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CATSketcherUseItf Interface CATISktUse2DWFFactory

Usage: an implementation of this interface is supplied and you must use it as is. You should not reimplement it.

interface CATISktUse2DWFFactory

Provides the client with the functionality for creating 2D geometric elements.
Role:

Method Index

o CreateArc(CATBaseUnknown*,CATBaseUnknown*,CATBaseUnknown*,IID&,CATBaseUnknown**): Creates an Arc on a 2D Curve.
o CreateCenterCircle(double*,double): Creates a 2D axis circle.
o CreateCenterLine(double*,double*): Creates a 2D axis line.
o CreateChamfer(CATISktUse2DCurve*,CATISktUse2DCurve*,double*,double*,double*,int): Creates a chamfer segment.
o CreateCircle(double*,double): Creates a 2D circle.
o CreateCircle(double*,double*,double*,int): Creates a 2D arc through three points.
o CreateCircle(double*,double,double,double): Creates a 2D arc.
o CreateCircleTgt(double*,double*,double*,int): Creates a 2D arc with two points and a tangent.
o CreateConicCurve(CATBaseUnknown*,CATBaseUnknown*,IID&,CATBaseUnknown**,CATBaseUnknown*,CATBaseUnknown*,CATBaseUnknown*,CATBaseUnknown*,CATBaseUnknown*,CATBaseUnknown*,CATBaseUnknown*,CATBaseUnknown*,double): Creates a 2D conic curve.
o CreateConnectCurve(CATBaseUnknown*,CATBaseUnknown*,CATBaseUnknown*,CATBaseUnknown*,IID&,CATBaseUnknown**,int,int,int,int,double,double): Creates a 2D connecting curve between two 2D curves.
o CreateConstructionCircle(double*,double): Creates a 2D construction circle.
o CreateConstructionLine(double*,double*): Creates a 2D construction line.
o CreateContour(CATISktUse2DCurve_var&,CATContourClass,CATAutosearchMode): Dedicated to curve connectivity detection using CATIA V4 tolerance.
o CreateCorner(CATISktUse2DCurve*,CATISktUse2DCurve*,double*,double*): Creates a bi-tangent arc.
o CreateCstPoint(double*,double*,double*): Creates a 2D control point.
o CreateCubicSplineCurve(CATLISTV(CATISktUse2DPoint_var)&,int): Creates a 2D cubic spline curve (degree = 3).
o CreateEllipse(double*,double*,double,double): Creates a 2D ellipse.
o CreateEllipse(double*,double*,double,double,double,double): Creates a 2D arc of ellipse.
o CreateHyperbola(double*,double*,double,double): Creates a 2D hyperbola.
o CreateHyperbola(double*,double*,double,double,double,double): Creates a 2D hyperbola.
o CreateLine(double*,double*): Creates a 2D line.
o CreateLine(double*,double*,double,double): Creates a 2D line.
o CreateOffsetCurve(int,CATBaseUnknown*,double): Creates a 2D offset curve of a 2D curve.
o CreateOutput(CATBaseUnknown*,IID&,CATBaseUnknown**): Creates a 2D Output Geometry from 2D Geometry.
o CreateOutputAxis(CATBaseUnknown*,IID&,CATBaseUnknown**): Creates a 2D Output axis Geometry from 2D point.
o CreateOutputPlane(CATBaseUnknown*,IID&,CATBaseUnknown**): Creates a 2D Output plane from 2D line.
o CreateOutputProfile(CATLISTV(CATBaseUnknown_var)&,IID&,CATBaseUnknown**): Creates a 2D Output Profile from 2D Geometries.
o CreateParabola(double*,double*,double): Creates a 2D parabola.
o CreateParabola(double*,double*,double,double,double): Creates a 2D parabola.
o CreatePoint(double*): Creates a 2D point.
o CreatePolyline(unsigned long,double*,boolean): Creates a 2D polyline.
o CreateSplineCurve(CATLISTV(CATISktUse2DPoint_var)&,int): Creates a 2D quintic spline curve (degree = 5).
o CreateUnspec(CATCurve_var&): Creates a curve from a CATPCurve object.
o Duplicate(CATLISTV(CATISktUse2DWFGeometry_var)&,CATMathTransformation2D&): Duplicates a set of 2D geometries and applies a transformation to the result.
o FixTogether(CATLISTV(CATISktUse2DWFGeometry_var)&,IID&,CATBaseUnknown**,int): Creates a Fix Together Constraint (rigid set) of 2D Geometries.
o IntersectGeometry(CATBaseUnknown_var&,CATLISTV(CATISktUse2DWFGeometry_var)&,int,CATBaseUnknown*,double*,int,int): Intersects 3D or 2D external geometry.
o OffsetGeometry(int,CATBaseUnknown*,double,int,CATBaseUnknown*,double*,int,int): Offsets 3D geometry.
o ProjectGeometry(CATBaseUnknown_var&,CATLISTV(CATISktUse2DWFGeometry_var)&,int,CATBaseUnknown*,double*,int,int): Projects 3D or 2D external geometry on a sketch.
o SilhouetteGeometry(CATBaseUnknown_var&,CATLISTV(CATISktUse2DWFGeometry_var)&,int,CATBaseUnknown*,double*,int): Creates the silhouette of a surface.

Methods

o CreateArc

public virtual CreateArc(		`iCurve1`,
		`iPoint1`,
		`iPoint2`,
	const	`iid`,
		`oArc`)

Creates an Arc on a 2D Curve.

Parameters:

iCurve: [in] The curve on which the arc must be created.
iPoint1: [in] 2D start point for the arc.
iPoint2: [in] 2D end point for the arc.
iIID: [in] Interface identifier for which a pointer is requested.
oArc: [out] Pointer to the created Arc.

o CreateCenterCircle

public virtual CreateCenterCircle(	const	`iPoint`,
	const	`iRadius`)

Creates a 2D axis circle.

Parameters:

iPoint: [in] 2D origin point coordinates.
iRadius: [in] Radius of the circle.

o CreateCenterLine

public virtual CreateCenterLine(	const	`iPoint`,
	const	`iDirection`)

Creates a 2D axis line.

Parameters:

iPoint: [in] 2D origin point coordinates.
iDirection: [in] 2D direction coordinates (will be normalized).

o CreateChamfer

public virtual CreateChamfer(		`iCurve1`,
		`iCurve2`,
	const	`iPoint`,
	const	`iParam1`	`=NULL`,
	const	`iParam2`	`=NULL`,
	const	`iChamfer`	`=1`)

Creates a chamfer segment.

Parameters:

iCurve1: [in] First geometric element.
iCurve2: [in] Second geometric element.
iPoint: [in] Indicated 2D point coordinates.
iParam1: [in] Optional first parameter of the chamfer segment.
iParam2: [in] Optional second parameter of the chamfer segment.
iChamfer: [in] Indicates the computation mode of the chamfer, thus the significance of the two parameters iParam1 and iParam2: If iChamfer == 1 (Length of the chamfer and its angle): iParam1 means the length of the chamfer segment. iParam2 means the angle of the chamfer segment with the tangent to the first curve at the nearest intersection point from the indicated 2D point. If iChamfer == 2 (Length1 and Length2 define the chamfer): iParam1 means the distance of the chamfer segment with either the intersecting point of the two curves, if it exists, or the end point of the first curve. iParam2 means the distance of the chamfer segment with either the intersecting point of the two curves, if it exists, or the end point of the second curve. If iChamfer == 3 (Length1 and Angle define the chamfer): iParam1 means the distance of the chamfer segment with either the intersecting point of the two curves, if it exists, or the end point of the first curve. iParam2 means the angle of the chamfer segment with the tangent of the first curve at the nearest intersection point from the indicated 2D point.

o CreateCircle

public virtual CreateCircle(	const	`iPoint`,
	const	`iRadius`)

Creates a 2D circle.

Parameters:

iPoint: [in] 2D center point coordinates.
iRadius: [in] Radius of the circle.

o CreateCircle

public virtual CreateCircle(	const	`iStartPoint`,
	const	`iPoint`,
	const	`iEndPoint`,
	const	`iRelimit`	`=1`)

Creates a 2D arc through three points.

Parameters:

iStartPoint

[in] 2D start point coordinates.

iPoint

[in] 2D second point coordinates.

iEndPoint

[in] 2D end point coordinates.

iRelimit

[in] Trimming mode.

1: The arc is trimmed on given points.
0: The arc is not trimmed.

o CreateCircle

public virtual CreateCircle(	const	`iPoint`,
	const	`iRadius`,
	const	`iStartParam`,
	const	`iEndParam`)

Creates a 2D arc.

Parameters:

iPoint: [in] 2D center point coordinates.
iRadius: [in] Radius of the circle.
iStartParam: [in] Parameter of the start point (0<=iStartParam<2*PI).
iEndParam: [in] Parameter of the end point (iStartParam

o CreateCircleTgt

public virtual CreateCircleTgt(	const	`iStartPoint`,
	const	`iStartTangent`,
	const	`iEndPoint`,
	const	`iRelimit`	`=1`)

Creates a 2D arc with two points and a tangent.

Parameters:

iStartPoint

[in] 2D start point coordinates.

iStartTangent

[in] 2D tangent coordinates.

iEndPoint

[in] 2D end point coordinates.

iRelimit

[in] Trimming mode.

1: The arc is trimmed on given points.
0: The arc is not trimmed.

o CreateConicCurve

public virtual CreateConicCurve(		`iStartPoint`,
		`iEndPoint`,
	const	`iIID`,
		`oConic`,
		`iStartTangent`	`=NULL`,
		`iEndTangent`	`=NULL`,
		`iFirstIntermediatePoint`	`=NULL`,
		`iFirstIntermediateTangent`	`=NULL`,
		`iSecondIntermediatePoint`	`=NULL`,
		`iSecondIntermediateTangent`	`=NULL`,
		`iThirdIntermediatePoint`	`=NULL`,
		`iTangentIntersectionPoint`	`=NULL`,
	const	`iConicParm`	`=0.5`)

Creates a 2D conic curve.

Parameters:

iStartPoint

[in] Starting point of conic curve.

iEndPoint

[in] Ending point of conic curve.

iIID

[in] Interface identifier for which a pointer is requested.

oConic

[out] Pointer to the created conic curve.

iFirstIntermediatePoint

[in] Optional: First intermediate passing thru point.

iFirstIntermediateTangent

[in] Optional: Tangent at the first intermediate passing thru point.

iSecondIntermediatePoint

[in] Optional: Second intermediate passing thru point.

iSecondIntermediateTangent

[in] Optional: Tangent at the second intermediate passing thru point.

iThirdIntermediatePoint

[in] Optional: Third intermediate passing thru point.

iTangentIntersectionPoint

[in] Optional: Tangent intersection point.

iConicParm

[in] Optional: Conic parameter.
Legal values:

>0: should be greater than 0
0.5: default value
<1: should be lower than 1

See also:

o CreateConnectCurve

public virtual CreateConnectCurve(		`iCurve1`,
		`iPoint1`,
		`iCurve2`,
		`iPoint2`,
	const	`iid`,
		`oConnect`,
	const	`iContinuity1`	`=2`,
	const	`iContinuity2`	`=2`,
	const	`iOrient1`	`=1`,
	const	`iOrient2`	`=1`,
	const	`iTension1`	`=1.0`,
	const	`iTension2`	`=1.0`)

Creates a 2D connecting curve between two 2D curves.

Parameters:

iCurve1

[in] First 2D curve to connect.

iPoint1

[in] 2D start point for the connecting curve.

iCurve2

[in] Second 2D curve to connect.

iPoint2

[in] 2D end point for the connecting curve.

iIID

[in] Interface identifier for which a pointer is requested.

oConnect

[out] Pointer to the created connecting curve

iContinuity1

[in] Optional: Continuity with first curve.
Legal values:

0: C0 - point continuity
1: C1 - tangent continuity
2: C2 - curvature continuity

iContinuity2

[in] Optional: Continuity with second curve.
Legal values:

0: C0 - point continuity
1: C1 - tangent continuity
2: C2 - curvature continuity

iOrientation1

[in] Optional: If same orientation, the connecting curve starts tangent to iCurve1 at iPoint1.
Legal values:

1: same orientation
-1: opposite orientation

iOrientation2

[in] Optional: If same orientation, the connecting curve ends tangent to iCurve2 at iPoint2.
Legal values:

1: same orientation
-1: opposite orientation

iTension1

[in] Optional: Standard tension = 1.0; increase this value to straighten the connecting curve.

iTension2

[in] Optional: Standard tension = 1.0; increase this value to straighten the connecting curve.

See also:

o CreateConstructionCircle

public virtual CreateConstructionCircle(	const	`iPoint`,
	const	`iRadius`)

Creates a 2D construction circle.

Parameters:

iPoint: [in] 2D center point coordinates.
iRadius: [in] Radius of the circle.

o CreateConstructionLine

public virtual CreateConstructionLine(	const	`iPoint`,
	const	`iDirection`)

Creates a 2D construction line.

Parameters:

iPoint: [in] 2D origin point coordinates.
iDirection: [in] 2D direction coordinates (will be normalized).

o CreateContour

public virtual CreateContour(	const	`i2DGeom`,
	const	`iClass`	`=ContourClass_Undefined`,
	const	`iMode`	`=AutosearchMode_NoMultipleSolutions`)

Dedicated to curve connectivity detection using CATIA V4 tolerance.

o CreateCorner

public virtual CreateCorner(		`iCurve1`,
		`iCurve2`,
	const	`iPoint`,
	const	`iRadius`	`=NULL`)

Creates a bi-tangent arc.

Parameters:

iCurve1: [in] First geometric element.
iCurve2: [in] Second geometric element.
iPoint: [in] Indicated 2D point coordinates.
iRadius: [in] Optional radius of the arc (unspecified by default).

o CreateCstPoint

public virtual CreateCstPoint(	const	`iPoint`,
	const	`iTangent`,
	const	`iCurvature`)

Creates a 2D control point.

Parameters:

iPoint: [in] 2D point coordinates.
iTangent: [in] 2D tangent coordinates or NULL.
iCurvature: [in] 2D curvature coordinates or NULL. The curvature direction has to be orthogonal to the tangent. Radius of curvature is 1/norm(curvature). The curvature vector can be (0,0), indicating an infinite radius of curvature (line).

o CreateCubicSplineCurve

public virtual CreateCubicSplineCurve(	const	`iPoints`,
	const	`iEvaluationType`)

Creates a 2D cubic spline curve (degree = 3).

Parameters:

iPoints: [in] List of spline control points.
iEvaluationType: [in] Evaluation mode (NOT USED).

o CreateEllipse

public virtual CreateEllipse(	const	`iPoint`,
	const	`iMajorDirection`,
	const	`iMajorRadius`,
	const	`iMinorRadius`)

Creates a 2D ellipse.

Parameters:

iPoint: [in] 2D center point coordinates.
iMajorDirection: [in] 2D major axis direction coordinates.
iMajorRadius: [in] Major semi-axis of the ellipse.
iMinorRadius: [in] Minor semi-axis of the ellipse.

o CreateEllipse

public virtual CreateEllipse(	const	`iPoint`,
	const	`iMajorDirection`,
	const	`iMajorRadius`,
	const	`iMinorRadius`,
	const	`iStartParam`,
	const	`iEndParam`)

Creates a 2D arc of ellipse.

Parameters:

iPoint: [in] 2D center point coordinates.
iMajorDirection: [in] 2D major axis direction coordinates.
iMajorRadius: [in] Major semi-axis of the ellipse.
iMinorRadius: [in] Minor semi-axis of the ellipse.
iStartParam: [in] Parameter of the start point (0<=iStartParam<2*PI).
iEndParam: [in] Parameter of the end point (iStartParam

o CreateHyperbola

public virtual CreateHyperbola(	const	`iPoint`,
	const	`iAxis`,
	const	`iRadius1`,
	const	`iRadius2`)

Creates a 2D hyperbola.

Parameters:

iPoint: [in] 2D center point coordinates.
iAxis: [in] 2D axis direction coordinates.
iRadius1: [in] Radius of the hyperbola.
iRadius2: [in] Imaginary radius of the hyperbola.

o CreateHyperbola

public virtual CreateHyperbola(	const	`iPoint`,
	const	`iAxis`,
	const	`iRadius1`,
	const	`iRadius2`,
	const	`iStartParam`,
	const	`iEndParam`)

Creates a 2D hyperbola.

Parameters:

iPoint: [in] 2D center point coordinates.
iAxis: [in] 2D axis direction coordinates.
iRadius1: [in] Radius of the hyperbola.
iRadius2: [in] Imaginary radius of the hyperbola.
iStartParam: [in] Parameter of the start point.
iEndParam: [in] Parameter of the end point.

o CreateLine

public virtual CreateLine(	const	`iStartPoint`,
	const	`iEndPoint`)

Creates a 2D line.

Parameters:

iStartPoint: [in] 2D start point coordinates.
iEndPoint: [in] 2D end point coordinates.

o CreateLine

public virtual CreateLine(	const	`iPoint`,
	const	`iDirection`,
	const	`iStartParam`,
	const	`iEndParam`)

Creates a 2D line.

Parameters:

iPoint: [in] 2D origin point coordinates.
iDirection: [in] 2D direction coordinates (will be normalized).
iStartParam: [in] Parameter of the start point (iPoint + iStartParam * iDirection).
iEndParam: [in] Parameter of the end point (iPoint + iEndParam * iDirection).

o CreateOffsetCurve

public virtual CreateOffsetCurve(	const	`iCornerType`,
		`iRefGeom`,
	const	`iValue`)

Creates a 2D offset curve of a 2D curve.

Parameters:

iCornerType: [in] Corner computation mode.
iRefGeom: [in] Offseted curve.
iValue: [in] Signed offset value.

o CreateOutput

public virtual CreateOutput(		`iGeom`,
	const	`iid`,
		`oOutput`)

Creates a 2D Output Geometry from 2D Geometry.

Parameters:

iGeom: [in] 2D Geometry of the current sketch.
iIID: [in] Interface identifier for which a pointer is requested.
oOutput: [out] Pointer to the created Output Geometry

o CreateOutputAxis

public virtual CreateOutputAxis(		`iGeom`,
	const	`iid`,
		`oOutput`)

Creates a 2D Output axis Geometry from 2D point.

Parameters:

iGeom: [in] 2D Geometry of the current sketch.
iIID: [in] Interface identifier for which a pointer is requested.
oOutput: [out] Pointer to the created Output Geometry

o CreateOutputPlane

public virtual CreateOutputPlane(		`iGeom`,
	const	`iid`,
		`oOutput`)

Creates a 2D Output plane from 2D line.

Parameters:

iGeom: [in] 2D Geometry of the current sketch.
iIID: [in] Interface identifier for which a pointer is requested.
oOutput: [out] Pointer to the created Output Geometry

o CreateOutputProfile

public virtual CreateOutputProfile(		`i2DGeoms`,
	const	`iIID`,
		`oOutput`)

Creates a 2D Output Profile from 2D Geometries.

Parameters:

io2DGeoms: [in/out] The set of geometries that defines the profile domain.
iIID: [in] Interface identifier for which a pointer is requested.
oOutput: [out] Pointer to the created Output Profile

o CreateParabola

public virtual CreateParabola(	const	`iPoint`,
	const	`iAxis`,
	const	`iFocalDistance`)

Creates a 2D parabola.

Parameters:

iPoint: [in] 2D center point coordinates.
iAxis: [in] 2D axis direction coordinates.
iFocalDistance: [in] Focal distance of the parabola.

o CreateParabola

public virtual CreateParabola(	const	`iPoint`,
	const	`iAxis`,
	const	`iFocalDistance`,
	const	`iStartParam`,
	const	`iEndParam`)

Creates a 2D parabola.

Parameters:

iPoint: [in] 2D center point coordinates.
iAxis: [in] 2D axis direction coordinates.
iFocalDistance: [in] Focal distance of the parabola.
iStartParam: [in] Parameter of the start point.
iEndParam: [in] Parameter of the end point.

o CreatePoint

public virtual CreatePoint( const iPoint)

Creates a 2D point.

Parameters:

iPoint: [in] 2D point coordinates.

o CreatePolyline

public virtual CreatePolyline(	const	`nPoints`,
	const	`pPoints`,
	const	`isClosed`)

Creates a 2D polyline.

Parameters:

nPoints: [in] number of 2D points.
pPoints: [in] 2D point coordinates.
isClosed: [in] if TRUE, an additional arc will be created between the last and the first points to close the polyline curve.

o CreateSplineCurve

public virtual CreateSplineCurve(	const	`iPoints`,
	const	`iEvaluationType`)

Creates a 2D quintic spline curve (degree = 5).

Parameters:

iPoints: [in] List of spline control points.
iEvaluationType: [in] Evaluation mode (NOT USED).

o CreateUnspec

public virtual CreateUnspec( const iCurve)

Creates a curve from a CATPCurve object.

Parameters:

iCurve: [in] CATPCurve (also a CATCurve) to create.

o Duplicate

public virtual Duplicate(	const	`iGeoms`,
		`ioTransfo`)

Duplicates a set of 2D geometries and applies a transformation to the result.

Parameters:

iGeoms: [in] List of geometric elements to duplicate.
ioTransfo: [inout] 2D transformation to apply to the duplicated elements.

o FixTogether

public virtual FixTogether(		`io2DGeoms`,
	const	`iIID`,
		`oFixTogether`,
	const	`iAddFamily`	`=1`)

Creates a Fix Together Constraint (rigid set) of 2D Geometries.

Parameters:

io2DGeoms: [in/out] The set of geometries on which the Fix Together must be created. The list of geometries with/without dependencies is returned after creation.
iIID: [in] Interface identifier for which a pointer is requested.
oFixTogether: [out] Pointer to the created Fix Together Constraint.
iAddFamily: [in] Optional: Dependencies management.
Legal values:
0: Not management of dependencies
<1: default value: the geometries will be added with their dependencies

See also:

o IntersectGeometry

public virtual IntersectGeometry(	const	`iGeom`,
		`oGeoms`,
	const	`iPhantom`	`=0`,
		`iNearGeom`	`=NULL`,
	const	`iSel2DPt`	`=NULL`,
	const	`iDatum`	`=0`,
	const	`iCanonic`	`=1`)

Intersects 3D or 2D external geometry.

Parameters:

iGeom

[in] External geometric element to intersect with the sketch plane.

oGeoms

[out] List of handlers on the created objects.

iPhantom

[in] Creation mode.

1: The geometric elements are created in phantom mode (invisible).
0: The geometric elements are created in standard mode (visible).

iNearGeom

[in] Optional external geometric element to keep the nearest solution.

iSel2DPt

[in] Optional 2D point coordinates to keep only the nearest solution for a canonical surface projection.

iDatum

[in] Datum mode.

1: The generated geometric elements are not associative.
0: The generated geometric elements are associative.

iCanonic

[in] To manage canonicity.

1: If possible the final geometry will be canonical.
0: No canonicity management.

o OffsetGeometry

public virtual OffsetGeometry(	const	`iCornerType`,
		`iRefGeom`,
	const	`iValue`,
	const	`iPropagType`	`=OffsetPropagType_None`,
		`iInitGeom`	`=NULL`,
	const	`iInitPt`	`=NULL`,
	const	`iOperMode`	`=0`,
	const	`iCanonical`	`=1`)

Offsets 3D geometry.

Parameters:

iCornerType: [in] Corner computation mode.
iRefGeom: [in] External geometric element.
iValue: [in] Signed offset value.
iPropagType: [in] Optional propagation mode. See CAT2DOffsetDefs.
iInitGeom: [in] Optional external geometric element to keep the nearest solution.
iIniPt: [in] Optional 2D point coordinates to keep the nearest solution.

iCanonic

[in] To manage canonicity.

o ProjectGeometry

public virtual ProjectGeometry(	const	`iGeom`,
		`oGeoms`,
	const	`iPhantom`	`=0`,
		`iNearGeom`	`=NULL`,
	const	`iSel2DPt`	`=NULL`,
	const	`iDatum`	`=0`,
	const	`iCanonic`	`=1`)

Projects 3D or 2D external geometry on a sketch.

Parameters:

iGeom

[in] External geometric element to project on the sketch plane.

oGeoms

[out] List of handlers on the created objects.

iPhantom

[in] Creation mode.

1: The geometric elements are created in phantom mode (invisible).
0: The geometric elements are created in standard mode (visible).

iNearGeom

[in] Optional external geometric element to keep the nearest solution.

iSel2DPt

[in] Optional 2D point coordinates to keep only the nearest solution for a canonical surface projection.

iDatum

[in] Datum mode.

1: The generated geometric elements are not associative.
0: The generated geometric elements are associative.

iCanonic

[in] To manage canonicity.

1: If possible the final geometry will be canonical.
0: No canonicity management.

o SilhouetteGeometry

public virtual SilhouetteGeometry(	const	`iGeom`,
		`oGeoms`,
	const	`iPhantom`	`=0`,
		`iNearGeom`	`=NULL`,
	const	`iSel2DPt`	`=NULL`,
	const	`iDatum`	`=0`)

Creates the silhouette of a surface.

Parameters:

iGeom

[in] External geometric element

oGeoms

[out] List of handlers on the created objects.

iPhantom

[in] Creation mode.

1: The geometric elements are created in phantom mode (invisible).
0: The geometric elements are created in standard mode (visible).

iNearGeom

[in] Optional external geometric element to keep the nearest solution.

iSel2DPt

[in] Optional 2D point coordinates to keep only the nearest solution

iDatum

[in] Datum mode.

1: The generated geometric elements are not associative.
0: The generated geometric elements are associative.

This object is included in the file: CATISktUse2DWFFactory.h
If needed, your Imakefile.mk should include the module: CATSketcherUseItf