Section Class

class NXOpen.Section

Bases: NXOpen.DisplayableObject

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 NXOpen.SectionCollection.CreateSection

New in version NX3.0.0.

Properties

Property Description
AngleTolerance Returns or sets the angle tolerance
ChainingTolerance Returns or sets the chaining tolerance
Color Returns or sets the color of the object.
DistanceTolerance Returns or sets the distance tolerance
IsBlanked Returns the blank status of this object.
IsOccurrence Returns whether this object is an occurrence or not.
JournalIdentifier Returns the identifier that would be recorded in a journal for this object.
Layer Returns or sets the layer that the object is in.
LineFont Returns or sets the line font of the object.
LineWidth Returns or sets the line width of the object.
Name Returns the custom name of the object.
NameLocation Returns the location of the object’s name.
OwningComponent Returns the owning component, if this object is an occurrence.
OwningPart Returns the owning part of this object
Prototype Returns the prototype of this object if it is an occurrence.
Tag Returns the Tag for this object.

Methods

Method Description
AddChainBetweenIntersectionPoints Adds a chain between given two intersection points to the section.
AddSmartPoint Add smart point into section.
AddToSection Adds selection intent rules to the section.
AlignDirectionOfLoop Set the direction of a single loop of the section along the given vector.
AllowSelfIntersection Allow self intersecting section or not.
Blank Blanks the object.
CleanMappingData Cleans Mapping Data
Clear Clear the section of all its constituents
CloneSection Clone section.
DeleteAllAttributesByType Deletes all attributes of a specific type.
DeleteAttributeByTypeAndTitle Deletes an attribute by type and title.
DeleteUserAttribute Deletes the first attribute encountered with the given Type, Title.
DeleteUserAttributes Deletes the attributes encountered with the given Type with option to update or not.
DeselectPortion Deselects Portion of the section depending on the option provided.
Destroy Destroy the section object
EvaluateAndAskOutputEntities Recalculates section collection.
FindObject Finds the NXOpen.NXObject with the given identifier as recorded in a journal.
GetAllowedEntityTypes Get the Allowed Entity Types.
GetAttributeTitlesByType Gets all the attribute titles of a specific type.
GetBooleanUserAttribute Gets a boolean attribute by Title and array Index.
GetComputationalTimeUserAttribute Gets a time attribute by Title and array Index.
GetIntegerAttribute Gets an integer attribute by title.
GetIntegerUserAttribute Gets an integer attribute by Title and array Index.
GetLoopIndex Returns the index of the section loop conatining the section element.
GetMultiComponent Gets the option set on Section for collection from multiple components.
GetNonFeatureMode Gets the option set on Section for collection in non-feature mode.
GetOldOutputCurves Gives the old output curves of the section.
GetOutputCurves Gives the output curves of the section.
GetRealAttribute Gets a real attribute by title.
GetRealUserAttribute Gets a real attribute by Title and array Index.
GetReferenceAttribute Gets the reference string (not the calculated value) of a string attribute that uses a reference string.
GetSectionData Gets the section data
GetStartAndDirection Gets the start element and the direction of the section.
GetStartAndDirectionOfLoop Gets the start point and the direction of a specified single loop of the section.
GetStringAttribute Gets a string attribute value by title.
GetStringUserAttribute Gets a string attribute by Title and array Index.
GetTimeAttribute Gets a time attribute by title.
GetTimeUserAttribute Gets a time attribute by Title and array Index.
GetUserAttribute Gets the first attribute encountered on the object, if any, with a given Title, Type and array Index.
GetUserAttributeAsString Gets the first attribute encountered on the object, if any, with a given title, type and array index.
GetUserAttributeCount Gets the count of set attributes on the object, if any, of the given type.
GetUserAttributeLock Determine the lock of the given attribute.
GetUserAttributeSize Gets the size of the first attribute encountered on the object, if any, with a given Title and Type.
GetUserAttributeSourceObjects Returns an array of objects from which this object presents attributes.
GetUserAttributes Gets all the attributes that have been set on the given object.
GetUserAttributesAsStrings Gets all the attributes that have been set on the given object.
HasUserAttribute Determines if an attribute with the given Title, Type and array Index is present on the object Unset attributes will not be detected by this function, as its purpose is to test for the actual presence of the attribute on the object.
Highlight Highlights the object.
MapSectionElements Maps old section curves to new section curves
PrepareMappingData Prepares Mapping Data
Print Prints a representation of this object to the system log file.
RedisplayObject Redisplays the object in all views.
RemoveMultipleCurves Removes multiple section elements that are either curves/edges.
RemoveMultipleElements Removes multiple section elements.
RemoveMultiplePoints Removes multiple section elements that are points.
RemoveRules Removes selection intent rules from the section.
RemoveSingleSectionElement Removes one section element curve.
RemoveUnderlyingChain Removes all the selection intent rules related to the chain on which the given point lies.
RemoveUnderlyingCurve Removes the single curve which is within tolerance to the given point, from the section.
RemoveViewDependency Remove dependency on all views from an object.
ReverseDirection Reverse the section direction
ReverseDirectionOfClosedLoop Reverse the loop direction of a closed loop while keeping the start curve same.
ReverseDirectionOfLoop Reverse the direction of of a specified single loop of the section.
SetAllowRefCrvs Sets to the section whether to allow reference curves or not.
SetAllowedEntityTypes Set the Allowed Entity Types.
SetAttribute Creates or modifies an integer attribute.
SetBooleanUserAttribute Creates or modifies a boolean attribute with the option to update or not.
SetInterpart Set inter-part state of section and make it empty.
SetMultiComponent Sets the true option on Section for collection from multiple components.
SetName Sets the custom name of the object.
SetNameLocation Sets the location of the object’s name.
SetNonFeatureMode Sets the true option on Section for collection in non-feature mode.
SetReferenceAttribute Creates or modifies a string attribute which uses a reference string.
SetStartAndDirection Sets the start element and the direction of the section.
SetStartCurveOfClosedLoop Set the curve on which the specified point lies as the start curve of a specified single loop of the section.
SetTimeAttribute Creates or modifies a time attribute.
SetTimeUserAttribute Creates or modifies a time attribute with the option to update or not.
SetUserAttribute Creates or modifies an attribute with the option to update or not.
SetUserAttributeLock Lock or unlock the given attribute.
SkipSorting Sets the option to skip sorting the section loops or not.
Unblank Unblanks the object.
Unhighlight Unhighlights the object.

Enumerations

SectionAllowTypes Enumeration Defines entity types allowed.
SectionDeselectOption Enumeration Defines type of deselect option.
SectionMode Enumeration Defines mode with respect to feature create or edit mode.

Property Detail

AngleTolerance

Section.AngleTolerance

Returns or sets the angle tolerance

-------------------------------------

Getter Method

Signature AngleTolerance()

Returns:angle tolerance
Return type:float

New in version NX3.0.0.

License requirements: gateway (“UG GATEWAY”)

-------------------------------------

Setter Method

Signature AngleTolerance(angleTolerance)

Parameters:angleTolerance (float) – angle tolerance

New in version NX3.0.0.

License requirements: gateway (“UG GATEWAY”)

ChainingTolerance

Section.ChainingTolerance

Returns or sets the chaining tolerance

-------------------------------------

Getter Method

Signature ChainingTolerance()

Returns:chaining tolerance
Return type:float

New in version NX3.0.0.

License requirements: gateway (“UG GATEWAY”)

-------------------------------------

Setter Method

Signature ChainingTolerance(chainingTolerance)

Parameters:chainingTolerance (float) – chaining tolerance

New in version NX3.0.0.

License requirements: gateway (“UG GATEWAY”)

DistanceTolerance

Section.DistanceTolerance

Returns or sets the distance tolerance

-------------------------------------

Getter Method

Signature DistanceTolerance()

Returns:distance tolerance
Return type:float

New in version NX3.0.0.

License requirements: gateway (“UG GATEWAY”)

-------------------------------------

Setter Method

Signature DistanceTolerance(distanceTolerance)

Parameters:distanceTolerance (float) – distance tolerance

New in version NX3.0.0.

License requirements: gateway (“UG GATEWAY”)

IsOccurrence

Section.IsOccurrence

Returns whether this object is an occurrence or not.

-------------------------------------

Getter Method

Signature IsOccurrence()

Returns:This object is an occurrence
Return type:bool

New in version NX3.0.0.

License requirements: None.

JournalIdentifier

Section.JournalIdentifier

Returns the identifier that would be recorded in a journal for this object.

This may not be the same across different releases of the software.

-------------------------------------

Getter Method

Signature JournalIdentifier()

Returns:
Return type:str

New in version NX3.0.0.

License requirements: None.

Name

Section.Name

Returns the custom name of the object.

-------------------------------------

Getter Method

Signature Name()

Returns:
Return type:str

New in version NX3.0.0.

License requirements: None.

OwningComponent

Section.OwningComponent

Returns the owning component, if this object is an occurrence.

-------------------------------------

Getter Method

Signature OwningComponent()

Returns:
Return type:NXOpen.Assemblies.Component

New in version NX3.0.0.

License requirements: None.

OwningPart

Section.OwningPart

Returns the owning part of this object

-------------------------------------

Getter Method

Signature OwningPart()

Returns:The owning part of this object or null if it does not have an owner
Return type:NXOpen.BasePart

New in version NX3.0.0.

License requirements: None.

Prototype

Section.Prototype

Returns the prototype of this object if it is an occurrence.

-------------------------------------

Getter Method

Signature Prototype()

Returns:The prototype of this object or null if this object is not an occurrence
Return type:NXOpen.INXObject

New in version NX3.0.0.

License requirements: None.

Method Detail

AddChainBetweenIntersectionPoints

Section.AddChainBetweenIntersectionPoints

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

Signature AddChainBetweenIntersectionPoints(rules, startConnector, startIntersectionPoint, endConnector, endIntersectionPoint, seed, helpPoint, featureMode, chainWithinFeature)

Parameters:
  • rules (list of NXOpen.SelectionIntentRule) – Selection intent rules. To create selection intent rules see documentation of ScRuleFactory for more details.
  • startConnector (NXOpen.NXObject) – It represents the start of the portion of the chain (or single entity) that is used. If “startConnector” is None, then the start point of the chained entity along its “natural” direction is used. It can be point, curve or edge
  • startIntersectionPoint (NXOpen.Point3d) – The point where the start connector intersects with the chain.
  • endConnector (NXOpen.NXObject) – Represents the end of the portion of the chain (or single entity) that is used. It can be point, curve or edge
  • endIntersectionPoint (NXOpen.Point3d) – The point where the end connector intersects with the chain.
  • seed (NXOpen.NXObject) – Seed curve, edge or face
  • helpPoint (NXOpen.Point3d) – The point which is used to determine which portion of the chain to use for creating section.
  • featureMode (NXOpen.SectionMode) – Feature create or edit mode.
  • chainWithinFeature (bool) – 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.

New in version NX7.5.0.

License requirements: gateway (“UG GATEWAY”)

AddSmartPoint

Section.AddSmartPoint

Add smart point into section.

This API is now deprecated. Please use ScRuleFactory.CreateRuleCurveDumb and Section.AddToSection instead.

Signature AddSmartPoint(smartPt, tol)

Parameters:
  • smartPt (NXOpen.Point) – Smart point tobe added into section.
  • tol (float) – Tolerance.

New in version NX4.0.0.

Deprecated since version NX7.5.0: Please use ScRuleFactory.CreateRuleCurveDumb followed by Section.AddToSection instead.

License requirements: gateway (“UG GATEWAY”)

AddToSection

Section.AddToSection

Overloaded method AddToSection

  • AddToSection(rules, seed, startConnector, endConnector, helpPoint, featureMode)
  • AddToSection(rules, seed, startConnector, endConnector, helpPoint, featureMode, chainWithinFeature)

-------------------------------------

Adds selection intent rules to the section.

Signature AddToSection(rules, seed, startConnector, endConnector, helpPoint, featureMode)

Parameters:
  • rules (list of NXOpen.SelectionIntentRule) – Selection intent rules. To create selection intent rules see documentation of ScRuleFactory for more details.
  • seed (NXOpen.NXObject) – Seed curve, edge or face
  • startConnector (NXOpen.NXObject) – 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 (NXOpen.NXObject) – It represents the end of the portion of the chain (or single entity) that is used. It can be point, curve or edge
  • helpPoint (NXOpen.Point3d) – When ambiguity in multiple solutions is encountered, help_point is used to determine which portion of the chain to use for creating section. It is most useful when used with non-NULL connectors or with Region Boundary Curves rule.
  • featureMode (NXOpen.SectionMode) – Feature create or edit mode.

New in version NX4.0.0.

License requirements: gateway (“UG GATEWAY”)

-------------------------------------

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

Signature AddToSection(rules, seed, startConnector, endConnector, helpPoint, featureMode, chainWithinFeature)

Parameters:
  • rules (list of NXOpen.SelectionIntentRule) – Selection intent rules. To create selection intent rules see documentation of ScRuleFactory for more details.
  • seed (NXOpen.NXObject) – Seed curve, edge or face
  • startConnector (NXOpen.NXObject) – 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 (NXOpen.NXObject) – It represents the end of the portion of the chain (or single entity) that is used. It can be point, curve or edge
  • helpPoint (NXOpen.Point3d) – When ambiguity in multiple solutions is encountered, help_point is used to determine which portion of the chain to use for creating section. It is most useful when used with non-NULL connectors or with Region Boundary Curves rule.
  • featureMode (NXOpen.SectionMode) – Feature create or edit mode.
  • chainWithinFeature (bool) – 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.

New in version NX5.0.0.

License requirements: gateway (“UG GATEWAY”)

-------------------------------------

AlignDirectionOfLoop

Section.AlignDirectionOfLoop

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

Signature AlignDirectionOfLoop(point, direction)

Parameters:
  • point (NXOpen.Point3d) – Any point on a the desired loop.
  • direction (NXOpen.Vector3d) – Desired tangent direction of the loop at the point.

New in version NX5.0.1.

License requirements: gateway (“UG GATEWAY”)

AllowSelfIntersection

Section.AllowSelfIntersection

Allow self intersecting section or not.

By default self intersection is allowed.

Signature AllowSelfIntersection(allowSelfIntersection)

Parameters:allowSelfIntersection (bool) – True if self-intersecting section is allowed else false

New in version NX4.0.0.

License requirements: gateway (“UG GATEWAY”)

CleanMappingData

Section.CleanMappingData

Cleans Mapping Data

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

Signature CleanMappingData()

New in version NX7.5.0.

License requirements: gateway (“UG GATEWAY”)

Clear

Section.Clear

Clear the section of all its constituents

Signature Clear()

New in version NX5.0.0.

License requirements: gateway (“UG GATEWAY”)

CloneSection

Section.CloneSection

Clone section.

Signature CloneSection()

Returns:the cloned section
Return type:NXOpen.Section

New in version NX7.0.0.

License requirements: None.

DeselectPortion

Section.DeselectPortion

Deselects Portion of the section depending on the option provided.

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

Signature DeselectPortion(seedPoint, startLimit, endLimit, deselectionType)

Parameters:

New in version NX7.5.0.

License requirements: gateway (“UG GATEWAY”)

Destroy

Section.Destroy

Destroy the section object

Signature Destroy()

New in version NX4.0.0.

License requirements: gateway (“UG GATEWAY”)

EvaluateAndAskOutputEntities

Section.EvaluateAndAskOutputEntities

Recalculates section collection.

This is JA API for recalculating the section collection and to get the section collection after recalculation.

Signature EvaluateAndAskOutputEntities()

Returns:The array of section elements.
Return type:list of NXOpen.NXObject

New in version NX9.0.0.

License requirements: gateway (“UG GATEWAY”)

FindObject

Section.FindObject

Finds the NXOpen.NXObject with the given identifier as recorded in a journal.

An object may not return the same value as its JournalIdentifier in different versions of the software. However newer versions of the software should find the same object when FindObject is passed older versions of its journal identifier. In general, this method should not be used in handwritten code and exists to support record and playback of journals.

An exception will be thrown if no object can be found with the given journal identifier.

Signature FindObject(journalIdentifier)

Parameters:journalIdentifier (str) – Journal identifier of the object
Returns:
Return type:NXOpen.INXObject

New in version NX3.0.0.

License requirements: None.

GetAllowedEntityTypes

Section.GetAllowedEntityTypes

Get the Allowed Entity Types.

Works only for UF_SC_CURVE_dumb_data_s and UF_SC_CURVE_feature_data_s

Signature GetAllowedEntityTypes()

Returns:allowed entity types
Return type:NXOpen.SectionAllowTypes

New in version NX7.5.0.

License requirements: gateway (“UG GATEWAY”)

GetLoopIndex

Section.GetLoopIndex

Overloaded method GetLoopIndex

  • GetLoopIndex(sectionElement)
  • GetLoopIndex(pointSpecifyingLoop, tolerance)

-------------------------------------

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.

Signature GetLoopIndex(sectionElement)

Parameters:sectionElement (NXOpen.NXObject) – an element that constructs the section
Returns:loop Index
Return type:int

New in version NX5.0.0.

License requirements: gateway (“UG GATEWAY”)

-------------------------------------

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

Signature GetLoopIndex(pointSpecifyingLoop, tolerance)

Parameters:
  • pointSpecifyingLoop (NXOpen.Point3d) – a point lying on the loop for which the loop index is being queried
  • tolerance (float) – Tolerance for specifying point on loop.
Returns:

loop Index
Return type:

int

New in version NX5.0.0.

License requirements: gateway (“UG GATEWAY”)

-------------------------------------

GetMultiComponent

Section.GetMultiComponent

Gets the option set on Section for collection from multiple components.

A multi-component Section can have collection from multiple components i.e., multiple parts or multiple instances of same part or both.

Signature GetMultiComponent()

Returns:Multi-component option set on Section
Return type:bool

New in version NX9.0.0.

License requirements: None.

GetNonFeatureMode

Section.GetNonFeatureMode

Gets the option set on Section for collection in non-feature mode.

A Section in non-feature mode does not reference the feature data of the part from which the collection is done.

Signature GetNonFeatureMode()

Returns:Non-feature mode set on Section
Return type:bool

New in version NX9.0.0.

License requirements: None.

GetOldOutputCurves

Section.GetOldOutputCurves

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.

Signature GetOldOutputCurves()

Returns:The array of old section elements.
Return type:list of NXOpen.NXObject

New in version NX7.5.0.

License requirements: gateway (“UG GATEWAY”)

GetOutputCurves

Section.GetOutputCurves

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.

Signature GetOutputCurves()

Returns:The array of section elements.
Return type:list of NXOpen.NXObject

New in version NX7.5.0.

License requirements: gateway (“UG GATEWAY”)

GetSectionData

Section.GetSectionData

Gets the section data

Signature GetSectionData()

Returns:Section data consists of selection intent rules,

section elements, start and end connector. :rtype: list of NXOpen.SectionData

New in version NX3.0.0.

License requirements: gateway (“UG GATEWAY”)

GetStartAndDirection

Section.GetStartAndDirection

Gets the start element and the direction of the section.

Signature GetStartAndDirection()

Returns:a tuple
Return type:A tuple consisting of (startElement, startPoint, direction). startElement is a NXOpen.ICurve. 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 is a NXOpen.Point3d. The origin of the vector that defines the direction of the section. This point has to be on the start_element. direction is a NXOpen.Vector3d. The direction of the vector defines the direction of the section.

New in version NX3.0.0.

License requirements: gateway (“UG GATEWAY”)

GetStartAndDirectionOfLoop

Section.GetStartAndDirectionOfLoop

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

Signature GetStartAndDirectionOfLoop(index)

Parameters:index (int) – The index of the loop of the section for which start point and direction are being queried.
Returns:a tuple
Return type:A tuple consisting of (startPoint, direction). startPoint is a NXOpen.Point3d. The origin of the vector that defines the direction of the loop of the section specified by the index. direction is a NXOpen.Vector3d. The direction of the vector defines the direction of the loop of the section specified by the index.

New in version NX5.0.0.

License requirements: gateway (“UG GATEWAY”)

MapSectionElements

Section.MapSectionElements

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

Signature MapSectionElements(oldWf, newWf)

Parameters:
  • oldWf (NXOpen.NXObject) – The old section curve which was removed and hence needs to be mapped.
  • newWf (NXOpen.NXObject) – The new section curve that would be mapped to the old section curve.

New in version NX7.5.0.

License requirements: gateway (“UG GATEWAY”)

PrepareMappingData

Section.PrepareMappingData

Prepares Mapping Data

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

Signature PrepareMappingData()

New in version NX7.5.0.

License requirements: gateway (“UG GATEWAY”)

Print

Section.Print

Prints a representation of this object to the system log file.

Signature Print()

New in version NX3.0.0.

License requirements: None.

RemoveMultipleCurves

Section.RemoveMultipleCurves

Removes multiple section elements that are either curves/edges.

This API is now deprecated. Please use Section.RemoveMultipleElements instead.

Signature RemoveMultipleCurves(wfs, startConnector, endConnector, featureMode)

Parameters:
  • wfs (list of NXOpen.ICurve) – The elements (curves/edges) that construct the section.
  • startConnector (list of NXOpen.NXObject) – The element that is connected to the curve/edge near its start point.
  • endConnector (list of NXOpen.NXObject) – The element that is connected to the curve/edge near its end point.
  • featureMode (NXOpen.SectionMode) – Feature create or edit mode.

New in version NX6.0.2.

Deprecated since version NX8.5.0: Please use Section.RemoveMultipleElements instead.

License requirements: None.

RemoveMultipleElements

Section.RemoveMultipleElements

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

Signature RemoveMultipleElements(wfs, startConnectors, endConnectors, isCombinationsResultIntoOnlyOneCurvePerCombination, pointsOnCurvesToBeRemoved, points, featureMode)

Parameters:
  • wfs (list of NXOpen.ICurve) – The elements (curves/edges) that construct the section.
  • startConnectors (list of NXOpen.NXObject) – The element that is connected to the curve/edge near its start point.
  • endConnectors (list of NXOpen.NXObject) – The element that is connected to the curve/edge near its end point.
  • isCombinationsResultIntoOnlyOneCurvePerCombination (list of bool) – 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 (list of NXOpen.Point3d) – 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 (list of NXOpen.Point) – The points that are part of section and to be removed from the section.
  • featureMode (NXOpen.SectionMode) – Feature create or edit mode.

New in version NX6.0.2.

License requirements: gateway (“UG GATEWAY”)

RemoveMultiplePoints

Section.RemoveMultiplePoints

Removes multiple section elements that are points.

This API is now deprecated. Please use Section.RemoveMultipleElements instead.

Signature RemoveMultiplePoints(points, featureMode)

Parameters:

New in version NX6.0.2.

Deprecated since version NX8.5.0: Please use Section.RemoveMultipleElements instead.

License requirements: gateway (“UG GATEWAY”)

RemoveRules

Section.RemoveRules

Overloaded method RemoveRules

  • RemoveRules(rules, startConnector, endConnector, featureMode)
  • RemoveRules(sectionElement, startConnector, endConnector, 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.

Signature RemoveRules(rules, startConnector, endConnector, featureMode)

Parameters:
  • rules (list of NXOpen.SelectionIntentRule) – Selection intent rules.
  • startConnector (NXOpen.NXObject) – 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 (NXOpen.NXObject) – 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 (NXOpen.SectionMode) – Feature create or edit mode

New in version NX3.0.0.

License requirements: gateway (“UG GATEWAY”)

-------------------------------------

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.

Signature RemoveRules(sectionElement, startConnector, endConnector, featureMode)

Parameters:
  • sectionElement (NXOpen.ICurve) – The element that constructs the section
  • startConnector (NXOpen.NXObject) – The element that is connected to the section_element near its start_point
  • endConnector (NXOpen.NXObject) – The element that is connected to the section_element near its end_point
  • featureMode (NXOpen.SectionMode) – Feature create or edit mode.

New in version NX4.0.0.

License requirements: gateway (“UG GATEWAY”)

-------------------------------------

RemoveSingleSectionElement

Section.RemoveSingleSectionElement

Overloaded method RemoveSingleSectionElement

  • RemoveSingleSectionElement(sectionElement, startConnector, endConnector, featureMode)
  • RemoveSingleSectionElement(sectionElement, featureMode)

-------------------------------------

Removes one section element curve.

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

Signature RemoveSingleSectionElement(sectionElement, startConnector, endConnector, featureMode)

Parameters:
  • sectionElement (NXOpen.ICurve) – The element that constructs the section
  • startConnector (NXOpen.NXObject) – The element that is connected to the section_element near its start_point
  • endConnector (NXOpen.NXObject) – The element that is connected to the section_element near its end_point
  • featureMode (NXOpen.SectionMode) – Feature create or edit mode

New in version NX4.0.0.

License requirements: gateway (“UG GATEWAY”)

-------------------------------------

Removes one section element that is a point.

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

Signature RemoveSingleSectionElement(sectionElement, featureMode)

Parameters:

New in version NX5.0.0.

License requirements: gateway (“UG GATEWAY”)

-------------------------------------

RemoveUnderlyingChain

Section.RemoveUnderlyingChain

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.

Signature RemoveUnderlyingChain(pointSpecifyingChain, tolerance, featureMode)

Parameters:
  • pointSpecifyingChain (NXOpen.Point3d) – The point should lie on the chain that is to be removed.
  • tolerance (float) – Tolerance for specifying point on chain.
  • featureMode (NXOpen.SectionMode) – Feature create or edit mode.

New in version NX5.0.0.

License requirements: gateway (“UG GATEWAY”)

RemoveUnderlyingCurve

Section.RemoveUnderlyingCurve

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.

Signature RemoveUnderlyingCurve(pointSpecifyingCurve, tolerance, featureMode)

Parameters:
  • pointSpecifyingCurve (NXOpen.Point3d) – The point should lie on the curve that is to be removed.
  • tolerance (float) – Tolerance for specifying point on curve.
  • featureMode (NXOpen.SectionMode) – Feature create or edit mode.

New in version NX6.0.2.

License requirements: gateway (“UG GATEWAY”)

ReverseDirection

Section.ReverseDirection

Reverse the section direction

Signature ReverseDirection()

New in version NX4.0.0.

License requirements: gateway (“UG GATEWAY”)

ReverseDirectionOfClosedLoop

Section.ReverseDirectionOfClosedLoop

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

This API can only be used closed loops.

Signature ReverseDirectionOfClosedLoop(index)

Parameters:index (int) – Index of the closed loop for which the direction is to be reversed.

New in version NX5.0.0.

License requirements: gateway (“UG GATEWAY”)

ReverseDirectionOfLoop

Section.ReverseDirectionOfLoop

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

Signature ReverseDirectionOfLoop(index)

Parameters:index (int) – The index of the loop of the section that is to be reversed.

New in version NX5.0.0.

License requirements: gateway (“UG GATEWAY”)

SetAllowRefCrvs

Section.SetAllowRefCrvs

Sets to the section whether to allow reference curves or not.

This is JA API for setting to the section whether to allow reference curves or not.

Signature SetAllowRefCrvs(allowRefCrvs)

Parameters:allowRefCrvs (bool) –

New in version NX10.0.0.

License requirements: None.

SetAllowedEntityTypes

Section.SetAllowedEntityTypes

Set the Allowed Entity Types.

Works only for UF_SC_CURVE_dumb_data_s and UF_SC_CURVE_feature_data_s

Signature SetAllowedEntityTypes(allowedEntityTypes)

Parameters:allowedEntityTypes (NXOpen.SectionAllowTypes) – Allowed entity types.

New in version NX7.5.0.

License requirements: gateway (“UG GATEWAY”)

SetInterpart

Section.SetInterpart

Set inter-part state of section and make it empty.

This function sets the value of interpart flag on Section. Error will be raised while setting this option on Section in following conditions: (1) Multi-component option is already set on Section.

Signature SetInterpart(interpart)

Parameters:interpart (bool) – True to set section interpart

New in version NX6.0.0.

License requirements: None.

SetMultiComponent

Section.SetMultiComponent

Sets the true option on Section for collection from multiple components.

A multi-component Section can have collection from multiple components i.e., multiple parts or multiple instances of same part or both. This method should be used only if such collection is desired. Error will be raised while setting this option on Section in following conditions: (1) Inter-part option is already set on Section.

Signature SetMultiComponent()

New in version NX9.0.0.

License requirements: None.

SetName

Section.SetName

Sets the custom name of the object.

NOTE: This method should not be used to edit a read-only object such as a Mirrored PMI object. If it is, the changes will be overridden when the part is updated.

Signature SetName(name)

Parameters:name (str) –

New in version NX3.0.0.

License requirements: None.

SetNonFeatureMode

Section.SetNonFeatureMode

Sets the true option on Section for collection in non-feature mode.

A Section in non-feature mode does not reference the feature data of the part from which the collection is done. The option should be set on an empty Section only. For a non-empty Section, setting this option will raise error in following conditions: (1) Section is referencing feature data and non-feature mode is set true. (2) Section is not referencing feature data and non-feature mode is set false.

Signature SetNonFeatureMode()

New in version NX9.0.0.

License requirements: None.

SetStartAndDirection

Section.SetStartAndDirection

Sets the start element and the direction of the section.

Signature SetStartAndDirection(startElement, startPoint, direction)

Parameters:
  • startElement (NXOpen.ICurve) – 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 (NXOpen.Point3d) – The origin of the vector that defines the direction of the section. This point has to be on the start_element.
  • direction (NXOpen.Vector3d) – The direction of the vector defines the direction of the section.

New in version NX3.0.0.

License requirements: gateway (“UG GATEWAY”)

SetStartCurveOfClosedLoop

Section.SetStartCurveOfClosedLoop

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

Signature SetStartCurveOfClosedLoop(index, pointOnStartCurve)

Parameters:
  • index (int) – Index of the loop for which the start curve is to be set.
  • pointOnStartCurve (NXOpen.Point3d) – Any point on a curve that is to be set as the start curve.

New in version NX5.0.0.

License requirements: gateway (“UG GATEWAY”)

SkipSorting

Section.SkipSorting

Sets the option to skip sorting the section loops or not.

This method should be used rare scenarios. In normal situation this method should never be used. If sort option is set to true then it should be set to false after required operation is done. If sort option is set to true then section loops are not sorted and output will not be in order.

Signature SkipSorting(skipSorting)

Parameters:skipSorting (bool) – True to skip sorting of section loops else false

New in version NX8.0.0.

License requirements: gateway (“UG GATEWAY”)