NX Open C++ Reference Guide
Public Types | Public Member Functions
NXOpen::Features::ThroughCurvesBuilder Class Reference

Represents a Features::ThroughCurves builder. More...

Inheritance diagram for NXOpen::Features::ThroughCurvesBuilder:
NXOpen::Features::FeatureBuilder NXOpen::Builder NXOpen::TaggedObject NXOpen::GeometricUtilities::IComponentBuilder

List of all members.

Public Types

enum  BodyPreferenceTypes { BodyPreferenceTypesSolid, BodyPreferenceTypesSheet }
 This enum represents the body type option. More...
enum  ConstructionMethod { ConstructionMethodNormal, ConstructionMethodSplinePoints, ConstructionMethodSimple }
 This enum represents the Construction options. More...
enum  PatchTypes { PatchTypesSingle, PatchTypesMultiple, PatchTypesMatchString }
 This enum represents the Patch options. More...

Public Member Functions

NXOpen::GeometricUtilities::AlignmentMethodBuilderAlignment ()
 Returns the alignment.
NXOpen::Features::ThroughCurvesBuilder::BodyPreferenceTypes BodyPreference ()
 Returns the body type options
Created in NX7.5.0.
bool ClosedInV ()
 Returns the closed in V.
NXOpen::Features::ThroughCurvesBuilder::ConstructionMethod Construction ()
 Returns the construction options.
double CurvatureTolerance ()
 Returns the curvature tolerance.
NXOpen::GeometricUtilities::ContinuityFirstSectionContinuity ()
 Returns the first section continuity.
NXOpen::GeometricUtilities::FlowDirectionFlowDirection ()
 Returns the flow direction.
NXOpen::GeometricUtilities::ContinuityLastSectionContinuity ()
 Returns the last section continuity.
NXOpen::GeometricUtilities::RebuildLoftingSurfaceRebuildData ()
 Returns the lofting surface rebuild data.
bool NormalToEndSections ()
 Returns the option of normal to end sections for Through Curves surface, which makes the output surface normal to the two end sections.If an end section is planar, the surface will be parallel to the plane normal at the end.If an end section is a 3D curve, an average normal vector will be computed, and the surface will be parallel to the average normal at the end.
NXOpen::Features::ThroughCurvesBuilder::PatchTypes PatchType ()
 Returns the patch type.
double PositionTolerance ()
 Returns the position tolerance.
bool PreserveShape ()
 Returns the preserve shape.
NXOpen::SectionListSectionsList ()
 Returns the sections list which is required.
NXOpen::GeometricUtilities::RebuildSectionSurfaceRebuildData ()
 Returns the section surface rebuild data.
NXOpen::SectionSectionTemplateString ()
 Returns the section template curve.
void SetBodyPreference (NXOpen::Features::ThroughCurvesBuilder::BodyPreferenceTypes bodyPreference)
 Sets the body type options
Created in NX7.5.0.
void SetClosedInV (bool closedInV)
 Sets the closed in V.
void SetConstruction (NXOpen::Features::ThroughCurvesBuilder::ConstructionMethod construction)
 Sets the construction options.
void SetCurvatureTolerance (double tolerance)
 Sets the curvature tolerance.
void SetNormalToEndSections (bool normalToEndSections)
 Sets the option of normal to end sections for Through Curves surface, which makes the output surface normal to the two end sections.If an end section is planar, the surface will be parallel to the plane normal at the end.If an end section is a 3D curve, an average normal vector will be computed, and the surface will be parallel to the average normal at the end.
void SetPatchType (NXOpen::Features::ThroughCurvesBuilder::PatchTypes patchType)
 Sets the patch type.
void SetPositionTolerance (double tolerance)
 Sets the position tolerance.
void SetPreserveShape (bool preserveShape)
 Sets the preserve shape.
void SetSectionTemplateString (NXOpen::Section *sectionTemplate)
 Sets the section template curve.
void SetTangentTolerance (double tolerance)
 Sets the tangent tolerance.
double TangentTolerance ()
 Returns the tangent tolerance.

Detailed Description

Represents a Features::ThroughCurves builder.


This builder lets you create or edit a body through a collection of curve outlines in one direction. The curve outlines are referred to as section strings.

To create a new instance of this class, use Features::FeatureCollection::CreateThroughCurvesBuilder
Default values.

Property Value

Alignment.AlignType

Parameter

ClosedInV

False

Construction

Normal

FirstSectionContinuity.ContinuityType

G0

FlowDirection.FlowDirectionType

NotSpecified

LastSectionContinuity.ContinuityType

G0

LoftingSurfaceRebuildData.Degree

3

LoftingSurfaceRebuildData.RebuildType

None

NormalToEndSections

False

PatchType

Multiple

PreserveShape

True

SectionSurfaceRebuildData.RebuildType

None


Created in NX5.0.0.


Member Enumeration Documentation

This enum represents the body type option.

If sections are all closed, if possible then a solid body can be created.

Enumerator:
BodyPreferenceTypesSolid 

Solid.

BodyPreferenceTypesSheet 

Sheet.

This enum represents the Construction options.

Enumerator:
ConstructionMethodNormal 

Use the standard procedures.

ConstructionMethodSplinePoints 

Use the points and tangent values at the points for reparameterizing curves.

ConstructionMethodSimple 

Build the simplest mesh surface possible.

This enum represents the Patch options.

Enumerator:
PatchTypesSingle 

single patch.

PatchTypesMultiple 

multiple patches.

PatchTypesMatchString 

patch match string.


Member Function Documentation

Returns the alignment.

See GeometricUtilities::AlignmentMethodBuilder for details.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the body type options
Created in NX7.5.0.



License requirements : None

Returns the closed in V.

When this option is ON, the sheet is closed along columns (that is, the V direction).


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the construction options.

Use one of three construction options when you create a Through Curves feature: Normal, Use Spline Points and Simple.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the curvature tolerance.

Control the curvature tolerance of the rebuild surface in relation to the input curves.
Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the first section continuity.

See GeometricUtilities::Continuity for details. Define continuity constraint at the first section side. It contains the continuity type and the constraint face.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the flow direction.

See GeometricUtilities::FlowDirection for details.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the last section continuity.

See GeometricUtilities::Continuity for details. Define continuity constraint at the last section side. It contains the continuity type and the constraint face.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the lofting surface rebuild data.

See GeometricUtilities::Rebuild for details.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the option of normal to end sections for Through Curves surface, which makes the output surface normal to the two end sections.If an end section is planar, the surface will be parallel to the plane normal at the end.If an end section is a 3D curve, an average normal vector will be computed, and the surface will be parallel to the average normal at the end.

If an end section is a line, the normal vector will be computed so that it points from the end section to the section next to the end section.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the patch type.

Lets you create a body containing a single patch or multiple patches.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the position tolerance.

Control the distance accuracy of the rebuild surface in relation to the input curves.
Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the preserve shape.

Allow you to keep sharp edges, overriding the default of approximating the output surface. Setting the Tolerance to 0.0 will achieve the same result.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the sections list which is required.

See ObjectList for details. The section strings define the rows of the body. A section string can consist of a single object or multiple objects, and each object can be one of the following: a curve or a solid edge.
Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the section surface rebuild data.

See GeometricUtilities::Rebuild for details.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Returns the section template curve.

Control the building of the simple surface in section curve direction. It is only available when the construction method is simple. If you leave it empty, the system will automatically choose the most complicated one for fitting.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Sets the body type options
Created in NX7.5.0.



License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Parameters:
bodyPreferencebodypreference

Sets the closed in V.

When this option is ON, the sheet is closed along columns (that is, the V direction).


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Parameters:
closedInVclosed in v

Sets the construction options.

Use one of three construction options when you create a Through Curves feature: Normal, Use Spline Points and Simple.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Parameters:
constructionconstruction

Sets the curvature tolerance.

Control the curvature tolerance of the rebuild surface in relation to the input curves.
Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Parameters:
tolerancetolerance

Sets the option of normal to end sections for Through Curves surface, which makes the output surface normal to the two end sections.If an end section is planar, the surface will be parallel to the plane normal at the end.If an end section is a 3D curve, an average normal vector will be computed, and the surface will be parallel to the average normal at the end.

If an end section is a line, the normal vector will be computed so that it points from the end section to the section next to the end section.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Parameters:
normalToEndSectionsnormal to end sections

Sets the patch type.

Lets you create a body containing a single patch or multiple patches.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Parameters:
patchTypepatch type

Sets the position tolerance.

Control the distance accuracy of the rebuild surface in relation to the input curves.
Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Parameters:
tolerancetolerance

Sets the preserve shape.

Allow you to keep sharp edges, overriding the default of approximating the output surface. Setting the Tolerance to 0.0 will achieve the same result.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Parameters:
preserveShapepreserve shape

Sets the section template curve.

Control the building of the simple surface in section curve direction. It is only available when the construction method is simple. If you leave it empty, the system will automatically choose the most complicated one for fitting.


Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Parameters:
sectionTemplatesectiontemplate

Sets the tangent tolerance.

Control the angular accuracy of the rebuild surface in relation to the input curves.It is expressed in degree.
Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")

Parameters:
tolerancetolerance

Returns the tangent tolerance.

Control the angular accuracy of the rebuild surface in relation to the input curves.It is expressed in degree.
Created in NX5.0.0.

License requirements : features_modeling ("FEATURES MODELING") OR nx_freeform_1 ("basic freeform modeling")


The documentation for this class was generated from the following file:
Copyright 2011 Siemens Product Lifecycle Management Software Inc. All Rights Reserved.