NX Open C++ Reference Guide
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Represents a section
Section consists of "chained_entity", a chain or a single entity of edge or curve.
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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::Section * | CloneSection () |
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 * > §ionData) |
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. |
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.
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")
rules | Selection intent rules. To create selection intent rules see documentation of ScRuleFactory for more details. |
startConnector | It 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 |
startIntersectionPoint | The point where the start connector intersects with the chain. |
endConnector | Represents the end of the portion of the chain (or single entity) that is used. It can be point, curve or edge |
endIntersectionPoint | The point where the end connector intersects with the chain. |
seed | Seed curve, edge or face |
helpPoint | The point which is used to determine which portion of the chain to use for creating section. |
featureMode | Feature create or edit mode. |
chainWithinFeature | True 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.
Created in NX4.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
smartPt | Smart point tobe added into section. |
tol | Tolerance. |
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")
rules | Selection intent rules. To create selection intent rules see documentation of ScRuleFactory for more details. |
seed | Seed curve, edge or face |
startConnector | 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. It can be point, curve or edge |
endConnector | It represents the end of the portion of the chain (or single entity) that is used. It can be point, curve or edge |
helpPoint | This is used to determine which portion of the chain to use for creating section. |
featureMode | Feature 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")
rules | Selection intent rules. To create selection intent rules see documentation of ScRuleFactory for more details. |
seed | Seed curve, edge or face |
startConnector | 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. It can be point, curve or edge |
endConnector | It represents the end of the portion of the chain (or single entity) that is used. It can be point, curve or edge |
helpPoint | This is used to determine which portion of the chain to use for creating section. |
featureMode | Feature create or edit mode. |
chainWithinFeature | True 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")
point | Any point on a the desired loop. |
direction | Desired 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")
allowSelfIntersection | True if self-intersecting section is allowed else false |
double NXOpen::Section::AngleTolerance | ( | ) |
Returns the angle tolerance
Created in NX3.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
double NXOpen::Section::ChainingTolerance | ( | ) |
Returns the chaining tolerance
Created in NX3.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
void NXOpen::Section::CleanMappingData | ( | ) |
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")
void NXOpen::Section::Clear | ( | ) |
Clear the section of all its constituents
Created in NX5.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
Clone section.
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")
seedPoint | The seed point of deselection |
startLimit | The element that is connected to the curve/edge near its start point. |
endLimit | The element that is connected to the curve/edge near its end point. |
deselectionType | The deselection type |
void NXOpen::Section::Destroy | ( | ) |
Destroy the section object
Created in NX4.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
double NXOpen::Section::DistanceTolerance | ( | ) |
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
int NXOpen::Section::GetLoopIndex | ( | NXOpen::NXObject * | sectionElement | ) |
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.
sectionElement | an 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.
pointSpecifyingLoop | a point lying on the loop for which the loop index is being queried |
tolerance | Tolerance 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")
oldOutputs | The 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")
outputs | The 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")
sectionData | Section 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")
startElement | The 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. |
startPoint | The origin of the vector that defines the direction of the section. This point has to be on the start_element. |
direction | The 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")
index | The index of the loop of the section for which start point and direction are being queried. |
startPoint | The origin of the vector that defines the direction of the loop of the section specified by the index. |
direction | The direction of the vector defines the direction of the loop of the section specified by the index. |
void NXOpen::Section::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.
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")
oldWf | The old section curve which was removed and hence needs to be mapped. |
newWf | The new section curve that would be mapped to the old section curve. |
void NXOpen::Section::PrepareMappingData | ( | ) |
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
wfs | The elements (curves/edges) that construct the section. |
startConnector | The element that is connected to the curve/edge near its start point. |
endConnector | The element that is connected to the curve/edge near its end point. |
featureMode | Feature 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")
wfs | The elements (curves/edges) that construct the section. |
startConnectors | The element that is connected to the curve/edge near its start point. |
endConnectors | The element that is connected to the curve/edge near its end point. |
isCombinationsResultIntoOnlyOneCurvePerCombination | Whether the combination of input curve/edge, Start Connector end Connector produces unique combination (i.e. they map to single section element) or not. |
pointsOnCurvesToBeRemoved | If 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 |
points | The points that are part of section and to be removed from the section. |
featureMode | Feature 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")
points | The points that construct the section. |
featureMode | Feature 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")
rules | Selection intent rules. |
startConnector | 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. It can be be point, curve or edge |
endConnector | It represents the end of the portion of the chain (or single entity) that is used. It can be be point, curve or edge |
featureMode | Feature 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")
sectionElement | The element that constructs the section |
startConnector | The element that is connected to the section_element near its start_point |
endConnector | The element that is connected to the section_element near its end_point |
featureMode | Feature 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")
sectionElement | The element that constructs the section |
startConnector | The element that is connected to the section_element near its start_point |
endConnector | The element that is connected to the section_element near its end_point |
featureMode | Feature create or edit mode |
void NXOpen::Section::RemoveSingleSectionElement | ( | NXOpen::Point * | sectionElement, |
NXOpen::Section::Mode | featureMode | ||
) |
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")
sectionElement | The point that constructs the section |
featureMode | Feature 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")
pointSpecifyingChain | The point should lie on the chain that is to be removed. |
tolerance | Tolerance for specifying point on chain. |
featureMode | Feature 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")
pointSpecifyingCurve | The point should lie on the curve that is to be removed. |
tolerance | Tolerance for specifying point on curve. |
featureMode | Feature create or edit mode. |
void NXOpen::Section::ReverseDirection | ( | ) |
Reverse the section direction
Created in NX4.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
void NXOpen::Section::ReverseDirectionOfClosedLoop | ( | int | index | ) |
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")
index | Index of the closed loop for which the direction is to be reversed. |
void NXOpen::Section::ReverseDirectionOfLoop | ( | int | index | ) |
Reverse the direction of of a specified single loop of the section.
Created in NX5.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
index | The index of the loop of the section that is to be reversed. |
void NXOpen::Section::SetAllowedEntityTypes | ( | NXOpen::Section::AllowTypes | allowedEntityTypes | ) |
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")
allowedEntityTypes | Allowed entity types. |
void NXOpen::Section::SetAngleTolerance | ( | double | angleTolerance | ) |
Sets the angle tolerance
Created in NX3.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
angleTolerance | angle tolerance |
void NXOpen::Section::SetChainingTolerance | ( | double | chainingTolerance | ) |
Sets the chaining tolerance
Created in NX3.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
chainingTolerance | chaining tolerance |
void NXOpen::Section::SetDistanceTolerance | ( | double | distanceTolerance | ) |
Sets the distance tolerance
Created in NX3.0.0.
License requirements : solid_modeling ("SOLIDS MODELING")
distanceTolerance | distance 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
interpart | True 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")
startElement | The 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. |
startPoint | The origin of the vector that defines the direction of the section. This point has to be on the start_element. |
direction | The 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")
index | Index of the loop for which the start curve is to be set. |
pointOnStartCurve | Any point on a curve that is to be set as the start curve. |