element used to start the extraction

Sub-element(s) supported (see

Boundary object): see Boundary.

oExt

The extracted object

Parameters:

element (Reference) –

Return type:

HybridShapeExtractMulti

add_new_extrapol_length(i_boundary: Reference, i_to_extrapol: Reference, i_length: float) → HybridShapeExtrapol

Note

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

o Func AddNewExtrapolLength(Reference iBoundary,

Reference iToExtrapol,

double iLength) As HybridShapeExtrapol

Creates a new Extrapol (specified by length) within the current

body.

Parameters:

iBoundary

Boundary point of curve to extrapolate or boundary curve of surface

to extrapolate.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iToExtrapol

Curve or surface to extrapolate.

Sub-element(s) supported (see Boundary object): see Face,

TriDimFeatEdge and BiDimFeatEdge.

iLength

Extrapolation length.

oExtrapol

Created Extrapolation.

Parameters:

• i_boundary (Reference) –

• i_to_extrapol (Reference) –

• i_length (float) –

Return type:

HybridShapeExtrapol

add_new_extrapol_until(i_boundary: Reference, i_to_extrapol: Reference, i_until: Reference) → HybridShapeExtrapol

Note

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

o Func AddNewExtrapolUntil(Reference iBoundary,

Reference iToExtrapol,

Reference iUntil) As HybridShapeExtrapol

Creates a new Extrapol (until an element) within the current

body.

Parameters:

iBoundary

Boundary point of curve to extrapolate or boundary curve of surface

to extrapolate.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iToExtrapol

Curve or surface to extrapolate.

Sub-element(s) supported (see Boundary object): see Face,

TriDimFeatEdge and BiDimFeatEdge.

iUntil

Extrapolation limit surface.

oExtrapol

Created Extrapolation.

Parameters:

• i_boundary (Reference) –

• i_to_extrapol (Reference) –

• i_until (Reference) –

Return type:

HybridShapeExtrapol

add_new_extremum(i_objet: Reference, i_dir: HybridShapeDirection, i_min_max: int) → HybridShapeExtremum

Note

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

o Func AddNewExtremum(Reference iObjet,

HybridShapeDirection iDir,

long iMinMax) As HybridShapeExtremum

Creates a new Extremum within the current body.

Parameters:

iObjet

Element onto extremum is computed

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge, BiDimFeatEdge and Face.

iDir

Extremum direction

iMinMax

Maximum (GSMMax) or Minimum (GSMMin)

oExt

The extremum object if succeded

Parameters:

• i_objet (Reference) –

• i_dir (HybridShapeDirection) –

• i_min_max (int) –

Return type:

HybridShapeExtremum

add_new_extremum_polar(i_type: int, ip_ia_contour: Reference) → HybridShapeExtremumPolar

Note

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

o Func AddNewExtremumPolar(short iType,

Reference ipIAContour) As HybridShapeExtremumPolar

Creates a new Extremum Polar within the current body.

Parameters:

iType

Type of extremum polar 0-Min Radius 1-Max Radius 2- Min Angle 3-

Maximum Angle

ipIAContour

Extremum Polar Contour. It should be non convex

opIAExtPolar

The extremum polar object if succeded

Parameters:

• i_type (int) –

• ip_ia_contour (Reference) –

Return type:

HybridShapeExtremumPolar

add_new_extrude(i_object_to_extrude: Reference, i_offset_debut: float, i_offset_fin: float, i_direction: HybridShapeDirection) → HybridShapeExtrude

Note

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

o Func AddNewExtrude(Reference iObjectToExtrude,

double iOffsetDebut,

double iOffsetFin,

HybridShapeDirection iDirection) As HybridShapeExtrude

Creates a new extrude within the current body.

Parameters:

iObjectToExtrude

Object to be extruded (point, line ,curve,or face)

Sub-element(s) supported (see

Boundary object): see Boundary.

iOffsetDebut

Length value

iOffsetFin

Length value ( iOffsetFin has to be larger than iOffsetDebut)

iDirection

Extrusion direction

oExtrudeObject

Extruded result

Parameters:

• i_object_to_extrude (Reference) –

• i_offset_debut (float) –

• i_offset_fin (float) –

• i_direction (HybridShapeDirection) –

Return type:

HybridShapeExtrude

add_new_fill() → HybridShapeFill

Note

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

o Func AddNewFill() As HybridShapeFill

Creates a new Fill within the current body.

Parameters:

oFill

Fill object

Return type:

HybridShapeFill

add_new_fillet_bi_tangent(i_element1: Reference, i_element2: Reference, i_radius: float, i_orientation1: int, i_orientation2: int, i_supports_trim_mode: int, i_ribbon_relimitation_mode: int) → HybridShapeFilletBiTangent

Note

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

o Func AddNewFilletBiTangent(Reference iElement1,

Reference iElement2,

double iRadius,

long iOrientation1,

long iOrientation2,

long iSupportsTrimMode,

long iRibbonRelimitationMode) As HybridShapeFilletBiTangent

Creates a new a sphere bitangent fillet between two skins.

Parameters:

iElement1

First support of fillet.

Sub-element(s) supported (see

Boundary object): see Face.

iElement2

Second support of fillet.

Sub-element(s) supported (see Boundary object): see

Face.

iRadius

Radius of the fillet.

iOrientation1

Manage the fillet center position.

iOrientation2

Manage the fillet center position.

iSupportsTrimMode

The 2 supports can be trimmed and assembled with the fillet. Value can

be 0 (No trim ) or 1 (Trim)

iRibbonRelimitationMode

Manage the relimition of fillet extremities.

Value can be : 0 (Smooth), 1 (Straight), 2 (Maximum) or 3 (Minimum)

oFillet

Created fillet.

Parameters:

• i_element1 (Reference) –

• i_element2 (Reference) –

• i_radius (float) –

• i_orientation1 (int) –

• i_orientation2 (int) –

• i_supports_trim_mode (int) –

• i_ribbon_relimitation_mode (int) –

Return type:

HybridShapeFilletBiTangent

add_new_fillet_tri_tangent(i_element1: Reference, i_element2: Reference, i_remove_elem: Reference, i_orientation1: int, i_orientation2: int, i_remove_orientation: int, i_supports_trim_mode: int, i_ribbon_relimitation_mode: int) → HybridShapeFilletTriTangent

Note

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

o Func AddNewFilletTriTangent(Reference iElement1,

Reference iElement2,

Reference iRemoveElem,

long iOrientation1,

long iOrientation2,

long iRemoveOrientation,

long iSupportsTrimMode,

long iRibbonRelimitationMode) As HybridShapeFilletTriTangent

Creates a new a tritangent fillet between three skins.

Parameters:

iElement1

First support of fillet.

Sub-element(s) supported (see

Boundary object): see Face.

iElement2

Second support of fillet.

Sub-element(s) supported (see Boundary object): see

Face.

iRemoveElem

Support to remove of fillet.

Sub-element(s) supported (see Boundary object): see

Face.

iOrientation1

Manage the fillet center position.

iOrientation2

Manage the fillet center position.

iRemoveOrientation

Manage the fillet center position.

iSupportsTrimMode

The 2 supports can be trimmed and assembled with the fillet. Value can

be 0 (No trim ) or 1 (Trim)

iRibbonRelimitationMode

Manage the relimition of fillet extremities.

Value can be : 0 (Smooth), 1 (Straight), 2 (Maximum) or 3 (Minimum)

oFillet

Created fillet.

Parameters:

• i_element1 (Reference) –

• i_element2 (Reference) –

• i_remove_elem (Reference) –

• i_orientation1 (int) –

• i_orientation2 (int) –

• i_remove_orientation (int) –

• i_supports_trim_mode (int) –

• i_ribbon_relimitation_mode (int) –

Return type:

HybridShapeFilletTriTangent

add_new_healing(i_body_toheal: Reference) → HybridShapeHealing

Note

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

o Func AddNewHealing(Reference iBodyToheal) As

HybridShapeHealing

Creates a new healing within the current body.

Parameters:

iBodyToHeal

The body to heal

oHealing

The created healing

Parameters:

i_body_toheal (Reference) –

Return type:

HybridShapeHealing

add_new_helix(i_axis: Reference, i_invert_axis: bool, i_starting_point: Reference, i_pitch: float, i_height: float, i_clockwise_revolution: bool, i_starting_angle: float, i_taper_angle: float, i_taper_outward: bool) → HybridShapeHelix

Note

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

o Func AddNewHelix(Reference iAxis,

boolean iInvertAxis,

Reference iStartingPoint,

double iPitch,

double iHeight,

boolean iClockwiseRevolution,

double iStartingAngle,

double iTaperAngle,

boolean iTaperOutward) As HybridShapeHelix

Creates a new Helix within the current body.

Parameters:

iAxis

The helix axis (always a line).

Sub-element(s) supported (see

Boundary object): see RectilinearTriDimFeatEdge and

RectilinearBiDimFeatEdge.

iInvertAxis

iStartingPoint

Starting Point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iPitch

Pitch.

iHeight

Helix height.

iClockwiseRevolution

Revolutions are clockwise if TRUE, counterclockwise if FALSE.

iStartingAngle

Starting angle from starting point measured on the helix itself. If no

starting angle is wanted, set it to 0.0.

iTaperAngle

0 <= Taper Angle < Pi/2 If no taper angle is wanted, set it to 0.0

(constant helix radius).

iTaperOutward

Helix radius increases if TRUE, decreases if FALSE.

oHelix

The Helix object if succeded

Parameters:

• i_axis (Reference) –

• i_invert_axis (bool) –

• i_starting_point (Reference) –

• i_pitch (float) –

• i_height (float) –

• i_clockwise_revolution (bool) –

• i_starting_angle (float) –

• i_taper_angle (float) –

• i_taper_outward (bool) –

Return type:

HybridShapeHelix

add_new_hybrid_scaling(i_elem_to_scale: Reference, i_center: Reference, i_ratio: float) → HybridShapeScaling

Note

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

o Func AddNewHybridScaling(Reference iElemToScale,

Reference iCenter,

double iRatio) As HybridShapeScaling

Creates a new scaling within the current body.

Parameters:

iElemToScale

Point, curve, surface or solid to transform.

Sub-element(s) supported (see

Boundary object): see Face, TriDimFeatEdge, BiDimFeatEdge and Vertex.

iCenter

Reference point or reference plane.

Sub-element(s) supported (see Boundary object): see PlanarFace and

Vertex.

iRatio

Scaling ratio.

oScaling

Created scaling.

Parameters:

• i_elem_to_scale (Reference) –

• i_center (Reference) –

• i_ratio (float) –

Return type:

HybridShapeScaling

add_new_hybrid_split(i_element1: Reference, i_element2: Reference, i_orientation: int) → HybridShapeSplit

Note

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

o Func AddNewHybridSplit(Reference iElement1,

Reference iElement2,

long iOrientation) As HybridShapeSplit

Creates a new Split within the current body.

Parameters:

iElement1

The feature to cut (curve or surface).

Sub-element(s) supported (see

Boundary object): see Face, TriDimFeatEdge and BiDimFeatEdge.

iElement2

The cutting feature (point, curve, surface).

Sub-element(s) supported (see Boundary object): see Face,

TriDimFeatEdge, BiDimFeatEdge and Vertex.

iOrientation

Manage the kept side of the feature to cut (value can be 1 or -1)

oSplit

Created split

Parameters:

• i_element1 (Reference) –

• i_element2 (Reference) –

• i_orientation (int) –

Return type:

HybridShapeSplit

add_new_hybrid_trim(i_element1: Reference, i_orientation1: int, i_element2: Reference, i_orientation2: int) → HybridShapeTrim

Note

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

o Func AddNewHybridTrim(Reference iElement1,

long iOrientation1,

Reference iElement2,

long iOrientation2) As HybridShapeTrim

Creates a new Trim within the current body by cutting and joining two

elements.

You can trim a surface by a surface or a curve by a curve.

Parameters:

iElement1

The feature to trim (curve or surface).

iOrientation1

Manage the kept side of iElement1 (value can be 1 or -1).

iElement2

The second feature to trim (curve or surface).

iOrientation2

Manage the kept side of iElement2 (value can be 1 or -1).

oTrim

Created trim.

Parameters:

• i_element1 (Reference) –

• i_orientation1 (int) –

• i_element2 (Reference) –

• i_orientation2 (int) –

Return type:

HybridShapeTrim

add_new_integrated_law(i_type: int) → HybridShapeIntegratedLaw

Note

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

o Func AddNewIntegratedLaw(long iType) As

HybridShapeIntegratedLaw

Creates Integrated Law.

Parameters:

iType

Type of law =

0 : None | 1 : Constant | 2 : Linear | 3 : SType | 4 : Advanced | 5 : Implicit

Parameters:

i_type (int) –

Return type:

HybridShapeIntegratedLaw

add_new_intersection(i_object1: Reference, i_object2: Reference) → HybridShapeIntersection

Note

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

o Func AddNewIntersection(Reference iObject1,

Reference iObject2) As HybridShapeIntersection

Creates a new Intersection within the current body.

Parameters:

iObject1

First element ( line, curve, plane, surface.

Sub-element(s) supported (see

Boundary object): see Face, RectilinearTriDimFeatEdge and

RectilinearBiDimFeatEdge.

iObject2

Second element ( line , curve, plane, surface.

Sub-element(s) supported (see Boundary object): see Face,

RectilinearTriDimFeatEdge and

RectilinearBiDimFeatEdge.

oIntersection

Intersection

Parameters:

• i_object1 (Reference) –

• i_object2 (Reference) –

Return type:

HybridShapeIntersection

add_new_inverse(element: Reference, inverse: int) → HybridShapeInverse

Note

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

o Func AddNewInverse(Reference Element,

long Inverse) As HybridShapeInverse

Creates a new Inverse within the current body.

Parameters:

iElement

The objet to inverse

iInverse

the type of inversion (see CATGSMOrientation.h) 1 for no inversion

-1 for inversion

oInv

The inverted object

Parameters:

• element (Reference) –

• inverse (int) –

Return type:

HybridShapeInverse

add_new_join(element1: Reference, element2: Reference) → HybridShapeAssemble

Note

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

o Func AddNewJoin(Reference Element1,

Reference Element2) As HybridShapeAssemble

Creates a new Join within the current body.

Parameters:

iElement1

First element to join ( curve or surface.

Sub-element(s) supported (see

Boundary object): see Face, TriDimFeatEdge and BiDimFeatEdge.

iElement2

Second element to join ( same type of the first

element)

Sub-element(s) supported (see Boundary object): see Face,

TriDimFeatEdge and BiDimFeatEdge.

oExt

Join result The default value used to join element is

0.001mm

Parameters:

• element1 (Reference) –

• element2 (Reference) –

Return type:

HybridShapeAssemble

add_new_law_dist_proj(i_reference: Reference, i_definition: Reference) → HybridShapeLawDistProj

Note

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

o Func AddNewLawDistProj(Reference iReference,

Reference iDefinition) As HybridShapeLawDistProj

Creates a new law within the current body.

Parameters:

iReference

Reference line of the law.

Sub-element(s) supported (see

Boundary object): see RectilinearTriDimFeatEdge and

RectilinearBiDimFeatEdge.

iDefinition

Definition curve of the law.

Sub-element(s) supported (see Boundary object): see TriDimFeatEdge and

BiDimFeatEdge.

oLaw

The Law object if succeded

Parameters:

• i_reference (Reference) –

• i_definition (Reference) –

Return type:

HybridShapeLawDistProj

add_new_line_angle(i_curve: Reference, i_surface: Reference, i_point: Reference, i_geodesic: bool, i_begin_offset: float, i_end_offset: float, i_angle: float, i_orientation: bool) → HybridShapeLineAngle

Note

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

o Func AddNewLineAngle(Reference iCurve,

Reference iSurface,

Reference iPoint,

boolean iGeodesic,

double iBeginOffset,

double iEndOffset,

double iAngle,

boolean iOrientation) As HybridShapeLineAngle

Creates a new angle line within the current body.

Parameters:

iCurve

Reference curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iSurface

Reference surface.

Sub-element(s) supported (see Boundary object): see

Face.

iPoint

reference point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iGeodesic

Puts the line on the surface

iBeginOffset

start offset

iEndOffset

end offset

iAngle

angle to reference curve

iOrientation

Orientation allows to reverse the line direction from the reference

point. For a line of L length, it is the same as creating this line with -L

length.

oLine

Created line

Parameters:

• i_curve (Reference) –

• i_surface (Reference) –

• i_point (Reference) –

• i_geodesic (bool) –

• i_begin_offset (float) –

• i_end_offset (float) –

• i_angle (float) –

• i_orientation (bool) –

Return type:

HybridShapeLineAngle

add_new_line_bi_tangent(i_curve1: Reference, i_element2: Reference, i_support: Reference) → HybridShapeLineBiTangent

Note

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

o Func AddNewLineBiTangent(Reference iCurve1,

Reference iElement2,

Reference iSupport) As HybridShapeLineBiTangent

Creates a new bitangent line within the current body.

Parameters:

iCurve1

First tangency curve lying on the support surface.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iCurve2

Second tangency element (point, curve) lying on the support

surface.

Sub-element(s) supported (see Boundary object): see TriDimFeatEdge,

BiDimFeatEdge and Vertex.

iSupport

The support surface of the two elements.

Sub-element(s) supported (see Boundary object): see

Face.

oLine

Created line

Parameters:

• i_curve1 (Reference) –

• i_element2 (Reference) –

• i_support (Reference) –

Return type:

HybridShapeLineBiTangent

add_new_line_bisecting(i_line1: Reference, i_line2: Reference, i_begin_offset: float, i_end_offset: float, i_orientation: bool, solution_nb: int) → HybridShapeLineBisecting

Note

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

o Func AddNewLineBisecting(Reference iLine1,

Reference iLine2,

double iBeginOffset,

double iEndOffset,

boolean iOrientation,

long SolutionNb) As HybridShapeLineBisecting

Creates a new bisecting line within the current body.

Parameters:

iLine1

First line.

Sub-element(s) supported (see

Boundary object): see RectilinearTriDimFeatEdge and

RectilinearBiDimFeatEdge.

iLine2

Second line.

Sub-element(s) supported (see Boundary object): see

RectilinearTriDimFeatEdge and

RectilinearBiDimFeatEdge.

iBeginOffset

start offset

iEndOffset

end offset

iOrientation

Orientation allows to reverse the line direction from the reference

point. For a line of L length, it is the same as creating this line with -L

length.

oLine

Created line

Parameters:

• i_line1 (Reference) –

• i_line2 (Reference) –

• i_begin_offset (float) –

• i_end_offset (float) –

• i_orientation (bool) –

• solution_nb (int) –

Return type:

HybridShapeLineBisecting

add_new_line_bisecting_on_support(i_line1: Reference, i_line2: Reference, i_surface: Reference, i_begin_offset: float, i_end_offset: float, i_orientation: bool, solution_nb: int) → HybridShapeLineBisecting

Note

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

o Func AddNewLineBisectingOnSupport(Reference iLine1,

Reference iLine2,

Reference iSurface,

double iBeginOffset,

double iEndOffset,

boolean iOrientation,

long SolutionNb) As HybridShapeLineBisecting

Creates a new bisecting line on a support within the current

body.

Parameters:

iLine1

First line.

Sub-element(s) supported (see

Boundary object): see RectilinearTriDimFeatEdge and

RectilinearBiDimFeatEdge.

iLine2

Second line.

Sub-element(s) supported (see Boundary object): see

RectilinearTriDimFeatEdge and

RectilinearBiDimFeatEdge.

iSurface

Reference surface.

Sub-element(s) supported (see Boundary object): see

Face.

iBeginOffset

start offset

iEndOffset

end offset

iOrientation

Orientation allows to reverse the line direction from the reference

point. For a line of L length, it is the same as creating this line with -L

length.

oLine

Created line

Parameters:

• i_line1 (Reference) –

• i_line2 (Reference) –

• i_surface (Reference) –

• i_begin_offset (float) –

• i_end_offset (float) –

• i_orientation (bool) –

• solution_nb (int) –

Return type:

HybridShapeLineBisecting

add_new_line_bisecting_on_support_with_point(i_line1: Reference, i_line2: Reference, i_ref_point: Reference, i_surface: Reference, i_begin_offset: float, i_end_offset: float, i_orientation: bool, solution_nb: int) → HybridShapeLineBisecting

Note

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

o Func AddNewLineBisectingOnSupportWithPoint(Reference

iLine1,

Reference iLine2,

Reference iRefPoint,

Reference iSurface,

double iBeginOffset,

double iEndOffset,

boolean iOrientation,

long SolutionNb) As HybridShapeLineBisecting

Creates a new bisecting line on a support with a atarting point within the

current body.

Parameters:

iLine1

First line.

Sub-element(s) supported (see

Boundary object): see RectilinearTriDimFeatEdge and

RectilinearBiDimFeatEdge.

iLine2

Second line.

Sub-element(s) supported (see Boundary object): see

RectilinearTriDimFeatEdge and

RectilinearBiDimFeatEdge.

iRefPoint

Starting point of the bisecting line.

Sub-element(s) supported (see Boundary object): see

Vertex.

iSurface

Reference surface.

Sub-element(s) supported (see Boundary object): see

Face.

iBeginOffset

start offset

iEndOffset

end offset

iOrientation

Orientation allows to reverse the line direction from the reference

point. For a line of L length, it is the same as creating this line with -L

length.

oLine

Created line

Parameters:

• i_line1 (Reference) –

• i_line2 (Reference) –

• i_ref_point (Reference) –

• i_surface (Reference) –

• i_begin_offset (float) –

• i_end_offset (float) –

• i_orientation (bool) –

• solution_nb (int) –

Return type:

HybridShapeLineBisecting

add_new_line_bisecting_with_point(i_line1: Reference, i_line2: Reference, i_ref_point: Reference, i_begin_offset: float, i_end_offset: float, i_orientation: bool, solution_nb: int) → HybridShapeLineBisecting

Note

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

o Func AddNewLineBisectingWithPoint(Reference iLine1,

Reference iLine2,

Reference iRefPoint,

double iBeginOffset,

double iEndOffset,

boolean iOrientation,

long SolutionNb) As HybridShapeLineBisecting

Creates a new bisecting line with a starting point within the current

body.

Parameters:

iLine1

First line.

Sub-element(s) supported (see

Boundary object): see RectilinearTriDimFeatEdge and

RectilinearBiDimFeatEdge.

iLine2

Second line.

Sub-element(s) supported (see Boundary object): see

RectilinearTriDimFeatEdge and

RectilinearBiDimFeatEdge.

iRefPoint

Starting point of the bisecting line.

Sub-element(s) supported (see Boundary object): see

Vertex.

iBeginOffset

start offset

iEndOffset

end offset

iOrientation

Orientation allows to reverse the line direction from the reference

point. For a line of L length, it is the same as creating this line with -L

length.

oLine

Created line

Parameters:

• i_line1 (Reference) –

• i_line2 (Reference) –

• i_ref_point (Reference) –

• i_begin_offset (float) –

• i_end_offset (float) –

• i_orientation (bool) –

• solution_nb (int) –

Return type:

HybridShapeLineBisecting

add_new_line_datum(i_object: Reference) → HybridShapeLineExplicit

Note

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

o Func AddNewLineDatum(Reference iObject) As

HybridShapeLineExplicit

Creates a new datum of line within the current body.

Parameters:

iObject

The object whose topological body will be duplicated and put into

created datum

oLine

Created datum Note2: the object passed as parameter to create the

datum has to be in the current container. Otherwise, an error

occurs.

Parameters:

i_object (Reference) –

Return type:

HybridShapeLineExplicit

add_new_line_normal(i_surface: Reference, i_point: Reference, i_begin_offset: float, i_end_offset: float, i_orientation: bool) → HybridShapeLineNormal

Note

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

o Func AddNewLineNormal(Reference iSurface,

Reference iPoint,

double iBeginOffset,

double iEndOffset,

boolean iOrientation) As HybridShapeLineNormal

Creates a new normal line within the current body.

Parameters:

iSurface

Reference surface.

Sub-element(s) supported (see

Boundary object): see Face.

iPoint

Reference point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iBeginOffset

start offset

iEndOffset

end offset

iOrientation

Orientation allows to reverse the line direction from the reference

point. For a line of L length, it is the same as creating this line with -L

length.

oLine

Created line

Parameters:

• i_surface (Reference) –

• i_point (Reference) –

• i_begin_offset (float) –

• i_end_offset (float) –

• i_orientation (bool) –

Return type:

HybridShapeLineNormal

add_new_line_pt_dir(i_pt: Reference, i_direction: HybridShapeDirection, i_begin_offset: float, i_end_offset: float, i_orientation: bool) → HybridShapeLinePtDir

Note

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

o Func AddNewLinePtDir(Reference iPt,

HybridShapeDirection iDirection,

double iBeginOffset,

double iEndOffset,

boolean iOrientation) As HybridShapeLinePtDir

Creates a new point-direction line within the current

body.

Parameters:

iPt

reference point.

Sub-element(s) supported (see

Boundary object): see Vertex.

iDirection

Direction

iBeginOffset

start offset

iEndOffset

end offset

iOrientation

Orientation allows to reverse the line direction from the reference

point. For a line of L length, it is the same as creating this line with -L

length.

oLine

Created line

Parameters:

• i_pt (Reference) –

• i_direction (HybridShapeDirection) –

• i_begin_offset (float) –

• i_end_offset (float) –

• i_orientation (bool) –

Return type:

HybridShapeLinePtDir

add_new_line_pt_dir_on_support(i_pt: Reference, i_direction: HybridShapeDirection, i_support: Reference, i_begin_offset: float, i_end_offset: float, i_orientation: bool) → HybridShapeLinePtDir

Note

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

o Func AddNewLinePtDirOnSupport(Reference iPt,

HybridShapeDirection iDirection,

Reference iSupport,

double iBeginOffset,

double iEndOffset,

boolean iOrientation) As HybridShapeLinePtDir

Creates a new point-direction line within the current

body.

Parameters:

iPt

reference point.

Sub-element(s) supported (see

Boundary object): see Vertex.

iDirection

Direction

iSupport

Support element (surface or plane)

Sub-element(s) supported (see Boundary object): see

Face.

iBeginOffset

start offset

iEndOffset

end offset

iOrientation

Orientation allows to reverse the line direction from the reference

point. For a line of L length, it is the same as creating this line with -L

length.

oLine

Created line

Parameters:

• i_pt (Reference) –

• i_direction (HybridShapeDirection) –

• i_support (Reference) –

• i_begin_offset (float) –

• i_end_offset (float) –

• i_orientation (bool) –

Return type:

HybridShapeLinePtDir

add_new_line_pt_pt(i_pt_origine: Reference, i_pt_extremite: Reference) → HybridShapeLinePtPt

Note

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

o Func AddNewLinePtPt(Reference iPtOrigine,

Reference iPtExtremite) As HybridShapeLinePtPt

Creates a new point-point line within the current body.

Parameters:

iPtOrigine

Origin point.

Sub-element(s) supported (see

Boundary object): see Vertex.

iPtExtremite

Extremity point.

Sub-element(s) supported (see Boundary object): see

Vertex.

oLine

Created line

Parameters:

• i_pt_origine (Reference) –

• i_pt_extremite (Reference) –

Return type:

HybridShapeLinePtPt

add_new_line_pt_pt_extended(i_pt_origine: Reference, i_pt_extremite: Reference, i_begin_offset: float, i_end_offset: float) → HybridShapeLinePtPt

Note

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

o Func AddNewLinePtPtExtended(Reference iPtOrigine,

Reference iPtExtremite,

double iBeginOffset,

double iEndOffset) As HybridShapeLinePtPt

Creates a new point-point line with extensions within the current

body.

Parameters:

iPtOrigine

Origin point.

Sub-element(s) supported (see

Boundary object): see Vertex.

iPtExtremite

Extremity point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iBeginOffset

start offset

iEndOffset

end offset

oLine

Created line

Parameters:

• i_pt_origine (Reference) –

• i_pt_extremite (Reference) –

• i_begin_offset (float) –

• i_end_offset (float) –

Return type:

HybridShapeLinePtPt

add_new_line_pt_pt_on_support(i_pt_origine: Reference, i_pt_extremite: Reference, i_support: Reference) → HybridShapeLinePtPt

Note

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

o Func AddNewLinePtPtOnSupport(Reference iPtOrigine,

Reference iPtExtremite,

Reference iSupport) As HybridShapeLinePtPt

Creates a new point-point line with support within the current

body.

Parameters:

iPtOrigine

Origin point.

Sub-element(s) supported (see

Boundary object): see Vertex.

iPtExtremite

Extremity point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iSupport

Support element (surface or plane)

Sub-element(s) supported (see Boundary object): see

Face.

oLine

Created line

Parameters:

• i_pt_origine (Reference) –

• i_pt_extremite (Reference) –

• i_support (Reference) –

Return type:

HybridShapeLinePtPt

add_new_line_pt_pt_on_support_extended(i_pt_origine: Reference, i_pt_extremite: Reference, i_support: Reference, i_begin_offset: float, i_end_offset: float) → HybridShapeLinePtPt

Note

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

o Func AddNewLinePtPtOnSupportExtended(Reference iPtOrigine,

Reference iPtExtremite,

Reference iSupport,

double iBeginOffset,

double iEndOffset) As HybridShapeLinePtPt

Creates a new point-point line with extensions and with support within the

current body.

Parameters:

iPtOrigine

Origin point.

Sub-element(s) supported (see

Boundary object): see Vertex.

iPtExtremite

Extremity point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iSupport

Support element (surface or plane)

Sub-element(s) supported (see Boundary object): see

Face.

iBeginOffset

start offset

iEndOffset

end offset

oLine

Created line

Parameters:

• i_pt_origine (Reference) –

• i_pt_extremite (Reference) –

• i_support (Reference) –

• i_begin_offset (float) –

• i_end_offset (float) –

Return type:

HybridShapeLinePtPt

add_new_line_tangency(i_curve: Reference, i_point: Reference, i_begin_offset: float, i_end_offset: float, i_orientation: bool) → HybridShapeLineTangency

Note

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

o Func AddNewLineTangency(Reference iCurve,

Reference iPoint,

double iBeginOffset,

double iEndOffset,

boolean iOrientation) As HybridShapeLineTangency

Creates a new tangent line within the current body.

Parameters:

iCurve

Reference curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iPoint

Reference point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iBeginOffset

start offset

iEndOffset

end offset

iOrientation

Orientation allows to reverse the line direction from the reference

point. For a line of L length, it is the same as creating this line with -L

length.

oLine

Created line

Parameters:

• i_curve (Reference) –

• i_point (Reference) –

• i_begin_offset (float) –

• i_end_offset (float) –

• i_orientation (bool) –

Return type:

HybridShapeLineTangency

add_new_line_tangency_on_support(i_curve: Reference, i_point: Reference, i_support: Reference, i_begin_offset: float, i_end_offset: float, i_orientation: bool) → HybridShapeLineTangency

Note

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

o Func AddNewLineTangencyOnSupport(Reference iCurve,

Reference iPoint,

Reference iSupport,

double iBeginOffset,

double iEndOffset,

boolean iOrientation) As HybridShapeLineTangency

Creates a new tangent line within the current body.

Parameters:

iCurve

Reference curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iPoint

Reference point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iSupport

Support element (surface or plane)

Sub-element(s) supported (see Boundary object): see

Face.

iBeginOffset

start offset

iEndOffset

end offset

iOrientation

Orientation allows to reverse the line direction from the reference

point. For a line of L length, it is the same as creating this line with -L

length.

oLine

Created line

Parameters:

• i_curve (Reference) –

• i_point (Reference) –

• i_support (Reference) –

• i_begin_offset (float) –

• i_end_offset (float) –

• i_orientation (bool) –

Return type:

HybridShapeLineTangency

add_new_loft() → HybridShapeLoft

Note

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

o Func AddNewLoft() As HybridShapeLoft

Creates a new Loft within the current body.

Parameters:

oExt

CATIAHybridShapeLoft created

Return type:

HybridShapeLoft

add_new_mid_surface(i_support: Reference, i_creation_mode: int, i_threshold: float) → HybridShapeMidSurface

Note

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

o Func AddNewMidSurface(Reference iSupport,

long iCreationMode,

double iThreshold) As HybridShapeMidSurface

Creates a new MidSurface in Automatic Creation Mode Only.

Parameters:

iSupport

support Body

iCreationMode

Creation Mode (Only Automatic Accepted)

iThreshold

Threshold Thickness

Returns:

oMidSurface Created MidSurface

Parameters:

• i_support (Reference) –

• i_creation_mode (int) –

• i_threshold (float) –

Return type:

HybridShapeMidSurface

add_new_mid_surface_with_auto_threshold(i_support: Reference, i_creation_mode: int, i_threshold: float, i_auto_thickness_threshold: int) → HybridShapeMidSurface

Note

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

o Func AddNewMidSurfaceWithAutoThreshold(Reference iSupport,

long iCreationMode,

double iThreshold,

long iAutoThicknessThreshold) As HybridShapeMidSurface

Creates a new MidSurface in Automatic Creation Mode Only.

Parameters:

iSupport

support Body

iCreationMode

Creation Mode (Only Automatic Accepted)

iThreshold

Threshold Thickness

iAutoThicknessThreshold

Automatic Thickness Threshold

Returns:

oMidSurface Created MidSurface

Parameters:

• i_support (Reference) –

• i_creation_mode (int) –

• i_threshold (float) –

• i_auto_thickness_threshold (int) –

Return type:

HybridShapeMidSurface

add_new_near(multi_element: Reference, reference_element: Reference) → HybridShapeNear

Note

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

o Func AddNewNear(Reference MultiElement,

Reference ReferenceElement) As HybridShapeNear

Creates a new Near within the current body.

Parameters:

iMultiElement

Non connex element (point,curve,surface.

Sub-element(s) supported (see

Boundary object): see Face, TriDimFeatEdge, BiDimFeatEdge and Vertex.

iReferenceElement

Reference element

Sub-element(s) supported (see Boundary object): see Face,

TriDimFeatEdge, BiDimFeatEdge and Vertex.

oNear

The result is the connex component that is the nearest from the

reference element

Parameters:

• multi_element (Reference) –

• reference_element (Reference) –

Return type:

HybridShapeNear

add_new_offset(i_object_to_offset: Reference, i_offset: float, i_orientation: bool, i_precision: float) → HybridShapeOffset

Note

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

o Func AddNewOffset(Reference iObjectToOffset,

double iOffset,

boolean iOrientation,

double iPrecision) As HybridShapeOffset

Creates a new offset within the current body.

Parameters:

iObjectToOffset

Surface to offset.

Sub-element(s) supported (see

Boundary object): see Face.

iOffset

Offset value

iOrientation

Offset orientation

iPrecision

This variable is no longer in use and any change in it’s value does not

impact the output.

oOffsetObject

Offset Surface

Parameters:

• i_object_to_offset (Reference) –

• i_offset (float) –

• i_orientation (bool) –

• i_precision (float) –

Return type:

HybridShapeOffset

add_new_plane1_curve(i_planar_curve: Reference) → HybridShapePlane1Curve

Note

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

o Func AddNewPlane1Curve(Reference iPlanarCurve) As

HybridShapePlane1Curve

Creates a new plane passing through one planar curve within the current

body.

Parameters:

iPlanarCurve

passing curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

oPlane

Created plane

Parameters:

i_planar_curve (Reference) –

Return type:

HybridShapePlane1Curve

add_new_plane1_line1_pt(i_ln: Reference, i_pt: Reference) → HybridShapePlane1Line1Pt

Note

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

o Func AddNewPlane1Line1Pt(Reference iLn,

Reference iPt) As HybridShapePlane1Line1Pt

Creates a new plane passing through 1 line and 1 point within the current

body.

Parameters:

iLn

passing line.

Sub-element(s) supported (see

Boundary object): see RectilinearTriDimFeatEdge,

RectilinearBiDimFeatEdge and RectilinearMonoDimFeatEdge.

iPt

passing point.

Sub-element(s) supported (see Boundary object): see

Vertex.

oPlane

Created plane

Parameters:

• i_ln (Reference) –

• i_pt (Reference) –

Return type:

HybridShapePlane1Line1Pt

add_new_plane2_lines(i_ln1: Reference, i_ln2: Reference) → HybridShapePlane2Lines

Note

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

o Func AddNewPlane2Lines(Reference iLn1,

Reference iLn2) As HybridShapePlane2Lines

Creates a new plane passing through 2 lines within the current

body.

Parameters:

iLn1

first passing line.

Sub-element(s) supported (see

Boundary object): see RectilinearTriDimFeatEdge,

RectilinearBiDimFeatEdge and RectilinearMonoDimFeatEdge.

iLn2

second passing line.

Sub-element(s) supported (see Boundary object): see

RectilinearTriDimFeatEdge, RectilinearBiDimFeatEdge and

RectilinearMonoDimFeatEdge.

oPlane

Created line

Parameters:

• i_ln1 (Reference) –

• i_ln2 (Reference) –

Return type:

HybridShapePlane2Lines

add_new_plane3_points(i_pt1: Reference, i_pt2: Reference, i_pt3: Reference) → HybridShapePlane3Points

Note

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

o Func AddNewPlane3Points(Reference iPt1,

Reference iPt2,

Reference iPt3) As HybridShapePlane3Points

Creates a new plane passing through 3 points within the current

body.

Parameters:

iPt1

first passing point.

Sub-element(s) supported (see

Boundary object): see Vertex.

iPt2

second passing point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iPt3

third passing point.

Sub-element(s) supported (see Boundary object): see

Vertex.

oPlane

Created plane

Parameters:

• i_pt1 (Reference) –

• i_pt2 (Reference) –

• i_pt3 (Reference) –

Return type:

HybridShapePlane3Points

add_new_plane_angle(i_plane: Reference, i_revol_axis: Reference, i_angle: float, i_orientation: bool) → HybridShapePlaneAngle

Note

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

o Func AddNewPlaneAngle(Reference iPlane,

Reference iRevolAxis,

double iAngle,

boolean iOrientation) As HybridShapePlaneAngle

Creates a new angle plane within the current body.

Parameters:

iPlane

reference plane

Sub-element(s) supported (see

Boundary object): see PlanarFace.

iRevolAxis

rotation axis

Sub-element(s) supported (see Boundary object): see

RectilinearTriDimFeatEdge, RectilinearBiDimFeatEdge and

RectilinearMonoDimFeatEdge.

iAngle

angle

iOrientation

Orientation to reverse the plane from the reference plane.

oPlane

Created plane

Parameters:

• i_plane (Reference) –

• i_revol_axis (Reference) –

• i_angle (float) –

• i_orientation (bool) –

Return type:

HybridShapePlaneAngle

add_new_plane_datum(i_object: Reference) → HybridShapePlaneExplicit

Note

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

o Func AddNewPlaneDatum(Reference iObject) As

HybridShapePlaneExplicit

Creates a new datum of plane within the current body.

Parameters:

iObject

The object whose topological body will be duplicated and put into

created datum

oPlane

Created datum Note2: the object passed as parameter to create the

datum has to be in the current container. Otherwise, an error

occurs.

Parameters:

i_object (Reference) –

Return type:

HybridShapePlaneExplicit

add_new_plane_equation(i_a_coeff: float, i_b_coeff: float, i_c_coeff: float, i_d_coeff: float) → HybridShapePlaneEquation

Note

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

o Func AddNewPlaneEquation(double iA_Coeff,

double iB_Coeff,

double iC_Coeff,

double iD_Coeff) As HybridShapePlaneEquation

Creates a new equation plane within the current body. Plane equation is Ax+By+Cz = D.

Parameters:

iA_Coeff

A coefficient

iB_Coeff

B coefficient

iC_Coeff

C coefficient

iD_Coeff

D coefficient

oPlane

Created plane

Parameters:

• i_a_coeff (float) –

• i_b_coeff (float) –

• i_c_coeff (float) –

• i_d_coeff (float) –

Return type:

HybridShapePlaneEquation

add_new_plane_mean(i_list_of_points: tuple, nb_point: int) → HybridShapePlaneMean

Note

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

o Func AddNewPlaneMean(CATSafeArrayVariant iListOfPoints,

long NbPoint) As HybridShapePlaneMean

Creates a new mean through points plane within the current

body.

Parameters:

oIListOfPoints

list of passing points Warning : Input and Output parameter for CATScript applications,

procedural type

iNbPoint

Number of points

oPlane

Created plane

Parameters:

• i_list_of_points (tuple) –

• nb_point (int) –

Return type:

HybridShapePlaneMean

add_new_plane_normal(i_curve: Reference, i_pt: Reference) → HybridShapePlaneNormal

Note

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

o Func AddNewPlaneNormal(Reference iCurve,

Reference iPt) As HybridShapePlaneNormal

Creates a new normal plane within the current body.

Parameters:

iCurve

Reference curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iPt

Reference point.

Sub-element(s) supported (see Boundary object): see

Vertex.

oPlane

Created plane

Parameters:

• i_curve (Reference) –

• i_pt (Reference) –

Return type:

HybridShapePlaneNormal

add_new_plane_offset(i_plane: Reference, i_offset: float, i_orientation: bool) → HybridShapePlaneOffset

Note

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

o Func AddNewPlaneOffset(Reference iPlane,

double iOffset,

boolean iOrientation) As HybridShapePlaneOffset

Creates a new offset plane within the current body.

Parameters:

iPlane

reference plane

Sub-element(s) supported (see

Boundary object): see PlanarFace.

iOffset

offset value

iOrientation

Orientation to reverse the plane from the reference plane.

oPlane

Created plane

Parameters:

• i_plane (Reference) –

• i_offset (float) –

• i_orientation (bool) –

Return type:

HybridShapePlaneOffset

add_new_plane_offset_pt(i_plane: Reference, i_pt: Reference) → HybridShapePlaneOffsetPt

Note

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

o Func AddNewPlaneOffsetPt(Reference iPlane,

Reference iPt) As HybridShapePlaneOffsetPt

Creates a new offset trough point plane within the current

body.

Parameters:

iPlane

reference plane

Sub-element(s) supported (see

Boundary object): see PlanarFace.

iPt

Reference point.

Sub-element(s) supported (see Boundary object): see

Vertex.

oPlane

Created plane

Parameters:

• i_plane (Reference) –

• i_pt (Reference) –

Return type:

HybridShapePlaneOffsetPt

add_new_plane_tangent(i_surface: Reference, i_pt: Reference) → HybridShapePlaneTangent

Note

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

o Func AddNewPlaneTangent(Reference iSurface,

Reference iPt) As HybridShapePlaneTangent

Creates a new tangent plane within the current body.

Parameters:

iSurface

reference surface.

Sub-element(s) supported (see

Boundary object): see Face.

iPt

reference point.

Sub-element(s) supported (see Boundary object): see

Vertex.

oPlane

Created plane

Parameters:

• i_surface (Reference) –

• i_pt (Reference) –

Return type:

HybridShapePlaneTangent

add_new_point_between(i_point1: Reference, i_point2: Reference, i_ratio: float, i_orientation: int) → HybridShapePointBetween

Note

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

o Func AddNewPointBetween(Reference iPoint1,

Reference iPoint2,

double iRatio,

long iOrientation) As HybridShapePointBetween

Creates a new PointBetween within the current body.

Parameters:

iPoint1

Reference point to compute the barycenter.

Sub-element(s) supported (see

Boundary object): see Vertex.

iPoint2

Second point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iRatio

barycenter parameter

iOrientation

To compute the barycenter of the segment [Pt1 - Pt2]

oPoint

PointBetween if succeded

Parameters:

• i_point1 (Reference) –

• i_point2 (Reference) –

• i_ratio (float) –

• i_orientation (int) –

Return type:

HybridShapePointBetween

add_new_point_center(i_curve: Reference) → HybridShapePointCenter

Note

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

o Func AddNewPointCenter(Reference iCurve) As

HybridShapePointCenter

Creates a new circle center point within the current body.

Parameters:

iCurve

Reference circle

Sub-element(s) supported (see

Boundary object): see Edge.

oPoint

Created point

Parameters:

i_curve (Reference) –

Return type:

HybridShapePointCenter

add_new_point_coord(i_x: float, i_y: float, i_z: float) → HybridShapePointCoord

Note

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

o Func AddNewPointCoord(double iX,

double iY,

double iZ) As HybridShapePointCoord

Creates a new point defined by its cartesian coordinates within the current

body.

Parameters:

iX

X coordinate for the point

iY

Y coordinate for the point

iZ

Z coordinate for the point

oPoint

Created point

Parameters:

• i_x (float) –

• i_y (float) –

• i_z (float) –

Return type:

HybridShapePointCoord

add_new_point_coord_with_reference(i_x: float, i_y: float, i_z: float, i_pt: Reference) → HybridShapePointCoord

Note

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

o Func AddNewPointCoordWithReference(double iX,

double iY,

double iZ,

Reference iPt) As HybridShapePointCoord

Creates a new point defined its the cartesian coordinates regarding a

reference point.

Parameters:

iX

X coordinate for the point

iY

Y coordinate for the point

iZ

Z coordinate for the point

iPt

Reference point.

Sub-element(s) supported (see

Boundary object): see Vertex.

oPoint

Created point

Parameters:

• i_x (float) –

• i_y (float) –

• i_z (float) –

• i_pt (Reference) –

Return type:

HybridShapePointCoord

add_new_point_coords(coord_list)

coord_list must be a list of iterables of length 3. Example: coord_list = [[0, 0, 1], [0, 1, 0]] :param list() coord_list: :returns: list[HybridShapePointCoord]

add_new_point_datum(i_object: Reference) → HybridShapePointExplicit

Note

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

o Func AddNewPointDatum(Reference iObject) As

HybridShapePointExplicit

Creates a new datum of point within the current body.

Parameters:

iObject

The object whose topological body will be duplicated and put into

created datum

oPoint

Created datum Note2: the object passed as parameter to create the

datum has to be in the current container. Otherwise, an error

occurs.

Parameters:

i_object (Reference) –

Return type:

HybridShapePointExplicit

add_new_point_on_curve_along_direction(i_crv: Reference, i_long: float, i_orientation: bool, i_direction: HybridShapeDirection) → HybridShapePointOnCurve

Note

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

o Func AddNewPointOnCurveAlongDirection(Reference iCrv,

double iLong,

boolean iOrientation,

HybridShapeDirection iDirection) As HybridShapePointOnCurve

Creates a new point on a curve with a deafult origin point and from a

distance along direction.

Parameters:

iCrv

support curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iLong

distance to default origin point.(origin of acurrent axis system)

iOrientation

Orientation = TRUE means that distance is measured in the other orientation of the curve.

iDirection

Direction = The distance at which point is created is measured in this direction.

oPoint

Created point

Parameters:

• i_crv (Reference) –

• i_long (float) –

• i_orientation (bool) –

• i_direction (HybridShapeDirection) –

Return type:

HybridShapePointOnCurve

add_new_point_on_curve_from_distance(i_crv: Reference, i_long: float, i_orientation: bool) → HybridShapePointOnCurve

Note

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

o Func AddNewPointOnCurveFromDistance(Reference iCrv,

double iLong,

boolean iOrientation) As HybridShapePointOnCurve

Creates a new point on a curve from a distance to an extremity within the

current body.

Parameters:

iCrv

support curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iLong

distance to extremity

iOrientation

Orientation = TRUE means that distance is measured in the other orientation of the curve and

from the other extremity.

oPoint

Created point

Parameters:

• i_crv (Reference) –

• i_long (float) –

• i_orientation (bool) –

Return type:

HybridShapePointOnCurve

add_new_point_on_curve_from_percent(i_crv: Reference, i_long: float, i_orientation: bool) → HybridShapePointOnCurve

Note

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

o Func AddNewPointOnCurveFromPercent(Reference iCrv,

double iLong,

boolean iOrientation) As HybridShapePointOnCurve

Creates a new point on a curve from a ratio of distance to an extremity

within the current body.

Parameters:

iCrv

support curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iLong

Ratio of curve length

iOrientation

Orientation = TRUE means that ratio is measured in the other orientation of the curve and

from the other extremity.

oPoint

Created point

Parameters:

• i_crv (Reference) –

• i_long (float) –

• i_orientation (bool) –

Return type:

HybridShapePointOnCurve

add_new_point_on_curve_with_reference_along_direction(i_crv: Reference, i_pt: Reference, i_long: float, i_orientation: bool, i_direction: HybridShapeDirection) → HybridShapePointOnCurve

Note

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

o Func AddNewPointOnCurveWithReferenceAlongDirection(Reference

iCrv,

Reference iPt,

double iLong,

boolean iOrientation,

HybridShapeDirection iDirection) As HybridShapePointOnCurve

Creates a new point on a curve with a reference point and from a distance

along direction.

Parameters:

iCrv

support curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iPt

reference point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iLong

distance (length) to reference point

iOrientation

Orientation = TRUE means that distance is measured in the other orientation of the curve

iDirection

Direction = The distance at which point is created is measured in this direction.

oPoint

Created point

Parameters:

• i_crv (Reference) –

• i_pt (Reference) –

• i_long (float) –

• i_orientation (bool) –

• i_direction (HybridShapeDirection) –

Return type:

HybridShapePointOnCurve

add_new_point_on_curve_with_reference_from_distance(i_crv: Reference, i_pt: Reference, i_long: float, i_orientation: bool) → HybridShapePointOnCurve

Note

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

o Func AddNewPointOnCurveWithReferenceFromDistance(Reference

iCrv,

Reference iPt,

double iLong,

boolean iOrientation) As HybridShapePointOnCurve

Creates a new point on a curve with a reference point and from a distance

within the current body.

Parameters:

iCrv

support curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iPt

reference point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iLong

distance (length) to reference point

iOrientation

Orientation = TRUE means that distance is measured in the other orientation of the curve

oPoint

Created point

Parameters:

• i_crv (Reference) –

• i_pt (Reference) –

• i_long (float) –

• i_orientation (bool) –

Return type:

HybridShapePointOnCurve

add_new_point_on_curve_with_reference_from_percent(i_crv: Reference, i_pt: Reference, i_long: float, i_orientation: bool) → HybridShapePointOnCurve

Note

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

o Func AddNewPointOnCurveWithReferenceFromPercent(Reference

iCrv,

Reference iPt,

double iLong,

boolean iOrientation) As HybridShapePointOnCurve

Creates a new point on a curve with a reference point and from a ratio of

distance within the current body.

Parameters:

iCrv

Support curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iPt

reference point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iLong

Ratio of curve length

iOrientation

Orientation = TRUE means that ratio is measured in the other orientation of the curve

oPoint

Created point

Parameters:

• i_crv (Reference) –

• i_pt (Reference) –

• i_long (float) –

• i_orientation (bool) –

Return type:

HybridShapePointOnCurve

add_new_point_on_plane(i_plane: Reference, i_x: float, i_y: float) → HybridShapePointOnPlane

Note

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

o Func AddNewPointOnPlane(Reference iPlane,

double iX,

double iY) As HybridShapePointOnPlane

Creates a new point on a plane within the current body.

Parameters:

iPlane

Support plane

Sub-element(s) supported (see

Boundary object): see PlanarFace.

iX

X cartesian coordinates in the plane.

iY

Y cartesian coordinates in the plane.

oPoint

Created point

Parameters:

• i_plane (Reference) –

• i_x (float) –

• i_y (float) –

Return type:

HybridShapePointOnPlane

add_new_point_on_plane_with_reference(i_plane: Reference, i_pt: Reference, i_x: float, i_y: float) → HybridShapePointOnPlane

Note

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

o Func AddNewPointOnPlaneWithReference(Reference iPlane,

Reference iPt,

double iX,

double iY) As HybridShapePointOnPlane

Creates a new point on a plane with a reference point within the current

body.

Parameters:

iPlane

Support plane

Sub-element(s) supported (see

Boundary object): see PlanarFace.

iPt

Reference plane

Sub-element(s) supported (see Boundary object): see

Vertex.

iX

X cartesian coordinates in the plane.

iY

Y cartesian coordinates in the plane.

oPoint

Created point

Parameters:

• i_plane (Reference) –

• i_pt (Reference) –

• i_x (float) –

• i_y (float) –

Return type:

HybridShapePointOnPlane

add_new_point_on_surface(i_surface: Reference, i_direction: HybridShapeDirection, i_x: float) → HybridShapePointOnSurface

Note

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

o Func AddNewPointOnSurface(Reference iSurface,

HybridShapeDirection iDirection,

double iX) As HybridShapePointOnSurface

Creates a new point on a surface within the current body.

Parameters:

iSurface

Support surface.

Sub-element(s) supported (see

Boundary object): see Face.

iDirection

Direction from the reference point in which the point is computed.

iX

geodesic length to reference point

oPoint

Created point

Parameters:

• i_surface (Reference) –

• i_direction (HybridShapeDirection) –

• i_x (float) –

Return type:

HybridShapePointOnSurface

add_new_point_on_surface_with_reference(i_surface: Reference, i_pt: Reference, i_direction: HybridShapeDirection, i_x: float) → HybridShapePointOnSurface

Note

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

o Func AddNewPointOnSurfaceWithReference(Reference iSurface,

Reference iPt,

HybridShapeDirection iDirection,

double iX) As HybridShapePointOnSurface

Creates a new point on a surface with a reference point within the current

body.

Parameters:

iSurface

Support surface.

Sub-element(s) supported (see

Boundary object): see Face.

iPt

reference point.

Sub-element(s) supported (see Boundary object): see

Vertex.

iDirection

Direction from the reference point in which the point is computed.

iX

geodesic length to reference point

oPoint

Created point

Parameters:

• i_surface (Reference) –

• i_pt (Reference) –

• i_direction (HybridShapeDirection) –

• i_x (float) –

Return type:

HybridShapePointOnSurface

add_new_point_tangent(i_curve: Reference, i_direction: HybridShapeDirection) → HybridShapePointTangent

Note

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

o Func AddNewPointTangent(Reference iCurve,

HybridShapeDirection iDirection) As HybridShapePointTangent

Creates a new tangent to curve point within the current

body.

Parameters:

iCurve

Reference curve.

Sub-element(s) supported (see

Boundary object): see Edge.

iDirection

Direction in which tangent points are computed

oPoint

Created point

Parameters:

• i_curve (Reference) –

• i_direction (HybridShapeDirection) –

Return type:

HybridShapePointTangent

add_new_polyline() → HybridShapePolyline

Note

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

o Func AddNewPolyline() As HybridShapePolyline

Creates a new Polyline within the current body.

Parameters:

oPolyline

The Polyline object if succeded

Return type:

HybridShapePolyline

add_new_position_transfo(i_mode: int) → HybridShapePositionTransfo

Note

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

o Func AddNewPositionTransfo(long iMode) As

HybridShapePositionTransfo

Creates a new PositionTransfo within the current body.

Parameters:

iMode

Positioning mode.

oExt

Created positioning transformation (i.e. positioned wire /

profile).

Parameters:

i_mode (int) –

Return type:

HybridShapePositionTransfo

add_new_project(i_element: Reference, i_support: Reference) → HybridShapeProject

Note

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

o Func AddNewProject(Reference iElement,

Reference iSupport) As HybridShapeProject

Creates a new Project within the current body.

Parameters:

iElement

Element to project (point, curve).

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge, BiDimFeatEdge and Vertex.

iSupport

Curve or surface support for projection.

Sub-element(s) supported (see Boundary object): see Face,

TriDimFeatEdge and BiDimFeatEdge.

oProjection

Created projection

Parameters:

• i_element (Reference) –

• i_support (Reference) –

Return type:

HybridShapeProject

add_new_reflect_line(i_support: Reference, i_dir: HybridShapeDirection, i_angle: float, i_orientation_support: int, i_orientation_direction: int) → HybridShapeReflectLine

Note

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

o Func AddNewReflectLine(Reference iSupport,

HybridShapeDirection iDir,

double iAngle,

long iOrientationSupport,

long iOrientationDirection) As HybridShapeReflectLine

Deprecated:

V5R17 CATIAHybridShapeFactory#AddNewReflectLineWithType Creates a new

ReflectLine within the current body.

Create a reflectline curve on a support surface along a direction with

an angle.

Parameters:

iSupport

Support surface.

Sub-element(s) supported (see

Boundary object): see Face.

iAngle

Angle of the reflectline.

iOrientationSupport

Manage the angle used to compute the reflectline. Value can be 1 or -1

iOrientationDirection

Manage the angle used to compute the reflectline. Value can be 1 or -1

oReflectLine

Created reflectline.

Parameters:

• i_support (Reference) –

• i_dir (HybridShapeDirection) –

• i_angle (float) –

• i_orientation_support (int) –

• i_orientation_direction (int) –

Return type:

HybridShapeReflectLine

add_new_reflect_line_with_type(i_support: Reference, i_dir: HybridShapeDirection, i_angle: float, i_orientation_support: int, i_orientation_direction: int, i_type: int) → HybridShapeReflectLine

Note

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

o Func AddNewReflectLineWithType(Reference iSupport,

HybridShapeDirection iDir,

double iAngle,

long iOrientationSupport,

long iOrientationDirection,

long iType) As HybridShapeReflectLine

Creates a new ReflectLine within the current body.

Create a reflectline curve on a support surface along a direction with an

angle.

Parameters:

iSupport

Support surface.

iAngle

Angle of the reflectline.

iOrientationSupport

Manage the angle used to compute the reflectline. Value can be 1 or

-1

iOrientationDirection

Manage the angle used to compute the reflectline. Value can be 1 or

-1

iType

Manage the type used to compute the reflectline. Value can be 0 or

1 Returns or sets whether the reflectline curve is or should be created with

the normal to the support or the tangent plane to the

support.

Role: The TypeSolution indicates whether the created reflectline

curve is compute with the angle between the normale to the support and the

direction or with the angle between the tangent plane to the support and the

direction..

Legal values: 0 for the normal and 1 for the tangent plane.

oReflectLine

Created reflectline.

Parameters:

• i_support (Reference) –

• i_dir (HybridShapeDirection) –

• i_angle (float) –

• i_orientation_support (int) –

• i_orientation_direction (int) –

• i_type (int) –

Return type:

HybridShapeReflectLine

add_new_revol(i_object_to_extrude: Reference, i_offset_debut: float, i_offset_fin: float, i_axis: Reference) → HybridShapeRevol

Note

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

o Func AddNewRevol(Reference iObjectToExtrude,

double iOffsetDebut,

double iOffsetFin,

Reference iAxis) As HybridShapeRevol

Creates a new revolution within the current body.

Parameters:

iObjectToExtrude

Profile to be revolved

Sub-element(s) supported (see

Boundary object): see Face, TriDimFeatEdge, BiDimFeatEdge and Vertex.

iOffsetDebut

Angle value

iOffsetFin

Angle value

iAxis

Revolution axis ( line that has to be in the profil

plane

Sub-element(s) supported (see Boundary object): see

RectilinearTriDimFeatEdge, RectilinearBiDimFeatEdge and

RectilinearMonoDimFeatEdge.

oRevolObject

Revolved result

Parameters:

• i_object_to_extrude (Reference) –

• i_offset_debut (float) –

• i_offset_fin (float) –

• i_axis (Reference) –

Return type:

HybridShapeRevol

add_new_rotate(i_to_rotate: Reference, i_axis: Reference, i_angle: float) → HybridShapeRotate

Note

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

o Func AddNewRotate(Reference iToRotate,

Reference iAxis,

double iAngle) As HybridShapeRotate

Creates a new Rotate within the current body.

Parameters:

iToRotate

point, curve, surface or solid to transform.

Sub-element(s) supported (see

Boundary object): see Face, TriDimFeatEdge, BiDimFeatEdge and Vertex.

iAxis

Rotation axis.

Sub-element(s) supported (see Boundary object): see

Edge.

iAngle

Rotation angle.

oRotate

Created rotation.

Parameters:

• i_to_rotate (Reference) –

• i_axis (Reference) –

• i_angle (float) –

Return type:

HybridShapeRotate

add_new_section() → HybridShapeSection

Note

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

o Func AddNewSection() As HybridShapeSection

Creates a new section.

Parameters:

oSection

Created Section

Return type:

HybridShapeSection

add_new_sphere(i_center: Reference, i_axis: Reference | VBANothing, i_radius: float, i_begin_parallel_angle: float, i_end_parallel_angle: float, i_begin_meridian_angle: float, i_end_meridian_angle: float) → HybridShapeSphere

Note

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

o Func AddNewSphere(Reference iCenter,

Reference iAxis,

double iRadius,

double iBeginParallelAngle,

double iEndParallelAngle,

double iBeginMeridianAngle,

double iEndMeridianAngle) As HybridShapeSphere

Creates a new Sphere within the current body.

Parameters:

iCenter

Sphere center.

Sub-element(s) supported (see

Boundary object): see Vertex.

iAxis

Sphere axis

iRadius

Radius

iBeginParallelAngle

Angle value

iEndParallelAngle

Angle value

iBeginMeridianAngle

Angle value

iEndMeridianAngle

Angle value

oSphereObject

Sphere result

Parameters:

• i_center (Reference) –

• i_axis (Reference or VBANothing) –

• i_radius (float) –

• i_begin_parallel_angle (float) –

• i_end_parallel_angle (float) –

• i_begin_meridian_angle (float) –

• i_end_meridian_angle (float) –

Return type:

HybridShapeSphere

add_new_spine() → HybridShapeSpine

Note

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

o Func AddNewSpine() As HybridShapeSpine

Creates a new spine within the current body.

Parameters:

oExt

CATIAHybridShapeSpine created

Return type:

HybridShapeSpine

add_new_spiral(i_type: int, i_support: Reference, i_center_point: Reference, i_axis: HybridShapeDirection, i_starting_radius: float, i_clockwise_revolution: bool) → HybridShapeSpiral

Note

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

o Func AddNewSpiral(long iType,

Reference iSupport,

Reference iCenterPoint,

HybridShapeDirection iAxis,

double iStartingRadius,

boolean iClockwiseRevolution) As HybridShapeSpiral

Creates a new Spiral within the current body.

Parameters:

iType

Spiral is defined by AngleRadius, AnglePitch or PitchRadius.

iSupport

Spiral planar support.

iCenterPoint

Center point.

iAxis

Axis.

iStartingRadius

Defines the starting point: distance from the center point on the

axis.

iClockwiseRevolution

Revolutions are clockwise if TRUE, counterclockwise if FALSE.

oSpiral

The Spiral object if succeded

Parameters:

• i_type (int) –

• i_support (Reference) –

• i_center_point (Reference) –

• i_axis (HybridShapeDirection) –

• i_starting_radius (float) –

• i_clockwise_revolution (bool) –

Return type:

HybridShapeSpiral

add_new_spline() → HybridShapeSpline

Note

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

o Func AddNewSpline() As HybridShapeSpline

Creates a new Spline within the current body.

Parameters:

oSpline

Created spline.

Return type:

HybridShapeSpline

add_new_surface_datum(i_object: Reference) → HybridShapeSurfaceExplicit

Note

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

o Func AddNewSurfaceDatum(Reference iObject) As

HybridShapeSurfaceExplicit

Creates a new datum of surface within the current body.

Parameters:

iObject

The object whose topological body will be duplicated and put into

created datum

oSurface

Created surface Note2: the object passed as parameter to create the

datum has to be in the current container. Otherwise, an error

occurs.

Parameters:

i_object (Reference) –

Return type:

HybridShapeSurfaceExplicit

add_new_sweep_circle(i_guide1: Reference) → HybridShapeSweepCircle

Note

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

o Func AddNewSweepCircle(Reference iGuide1) As

HybridShapeSweepCircle

Creates a new SweepCircle within the current body.

Parameters:

iGuide1

First guide or center curve.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

oExt

Created swept surface.

Parameters:

i_guide1 (Reference) –

Return type:

HybridShapeSweepCircle

add_new_sweep_conic(ip_ia_guide1: Reference) → HybridShapeSweepConic

Note

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

o Func AddNewSweepConic(Reference ipIAGuide1) As

HybridShapeSweepConic

Creates a new SweepConic within the current body.

Parameters:

iGuide1

First guide curve.

opIASweepConic

Created swept surface.

Parameters:

ip_ia_guide1 (Reference) –

Return type:

HybridShapeSweepConic

add_new_sweep_explicit(i_profile: Reference, i_guide: Reference) → HybridShapeSweepExplicit

Note

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

o Func AddNewSweepExplicit(Reference iProfile,

Reference iGuide) As HybridShapeSweepExplicit

Creates a new SweepExplicit within the current body.

Parameters:

iProfile

Profile.

Sub-element(s) supported (see

Boundary object): see TriDimFeatEdge and BiDimFeatEdge.

iGuide

First guide curve.

Sub-element(s) supported (see Boundary object): see TriDimFeatEdge and

BiDimFeatEdge.

oExt

Created swept surface.

Parameters:

• i_profile (Reference) –

• i_guide (Reference) –

Return type:

HybridShapeSweepExplicit

add_new_sweep_line(i_guide1: Reference) → HybridShapeSweepLine

Note

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

o Func AddNewSweepLine(Reference iGuide1) As

HybridShapeSweepLine

Creates a new SweepLine within the current body.

Parameters:

iGuide1

First guide curve.

oExt

Created swept surface.

Parameters:

i_guide1 (Reference) –

Return type:

HybridShapeSweepLine

add_new_symmetry(i_object: Reference, i_reference: Reference) → HybridShapeSymmetry

Note

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

o Func AddNewSymmetry(Reference iObject,

Reference iReference) As HybridShapeSymmetry

Creates a new Symmetry within the current body.

Parameters:

iObject

Point, curve, surface or solid to transform.

Sub-element(s) supported (see

Boundary object): see Face, TriDimFeatEdge, BiDimFeatEdge and Vertex.

iReference

Point, line or reference plane.

Sub-element(s) supported (see Boundary object): see PlanarFace, Edge

and Vertex.

oSymmetry

Created symmetry.

Parameters:

• i_object (Reference) –

• i_reference (Reference) –

Return type:

HybridShapeSymmetry

add_new_transfer(i_element_to_transfer: Reference, i_type_of_transfer: int) → HybridShapeTransfer

Note

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

o Func AddNewTransfer(Reference iElementToTransfer,

long iTypeOfTransfer) As HybridShapeTransfer

Creates a new Transfer within the current body.

Note: require DL1 license.

Parameters:

iElementToTransfer

The element to transfer

iTypeOfTransfer

The type of transfer

oExt

Created Transfer operation.

Parameters:

• i_element_to_transfer (Reference) –

• i_type_of_transfer (int) –

Return type:

HybridShapeTransfer

add_new_translate(i_element: Reference, i_direction: HybridShapeDirection, i_distance: float) → HybridShapeTranslate

Note

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

o Func AddNewTranslate(Reference iElement,

HybridShapeDirection iDirection,

double iDistance) As HybridShapeTranslate

Creates a new Translate within the current body.

Parameters:

iElement

Point, curve, surface or solid to translate.

iDirection

Translation direction.

iDistance

Translation Distance.

oTranslate

Created translation

oTranslate

Created Translate (Empty feature)

Note: Then translate mode and inputs has to be initialized

See also:

HybridShapeTranslate

Parameters:

• i_element (Reference) –

• i_direction (HybridShapeDirection) –

• i_distance (float) –

Return type:

HybridShapeTranslate

add_new_unfold() → HybridShapeUnfold

Note

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

o Func AddNewUnfold() As HybridShapeUnfold

Creates a new Unfold within the current body.

Note: require DL1 license.

Parameters:

oExt

Created unfold operation.

Return type:

HybridShapeUnfold

add_new_volume_datum(i_object: Reference) → HybridShapeVolumeExplicit

Note

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

o Func AddNewVolumeDatum(Reference iObject) As

HybridShapeVolumeExplicit

Creates a new datum of volume within the current body.

Note: requires GSO License

Parameters:

iObject

The object whose topological body will be duplicated and put into

created datum

oVolume

Created Volume Note2: the object passed as parameter to create the

datum has to be in the current container. Otherwise, an error

occurs.

Parameters:

i_object (Reference) –

Return type:

HybridShapeVolumeExplicit

add_new_wrap_curve() → HybridShapeWrapCurve

Note

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

o Func AddNewWrapCurve() As HybridShapeWrapCurve

Creates a new Wrap Curve Surface within the current body.

Note: require GSO license.

Parameters:

oWrapCurve

The Wrap Curve object if succeded

Return type:

HybridShapeWrapCurve

add_new_wrap_surface(i_body_to_deform: Reference) → HybridShapeWrapSurface

Note

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

o Func AddNewWrapSurface(Reference iBodyToDeform) As

HybridShapeWrapSurface

Creates a new Wrap Surface within the current body.

Note: require GSO license.

Parameters:

:

iBodyToDeform Body to deform with a Wrap Surface

oWrapSurface

The Wrap Surface object if succeded

Parameters:

i_body_to_deform (Reference) –

Return type:

HybridShapeWrapSurface

change_feature_name(i_elem: Reference, name: str) → None

Note

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

o Sub ChangeFeatureName(Reference iElem,

CATBSTR Name)

Set display name for Shape Design Features.

Parameters:

iElem

Element to rename

Name

User name

Parameters:

• i_elem (Reference) –

• name (str) –

Return type:

None

delete_object_for_datum(i_object: Reference) → None

Note

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

o Sub DeleteObjectForDatum(Reference iObject)

Deletes an object within the current body.

Parameters:

iObject

Object to delete

Parameters:

i_object (Reference) –

Return type:

None

get_geometrical_feature_type(i_elem: Reference) → int

Note

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

o Func GetGeometricalFeatureType(Reference iElem) As short

Returns type of “geometrical” shape Design feature .

Parameters:

iElem

Reference element

oType

Type of feature

0 = Unknown, 1 = Point, 2 = Curve, 3 = Line, 4 = Circle,

5 = Surface, 6 = Plane, 7 = Solid / Volume

Level of availability = V5R14

See enumeration.enumeration_types.geometrical_feature_type() for enums.

Parameters:

i_elem (Reference) –

Returns:

0 = Unknown, 1 = Point, 2 = Curve, 3 = Line, 4 = Circle, 5 = Surface, 6 = Plane, 7 = Solid, Volume

Return type:

int

gsm_visibility(i_elem: Reference, show: int) → None

Note

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

o Sub GSMVisibility(Reference iElem,

long Show)

Set Visibility attribut for Shape Design Features.

Parameters:

iElem

Element to show/NoShow

Show

= 0 NoShow , 1= Show

Parameters:

• i_elem (Reference) –

• show (int) –

Return type:

None