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

Represents a section
Section consists of "chained_entity", a chain or a single entity of edge or curve. More...

Inheritance diagram for NXOpen::Section:
NXOpen::DisplayableObject NXOpen::NXObject NXOpen::IFitTo NXOpen::TaggedObject NXOpen::INXObject NXOpen::INXObject

List of all members.

Public Types

enum  AllowTypes { AllowTypesUninitialized, AllowTypesOnlyCurves, AllowTypesOnlyPoints, AllowTypesCurvesAndPoints }
 Defines entity types allowed. More...
enum  DeselectOption { DeselectOptionSectionBetweenIntersection, DeselectOptionCurveBetweenIntersection }
 Defines type of deselect option. More...
enum  Mode { ModeCreate, ModeEdit }
 Defines mode with respect to feature create or edit mode. More...

Public Member Functions

void AddChainBetweenIntersectionPoints (const std::vector< NXOpen::SelectionIntentRule * > &rules, NXOpen::NXObject *startConnector, const NXOpen::Point3d &startIntersectionPoint, NXOpen::NXObject *endConnector, const NXOpen::Point3d &endIntersectionPoint, NXOpen::NXObject *seed, const NXOpen::Point3d &helpPoint, NXOpen::Section::Mode featureMode, bool chainWithinFeature)
 Adds a chain between given two intersection points to the section.
void AddSmartPoint (NXOpen::Point *smartPt, double tol)
 Add smart point into section.
void AddToSection (const std::vector< NXOpen::SelectionIntentRule * > &rules, NXOpen::NXObject *seed, NXOpen::NXObject *startConnector, NXOpen::NXObject *endConnector, const NXOpen::Point3d &helpPoint, NXOpen::Section::Mode featureMode)
 Adds selection intent rules to the section.
void AddToSection (const std::vector< NXOpen::SelectionIntentRule * > &rules, NXOpen::NXObject *seed, NXOpen::NXObject *startConnector, NXOpen::NXObject *endConnector, const NXOpen::Point3d &helpPoint, NXOpen::Section::Mode featureMode, bool chainWithinFeature)
 Adds selection intent rules to the section with the option of restricting chaining and limit discovery to a single feature.
void AlignDirectionOfLoop (const NXOpen::Point3d &point, const NXOpen::Vector3d &direction)
 Set the direction of a single loop of the section along the given vector.
void AllowSelfIntersection (bool allowSelfIntersection)
 Allow self intersecting section or not.
double AngleTolerance ()
 Returns the angle tolerance
Created in NX3.0.0.
double ChainingTolerance ()
 Returns the chaining tolerance
Created in NX3.0.0.
void CleanMappingData ()
 Cleans Mapping Data
This method should be used to clean mapping data after mapping is done

void Clear ()
 Clear the section of all its constituents
Created in NX5.0.0.
NXOpen::SectionCloneSection ()
 Clone section.
void DeselectPortion (const NXOpen::Point3d &seedPoint, NXOpen::NXObject *startLimit, NXOpen::NXObject *endLimit, NXOpen::Section::DeselectOption deselectionType)
 Deselects Portion of the section depending on the option provided.
void Destroy ()
 Destroy the section object
Created in NX4.0.0.
double DistanceTolerance ()
 Returns the distance tolerance
Created in NX3.0.0.
NXOpen::Section::AllowTypes GetAllowedEntityTypes ()
 Get the Allowed Entity Types.
int GetLoopIndex (NXOpen::NXObject *sectionElement)
 Returns the index of the section loop conatining the section element.
int GetLoopIndex (const NXOpen::Point3d &pointSpecifyingLoop, double tolerance)
 Returns the index of the loop on which the given point lies.
void GetOldOutputCurves (std::vector< NXOpen::NXObject * > &oldOutputs)
 Gives the old output curves of the section.
void GetOutputCurves (std::vector< NXOpen::NXObject * > &outputs)
 Gives the output curves of the section.
void GetSectionData (std::vector< NXOpen::SectionData * > &sectionData)
 Gets the section data
Created in NX3.0.0.
void GetStartAndDirection (NXOpen::ICurve **startElement, NXOpen::Point3d *startPoint, NXOpen::Vector3d *direction)
 Gets the start element and the direction of the section.
void GetStartAndDirectionOfLoop (int index, NXOpen::Point3d *startPoint, NXOpen::Vector3d *direction)
 Gets the start point and the direction of a specified single loop of the section.
void MapSectionElements (NXOpen::NXObject *oldWf, NXOpen::NXObject *newWf)
 Maps old section curves to new section curves
This method should be used to map old section curves to new section curves when some or all curves from section are removed and some or all new curves are added.
void PrepareMappingData ()
 Prepares Mapping Data
This method should be used to create mapping data if mapping is to be done

Created in NX7.5.0.
void RemoveMultipleCurves (const std::vector< NXOpen::ICurve * > &wfs, const std::vector< NXOpen::NXObject * > &startConnector, const std::vector< NXOpen::NXObject * > &endConnector, NXOpen::Section::Mode featureMode)
 Removes multiple section elements that are either curves/edges.
void RemoveMultipleElements (const std::vector< NXOpen::ICurve * > &wfs, const std::vector< NXOpen::NXObject * > &startConnectors, const std::vector< NXOpen::NXObject * > &endConnectors, const std::vector< bool > &isCombinationsResultIntoOnlyOneCurvePerCombination, const std::vector< NXOpen::Point3d > &pointsOnCurvesToBeRemoved, const std::vector< NXOpen::Point * > &points, NXOpen::Section::Mode featureMode)
 Removes multiple section elements.
void RemoveMultiplePoints (const std::vector< NXOpen::Point * > &points, NXOpen::Section::Mode featureMode)
 Removes multiple section elements that are points.
void RemoveRules (const std::vector< NXOpen::SelectionIntentRule * > &rules, NXOpen::NXObject *startConnector, NXOpen::NXObject *endConnector, NXOpen::Section::Mode featureMode)
 Removes selection intent rules from the section.
void RemoveRules (NXOpen::ICurve *sectionElement, NXOpen::NXObject *startConnector, NXOpen::NXObject *endConnector, NXOpen::Section::Mode featureMode)
 Removes all the selection intent rules related to the section element.
void RemoveSingleSectionElement (NXOpen::ICurve *sectionElement, NXOpen::NXObject *startConnector, NXOpen::NXObject *endConnector, NXOpen::Section::Mode featureMode)
 Removes one section element curve.
void RemoveSingleSectionElement (NXOpen::Point *sectionElement, NXOpen::Section::Mode featureMode)
 Removes one section element that is a point.
void RemoveUnderlyingChain (const NXOpen::Point3d &pointSpecifyingChain, double tolerance, NXOpen::Section::Mode featureMode)
 Removes all the selection intent rules related to the chain on which the given point lies.
void RemoveUnderlyingCurve (const NXOpen::Point3d &pointSpecifyingCurve, double tolerance, NXOpen::Section::Mode featureMode)
 Removes the single curve which is within tolerance to the given point, from the section.
void ReverseDirection ()
 Reverse the section direction
Created in NX4.0.0.
void ReverseDirectionOfClosedLoop (int index)
 Reverse the loop direction of a closed loop while keeping the start curve same.
void ReverseDirectionOfLoop (int index)
 Reverse the direction of of a specified single loop of the section.
void SetAllowedEntityTypes (NXOpen::Section::AllowTypes allowedEntityTypes)
 Set the Allowed Entity Types.
void SetAngleTolerance (double angleTolerance)
 Sets the angle tolerance
Created in NX3.0.0.
void SetChainingTolerance (double chainingTolerance)
 Sets the chaining tolerance
Created in NX3.0.0.
void SetDistanceTolerance (double distanceTolerance)
 Sets the distance tolerance
Created in NX3.0.0.
void SetInterpart (bool interpart)
 Set inter-part state of section and make it empty
Created in NX6.0.0.
void SetStartAndDirection (NXOpen::ICurve *startElement, const NXOpen::Point3d &startPoint, const NXOpen::Vector3d &direction)
 Sets the start element and the direction of the section.
void SetStartCurveOfClosedLoop (int index, const NXOpen::Point3d &pointOnStartCurve)
 Set the curve on which the specified point lies as the start curve of a specified single loop of the section.

Detailed Description

Represents a section
Section consists of "chained_entity", a chain or a single entity of edge or curve.

The entire chain(or a single entity) may be used by the section or only a portion of the chain (or single entity) might be used. The portion of the chain (or single entity) that is used is defined by the "start_connector" and "end_connector".

start_connector: It represents the start of the portion of the chain (or single entity) that is used. If "start_connector" is null (Nothing), then the start point of the chained_entity along its "natural" direction is used.

start_connector_intersection_point: The point of intersection of the "chained_entity" and the "start_connector". This is used to determine what portion of the chain to use in case the "start_connector" intersects the "chained_entity" in multiple locations.

end_connector: It represents the end of the portion of the chain (or single entity) that is used.

end_connector_intersection_point: The point of intersection of the "chained_entity" and the "end_connector". This is used to determine what portion of the chain to use in case the "end_connector" intersects the "chained_entity" in multiple locations.

To create a new instance of this class, use SectionCollection::CreateSection

Created in NX3.0.0.


Member Enumeration Documentation

Defines entity types allowed.

Enumerator:
AllowTypesUninitialized 

This is uninitialized state.

Do not use this.

AllowTypesOnlyCurves 

Allow only curves in section.

AllowTypesOnlyPoints 

Allow only points in section.

AllowTypesCurvesAndPoints 

Allow both points and curves in section.

Defines type of deselect option.

Enumerator:
DeselectOptionSectionBetweenIntersection 

Potion of the loop between intersections will be deselected this may contain multiple chains.

DeselectOptionCurveBetweenIntersection 

Portion of curve between intersection.

Defines mode with respect to feature create or edit mode.

Enumerator:
ModeCreate 

Feature is being created.

ModeEdit 

Feature is being edited.


Member Function Documentation

void NXOpen::Section::AddChainBetweenIntersectionPoints ( const std::vector< NXOpen::SelectionIntentRule * > &  rules,
NXOpen::NXObject startConnector,
const NXOpen::Point3d startIntersectionPoint,
NXOpen::NXObject endConnector,
const NXOpen::Point3d endIntersectionPoint,
NXOpen::NXObject seed,
const NXOpen::Point3d helpPoint,
NXOpen::Section::Mode  featureMode,
bool  chainWithinFeature 
)

Adds a chain between given two intersection points to the section.


Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
rulesSelection intent rules. To create selection intent rules see documentation of ScRuleFactory for more details.
startConnectorIt represents the start of the portion of the chain (or single entity) that is used. If "startConnector" is NULL, then the start point of the chained entity along its "natural" direction is used. It can be point, curve or edge
startIntersectionPointThe point where the start connector intersects with the chain.
endConnectorRepresents the end of the portion of the chain (or single entity) that is used. It can be point, curve or edge
endIntersectionPointThe point where the end connector intersects with the chain.
seedSeed curve, edge or face
helpPointThe point which is used to determine which portion of the chain to use for creating section.
featureModeFeature create or edit mode.
chainWithinFeatureTrue if chaining and discovery of intersection limits is to be restricted to the feature of the seed. This is effective only when the seed belongs to a curve feature.
void NXOpen::Section::AddSmartPoint ( NXOpen::Point smartPt,
double  tol 
)

Add smart point into section.


Deprecated:
Deprecated in NX7.5.0.


Created in NX4.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
smartPtSmart point tobe added into section.
tolTolerance.
void NXOpen::Section::AddToSection ( const std::vector< NXOpen::SelectionIntentRule * > &  rules,
NXOpen::NXObject seed,
NXOpen::NXObject startConnector,
NXOpen::NXObject endConnector,
const NXOpen::Point3d helpPoint,
NXOpen::Section::Mode  featureMode 
)

Adds selection intent rules to the section.


Created in NX4.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
rulesSelection intent rules. To create selection intent rules see documentation of ScRuleFactory for more details.
seedSeed curve, edge or face
startConnectorIt represents the start of the portion of the chain (or single entity) that is used. If "start_connector" is null (Nothing), then the start point of the chained_entity along its "natural" direction is used. It can be point, curve or edge
endConnectorIt represents the end of the portion of the chain (or single entity) that is used. It can be point, curve or edge
helpPointThis is used to determine which portion of the chain to use for creating section.
featureModeFeature create or edit mode.
void NXOpen::Section::AddToSection ( const std::vector< NXOpen::SelectionIntentRule * > &  rules,
NXOpen::NXObject seed,
NXOpen::NXObject startConnector,
NXOpen::NXObject endConnector,
const NXOpen::Point3d helpPoint,
NXOpen::Section::Mode  featureMode,
bool  chainWithinFeature 
)

Adds selection intent rules to the section with the option of restricting chaining and limit discovery to a single feature.


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
rulesSelection intent rules. To create selection intent rules see documentation of ScRuleFactory for more details.
seedSeed curve, edge or face
startConnectorIt represents the start of the portion of the chain (or single entity) that is used. If "start_connector" is null (Nothing), then the start point of the chained_entity along its "natural" direction is used. It can be point, curve or edge
endConnectorIt represents the end of the portion of the chain (or single entity) that is used. It can be point, curve or edge
helpPointThis is used to determine which portion of the chain to use for creating section.
featureModeFeature create or edit mode.
chainWithinFeatureTrue if chaining and discovery of intersection limits is to be restricted to the feature of the seed. This is effective only when the seed belongs to a curve feature.
void NXOpen::Section::AlignDirectionOfLoop ( const NXOpen::Point3d point,
const NXOpen::Vector3d direction 
)

Set the direction of a single loop of the section along the given vector.


Created in NX5.0.1.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
pointAny point on a the desired loop.
directionDesired tangent direction of the loop at the point.
void NXOpen::Section::AllowSelfIntersection ( bool  allowSelfIntersection)

Allow self intersecting section or not.

By default self intersection is allowed.
Created in NX4.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
allowSelfIntersectionTrue if self-intersecting section is allowed else false

Returns the angle tolerance
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Returns the chaining tolerance
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Cleans Mapping Data
This method should be used to clean mapping data after mapping is done


Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Clear the section of all its constituents
Created in NX5.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Clone section.

Returns:
the cloned section
Created in NX7.0.0.

License requirements : None
void NXOpen::Section::DeselectPortion ( const NXOpen::Point3d seedPoint,
NXOpen::NXObject startLimit,
NXOpen::NXObject endLimit,
NXOpen::Section::DeselectOption  deselectionType 
)

Deselects Portion of the section depending on the option provided.


This method should be used to deselect portion of the section.


Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
seedPointThe seed point of deselection
startLimitThe element that is connected to the curve/edge near its start point.
endLimitThe element that is connected to the curve/edge near its end point.
deselectionTypeThe deselection type

Destroy the section object
Created in NX4.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Returns the distance tolerance
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Get the Allowed Entity Types.


Works only for UF_SC_CURVE_dumb_data_s and UF_SC_CURVE_feature_data_s

Returns:
allowed entity types
Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Returns the index of the section loop conatining the section element.

If the section element does not exist in the section or is part of more than one loops, this method will return an error.

Returns:
loop Index
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")
Parameters:
sectionElementan element that constructs the section
int NXOpen::Section::GetLoopIndex ( const NXOpen::Point3d pointSpecifyingLoop,
double  tolerance 
)

Returns the index of the loop on which the given point lies.

Returns:
loop Index
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")
Parameters:
pointSpecifyingLoopa point lying on the loop for which the loop index is being queried
toleranceTolerance for specifying point on loop.
void NXOpen::Section::GetOldOutputCurves ( std::vector< NXOpen::NXObject * > &  oldOutputs)

Gives the old output curves of the section.


This method returns an array of old section curves. They were created internally and are different from the parent curves used to build the section. These curves should not be modified or deleted, doing so may result in part corruption and session may become unstable.


Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
oldOutputsThe array of old section elements.
void NXOpen::Section::GetOutputCurves ( std::vector< NXOpen::NXObject * > &  outputs)

Gives the output curves of the section.


This method returns an array of existing section curves. They are created internally and are different from the parent curves used to build the section. These curves should not be modified or deleted, doing so may result in part corruption and session may become unstable.


Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
outputsThe array of section elements.
void NXOpen::Section::GetSectionData ( std::vector< NXOpen::SectionData * > &  sectionData)

Gets the section data
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
sectionDataSection data consists of selection intent rules, section elements, start and end connector.
void NXOpen::Section::GetStartAndDirection ( NXOpen::ICurve **  startElement,
NXOpen::Point3d startPoint,
NXOpen::Vector3d direction 
)

Gets the start element and the direction of the section.


Created in NX3.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
startElementThe element, curve or edge, specifying the starting of the section. If the section is a loop, then the loop is started by start_element and the direction is followed the input direction. If the section is not a loop, then the section can be started by other element, but the direction of the section is defined by the start_element and direction.
startPointThe origin of the vector that defines the direction of the section. This point has to be on the start_element.
directionThe direction of the vector defines the direction of the section.
void NXOpen::Section::GetStartAndDirectionOfLoop ( int  index,
NXOpen::Point3d startPoint,
NXOpen::Vector3d direction 
)

Gets the start point and the direction of a specified single loop of the section.


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
indexThe index of the loop of the section for which start point and direction are being queried.
startPointThe origin of the vector that defines the direction of the loop of the section specified by the index.
directionThe direction of the vector defines the direction of the loop of the section specified by the index.

Maps old section curves to new section curves
This method should be used to map old section curves to new section curves when some or all curves from section are removed and some or all new curves are added.



To find old section curves see documentation for Section::GetOldOutputCurves and to find current section curves see documentation for Section::GetOutputCurves

Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
oldWfThe old section curve which was removed and hence needs to be mapped.
newWfThe new section curve that would be mapped to the old section curve.

Prepares Mapping Data
This method should be used to create mapping data if mapping is to be done

Created in NX7.5.0.



License requirements : solid_modeling ("SOLIDS MODELING")

void NXOpen::Section::RemoveMultipleCurves ( const std::vector< NXOpen::ICurve * > &  wfs,
const std::vector< NXOpen::NXObject * > &  startConnector,
const std::vector< NXOpen::NXObject * > &  endConnector,
NXOpen::Section::Mode  featureMode 
)

Removes multiple section elements that are either curves/edges.


Created in NX6.0.2.

License requirements : None

Parameters:
wfsThe elements (curves/edges) that construct the section.
startConnectorThe element that is connected to the curve/edge near its start point.
endConnectorThe element that is connected to the curve/edge near its end point.
featureModeFeature create or edit mode.
void NXOpen::Section::RemoveMultipleElements ( const std::vector< NXOpen::ICurve * > &  wfs,
const std::vector< NXOpen::NXObject * > &  startConnectors,
const std::vector< NXOpen::NXObject * > &  endConnectors,
const std::vector< bool > &  isCombinationsResultIntoOnlyOneCurvePerCombination,
const std::vector< NXOpen::Point3d > &  pointsOnCurvesToBeRemoved,
const std::vector< NXOpen::Point * > &  points,
NXOpen::Section::Mode  featureMode 
)

Removes multiple section elements.


This method should be used to remove the multiple section elements from section when elements to be removed contains points, and some or all curves that can not be uniquely mapped with wireframe , start connector and end connector. For Such curves point laying on the curve should be specified


Created in NX6.0.2.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
wfsThe elements (curves/edges) that construct the section.
startConnectorsThe element that is connected to the curve/edge near its start point.
endConnectorsThe element that is connected to the curve/edge near its end point.
isCombinationsResultIntoOnlyOneCurvePerCombinationWhether the combination of input curve/edge, Start Connector end Connector produces unique combination (i.e. they map to single section element) or not.
pointsOnCurvesToBeRemovedIf Combination can not define curve to be deselected uniquely, then point which lies on the curve to be removed should be provided, otherwise point must be given as (0, 0, 0) for corresponding combination
pointsThe points that are part of section and to be removed from the section.
featureModeFeature create or edit mode.
void NXOpen::Section::RemoveMultiplePoints ( const std::vector< NXOpen::Point * > &  points,
NXOpen::Section::Mode  featureMode 
)

Removes multiple section elements that are points.


Created in NX6.0.2.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
pointsThe points that construct the section.
featureModeFeature create or edit mode.
void NXOpen::Section::RemoveRules ( const std::vector< NXOpen::SelectionIntentRule * > &  rules,
NXOpen::NXObject startConnector,
NXOpen::NXObject endConnector,
NXOpen::Section::Mode  featureMode 
)

Removes selection intent rules from the section.


To get selection intent rules of the section see documentation for Section::GetSectionData and SectionData::GetRules for more details.


Created in NX3.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
rulesSelection intent rules.
startConnectorIt represents the start of the portion of the chain (or single entity) that is used. If "start_connector" is null (Nothing), then the start point of the chained_entity along its "natural" direction is used. It can be be point, curve or edge
endConnectorIt represents the end of the portion of the chain (or single entity) that is used. It can be be point, curve or edge
featureModeFeature create or edit mode
void NXOpen::Section::RemoveRules ( NXOpen::ICurve sectionElement,
NXOpen::NXObject startConnector,
NXOpen::NXObject endConnector,
NXOpen::Section::Mode  featureMode 
)

Removes all the selection intent rules related to the section element.


To get selection elements of the section, see documentation for Section::GetSectionData and SectionData::GetSectionElementsData for more details.


Created in NX4.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
sectionElementThe element that constructs the section
startConnectorThe element that is connected to the section_element near its start_point
endConnectorThe element that is connected to the section_element near its end_point
featureModeFeature create or edit mode.
void NXOpen::Section::RemoveSingleSectionElement ( NXOpen::ICurve sectionElement,
NXOpen::NXObject startConnector,
NXOpen::NXObject endConnector,
NXOpen::Section::Mode  featureMode 
)

Removes one section element curve.


To get selection element see documentation for Section::GetSectionData and SectionData::GetSectionElementsData for more details.


Created in NX4.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
sectionElementThe element that constructs the section
startConnectorThe element that is connected to the section_element near its start_point
endConnectorThe element that is connected to the section_element near its end_point
featureModeFeature create or edit mode

Removes one section element that is a point.


To get selection element see documentation for Section::GetSectionData and SectionData::GetSectionElementsData for more details.


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
sectionElementThe point that constructs the section
featureModeFeature create or edit mode
void NXOpen::Section::RemoveUnderlyingChain ( const NXOpen::Point3d pointSpecifyingChain,
double  tolerance,
NXOpen::Section::Mode  featureMode 
)

Removes all the selection intent rules related to the chain on which the given point lies.


This method should be used in place of Section::RemoveRules when the part containing the section element is not loaded.


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
pointSpecifyingChainThe point should lie on the chain that is to be removed.
toleranceTolerance for specifying point on chain.
featureModeFeature create or edit mode.
void NXOpen::Section::RemoveUnderlyingCurve ( const NXOpen::Point3d pointSpecifyingCurve,
double  tolerance,
NXOpen::Section::Mode  featureMode 
)

Removes the single curve which is within tolerance to the given point, from the section.


This method should be used in place of Section::RemoveSingleSectionElement in any of the conditions: when the part containing the section element is not loaded, when the combination of input curve, start connector and end connector maps to multiple section element, or when underlying parent is invalid.


Created in NX6.0.2.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
pointSpecifyingCurveThe point should lie on the curve that is to be removed.
toleranceTolerance for specifying point on curve.
featureModeFeature create or edit mode.

Reverse the section direction
Created in NX4.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Reverse the loop direction of a closed loop while keeping the start curve same.

This API can only be used closed loops.
Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
indexIndex of the closed loop for which the direction is to be reversed.

Reverse the direction of of a specified single loop of the section.


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
indexThe index of the loop of the section that is to be reversed.

Set the Allowed Entity Types.


Works only for UF_SC_CURVE_dumb_data_s and UF_SC_CURVE_feature_data_s


Created in NX7.5.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
allowedEntityTypesAllowed entity types.
void NXOpen::Section::SetAngleTolerance ( double  angleTolerance)

Sets the angle tolerance
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
angleToleranceangle tolerance
void NXOpen::Section::SetChainingTolerance ( double  chainingTolerance)

Sets the chaining tolerance
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
chainingTolerancechaining tolerance
void NXOpen::Section::SetDistanceTolerance ( double  distanceTolerance)

Sets the distance tolerance
Created in NX3.0.0.



License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
distanceTolerancedistance tolerance
void NXOpen::Section::SetInterpart ( bool  interpart)

Set inter-part state of section and make it empty
Created in NX6.0.0.



License requirements : None

Parameters:
interpartTrue to set section interpart
void NXOpen::Section::SetStartAndDirection ( NXOpen::ICurve startElement,
const NXOpen::Point3d startPoint,
const NXOpen::Vector3d direction 
)

Sets the start element and the direction of the section.


Created in NX3.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
startElementThe element, curve or edge, specifying the starting of the section. If the section is a loop, then the loop is started by start_element and the direction is followed the input direction. If the section is not a loop, then the section can be started by other element, but the direction of the section is defined by the start_element and direction.
startPointThe origin of the vector that defines the direction of the section. This point has to be on the start_element.
directionThe direction of the vector defines the direction of the section.
void NXOpen::Section::SetStartCurveOfClosedLoop ( int  index,
const NXOpen::Point3d pointOnStartCurve 
)

Set the curve on which the specified point lies as the start curve of a specified single loop of the section.


Created in NX5.0.0.

License requirements : solid_modeling ("SOLIDS MODELING")

Parameters:
indexIndex of the loop for which the start curve is to be set.
pointOnStartCurveAny point on a curve that is to be set as the start curve.

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