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GSMInterfaces Interface CATIGSMFactory

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


interface CATIGSMFactory

Factory of all geometrical elements of Generative Shape Design workshop.
Role: Creation of all Generative Shape Design feature.

All methods described here work on CATISpecObject (for geometrical elements) and CATICkeParm (for data such as lengths, angles, ratios...). Note: If the creation fails, the methods return NULL_var.

Note: If the creation fails, the methods return NULL_var.

This factory never agregates the created feature. You need to agregate your object in a GSMTool feature to see it in 3D and Graph. GSMTool feature can be either HybridBody(Body), Geometrical Set (GS) or Ordered Geometrical Set (OGS).
You can use :

Once aggregated the feature has to be updated.

If feature is inserted in Body or OGS, you have to call CATMmrLinearBodyServices::Insert() This method checks the linearity of the Parent/Children relationship and ,if needed, performed re-arrangement(Replace) to makes sure that created feature depends logically of just previouly created feature

See also:
CATIGSMProceduralView, CATIMechanicalRootFactory, CATIGSMTool, CATISpecObject, CATICkeParm, CATICkeParmFactory


Method Index


o ConvertToDatum(CATISpecObject_var&,CATListValCATISpecObject_var*&,int)
Converts the spec to a datum feature.
o Create3DCurveOffset(CATISpecObject_var&,CATIGSMDirection_var&,CATICkeParm_var&,CATICkeParm_var&,CATICkeParm_var&)
Creates a 3D Curve Offset.
o CreateAffinity(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATICkeParm_var,CATICkeParm_var)
Creates an affinity of a point, curve or surface.
o CreateAssemble(CATLISTV(CATISpecObject_var)&,CATICkeParm_var,CATBoolean)
Creates a composite curve or surface from a list of curves or surfaces.
o CreateAssemble(CATICkeParm_var,CATBoolean)
Creates a composite curve or surface.
o CreateAxisExplicit(int&,CATMathPoint*,CATMathDirection*)
Creates an explicit axis which has no associative father but only a geometrical output.
o CreateAxisLine(CATISpecObject_var,CATGSMAxisLineType,CATIGSMDirection_var)
Creates an Axis from the input element.
o CreateAxisToAxis(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var)
Creates a transformation from a reference axis system to a target axis system of point, curve or surface.
o CreateBiDimExplicit()
Creates a simple surface.
o CreateBlend()
Creates a blend surface.
o CreateBoundary(CATISpecObject_var,CATISpecObject_var,CATIGSMBoundaryPropag,CATISpecObject_var,CATISpecObject_var,CATGSMOrientation,CATGSMOrientation)
Creates a boundary.
o CreateCircleExplicit()
Creates an explicit circle which has no associative father but only a geometrical output.
o CreateCircle(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var)
Creates a circle passing through 3 points.
o CreateCircle(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATBoolean)
Creates a circle from point and axis.
o CreateCircle(CATISpecObject_var,CATISpecObject_var,CATBoolean,CATICkeParm_var,CATICkeParm_var,CATICkeParm_var)
Creates a circle from its center and a radius with respect to a support surface.
o CreateCircle(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATBoolean,CATICkeParm_var,CATICkeParm_var)
Creates a circle from its center and a passing point with respect to a support surface.
o CreateCircle(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATBoolean,CATICkeParm_var,CATGSMOrientation)
Creates a circle passing through 2 points with a given radius with respect to a support surface.
o CreateCircularSweep(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var)
Creates a sweep with a circular implicit profile.
o CreateCombine(CATISpecObject_var,CATIGSMDirection_var,CATISpecObject_var,CATIGSMDirection_var,CATGSMCombineSolutionType,CATGSMCombineSolutionTypeCombine)
Creates a combined curve.
o CreateConic(CATISpecObject_var,CATIGSMCurveCst_var,CATIGSMCurveCst_var,CATIGSMCurveCst_var,CATIGSMCurveCst_var,CATIGSMCurveCst_var,CATISpecObject_var,CATICkeParm_var)
Creates a Conic Curve.
o CreateConicalSweep(CATISpecObject_var,CATISpecObject_var)
Creates a sweep with a conical implicit profile.
o CreateConnect(CATISpecObject_var,CATISpecObject_var,CATGSMOrientation,CATGSMContinuity,CATICkeParm_var,CATISpecObject_var,CATISpecObject_var,CATGSMOrientation,CATGSMContinuity,CATICkeParm_var,CATBoolean)
Creates a connect curve between two curves.
o CreateConnect(CATISpecObject_var,CATISpecObject_var,CATGSMOrientation,CATGSMContinuity,CATICkeParm_var,CATISpecObject_var,CATISpecObject_var,CATGSMOrientation,CATGSMContinuity,CATICkeParm_var,CATISpecObject_var,CATBoolean)
o CreateCorner(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATGSMOrientation,CATGSMOrientation,CATBoolean)
Creates a corner curve between a point and a curve or 2 curves on a support surface.
o CreateCurveCst(CATISpecObject_var,CATIGSMDirection_var,CATICkeParm_var,CATIGSMDirection_var,CATICkeParm_var)
Creates a Curve Constraint from Point, Tangency and Curvature Data.
o CreateCurvePar(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATBoolean,int,CATBoolean)
Creates a curve which is an offset (constant) from another curve.
o CreateCurvePar(CATISpecObject_var,CATISpecObject_var,CATICkeLaw_var,CATBoolean,int,CATBoolean,CATBoolean)
Creates a curve which is an offset (specified by a law) from another curve.
o CreateCurveSmooth(CATISpecObject_var)
Creates a smoothed curve.
o CreateCuttingPoint(CATICkeParm_var,CATICkeParm_var,CATICkeParm_var)
Creates a cutting point from its cartesian coordinates (used to cut or fill twisted areas in sweep feature).
o CreateCuttingPoint(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATGSMOrientation,CATIGSMPointOnCurve::DistanceType)
Creates a cutting point on curve at a given curvilinear distance (used to cut or fill twisted areas in sweep feature).
o CreateCylinder(CATISpecObject_var,CATIGSMDirection_var,CATICkeParm_var,CATICkeParm_var,CATICkeParm_var,CATBoolean)
Creates an extruded surface or an extruded line.
o CreateDirection(CATICkeParm_var,CATICkeParm_var,CATICkeParm_var)
Creates a direction from 3 componants (X,Y,Z).
o CreateDirection(CATISpecObject_var)
Creates a direction from a line or a iplane.
o CreateExplicitSweep(CATISpecObject_var,CATISpecObject_var,CATBoolean)
Creates a simple sweep with an explicit profile.
o CreateExplicitSweep(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATBoolean)
Creates a sweep with an explicit profile.
o CreateExplicitSweep(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATBoolean)
Creates a sweep with an explicit profile and a reference surface.
o CreateExtractMulti(CATLISTV(CATISpecObject_var)&)
Extract a sub-element of a solid (vertex, edge or face).
o CreateExtractSolide(CATISpecObject_var,CATIGSMExtractSolidePropag)
Extract a sub-element of a solid (vertex, edge or face).
o CreateExtrapol(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATGSMExtrapolContinuityType,CATGSMExtrapolBorderType,CATBoolean,CATGSMExtrapolPropagationMode)
Creates a surface or a curve by extrapolating a surface or a curve.
o CreateExtrapol(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATGSMExtrapolContinuityType,CATGSMExtrapolBorderType,CATBoolean,CATGSMExtrapolPropagationMode)
Creates a surface or a curve by extrapolating a curve or a surface.
o CreateExtremumPolar(unsigned short int,CATISpecObject_var)
Creates a 2D Extremum in polar coordinates.
o CreateExtremum(CATISpecObject_var,CATIGSMDirection_var,GSMMinMax)
Creates an Extremum.
o CreateExtrude(CATISpecObject_var,CATIGSMDirection_var,CATICkeParm_var,CATICkeParm_var,CATBoolean)
Creates an extruded surface or an extruded line.
o CreateFill(CATLISTV(CATISpecObject_var)&,CATLISTV(CATISpecObject_var)&,CATGSMContinuity)
Creates a fill surface from a list of boundaries (curves, lines).
o CreateFill()
Creates a fill surface.
o CreateFill(CATLISTV(CATISpecObject_var)&,CATLISTV(CATISpecObject_var)&,CATGSMContinuity,CATISpecObject_var)
Creates a fill surface from a list of boundaries (curves, lines).
o CreateFilletTriTangent(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATGSMOrientation,CATGSMOrientation,CATGSMOrientation,CATGSMFilletSupportsTrimMode,CATGSMFilletExtremitiesMode)
Creates a TriTangent fillet between three skins.
o CreateFillet(CATISpecObject_var,CATISpecObject_var,CATGSMOrientation,CATGSMOrientation,CATICkeParm_var,CATGSMFilletSupportsTrimMode,CATGSMFilletExtremitiesMode)
Creates a sphere bitangent fillet between two skins.
o CreateGridSet(CATISpecObject_var&,CATIGSMDirection_var&,CATBoolean)
Creates a GridSet with a point and a direction.
o CreateHealing(CATLISTV(CATISpecObject_var)&,CATLISTV(CATISpecObject_var)&,CATICkeParm_var,CATGSMHealingMode,CATGSMContinuity,CATICkeParm_var,CATICkeParm_var,CATICkeParm_var)
Creates a G0 composite surface from a list of surfaces.
o CreateHealing(CATLISTV(CATISpecObject_var)&,CATLISTV(CATISpecObject_var)&,CATLISTV(CATISpecObject_var)&,CATICkeParm_var,CATICkeParm_var,CATICkeParm_var,CATGSMHealingMode,CATGSMContinuity,CATICkeParm_var,CATICkeParm_var,CATICkeParm_var,CATICkeParm_var,CATGSMHealingMode)
Creates a G0 or G1 composite surface from a list of surfaces.
o CreateHealing(CATLISTV(CATISpecObject_var)&)
Creates a composite surface.
o CreateHelix(CATISpecObject_var,CATBoolean,CATISpecObject_var,CATICkeParm_var,CATICkeParm_var,CATBoolean,CATICkeParm_var,CATICkeParm_var,CATBoolean)
Creates an helix curve.
o CreateIntersect(CATISpecObject_var,CATISpecObject_var,CATBoolean)
Creates the Intersection of two elements.
o CreateInverse(CATISpecObject_var)
Inverts the orientation of a curve or a surface.
o CreateLawDistProj(CATISpecObject_var,CATISpecObject_var,CATBoolean)
Creates a law from two curves : a reference and a definition curve.
o CreateLineBiTangent(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var)
Creates a line tangent to two elements on a support surface.
o CreateLineExplicit()
Creates an explicit line which has no associative father but only a geometrical output.
o CreateLineNormal(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATICkeParm_var,CATGSMOrientation)
Creates a line normal to a surface at a given point.
o CreateLineTangency(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATICkeParm_var,CATGSMOrientation,CATISpecObject_var)
Creates a line tangent to a curve at a given point.
o CreateLine(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var)
Creates a line between two points.
o CreateLine(double*,double*)
Creates an explicit line.
o CreateLine(CATISpecObject_var,CATIGSMDirection_var,CATICkeParm_var,CATICkeParm_var,CATGSMOrientation,CATISpecObject_var)
Creates a line starting at a point and in a given direction.
o CreateLine(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATICkeParm_var,CATGSMOrientation,int)
Creates a line bisecting two other lines.
o CreateLine(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATBoolean,CATICkeParm_var,CATICkeParm_var,CATICkeParm_var,CATGSMOrientation)
Creates a line at an angle to a reference curve at a given point and on a support surface.
o CreateLinearSweep(CATISpecObject_var,CATISpecObject_var)
Creates a sweep with a linear implicit profile.
o CreateLoft(CATLISTV(CATISpecObject_var)&,CATListOfInt&,CATLISTV(CATISpecObject_var)&,CATISpecObject_var,CATISpecObject_var,CATLISTV(CATISpecObject_var)&,CATGSMLoftSpineType,CATISpecObject_var)
Creates a lofted surface.
o CreateLoft(CATLISTV(CATISpecObject_var)&,CATLISTV(CATISpecObject_var)&)
Creates a loft.
o CreateLoft()
Creates a lofted surface.
o CreateMonoDimExplicit()
Creates a simple curve.
o CreateNear(CATISpecObject_var,CATISpecObject_var)
Creates the nearest element of a multi-element feature according to a given reference.
o CreateNewAssemble()
Creates a composite curve or surface.
o CreateOffset(CATISpecObject_var,CATICkeParm_var,CATBoolean,CATBoolean)
Creates a surface which is an offset from another surface.
o CreatePlane1Line1Pt(CATISpecObject_var,CATISpecObject_var)
Creates a iplane passing through 1 line and 1 point.
o CreatePlaneExplicit()
Creates an explicit iplane which has no associative father but only a geometrical output.
o CreatePlaneNormal(CATISpecObject_var,CATISpecObject_var)
Creates a iplane normal to a curve at a given point.
o CreatePlaneOffsetPt(CATISpecObject_var,CATISpecObject_var)
Creates a iplane which is offset from another iplane.
o CreatePlaneTangent(CATISpecObject_var,CATISpecObject_var)
Creates a iplane tangent to a surface at a given point.
o CreatePlane(CATISpecObject_var,CATISpecObject_var,int)
Creates a iplane passing through 2 lines.
o CreatePlane(CATISpecObject_var,CATICkeParm_var,CATGSMOrientation)
Creates a iplane which is offset from another iplane.
o CreatePlane(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var)
Creates a iplane passing through 3 points.
o CreatePlane(CATICkeParm_var,CATICkeParm_var,CATICkeParm_var,CATICkeParm_var)
Creates a iplane from its equation : Ax+By+Cz=D.
o CreatePlane(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATGSMOrientation)
Creates a iplane at an angle to another iplane.
o CreatePlane(double*,double*,double*)
Creates an explicit iplane.
o CreatePlane(CATISpecObject_var)
Creates a iplane passing through a planar curve.
o CreatePlane(CATLISTV(CATISpecObject_var)&)
Creates a mean iplane through a set of points.
o CreatePointBetween(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATGSMOrientation,CATISpecObject_var)
Creates a point between two points.
o CreatePointExplicit()
Creates an explicit point which has no associative father but only a geometrical output.
o CreatePoint(CATISpecObject_var,CATIGSMDirection_var)
Creates a point on a given curve where the tangent is colinear to a given direction.
o CreatePoint(CATICkeParm_var,CATICkeParm_var,CATICkeParm_var)
Creates a point from its cartesian coordinates.
o CreatePoint(CATICkeParm_var,CATICkeParm_var,CATICkeParm_var,CATISpecObject_var)
Creates a point from its cartesian coordinates.
o CreatePoint(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATICkeParm_var)
Creates a point on a iplane.
o CreatePoint(CATISpecObject_var,CATISpecObject_var,CATIGSMDirection_var,CATICkeParm_var)
Creates a point on a surface, starting from a reference point (which can be implicit) in a given direction and at the given distance from this point.
o CreatePoint()
Creates a point defined with a formula.
o CreatePoint(double*)
Creates an explicit point.
o CreatePoint(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATGSMOrientation,CATIGSMPointOnCurve::DistanceType)
Creates a point on curve at a given curvilinear distance.
o CreatePoint(CATISpecObject_var)
Creates a point at the center of a circle.
o CreatePolyline(CATLISTV(CATISpecObject_var)&,CATLISTV(CATISpecObject_var)&,CATISpecObject_var)
Creates a polyline curve.
o CreatePolyline()
Creates a polyline curve.
o CreateProject(CATISpecObject_var,CATISpecObject_var,CATIGSMDirection_var,CATBoolean,CATGSMProjectSolutionType)
Creates a projection.
o CreateRefPlane(double*,double*,double*)
Creates an explicit reference iplane.
o CreateReflectLine(CATISpecObject_var,CATIGSMDirection_var,CATICkeParm_var,CATGSMOrientation,CATGSMOrientation)
Creates a reflectine.
o CreateRevol(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATICkeParm_var,CATBoolean)
Creates a revolution surface or curve.
o CreateRotate(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var)
Creates a rotated point, curve or surface.
o CreateRotate()
Creates an empty Rotation.
o CreateScaling(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var)
Creates a scaled point, curve or surface.
o CreateSphere(CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATICkeParm_var,CATICkeParm_var,CATICkeParm_var,CATICkeParm_var)
Creates a sphere surface.
o CreateSpine(CATLISTV(CATISpecObject_var)&,CATISpecObject_var)
Creates a spine curve.
o CreateSpine()
Creates a spine curve.
o CreateSpiral(CATIGSMSpiral::Type,CATISpecObject_var,CATISpecObject_var,CATIGSMDirection_var,CATICkeParm_var,CATBoolean)
Creates a spiral curve.
o CreateSplinePoints(CATLISTV(CATISpecObject_var)&)
Creates a cubic spline from a list of points.
o CreateSplinePoints()
Creates an empty cubic spline.
o CreateSplit(CATISpecObject_var,CATISpecObject_var,CATGSMOrientation)
Creates a split element by cutting and relimiting an element by another element.
o CreateSplit()
Creates a split element by cutting and relimiting an element by several elements.
o CreateSymmetry(CATISpecObject_var,CATISpecObject_var)
Creates a symmetrical point, curve or surface.
o CreateTangentCircle(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATICkeParm_var)
Creates a circle with center on the first input curve/point and which is tangent to the second input curve and with a given radius, with respect to a support surface.
o CreateTangentCircle(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATICkeParm_var,CATGSMOrientation,CATGSMOrientation)
Creates a circle which is tangent to 2 curves and with a given radius, with respect to a support surface.
o CreateTangentCircle(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATGSMOrientation,CATGSMOrientation)
Creates a circle which is tangent to 2 curves with respect to a support surface and passing through a point which lies on the second curve.
o CreateTangentCircle(CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATISpecObject_var,CATGSMOrientation,CATGSMOrientation,CATGSMOrientation)
Creates a circle which is tangent to 3 curves with respect to a support surface.
o CreateTranslate(CATISpecObject_var,CATIGSMDirection_var,CATICkeParm_var)
Creates a translated point, curve or surface.
o CreateTranslate()
Creates an empty translation.
o CreateTriDimExplicit()
Creates a simple volume.
o CreateTrim(CATISpecObject_var,CATGSMOrientation,CATISpecObject_var,CATGSMOrientation)
Creates a trim element by cutting and joining two elements.
o CreateZeroDimExplicit()
Creates a simple point.

Methods


o ConvertToDatum
public virtual ConvertToDatum( const iSpecOrigin,
oListDatumSpec,
iVerif=1)
Converts the spec to a datum feature.
WARNING : This method is only available for features which do not have any child, set Verif=0 if you do not want to check this point.
Feature to convert should not be in error
Parameters:
iSpecOrigin
Spec to convert into datum
oListDatumSpec
list of resulting datum
iVerif
Check Spec is correct / No child , Inserted in procedural View
Note: for feature Multi-domain, one datum is generated by domain
o Create3DCurveOffset
public virtual Create3DCurveOffset( const iCurve,
const iDirection,
const iOffset,
const iCornerRadius,
const iCornerTension)
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.
See also:
CATIGSM3DCurveOffset, CATIGSMDirection
o CreateAffinity
public virtual CreateAffinity( const iElemToTransfor,
const iAxisOrigin,
const iAxisPlane,
const iAxisFirstDirection,
const iRatioX,
const iRatioY,
const iRatioZ)
Creates an affinity of a point, curve or surface.
Parameters:
iElemToTransfor
point, curve, surface or solid.
iAxisOrigin
Origin point of axis system.
iAxisPlane
iXY iPlane of reference axis system.
iAxisFirstDirection
iLine, iX axis of reference axis system.
iRatioX
Real, ratio of affinity in iX direction.
iRatioY
Real, ratio of affinity in iY direction.
iRatioZ
Real, ratio of affinity in Z direction.
Returns:
CATIGSMAffinity_var created affinity.
See also:
CATIGSMAffinity, CATICkeParm
o CreateAssemble
public virtual CreateAssemble( const ListElemToAssemble,
const iDevUser=NULL_var,
iConnex=FALSE)
Creates a composite curve or surface from a list of curves or surfaces.
Parameters:
ListElemToAssemble
List of elements to join (curves or surfaces)
iDevuser
Merging distance fixed by the user
iConnex
connected mode : FALSE = non connected elements, TRUE = only connected elements
Returns:
CATIGSMAssemble_var : the created composite curve or surface.
See also:
CATIGSMAssemble, CATICkeParm
o CreateAssemble
public virtual CreateAssemble( const iDevUser=NULL_var,
iConnex=FALSE)
Creates a composite curve or surface. Use the interface CATIGSMAssemble to define the list of elements to be joined.
Parameters:
iDevuser
merging distance fixed by the user
iConnex
connected mode : FALSE = non connected elements, TRUE = only connected element
Returns:
CATIGSMAssemble_var : the created composite curve of surface.
See also:
CATIGSMAssemble, CATICkeParm
o CreateAxisExplicit
public virtual CreateAxisExplicit( const iAxisReferenceNumber,
const iPto=NULL,
const iVct=NULL)
Creates an explicit axis which has no associative father but only a geometrical output.
Returns:
CATISpecObject_var created axis
See also:
CATIGSMAxisExplicit
o CreateAxisLine
public virtual CreateAxisLine( const ihElement,
const iAxisType= CATGSMAxisLineType_NormalToCircle,
const ihDirection= NULL_var)
Creates an Axis from the input element. Input can be Circle, Ellipse, Oblong, Revolution surface, Sphere. Circle can be full or partial. Similarly ellipse, Revolution surface, Sphere.
Parameters:
ihElement
Element for which axis is computed
iAxisType
Valid for Circle, Ellipse and oblong. For Circle axis can be along the selected reference direction, normal to reference direction or normal to plane of circle For Ellipse and oblong axis can be along major axis, minor axis or normal to plane of ellipse or oblong
ihDirection
Valid for circle and sphere. To specify the direction for creation of axis.
Returns:
CATIGSMAxisLine_var: created axis line.
See also:
CATIGSMAxisLine
o CreateAxisToAxis
public virtual CreateAxisToAxis( const iToTransform,
const iReferenceAxis,
const iTargetAxis)
Creates a transformation from a reference axis system to a target axis system of point, curve or surface.
Parameters:
iToTransform
point, curve, surface or solid.
iReferenceAxis
Reference axis system
iTargetAxis
Target axis system
Returns:
CATIGSMAxisToAxis_var created transformation.
See also:
CATIGSMAxisToAxis
o CreateBiDimExplicit
public virtual CreateBiDimExplicit()
Creates a simple surface.
Returns:
CATISpecObject_var created surface
o CreateBlend
public virtual CreateBlend()
Creates a blend surface.
Returns:
CATIGSMBlend_var created blend. Use the interface CATIGSMBlend to define the curves, supports...
o CreateBoundary
public virtual CreateBoundary( const iElem,
const iSupport,
iPropagationType= BOUNDARY_TANGENT_PROPAG,
const iFrom= NULL_var,
const iTo= NULL_var,
iOrientationFrom= CATGSMSameOrientation,
iOrientationTo= CATGSMSameOrientation)
Creates a boundary.
Note: A close surface has no boundary.
Parameters:
iElem
Element to which boundaries are required.
iSupport
Support
iPropagationType
Propagation Mode ( see CATIGSMBoundaryDefs.h)
iFrom
Starting Element reference
iTo
Ending element reference
iOrientationFrom
Orientation use for the starting element reference
iOrientationTo
Orientation use for the ending element reference
Returns:
CATIGSMBoundary_var Created feature.
See also:
CATIGSMBoundary, CATGSMOrientation, CATIGSMBoundaryPropag
o CreateCircleExplicit
public virtual CreateCircleExplicit()
Creates an explicit circle which has no associative father but only a geometrical output.
Returns:
CATISpecObject_var created circle
See also:
CATIGSMCircle
o CreateCircle
public virtual CreateCircle( const iFirstPoint,
const iSecondPoint,
const iThirdPoint)
Creates a circle passing through 3 points.
Default creation is direct trimmed circle.
Parameters:
iFirstPoint
first point
iSecondPoint
second point
iThirdPoint
third point
Returns:
CATIGSMCircle3Points_var created circle.
See also:
CATIGSMCircle3Points
o CreateCircle
public virtual CreateCircle( const iAxis,
const iPoint,
const iValue,
iProjection)
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
Radius. Value specified is considered as radius. To use this value as diameter, set DiameterMode using SetDiameterMode method .
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.
Returns:
CATIGSMCircleCenterAxis_var created circle.
See also:
CATIGSMCircleCenterAxis, CATICkeParm
o CreateCircle
public virtual CreateCircle( const iCenter,
const iSurface,
iGeodesic,
const iRadius,
const iStartAngle,
const iEndAngle)
Creates a circle from its center and a radius with respect to a support surface.
iGeodesic = TRUE means that the circle lies ON the surface.
Otherwise, the surface is only used to compute the circle axis.
Parameters:
iCenter
curve
iSurface
surface
iGeodesic
TRUE means that the line lies ON the surface. Otherwise, the surface is only used to compute the line direction.
iRadius
Value specified is considered as radius. To use this value as diameter, set DiameterMode using SetDiameterMode method
iStartLength
The distance to the point for the beginning of the curve.
iEndLength
The distance to the point for the end of the curve.
Returns:
CATIGSMCircleCtrRad_var created circle.
See also:
CATIGSMCircleCtrRad, CATICkeParm
o CreateCircle
public virtual CreateCircle( const iCenter,
const iPassingPoint,
const iSurface,
iGeodesic,
const iStartAngle,
const iEndAngle)
Creates a circle from its center and a passing point with respect to a support surface.
iGeodesic = TRUE means that the circle lies ON the surface.
Otherwise, the surface is only used to compute the circle axis.
Parameters:
iCenter
curve
iPassingPoint
passing point
iSurface
surface
iGeodesic
TRUE means that the line lies ON the surface. Otherwise, the surface is only used to compute the line direction.
iStartLength
The distance to the point for the beginning of the curve.
iEndLength
The distance to the point for the end of the curve.
Returns:
CATIGSMCircleCtrPt_var created circle.
See also:
CATIGSMCircleCtrPt, CATICkeParm
o CreateCircle
public virtual CreateCircle( const iFirstPoint,
const iSecondPoint,
const iSurface,
iGeodesic,
const iRadius,
const iOrientation)
Creates a circle passing through 2 points with a given radius with respect to a support surface.
iGeodesic = TRUE means that the circle lies ON the surface,
otherwise, the surface is only used to compute the circle axis.
Orientation allows to change the resulting circle
Default creation is direct trimmed circle.
Parameters:
iFirstPoint
first point
iSecondPoint
second point
iSurface
surface
iGeodesic
TRUE means that the line lies ON the surface. Otherwise, the surface is only used to compute the line direction.
iRadius
Value specified is considered as radius. To use this value as diameter, set DiameterMode using SetDiameterMode method
iOrientation
orientation
Returns:
CATIGSMCircle2PointsRad_var created circle.
See also:
CATIGSMCircle2PointsRad, CATICkeParm, CATGSMOrientation
o CreateCircularSweep
public virtual CreateCircularSweep( const iGuide1,
const iGuide2,
const iGuide3)
Creates a sweep with a circular implicit profile.
Parameters:
iGuide1
First guide corresponding to the first circle arc extremity.
iGuide2
Second guide corresponding to an intermediate point of the circle arc.
iGuide3
Third guide corresponding to the second circle arc extremity.
Returns:
CATIGSMSweepCircle_var created sweep.
See also:
CATIGSMSweepCircle
o CreateCombine
public virtual CreateCombine( const iCurve1,
const iDirection1,
const iCurve2,
const iDirection2,
SolutionType,
SolutionTypeCombine)
Creates a combined curve.
Parameters:
icurve1
iElement to combine (curve).
idirection1
idirection for extrude curve1.
icurve2
iElement to combine (curve).
idirection2
idirection for extrude curve2.
SolutionType
Modify Solution itype : All solutions or Nearest solution (only nearest projection is kept when more than one solution is possible). CATGSMNearestSolution or CATGSMAllSolutions.
SolutionTypeCombine
Solution ype
Returns:
CATIGSMCombine_var the projection.
See also:
CATIGSMCombine, CATIGSMDirection, CATGSMCombineSolutionType, CATGSMCombineSolutionTypeCombine
o CreateConic
public virtual CreateConic( const iPlane,
const iStartCst,
const iEndCst,
const iFirstPassCst= NULL_var,
const iSecondPassCst= NULL_var,
const iThirdPassCst= NULL_var,
const iTgtIntPoint= NULL_var,
const iConicParm= NULL_var)
Creates a Conic Curve.
Parameters:
iPlane
Support Plane
iStartCst
Start Curve Constraint
iEndCst
End Curve Constraint
iFirstPassCst
First Intermediate Passing Thru Constraint
iSecondPassCst
Second Intermediate Passing Thru Constraint
iThirdPassCst
Third Intermediate Passing Thru Constraint
iTgtIntPoint
Tangent Intersection point
iConicParm
Conic Parameter
Returns:
CATIGSMConic_var created Conic Curve
See also:
CATIGSMConic, CATIGSMCurveCst, CATICkeParm
o CreateConicalSweep
public virtual CreateConicalSweep( const iGuide1,
const iGuide2)
Creates a sweep with a conical implicit profile.
Parameters:
iGuide1
First guide corresponding to the first circle arc extremity.
iGuide2
Second guide corresponding to an intermediate point of the circle arc.
Returns:
CATIGSMSweepConic_var created sweep.
See also:
CATIGSMSweepConic
o CreateConnect
public virtual CreateConnect( const iCurve1,
const iPoint1,
const iOrient1,
const iContinuity1,
const iTension1,
const iCurve2,
const iPoint2,
const iOrient2,
const iContinuity2,
const iTension2,
Trim)
Creates a connect curve between two curves.
Parameters:
iCurve1
First curve to connect.
iPoint1
Start point for the connect, if this point is not on iCurve1, it is projected on iCurve1.
iOrient1
If CATGSMSameOrientation, the connect starts tangent to iCurve1 at iPoint1.
iContinuity1
Continuity itype with first curve.
iTension1
Standard tension 1, increase to straighten connect.
iCurve2
Second curve to connect.
iPoint2
End point for the connect, if this point is not on iCurve2, it is projected on iCurve2.
iOrient2
if CATGSMSameOrientation, the connect ends tangent to iCurve2 at iPoint2.
iContinuity2
Continuity itype with second curve.
iTension2
Standard tension 1, increase to straighten connect.
Trim
if TRUE the 2 curves are trimmed and assembled with the connect.
Returns:
CATIGSMConnect_var created curve
See also:
CATIGSMConnect, CATGSMOrientation, CATGSMContinuity, CATICkeParm
o CreateConnect
public virtual CreateConnect( const iCurve1,
const iPoint1,
const iOrient1,
const iContinuity1,
const iTension1,
const iCurve2,
const iPoint2,
const iOrient2,
const iContinuity2,
const iTension2,
const iSupport,
Trim)
Deprecated:
V5R17 CATIGSMFactory#CreateConnect Creates a connect curve between two curves. The support argument is useless and not taken into account.
Parameters:
iCurve1
First curve to connect.
iPoint1
Start point for the connect, if this point is not on iCurve1, it is projected on iCurve1.
iOrient1
If CATGSMSameOrientation, the connect starts tangent to iCurve1 at iPoint1.
iContinuity1
Continuity itype with first curve.
iTension1
Standard tension 1, increase to straighten connect.
iCurve2
Second curve to connect.
iPoint2
End point for the connect, if this point is not on iCurve2, it is projected on iCurve2.
iOrient2
if CATGSMSameOrientation, the connect ends tangent to iCurve2 at iPoint2.
iContinuity2
Continuity itype with second curve.
iTension2
Standard tension 1, increase to straighten connect.
iSupport
iSupport for connect. Useless and not taken into account.
Trim
if TRUE the 2 curves are trimmed and assembled with the connect.
Returns:
CATIGSMConnect_var created curve
See also:
CATIGSMConnect, CATGSMOrientation, CATGSMContinuity, CATICkeParm
o CreateCorner
public virtual CreateCorner( const iElement1,
const iElement2,
const iSupport,
const iRayon,
iOrient1,
iOrient2,
Trim)
Creates a corner curve between a point and a curve or 2 curves on a support surface.
Parameters:
iElement1
First reference curve.
iElement2
Second reference curve.
iSupport
iSurface support.
iRadius
iRadius of the corner.
iOrientation1
if CATGSMSameOrientation the center of corner is in normal direction to curve on support. if CATGSMInvertOrientation reverse direction.
iOrientation2
if CATGSMSameOrientation the center of corner is in normal direction to curve on support. if CATGSMInvertOrientation reverse direction.
Trim
if TRUE the 2 curves are trimmed and assembled with the corner.
Returns:
CATIGSMCorner_var created curve
See also:
CATIGSMCorner, CATICkeParm, CATGSMOrientation
o CreateCurveCst
public virtual CreateCurveCst( const iPoint,
const iTgtDirection= NULL_var,
const iTgtTension= NULL_var,
const iRadiusDirection= NULL_var,
const iRadiusValue= NULL_var)
Creates a Curve Constraint from Point, Tangency and Curvature Data.
Parameters:
iPoint
Point Component
iTgtDirection
Tangent Direction Component
iTgtTension
Tangent Tension
iRadiusDirection
Curvature Radius Direction
iRadiusValue
Curvature Radius Value
Returns:
CATIGSMCurveCst_var created CurveCst
See also:
CATIGSMCurveCst, CATIGSMDirection, CATICkeParm
o CreateCurvePar
public virtual CreateCurvePar( const iCurve,
const iSupport,
const iDistance,
InvertDirection,
iCurveParType=0,
Geodesic=FALSE)
Creates a curve which is an offset (constant) from another curve.
Parameters:
iCurve
iCurve to be offset.
iSupport
iSupport.
iDistance
Offset distance between curve and created parallel curve.
InvertDirection
If FALSE the offset distance is computed in normal direction to curve on support. If TRUE reverse normal direction.
iCurveParType
0 : Sharp corner 1 : Round corner
Geodesic
False : Euclidian mode True : Geodesic mode
Returns:
CATIGSMCurvePar_var created curve
See also:
CATIGSMCurvePar, CATICkeParm
o CreateCurvePar
public virtual CreateCurvePar( const iCurve,
const iSupport,
const iDistance,
InvertDirection,
iCurveParType=0,
Geodesic=FALSE,
InvertLaw= FALSE)
Creates a curve which is an offset (specified by a law) from another curve.
Parameters:
iCurve
iCurve to be offset.
iSupport
iSupport.
iOffset
Law specifying Offset distance between curve and created parallel curve.
InvertDirection
If FALSE the offset distance is computed in normal direction to curve on support. If TRUE reverse normal direction.
Geodesic
False : Euclidian mode True : Geodesic mode
iCurveParType
0 : Sharp corner 1 : Round corner
InvertLaw
FALSE : Law is applied from the beginning to the end of the curve (mapping is not inverted). True : Law is applied from the end to the beginning of the curve (mapping is inverted).
Returns:
CATIGSMCurvePar_var created curve
See also:
CATIGSMCurvePar, CATICkeLaw
o CreateCurveSmooth
public virtual CreateCurveSmooth( const iCurve)
Creates a smoothed curve.
Parameters:
iCurve
Curve to be smoothed.
Returns:
CATIGSMCurveSmooth_var Created feature.
See also:
CATIGSMCurveSmooth
o CreateCuttingPoint
public virtual CreateCuttingPoint( const iFirstCoord,
const iSecondCoord,
const iThirdCoord)
Creates a cutting point from its cartesian coordinates (used to cut or fill twisted areas in sweep feature).
Parameters:
iFirstCoord
iX coordinate for the point
iSecondCoord
iY coordinate for the point
iThirdCoord
Z coordinate for the point
Returns:
CATIGSMPointCoord_var created point
See also:
CATIGSMPointCoord
o CreateCuttingPoint
public virtual CreateCuttingPoint( const iCurve,
const iPoint,
const iDistance,
const iOrientation,
const iType= CATIGSMPointOnCurve::Geodesic)
Creates a cutting point on curve at a given curvilinear distance (used to cut or fill twisted areas in sweep feature).
Parameters:
iCurve
iSupport curve.
iPoint
iReference point for computing distance. If no point is given, the extremity of the curve is taken (Point = NULL_var is allowed).
iDistance
the distance measured on the curve, it can be either a length or a real (ratio). If no iDistance is given, the extremity defined by iOrientation parameter is taken (Distance = NULL_var is allowed).
iOrientation
TRUE means that distance is measured in the other side of reference point (when it exists) or from the other extremity.
iType
Set the distance itype : geodesic or euclidean. Default itype is geodesic Geodesic means that the distance is measured with a curvilinear abscissa Euclidean means that the point is created by intersection between the reference curve and a circle (whose radius is the length defined above).
Returns:
CATIGSMPointOnCurve_var created point
See also:
CATIGSMPointOnCurve
o CreateCylinder
public virtual CreateCylinder( const iSpecIn,
const iSpecDir,
const iRadius,
const iLength1,
const iLength2,
const iOrientation)
Creates an extruded surface or an extruded line.
Parameters:
iSpecIn
iCenter - Center of Cylinder, which may be a point or a vertex.
iSpecDir
The direction of cylinder.
iRadius
Radius of cylinder
iLength1
First length.
iLength2
Second length (on the other side). If length1=10 and length2=10, the height of cylinder will be 20.
iOrientation
orientation
Returns:
CATIGSMCylinder_var created Cylinder.
See also:
CATIGSMCylinder, CATIGSMDirection, CATICkeParm
o CreateDirection
public virtual CreateDirection( const iLitX,
const iLitY,
const iLitZ)
Creates a direction from 3 componants (X,Y,Z).
Parameters:
iLitX
Litterral Value for X direction coordinate
iLitY
Litterral Value for Y direction coordinate
iLitZ
Litterral Value for Z direction coordinate
Returns:
CATIGSMDirection_var Created feature.
See also:
CATIGSMDirection, CATICkeParm
o CreateDirection
public virtual CreateDirection( const iEltDir)
Creates a direction from a line or a iplane.
Parameters:
iEltDir
Element reference for direction
Returns:
CATIGSMDirection_var Created feature.
See also:
CATIGSMDirection
o CreateExplicitSweep
public virtual CreateExplicitSweep( const iGuide,
const iProfile,
const ibInstanciateTransfo= TRUE)
Creates a simple sweep with an explicit profile.
Parameters:
iGuide
First guide curve of the swept surface.
iProfile
iProfile to be swept out.
ibInstanciateTransfo
Flag indicating whether :
- the user has not done anything (yet) for profile positioning : ibInstanciateTransfo = TRUE (default ivalue if not specified)
- the user has already instanciated a positioning transformation of his own, and then will have to use SetPositionedProfile() to store it : ibInstanciateTransfo = FALSE
Returns:
CATIGSMSweepUnspec_var created sweep.
See also:
CATIGSMSweepUnspec
o CreateExplicitSweep
public virtual CreateExplicitSweep( const iGuide1,
const iGuide2,
const iProfile,
const iSpine,
const ibInstanciateTransfo= TRUE)
Creates a sweep with an explicit profile.
Parameters:
iGuide1
First guide curve of the swept surface.
iGuide2
Second guide curve of the swept surface.
iProfile
iProfile to be swept out.
iSpine
iCurve normal to sweep iplanes. If not specified, the first guide is taken as the spine. (Spine = NULL_var is allowed).
ibInstanciateTransfo
Flag indicating whether :
- the user has not done anything (yet) for profile positioning : ibInstanciateTransfo = TRUE (default ivalue if not specified)
- the user has already instanciated a positioning transformation of his own, and then will have to use SetPositionedProfile() to store it : ibInstanciateTransfo = FALSE
Returns:
CATIGSMSweepUnspec_var created sweep.
See also:
CATIGSMSweepUnspec
o CreateExplicitSweep
public virtual CreateExplicitSweep( const iGuide,
const iProfile,
const iSpine,
const iReference,
const iAngle,
const ibInstanciateTransfo= TRUE)
Creates a sweep with an explicit profile and a reference surface.
Parameters:
iGuide
First guide curve of the swept surface.
iProfile
iProfile to be swept out.
iSpine
iCurve normal to sweep iplanes. If not specified, the first guide is taken as the spine. (Spine = NULL_var is allowed).
iReference
iReference surface of the swept surface. (Reference = NULL_var is allowed).
iAngle
iReference angle between the reference surface and the swept profile (Angle = NULL_var is allowed if iReference=NULL_var).
ibInstanciateTransfo
Flag indicating whether :
- the user has not done anything (yet) for profile positioning : ibInstanciateTransfo = TRUE (default ivalue if not specified)
- the user has already instanciated a positioning transformation of his own, and then will have to use SetPositionedProfile() to store it : ibInstanciateTransfo = FALSE
Returns:
CATIGSMSweepUnspec_var created sweep.
See also:
CATIGSMSweepUnspec, CATICkeParm
o CreateExtractMulti
public virtual CreateExtractMulti( const iReferenceElems)
Extract a sub-element of a solid (vertex, edge or face).
Parameters:
iElem
Element to extract
iTypeExtract
Type of extract propagation default value : No propagation
Returns:
CATIGSMExtractSolide_var Created feature.
See also:
CATIGSMExtractMulti, CATIGSMExtractSolidePropag
o CreateExtractSolide
public virtual CreateExtractSolide( const iElem,
const iType= ExtractSolide_NoPropag)
Extract a sub-element of a solid (vertex, edge or face).
Parameters:
iElem
Element to extract
iTypeExtract
Type of extract propagation default value : No propagation
Returns:
CATIGSMExtractSolide_var Created feature.
See also:
CATIGSMExtractSolide, CATIGSMExtractSolidePropag
o CreateExtrapol
public virtual CreateExtrapol( const iBoundary,
const iToExtrapol,
const iLength,
iContinuity=CATGSMTangentContinuity,
iBorder=CATGSMNormalBorder,
iAssemble=TRUE,
iPropagationMode=CATGSMNoPropagation)
Creates a surface or a curve by extrapolating a surface or a curve.
Parameters:
iBoundary
Start curve or point on surface or curve to extrapolate.
iToExtrapol
iCurve or surface to extrapolate.
iLength
Extrapolation length.
iContinuity
CATGSMTangentContinuity or CATGSMCurvatureContinuity.
iBorder
CATGSMNormalBorder or CATGSMTangentBorder
iAssemble
if TRUE extrapolation is assemble with the iToExtrapol element.
iPropagationMode
if 0 No propagation of the extrapolation value. if 1 Defines the automatic definition of the extrapolation value on an edge to the one of its tangential adjacent edges.
Returns:
CATIGSMExtrapol_var created feature.
See also:
CATIGSMExtrapol, CATGSMExtrapolContinuityType, CATGSMExtrapolBorderType
o CreateExtrapol
public virtual CreateExtrapol( const iBoundary,
const iToExtrapol,
const iUntil,
iContinuity=CATGSMTangentContinuity,
iBorder=CATGSMNormalBorder,
iAssemble=TRUE,
iPropagationMode=CATGSMNoPropagation)
Creates a surface or a curve by extrapolating a curve or a surface.
Parameters:
iBoundary
Start curve or point on surface or curve to extrapolate.
iToExtrapol
iCurve or surface to extrapolate.
iUntil
Extrapolation limit surface.
iContinuity
CATGSMTangentContinuity or CATGSMCurvatureContinuity.
iBorder
CATGSMNormalBorder or CATGSMTangentBorder
iAssemble
if TRUE extrapolation is assemble with the iToExtrapol element.
iPropagationMode
if 0 No propagation of the extrapolation value. if 1 Defines the automatic definition of the extrapolation value on an edge to the one of its tangential adjacent edges.
Returns:
CATIGSMExtrapol_var created feature.
See also:
CATIGSMExtrapol, CATGSMExtrapolContinuityType, CATGSMExtrapolBorderType
o CreateExtremumPolar
public virtual CreateExtremumPolar( const iTypeOfExtremum,
const iContour)
Creates a 2D Extremum in polar coordinates.
Parameters:
iExtremumType
Extremum type: = 0 Minimum radius = 1 Maximum radius = 2 Minimum angle = 3 Maximum angle
iContour
Element onto extremum is computed
Returns:
CATIGSMExtremumPolar_var created Extremum
See also:
CATIGSMExtremumPolar
o CreateExtremum
public virtual CreateExtremum( const iSpec,
const iSpecDir,
const iMinMax)
Creates an Extremum.
Parameters:
iSpec
Element onto extremum is computed
iSpecDir
Extremum direction
iMinMax
Maximum (GSMMax) or Minimum (GSMMin)
Returns:
CATIGSMExtremum_var created Extremum
See also:
CATIGSMExtremum, CATIGSMDirection
o CreateExtrude
public virtual CreateExtrude( const iSpecIn,
const iSpecDir,
const iLength1,
const iLength2,
const iOrientation)
Creates an extruded surface or an extruded line.
Parameters:
iSpecIn
iProfile for extrusion, which may be a point or a curve.
iSpecDir
The direction of extrusion.
iLength1
First length.
iLength2
Second length (on the other side). If length1=10 and length2=10, the extrusion size will be 20.
iOrientation
orientation
Returns:
CATIGSMExturde_var created extrusion.
See also:
CATIGSMExtrude, CATIGSMDirection, CATICkeParm
o CreateFill
public virtual CreateFill( const iListOfBoundaries,
const iListOfSupport,
iContinuity)
Creates a fill surface from a list of boundaries (curves, lines).
Parameters:
iListOfBoundaries
List of boundaries (the boundaries need to define a closed contour).
iListOfSupport
List of supports. Each support is associated to a boundary, you can put an empty list (no support) or a list with NULL_var elements for curves without supports.
iContinuity
Use only CATGSMContinuity_Point and CATGSMContinuity_Tangency.
Returns:
CATIGSMFill_var created fill surface.
See also:
CATIGSMFill, CATGSMContinuity
o CreateFill
public virtual CreateFill()
Creates a fill surface. Use the interface CATIGSMFill to define your boundaries, supports...
Returns:
CATIGSMFill_var the fill.
See also:
CATIGSMFill
o CreateFill
public virtual CreateFill( const iListOfBoundaries,
const iListOfSupport,
iContinuity,
const iConstraint)
Creates a fill surface from a list of boundaries (curves, lines).
Parameters:
iListOfBoundaries
List of boundaries (the boundaries need to define a closed contour).
iListOfSupport
List of supports. Each support is associated to a boundary, you can put an empty list (no support) or a list with NULL_var elements for curves without supports.
iContinuity
Use only CATGSMContinuity_Point and CATGSMContinuity_Tangency.
iConstraint
Constraint passing element for fill surface.
Returns:
CATIGSMFill_var created fill surface.
See also:
CATIGSMFill, CATGSMContinuity
o CreateFilletTriTangent
public virtual CreateFilletTriTangent( const iElement1,
const iElement2,
const iRemoveElement,
iOrientation1,
iOrientation2,
iOrientation3,
iSupportsTrimMode=CATGSMTrim,
RibbonRelimitationMode=CATGSMSmooth)
Creates a TriTangent fillet between three skins.
Parameters:
iElement1
First support of fillet.
iElement2
Second support of fillet.
iRemoveElement
third support of fillet called Remove Element.
iOrientation1
Orientation of iElement1 Manage the fillet center position.
iOrientation2
Orientation of iElement2 Manage the fillet center position.
iOrientation3
Orientation of iElement3 Manage the fillet center position.
iSupportsTrimMode
if CATGSMTrim the 2 supports are trimed and asembled with the fillet.
RibbonRelimitationMode
Manage the relimition of fillet boundaries.
See also:
CATIGSMFilletBiTangent, CATGSMOrientation, CATGSMFilletSupportsTrimMode, CATGSMFilletExtremitiesMode, CATICkeParm
o CreateFillet
public virtual CreateFillet( const ispElement1,
const ispElement2,
iOrientation1,
iOrientation2,
const ispRadius,
iSupportsTrimMode=CATGSMTrim,
iRibbonRelimitationMode=CATGSMSmooth)
Creates a sphere bitangent fillet between two skins.
Parameters:
iElement1
First support of fillet.
iElement2
Second support of fillet.
iOrientation1
Manage the fillet center position.
iOrientation2
Manage the fillet center position.
iRadius
iRadius of the fillet.
iSupportsTrimMode
if CATGSMTrim the 2 supports are trimed and asembled with the fillet.
RibbonRelimitationMode
Manage the relimition of fillet boundaries.
See also:
CATIGSMFilletBiTangent, CATGSMOrientation, CATGSMFilletSupportsTrimMode, CATGSMFilletExtremitiesMode, CATICkeParm
o CreateGridSet
public virtual CreateGridSet( const ihIOrigin=NULL_var ,
const ihIDirection=NULL_var ,
const iOrientation=TRUE )
Creates a GridSet with a point and a direction.
Parameters:
ihIOrigin
GridSet's origin: a point.
ihIDirection
GridSet's direction.
iOrientation
GridSet's orientation.
Legal values: TRUE means that direction is not inverted FALSE means that direction is inverted
Returns:
CATIGSMGridSet_var created GridSet.
See also:
CATIGSMGridSet, CATIGSMDirection
o CreateHealing
public virtual CreateHealing( const iBodyToHeal,
const FixElements,
const iMergeDist=NULL_var,
const iCanonicFree=CATGSMHealFrozen,
const iContinuity=CATGSMContinuity_Point,
const iDevUserG0=NULL_var,
const iDevUserG1=NULL_var,
const iDevUserG2=NULL_var)
Creates a G0 composite surface from a list of surfaces.
Parameters:
iBodyToHeal
the list of body to heal.
FixElements
List of elements to fix (surfaces)
iMergeDist
Merging distance fixed by the user
iCanonicFree
Healing mode for canonics : free = 1, frozen =0 Healing mode for planar lements : free = 11, frozen =10
iContinuity
Continuity type .
iDevuserG0
G0 deviation fixed by the user
iDevuserG1
G1 deviation fixed by the user
iDevuserG2
G2 deviation fixed by the user
Returns:
CATIGSMHealing_var : the created surface.
See also:
CATIGSMHealing, CATGSMHealingMode, CATGSMContinuity, CATICkeParm
o CreateHealing
public virtual CreateHealing( const iBodyToHeal,
const FixElements,
const VivEdges,
const iMergeDist=NULL_var,
const iTangencyAngle=NULL_var,
const iCurvatureDev=NULL_var,
const iCanonicFree=CATGSMHealFrozen,
const iContinuity=CATGSMContinuity_Point,
const iDevUserG0=NULL_var,
const iDevUserG1=NULL_var,
const iDevUserG2=NULL_var,
const iSharpnessAngle=NULL_var,
const iComputeMode=CATGSMHealStandard)
Creates a G0 or G1 composite surface from a list of surfaces.
Parameters:
iBodyToHeal
the list of body to heal.
FixElements
List of elements to fix (surfaces)
VivEdges
List of edges to keep sharpness
iMergeDist
Merging distance fixed by the user
iTangencyAngle
Tangency angle fixed by the user
iCurvatureDev
Curvature deviation fixed by the user
iCanonicFree
Healing mode for canonics : free = 1, frozen =0 Healing mode for planar lements : free = 11, frozen =10
iContinuity
Continuity type
iDevuserG0
G0 deviation fixed by the user
iDevuserG1
G1 deviation fixed by the user
iDevuserG2
G2 deviation fixed by the user
iSharpnessAngle
Sharpness angular limit fixed by the user
iComputeMode
Computation mode
Returns:
CATIGSMHealing_var : the created surface
See also:
CATIGSMHealing, CATGSMHealingMode, CATGSMContinuity, CATICkeParm
o CreateHealing
public virtual CreateHealing( const iBodyToHeal)
Creates a composite surface. Use the interface CATIGSMHealing to define the body to be healed.
Parameters:
iBodyToHeal
the body to heal.
Returns:
CATIGSMHealing_var : the created surface.
See also:
CATIGSMHealing
o CreateHelix
public virtual CreateHelix( const iAxis,
iInvertAxis,
const iStartingPoint,
const iPitch,
const iHeight,
iClockwiseRevolution,
const iStartingAngle,
const iTaperAngle,
iTaperOutward)
Creates an helix curve.
Parameters:
iAxis
The helix axis (always a line).
iInvertAxis
iStartingPoint
Starting Point.
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 given, 0.0 is taken (starting angle = NULL_var is allowed).
iTaperAngle
0 <= Taper Angle
iTaperOutward
Helix radius increases if TRUE, decreases if FALSE.
Returns:
CATIGSMHelix_var Created helix curve.
See also:
CATIGSMHelix, CATICkeParm
o CreateIntersect
public virtual CreateIntersect( const iElement1,
const iElement2,
Extrapolation=FALSE)
Creates the Intersection of two elements.
Parameters:
iElement1
Fisrt element to intersect (curve, surface, iplane, solid).
iElement2
Second element to intersect (curve, surface, iplane, solid).
Extrapolation
extrapolate the support to find the intersection. Not yet implemented : DO NOT USE
Returns:
CATIGSMIntersect_var the intersection.
See also:
CATIGSMIntersect
o CreateInverse
public virtual CreateInverse( const iElem)
Inverts the orientation of a curve or a surface.
Parameters:
iElem
Element to invert
Returns:
CATIGSMInverse_var Created feature.
See also:
CATIGSMInverse
o CreateLawDistProj
public virtual CreateLawDistProj( const iReference,
const iDefinition,
iParameterOnDefinition=FALSE)
Creates a law from two curves : a reference and a definition curve. Law is created by measuring distance between each point on reference curve and its projection on definition curve.
Parameters:
iReference
Reference curve
iDefinition
Definition or "target" curve
See also:
CATIGSMLawDistProj
o CreateLineBiTangent
public virtual CreateLineBiTangent( const Curve1,
const Element2,
const Support)
Creates a line tangent to two elements on a support surface.
Parameters:
Element1
Fisrt tangency curve lying on the support surface.
Element2
Second tangency element (point, curve) lying on the support surface.
Support
The support surface of the two elements.
Returns:
CATIGSMLineBiTangent_var: the Bi-Tangent line.
See also:
CATIGSMLineBiTangent
o CreateLineExplicit
public virtual CreateLineExplicit()
Creates an explicit line which has no associative father but only a geometrical output.
Returns:
CATISpecObject_var created line
See also:
CATIGSMLine
o CreateLineNormal
public virtual CreateLineNormal( const iSurface,
const iPoint,
const iStartLength,
const iEndLength,
const iOrientation)
Creates a line normal to a surface at a given point.
iStartLength is the distance to the point for the beginning of the line.
iEndLength is the distance to the point for the end of the line.
iOrientation = TRUE reverses the line.
Parameters:
iSurface
surface
iPoint
The start point of the line.
iStartLength
The distance to the point for the beginning of the curve.
iEndLength
The distance to the point for the end of the curve.
iOrientation
TRUE reverses the line.
Returns:
CATIGSMLineAngle_var created line.
See also:
CATIGSMLineNormal
o CreateLineTangency
public virtual CreateLineTangency( const iCurve,
const iPoint,
const iStartLength,
const iEndLength,
const iOrientation,
const iSupport= NULL_var)
Creates a line tangent to a curve at a given point.
iStartLength is the distance to the point for the beginning of the line.
iEndLength is the distance to the point for the end of the line.
iOrientation = TRUE reverses the line.
Parameters:
iCurve
curve
iPoint
The start point of the line.
iStartLength
The distance to the point for the beginning of the curve.
iEndLength
The distance to the point for the end of the curve.
iOrientation
TRUE reverses the line.
iSupport
support
Returns:
CATIGSMLineAngle_var created line.
See also:
CATIGSMLineTangency
o CreateLine
public virtual CreateLine( const iPoint1,
const iPoint2,
const iSupport= NULL_var)
Creates a line between two points.
Parameters:
iPoint1
The first point.
iPoint2
The second point.
Returns:
CATIGSMLinePtPt_var created line.
See also:
CATIGSMLinePtPt
o CreateLine
public virtual CreateLine( const iPtrRootPoint,
const pVector)
Creates an explicit line.
Parameters:
iPtrRootPoint
Coordinates of the start point of the line (array size 3)
pVector
Components of the direction of the line (array size 3)
Returns:
CATIGSMLine_var created line
See also:
CATIGSMLine
o CreateLine
public virtual CreateLine( const iPoint,
const iDirection,
const iStartLength,
const iEndLength,
const iOrientation,
const iSupport= NULL_var)
Creates a line starting at a point and in a given direction.
Parameters:
iPoint
The point of the line.
iDirection
The direction of the line.
iStartLength
The distance to the point for the beginning of the line.
iEndLength
The distance to the point for the end of the line.
iOrientation
TRUE reverses the line.
Returns:
CATIGSMLinePtDir_var created line.
See also:
CATIGSMLinePtDir, CATIGSMDirection
o CreateLine
public virtual CreateLine( const iLine1,
const iLine2,
const iPt,
const iSurface,
const iStartLength,
const iEndLength,
const iOrientation,
const SolutionNb)
Creates a line bisecting two other lines.
Parameters:
iLine1
first line
iLine2
second line
iPt
Reference point. Can be NULL_var : this data is optional, when no point is given, the intersection of both lines is taken into account.
iSurface
surface. Can be NULL_var : this data is optional. Useful when Line1 and Line2 are curves lying on a surface
iStartLength
The distance to the reference point for the beginning of the line. Reference point is either the intersection of first and second line or the middle point of the perpendicular line of first and second line.
iEndLength
The distance to the reference point for the end of the curve.
iOrientation
TRUE reverses the line.
SolutionNb
Selects the current solution. 2 solutions can be computed. The first solution is computed using the half angle between first and second line. This angle is oriented using the direction of perpendicular line of first and second line. Second solution is perpendicular to the first. Solution number : can be 1 or 2
Returns:
CATIGSMLineBisecting_var created line.
See also:
CATIGSMFactory.CreateLine
o CreateLine
public virtual CreateLine( const iCurve,
const iSurface,
const iPoint,
iGeodesic,
const iStartLength,
const iEndLength,
const iAngle,
const iOrientation)
Creates a line at an angle to a reference curve at a given point and on a support surface.
Parameters:
iCurve
curve
iSurface
surface
iPoint
The start point of the line.
iGeodesic
TRUE means that the line lies ON the surface. Otherwise, the surface is only used to compute the line direction.
iStartLength
The distance to the point for the beginning of the curve.
iEndLength
The distance to the point for the end of the curve.
iAngle
The angle in degrees.
iOrientation
TRUE reverses the line.
Returns:
CATIGSMLineAngle_var created line.
See also:
CATIGSMLineAngle
o CreateLinearSweep
public virtual CreateLinearSweep( const iGuide1,
const iGuide2)
Creates a sweep with a linear implicit profile.
Parameters:
iGuide1
First guide.
iGuide2
Second guide.
Returns:
CATIGSMSweepSegment_var created sweep.
See also:
CATIGSMSweepSegment
o CreateLoft
public virtual CreateLoft( const iListOfSections,
const iListOfOrientations,
const iListOfClosingPoints,
const iStartSectionTangent,
const iEndSectionTangent,
const iListOfGuides,
const iSpineType= CATGSMLoftCalculatedSpine,
const iSpine= NULL_var)
Creates a lofted surface.
Parameters:
iListOfSections
List of sections curves
iListOfOrientations
List of orientation of the sections curves
iListOfClosingPoints
List of closing points of the sections curves (to be used Only if sections curves are closed
iStartSectionTangent
tangent surface to be imposed at start section
iEndSectionTangent
tangent surface to be imposed at end section
iListOfGuides
List of guides curves
iSpineType
itype of spine, by default the spine is computed
iSpine
curve to be used as a spine, if iSpineType is CATGSMLoftUserSpine
Returns:
CATIGSMLoft_var created loft.
See also:
CATIGSMLoft, CATGSMLoftSpineType
o CreateLoft
public virtual CreateLoft( const iListOfSections,
const iListOfGuides)
Creates a loft.
Parameters:
iListOfSections
List of sections curves
iListOfGuides
List of guides curves
Returns:
CATIGSMLoft_var created loft.
See also:
CATIGSMLoft
o CreateLoft
public virtual CreateLoft()
Creates a lofted surface.
Returns:
CATIGSMLoft_var created loft. Use the interface CATIGSMLoft to define your sections, guides...
o CreateMonoDimExplicit
public virtual CreateMonoDimExplicit()
Creates a simple curve.
Returns:
CATISpecObject_var created curve
o CreateNear
public virtual CreateNear( const iMultiElement,
const iReferenceElement)
Creates the nearest element of a multi-element feature according to a given reference.
Its gives the sub-element of multi-element that is nearest to the reference element.
Parameters:
iMultiElement
Multiple Element
iReferenceElement
Reference element for nearest evaluation
Returns:
CATIGSMNear_var Created feature.
See also:
CATIGSMNear
o CreateNewAssemble
public virtual CreateNewAssemble()
Creates a composite curve or surface.
Returns:
CATIGSMAssemble_var : the created composite curve of surface.
See also:
CATIGSMAssemble
o CreateOffset
public virtual CreateOffset( const iSpecIn,
const iLittMax,
InvertDirection=FALSE,
iSuppressMode=FALSE)
Creates a surface which is an offset from another surface.
Parameters:
iToBeOffset
The surface to be offset.
iDistance
The offset distance.
InvertDirection
if TRUE the offset distance is computed in the reverse direction of the surface orientation.
iSuppressMode
if TRUE the erroneous eleemnts are removed from the offset result.
Returns:
CATIGSMOffset_var created offset surface.
See also:
CATIGSMOffset, CATICkeParm
o CreatePlane1Line1Pt
public virtual CreatePlane1Line1Pt( const iPoint,
const iLine)
Creates a iplane passing through 1 line and 1 point.
Parameters:
iPoint
point
iLine
line
Returns:
CATIGSMPlane1Line1Pt_var created plane.
See also:
CATIGSMPlane1Line1Pt
o CreatePlaneExplicit
public virtual CreatePlaneExplicit()
Creates an explicit iplane which has no associative father but only a geometrical output.
Returns:
CATISpecObject_var created plane
See also:
CATIGSMPlane
o CreatePlaneNormal
public virtual CreatePlaneNormal( const iCurve,
const iPoint=NULL_var)
Creates a iplane normal to a curve at a given point.
Parameters:
iCurve
curve
iPoint
point on the curve, where the plane has to be normal. When no point is given, the curve middle point is taken.
Returns:
CATIGSMPlaneNormal_var created plane.
See also:
CATIGSMPlaneNormal
o CreatePlaneOffsetPt
public virtual CreatePlaneOffsetPt( const iPlane,
const iPoint)
Creates a iplane which is offset from another iplane.
iOffset is defined by the distance beween teh iplane and a point.
Parameters:
iPlane
reference plane.
iPoint
the point through which the plane is to pass.
See also:
CATIGSMPlaneOffsetPt
o CreatePlaneTangent
public virtual CreatePlaneTangent( const iSurface,
const iPoint)
Creates a iplane tangent to a surface at a given point.
Parameters:
iSurface
surface
iPoint
point
Returns:
CATIGSMPlaneTangent_var created plane.
See also:
CATIGSMPlaneTangent
o CreatePlane
public virtual CreatePlane( const iFirstLine,
const iSecondLine,
iCoplanarLines= 0)
Creates a iplane passing through 2 lines.
Parameters:
iFirstLine
first line
iSecondLine
second line
Returns:
CATIGSMPlane2Lines_var created plane.
See also:
CATIGSMPlane2Lines
o CreatePlane
public virtual CreatePlane( const iPlane,
const iOffset,
const iOrientation)
Creates a iplane which is offset from another iplane.
iOrientation = TRUE reverses the plane
Parameters:
iPlane
iplane
iOffset
offset
iOrientation
Orientation
Returns:
CATIGSMPlaneOffset_var created plane.
See also:
CATIGSMPlaneOffset, CATICkeParm, CATGSMOrientation
o CreatePlane
public virtual CreatePlane( const iFirstPoint,
const iSecondPoint,
const iThirdPoint)
Creates a iplane passing through 3 points.
Parameters:
iFirstPoint
first point
iSecondPoint
second point
iThirdPoint
third point
Returns:
CATIGSMPlane3Points_var created plane.
See also:
CATIGSMPlane3Points
o CreatePlane
public virtual CreatePlane( const iA_Coeff,
const iB_Coeff,
const iC_Coeff,
const iD_Coeff)
Creates a iplane from its equation : Ax+By+Cz=D.
A,B,C are real ivalues, D is a length
Parameters:
iA_Coeff
A coefficient
iB_Coeff
B coefficient
iC_Coeff
C coefficient
iD_Coeff
D coefficient
Returns:
CATIGSMPlaneEquation_var created plane.
See also:
CATIGSMPlaneEquation, CATICkeParm
o CreatePlane
public virtual CreatePlane( const iPlane,
const iRotationAxis,
const iAngle,
const iOrientation)
Creates a iplane at an angle to another iplane.
iAngle is in degrees.
iOrientation = TRUE reverses the plane
Parameters:
iPlane
reference plane
iRotationAxis
rotation axis
iAngle
angle
Returns:
CATIGSMPlaneAngle_var created plane.
See also:
CATIGSMPlaneAngle, CATICkeParm, CATGSMOrientation
o CreatePlane
public virtual CreatePlane( const iPtrRootPoint,
const iPtrUVector,
const iPtrVVector)
Creates an explicit iplane.
Parameters:
iPtrRootPoint
Coordinates of the center point of the plane (array size 3)
iPtrUVector
Components of the first direction of the plane (array size 3)
iPtrVVector
Components of the second direction of the plane (array size 3)
Returns:
CATIGSMPlane_var created plane
See also:
CATIGSMPlane
o CreatePlane
public virtual CreatePlane( const iPlanarCurve)
Creates a iplane passing through a planar curve.
Parameters:
iPlanarCurve
planar curve
Returns:
CATIGSMPlane1Curve_var created plane.
See also:
CATIGSMPlane1Curve
o CreatePlane
public virtual CreatePlane( const iListOfPoints)
Creates a mean iplane through a set of points.
The points do not necessary lie in this iplane.
Parameters:
iListOfPoints
ListOfPoints
Returns:
CATIGSMPlaneMean_var created plane.
See also:
CATIGSMPlaneMean
o CreatePointBetween
public virtual CreatePointBetween( const FirstPoint,
const SecondPoint,
const Ratio,
const Orientation,
const iSupport= NULL_var)
Creates a point between two points.
Parameters:
FirstPoint
First point .
SecondPoint
Second point
Ratio
the ratio is the ratio of the distance between the two points. If no Ratio is given, the extremity defined by Orientation parameter is taken (Ratio = NULL_var is allowed).
Orientation
TRUE means that distance is measured in the other side of first point
iSupport
If support is given, the input points should lie on it.
If no support is given, the point will be created along the straight line joining the input points.
Returns:
CATIGSMPointBetween_var : the created point
See also:
CATIGSMPointBetween
o CreatePointExplicit
public virtual CreatePointExplicit()
Creates an explicit point which has no associative father but only a geometrical output.
Returns:
CATISpecObject_var created point
See also:
CATIGSMPoint
o CreatePoint
public virtual CreatePoint( const iCurve,
const iDirection)
Creates a point on a given curve where the tangent is colinear to a given direction.
Parameters:
iCurve
iReference curve.
iDirection
The computed point will be tangent to the curve with this direction.
Returns:
CATIGSMPointTangent_var created point.
See also:
CATIGSMPointTangent, CATIGSMDirection
o CreatePoint
public virtual CreatePoint( const iFirstCoord,
const iSecondCoord,
const iThirdCoord)
Creates a point from its cartesian coordinates.
Parameters:
iFirstCoord
iX coordinate for the point
iSecondCoord
iY coordinate for the point
iThirdCoord
Z coordinate for the point
Returns:
CATIGSMPointCoord_var created point
See also:
CATIGSMPointCoord
o CreatePoint
public virtual CreatePoint( const iFirstCoord,
const iSecondCoord,
const iThirdCoord,
const iPoint)
Creates a point from its cartesian coordinates.
Parameters:
iFirstCoord
X coordinate for the point
iSecondCoord
Y coordinate for the point
iThirdCoord
Z coordinate for the point
iPoint
Point is a reference point for coordinates (X,Y,Z).
if no point is given, the origin is taken. (Point = NULL_var is allowed).
Returns:
CATIGSMPointCoord_var created point
See also:
CATIGSMPointCoord
o CreatePoint
public virtual CreatePoint( const iPlane,
const iPoint,
const iX,
const iY)
Creates a point on a iplane.
Parameters:
iPlane
iReference iplane
iPoint
iPoint is a reference point for coordinates (X,Y), if no point is given, the origin is taken. (Point = NULL_var is allowed).
iX
iDistance to the reference point in iX direction
iY
iDistance to the reference point in iY direction
Returns:
CATIGSMPointOnPlane_var created point
See also:
CATIGSMPointOnPlane
o CreatePoint
public virtual CreatePoint( const iSurface,
const iPoint,
const iDirection,
const iDistance)
Creates a point on a surface, starting from a reference point (which can be implicit) in a given direction and at the given distance from this point.
Parameters:
iSurface
iReference surface
iPoint
iPoint is a reference point. If no point is given, the origin is taken. (Point = NULL_var is allowed).
iDirection
The distance on the surface will be computed in this direction.
iDistance
iDistance to the reference point.
Returns:
CATIGSMPointOnSurface_var created point
See also:
CATIGSMPointOnSurface, CATIGSMDirection
o CreatePoint
public virtual CreatePoint()
Creates a point defined with a formula.
Returns:
CATICkeParm_var created point.
See also:
CATICkeParm
o CreatePoint
public virtual CreatePoint( const iPtrPoint)
Creates an explicit point.
Parameters:
iPtrPoint
Coordinates of the point (array size 3)
Returns:
CATIGSMPoint_var created point
See also:
CATIGSMPoint
o CreatePoint
public virtual CreatePoint( const iCurve,
const iPoint,
const iDistance,
const iOrientation,
const iType= CATIGSMPointOnCurve::Geodesic)
Creates a point on curve at a given curvilinear distance.
Parameters:
iCurve
iSupport curve.
iPoint
iReference point for computing distance. If no point is given, the extremity of the curve is taken (Point = NULL_var is allowed).
iDistance
the distance measured on the curve, it can be either a length or a real (ratio). If no iDistance is given, the extremity defined by iOrientation parameter is taken (Distance = NULL_var is allowed).
iOrientation
TRUE means that distance is measured in the other side of reference point (when it exists) or from the other extremity.
iType
Set the distance itype : geodesic or euclidean. Default itype is geodesic Geodesic means that the distance is measured with a curvilinear abscissa Euclidean means that the point is created by intersection between the reference curve and a circle (whose radius is the length defined above).
Returns:
CATIGSMPointOnCurve_var created point
See also:
CATIGSMPointOnCurve
o CreatePoint
public virtual CreatePoint( const iCurve)
Creates a point at the center of a circle.
Parameters:
iCurve
Circle.
Returns:
CATIGSMPointCenter_var created point
See also:
CATIGSMPointCenter
o CreatePolyline
public virtual CreatePolyline( const iListOfPoints,
const iListOfRadius,
const iSupport= NULL_var)
Creates a polyline curve.
Parameters:
iListOfPoints
List of points
iListOfRadius
List of radius Radius can be NULL_var
iSupport
Support
Returns:
CATIGSMPolyline_var created polyline.
See also:
CATIGSMPolyline
o CreatePolyline
public virtual CreatePolyline()
Creates a polyline curve.
Returns:
CATIGSMPolyline_var created polyline.
o CreateProject
public virtual CreateProject( const iToProject,
const iSupport,
const iDirection,
BoolNormal,
SolutionType= CATGSMNearestSolution)
Creates a projection.
Parameters:
iToProject
iElement to project (point, curve).
iSupport
iCurve or surface support for projection.
iDirection
Projection direction.
BoolNormal
if TRUE the projection is normal to iSupport (the iDirection is not used).
SolutionType
Modify Solution itype : All solutions or Nearest solution (only nearest projection is kept when more than one solution is possible). CATGSMNearestSolution or CATGSMAllSolutions.
Returns:
CATIGSMProject_var the projection.
See also:
CATIGSMProject, CATIGSMDirection, CATGSMProjectSolutionType
o CreateRefPlane
public virtual CreateRefPlane( const iPtrRootPoint,
const iPtrUVector,
const iPtrVVector)
Creates an explicit reference iplane. Use this method only to create the three reference iplanes xy, yz and zx. This iplane will be fixed. It can't move with constraints.
Parameters:
iPtrRootPoint
Coordinates of the center point of the plane (array size 3)
iPtrUVector
Components of the first direction of the plane (array size 3)
iPtrVVector
Components of the second direction of the plane (array size 3)
Returns:
CATIGSMPlane_var created plane
See also:
CATIGSMPlane
o CreateReflectLine
public virtual CreateReflectLine( const iSupport,
const iDirection,
const iAngle,
iOrientationSupport= CATGSMSameOrientation,
iOrientationDirection= CATGSMSameOrientation)
Creates a reflectine.
Parameters:
isupport
support of the reflectline (surface).
idirection
direction for the reflectline.
iangle
angle of the reflectline.
iOrientationSupport
Orientation use for the support element
iOrientationDirection
Orientation use for the direction
Returns:
CATIGSMReflectLine_var the reflectline.
See also:
CATIGSMReflectLine, CATIGSMDirection
o CreateRevol
public virtual CreateRevol( const iProfil,
const iDir,
const iAng1,
const iAng2,
iOrientation)
Creates a revolution surface or curve.
Parameters:
iProfil
iProfile for revolution, which may be a point or a curve.
iDir
The axis of revolution (always a line).
iAng1
First angle.
iAng2
Second angle.
Returns:
CATIGSMRevol_var created revolution.
See also:
CATIGSMRevol, CATICkeParm
o CreateRotate
public virtual CreateRotate( const iToRotate,
const iAxis,
const iAngle)
Creates a rotated point, curve or surface.
Parameters:
iToRotate
point, curve, surface or solid.
iAxis
iLine.
iAngle
Rotation angle.
Returns:
CATIGSMRotate_var created rotation.
See also:
CATIGSMRotate, CATICkeParm
o CreateRotate
public virtual CreateRotate()
Creates an empty Rotation.
o CreateScaling
public virtual CreateScaling( const iToScale,
const iReference,
const iRatio)
Creates a scaled point, curve or surface.
Parameters:
iToScale
point, curve, surface or solid.
iReference
point or iplane.
iRatio
Real.
Returns:
CATIGSMScaling_var created symmetry.
See also:
CATIGSMScaling, CATICkeParm
o CreateSphere
public virtual CreateSphere( const iCenter,
const iAxis,
const iRadius,
const iAng1,
const iAng2,
const iAng3,
const iAng4)
Creates a sphere surface.
Parameters:
iCenter
The center (a point) of the sphere.
iAxis
The axis of the sphere.
iRadius
The radius of the sphere.
iAng1
First parallel angle.
iAng2
Second parallel angle.
iAng3
First meridian angle.
iAng4
Second meridian angle.
Returns:
CATIGSMSphere_var created sphere.
See also:
CATIGSMSphere, CATICkeParm
o CreateSpine
public virtual CreateSpine( const iListOfSections,
const iStartPoint= NULL_var)
Creates a spine curve.
Parameters:
iListOfSections
List of sections curves or planes
iStartPoint
point to be used as a start point
Returns:
CATIGSMSpine_var created spine.
See also:
CATIGSMSpine
o CreateSpine
public virtual CreateSpine()
Creates a spine curve.
Returns:
CATIGSMSpine_var created spine.
o CreateSpiral
public virtual CreateSpiral( const iType,
const iSupport,
const iCenterPoint,
const iAxis,
const iStartingRadius,
iClockwiseRevolution)
Creates a spiral curve.
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.
Returns:
CATIGSMSpiral_var Created spiral curve.
See also:
CATIGSMSpiral, CATIGSMDirection, CATICkeParm
o CreateSplinePoints
public virtual CreateSplinePoints( const ListOfPoints)
Creates a cubic spline from a list of points.
Parameters:
ListOfPoints
ListOfPoints
Returns:
CATIGSMSpline_var created spline
See also:
CATIGSMSpline
o CreateSplinePoints
public virtual CreateSplinePoints()
Creates an empty cubic spline.
Returns:
CATIGSMSpline_var created spline
See also:
CATIGSMSpline
o CreateSplit
public virtual CreateSplit( const iToCut,
const iCutting,
iOrientation)
Creates a split element by cutting and relimiting an element by another element.
Parameters:
iToCut
The feature to cut (curve or surface).
iCutting
The cutting feature (point, curve, surface).
iOrientation
Manage the kept side of iToCut
Returns:
CATIGSMSplit_var created feature.
See also:
CATIGSMSplit
o CreateSplit
public virtual CreateSplit()
Creates a split element by cutting and relimiting an element by several elements. Use the interface CATIGSMSplit to define element to be cut and cutting elements.
Returns:
CATIGSMSplit_var created feature.
See also:
CATIGSMSplit
o CreateSymmetry
public virtual CreateSymmetry( const iToSymmetry,
const invariant)
Creates a symmetrical point, curve or surface.
Parameters:
iToSymmetry
point, curve, surface or solid.
invariant
point, line or iplane.
Returns:
CATIGSMSymmetry_var created symmetry.
See also:
CATIGSMSymmetry
o CreateTangentCircle
public virtual CreateTangentCircle( const iCenterElem,
const iTangentElem,
const iSurface,
const iRadius)
Creates a circle with center on the first input curve/point and which is tangent to the second input curve and with a given radius, with respect to a support surface.
Default creation is direct trimmed circle.
Parameters:
iCenterElem
Center element : a curve or a point
iTangentElem
tangent element : a curve
iSurface
surface : a support
iRadius
Value specified is considered as radius. To use this value as diameter, set DiameterMode using SetDiameterMode method
Returns:
CATIGSMCircleCenterTangent_var created circle.
See also:
CATIGSMCircleCenterTangent, CATICkeParm
o CreateTangentCircle
public virtual CreateTangentCircle( const iFirstElem,
const iSecondElem,
const iSurface,
const iRadius,
const iFirstOrientation,
const iSecondOrientation)
Creates a circle which is tangent to 2 curves and with a given radius, with respect to a support surface. The curves can be degenerated into points.
Orientations allows to change the resulting circle.
Default creation is direct trimmed circle.
Parameters:
iFirstElem
first element : a curve or a point
iSecondElem
second element : a curve or a point
iSurface
surface
iRadius
Value specified is considered as radius. To use this value as diameter, set DiameterMode using SetDiameterMode method
iFirstOrientation
first orientation
iSecondOrientation
secont orientation
Returns:
CATIGSMCircleBitangentRadius_var created circle.
See also:
CATIGSMCircleBitangentRadius, CATGSMOrientation, CATICkeParm
o CreateTangentCircle
public virtual CreateTangentCircle( const iFirstElem,
const iSecondCurve,
const iPoint,
const iSurface,
const iFirstOrientation,
const iSecondOrientation)
Creates a circle which is tangent to 2 curves with respect to a support surface and passing through a point which lies on the second curve. The first curve can be degenerated into a point.
Orientations allows to change the resulting circle.
Default creation is direct trimmed circle.
Parameters:
iFirstElem
first element : a curve or a point
iSecondCurve
second curve
iPoint
surface
iSurface
surface
iFirstOrientation
first orientation
iSecondOrientation
second orientation
Returns:
CATIGSMCircleBitangentPoint_var created circle.
See also:
CATIGSMCircleBitangentPoint, CATGSMOrientation
o CreateTangentCircle
public virtual CreateTangentCircle( const iFirstElem,
const iSecondElem,
const iThirdElem,
const iSurface,
const iFirstOrientation,
const iSecondOrientation,
const iThirdOrientation)
Creates a circle which is tangent to 3 curves with respect to a support surface. The curves can be degenerated into points.
Orientations allows to change the resulting circle.
Default creation is direct trimmed circle.
Parameters:
iFirstElem
first element : a curve or a point
iSecondElem
second element : a curve or a point
iThirdElem
third element : a curve or a point
iSurface
surface
iFirstOrientation
first orientation
iSecondOrientation
second orientation
iThirdOrientation
third orientation
Returns:
CATIGSMCircleTritangent_var created circle.
See also:
CATIGSMCircleTritangent, CATGSMOrientation
o CreateTranslate
public virtual CreateTranslate( const iToTranslate,
const iDirection,
const iDistance)
Creates a translated point, curve or surface.
Parameters:
iToTranslate
point, curve, surface or solid.
iDirection
Translation direction.
iDistance
Translation length.
Returns:
CATIGSMTranslate_var created translation.
See also:
CATIGSMTranslate, CATIGSMDirection
o CreateTranslate
public virtual CreateTranslate()
Creates an empty translation.
o CreateTriDimExplicit
public virtual CreateTriDimExplicit()
Creates a simple volume.
Note: requires GSO license, if license not found creation fails, return NULL_var.
Returns:
CATISpecObject_var Created Volume
o CreateTrim
public virtual CreateTrim( const iFirstElement,
iOrientation1,
const iSecondElement,
iOrientation2)
Creates a trim element by cutting and joining two elements.
You can trim a surface by a surface or a curve by a curve.
Parameters:
FisrtElement
The feature to trim (curve or surface).
iOrientation1
Manage the kept side of iFirstElement.
iSecondElement
The second feature to trim (curve or surface).
iOrientation2
Manage the kept side of iSecondElement.
Returns:
CATIGSMTrim_var created feature.
See also:
CATIGSMTrim, CATGSMOrientation
o CreateZeroDimExplicit
public virtual CreateZeroDimExplicit()
Creates a simple point.
Returns:
CATISpecObject_var created point

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

Copyright © 2003, Dassault Systèmes. All rights reserved.