NX Open C++ Reference Guide
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Represents a RPO builder. More...
Public Types | |
enum | AssociativityType { AssociativityTypeEndPoint, AssociativityTypeArcCenter, AssociativityTypeTangency, AssociativityTypeEndPoint1, AssociativityTypeEndPoint2, AssociativityTypeVerticalCenterline1, AssociativityTypeVerticalCenterline2, AssociativityTypeHorizontalCenterline1, AssociativityTypeHorizontalCenterline2 } |
Represents the associativity type for a dimension entity. More... | |
Public Member Functions | |
void | ApplyDimensions () |
Transforms the feature by applying the positioning dimensions Created in NX3.0.0. | |
NXOpen::Features::RPODimension * | CreateDimension () |
Creates a new empty RPODimension object. | |
void | CreatePositioningDimension () |
Creates a positioning dimension. | |
void | GetReferenceDirection (NXOpen::IReferenceAxis **reference, NXOpen::AxisOrientation *orientation) |
Query/Set a horizontal or vertical reference for the feature. | |
std::vector < NXOpen::Features::RPODimension * > | GetRpoDimensions () |
Gets the list of RPO dimemsions. | |
void | HidePositioningDimensions () |
Hides display of all the positioning dimensions Created in NX3.0.0. | |
void | SetExpression (const NXString &expression) |
Sets the expression value in order to constrain the target and tool entities which are set using NXOpen::Features::RPOBuilder::SetTargetAndTool . | |
void | SetReferenceDirection (NXOpen::IReferenceAxis *reference, NXOpen::AxisOrientation orientation) |
Sets a horizontal or vertical reference for the feature. | |
void | SetRpoDimensions (const std::vector< NXOpen::Features::RPODimension * > &dimensions) |
Sets the list of RPO dimemsions. | |
void | SetTargetAndTool (NXOpen::PositioningDimension::Subtype subtype, NXOpen::NXObject *target, NXOpen::Features::RPOBuilder::AssociativityType targetAssociativity, const NXOpen::Point3d &targetHelpPoint, NXOpen::NXObject *tool, NXOpen::Features::RPOBuilder::AssociativityType toolAssociativity, const NXOpen::Point3d &toolHelpPoint) |
Sets the target and tool entities. | |
void | ShowPositioningDimensions () |
Displays all the positioning dimensions Created in NX3.0.0. | |
void | UndoLastDimension () |
Undo the last positioning dimension Created in NX3.0.0. |
Represents a RPO builder.
It provides methods to create positioning dimensions to position the feature which is being created.
This is an abstract class, and cannot be instantiated
Created in NX3.0.0.
Represents the associativity type for a dimension entity.
Transforms the feature by applying the positioning dimensions
Created in NX3.0.0.
License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")
Creates a new empty RPODimension object.
Creates a positioning dimension.
This is third and the last step in creating a positioning dimension.
Created in NX3.0.0.
License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")
void NXOpen::Features::RPOBuilder::GetReferenceDirection | ( | NXOpen::IReferenceAxis ** | reference, |
NXOpen::AxisOrientation * | orientation | ||
) |
Query/Set a horizontal or vertical reference for the feature.
A reference is required to be set before creating a Horizontal or Vertical positioning dimension.
Created in NX4.0.0.
License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")
reference | Reference entity |
orientation | Orientation of reference |
std::vector<NXOpen::Features::RPODimension *> NXOpen::Features::RPOBuilder::GetRpoDimensions | ( | ) |
Hides display of all the positioning dimensions
Created in NX3.0.0.
License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")
void NXOpen::Features::RPOBuilder::SetExpression | ( | const NXString & | expression | ) |
Sets the expression value in order to constrain the target and tool entities which are set using NXOpen::Features::RPOBuilder::SetTargetAndTool .
This is the second step in creating a positioning dimension. This step is not needed for PositioningDimension::SubtypePointOntoPoint , PositioningDimension::SubtypePointOntoLine and PositioningDimension::SubtypeLineOntoLine
Created in NX3.0.0.
License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")
expression | Expression string |
void NXOpen::Features::RPOBuilder::SetReferenceDirection | ( | NXOpen::IReferenceAxis * | reference, |
NXOpen::AxisOrientation | orientation | ||
) |
Sets a horizontal or vertical reference for the feature.
A reference is required to be set before creating a PositioningDimension::SubtypeHorizontal or PositioningDimension::SubtypeVertical subtype of positioning dimension.
Created in NX3.0.0.
License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")
reference | Reference entity |
orientation | Orientation of reference |
void NXOpen::Features::RPOBuilder::SetRpoDimensions | ( | const std::vector< NXOpen::Features::RPODimension * > & | dimensions | ) |
void NXOpen::Features::RPOBuilder::SetTargetAndTool | ( | NXOpen::PositioningDimension::Subtype | subtype, |
NXOpen::NXObject * | target, | ||
NXOpen::Features::RPOBuilder::AssociativityType | targetAssociativity, | ||
const NXOpen::Point3d & | targetHelpPoint, | ||
NXOpen::NXObject * | tool, | ||
NXOpen::Features::RPOBuilder::AssociativityType | toolAssociativity, | ||
const NXOpen::Point3d & | toolHelpPoint | ||
) |
Sets the target and tool entities.
This is the first step in creating a positioning dimension. A positioning dimension constraints two entities. These two entities are referred to as target and tool enitities. The tool entity is selected from the tool body which is being created. For example, if a Pad is being created then the tool entity can be an edge of the Pad. The target entity is an entity which does not belong to the tool body which is being created.
Created in NX3.0.0.
License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")
subtype | Subtype of dimension |
target | Target entity |
targetAssociativity | Associativity for target entity |
targetHelpPoint | Help point for taregt entity |
tool | Tool entity |
toolAssociativity | Associativity for tool entity |
toolHelpPoint | Help point for tool entity |
Displays all the positioning dimensions
Created in NX3.0.0.
License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")
Undo the last positioning dimension
Created in NX3.0.0.
License requirements : features_modeling ("FEATURES MODELING"), solid_modeling ("SOLIDS MODELING")