NXOpen .NET Reference
12.0.0
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Represents the set of NXOpen.Assemblies.Component s that make up an assembly. More...
Public Types | |
enum | SubstitutionMode { NonAssociative, SingleComponent, All } |
Defines how a component substitution operation is performed. More... | |
enum | OpenOption { ComponentOnly, ImmediateChildren, WholeAssembly, ReapplyRevRule } |
Open options for open_components More... | |
enum | OpenComponentStatus { SuccessfullyOpened, DeletedByOpen, CouldNotOpen } |
Open Component Status More... | |
enum | CheckinCheckoutOption { DesignElement, SourceItem, Both, Default } |
Check in and Check out options for components More... | |
enum | CloseModified { False, True } |
Indicates how close component should handle component parts when they are modified More... | |
enum | SuppressedState { Inherit, Suppressed, Unsuppressed, SuppressedByExp, UnsuppressedByExp } |
Defines the component supression states. More... | |
enum | OrderTargetLocation { PlaceBefore, PlaceAfter } |
Option controls whether reordered NXOpen.Assemblies.Component s are placed before or after the target NXOpen.Assemblies.Component More... | |
Public Types inherited from NXOpen.NXObject | |
enum | AttributeType { Invalid, Null, Boolean, Integer, Real, String, Time, Reference, Any = 100 } |
Specifies attribute type. More... | |
enum | DateAndTimeFormat { Numeric, Textual } |
Specifies the format of the date and time attribute. More... | |
Public Member Functions | |
unsafe NXOpen.Assemblies.Component | AddComponent (string partToAdd, string referenceSetName, string componentName, NXOpen.Point3d basePoint, NXOpen.Matrix3x3 orientation, int layer, out NXOpen.PartLoadStatus loadStatus) |
Creates a new NXOpen.Assemblies.Component in this assembly, based on an existing part file. More... | |
unsafe NXOpen.Assemblies.Component | AddComponent (string partToAdd, string referenceSetName, string componentName, NXOpen.Point3d basePoint, NXOpen.Matrix3x3 orientation, int layer, out NXOpen.PartLoadStatus loadStatus, bool uomAsNgc) |
Creates a new NXOpen.Assemblies.Component in this assembly, based on an existing part file. More... | |
unsafe void | AddComponents (NXOpen.Part[] partsToAdd, NXOpen.Point3d point, NXOpen.Matrix3x3 orientation, int layer, string referenceSetName, int count, bool scatter, out NXOpen.Assemblies.Component[] components) |
Creates new NXOpen.Assemblies.Component in this assembly, based on existing part files. More... | |
unsafe NXOpen.Assemblies.Component | AddComponent (NXOpen.BasePart partToAdd, string referenceSetName, string componentName, NXOpen.Point3d basePoint, NXOpen.Matrix3x3 orientation, int layer, out NXOpen.PartLoadStatus loadStatus) |
Creates a new NXOpen.Assemblies.Component in this assembly, based on an existing part file. More... | |
unsafe NXOpen.Assemblies.Component | AddMasterPartComponent (string partToAdd, string referenceSetName, string componentName, NXOpen.Point3d basePoint, NXOpen.Matrix3x3 orientation, int layer, out NXOpen.PartLoadStatus loadStatus) |
Creates a new NXOpen.Assemblies.Component in this assembly as master part. More... | |
unsafe NXOpen.Assemblies.Component | AddMasterPartComponent (NXOpen.Part partToAdd, string referenceSetName, string componentName, NXOpen.Point3d basePoint, NXOpen.Matrix3x3 orientation, int layer, out NXOpen.PartLoadStatus loadStatus) |
Creates a new NXOpen.Assemblies.Component in this assembly as master part. More... | |
unsafe NXOpen.Assemblies.Component | InsertProduct (NXOpen.Part productPart, int layer, out NXOpen.PartLoadStatus loadStatus) |
Adds a product into workset part at identity location. More... | |
unsafe NXOpen.Assemblies.Component | SubstituteComponent (NXOpen.Assemblies.Component component, NXOpen.BasePart part, string newName, string referenceSet, int layer, NXOpen.Assemblies.ComponentAssembly.SubstitutionMode mode) |
Substitutes an old component with a new component. More... | |
unsafe void | RemoveComponent (NXOpen.Assemblies.Component component) |
Removes a component from this assemebly. More... | |
unsafe NXOpen.Assemblies.Component | MapComponentFromParent (NXOpen.Assemblies.Component component) |
Maps a component in a parent assembly onto a corresponding component in this assembly. More... | |
unsafe NXOpen.Assemblies.Component[] | MapComponentsFromSubassembly (NXOpen.Assemblies.Component component) |
Maps a component in a subassembly onto the corresponding components in this parent assembly. More... | |
unsafe void | ChangeByName (string name, NXOpen.Assemblies.Component[] partOccs) |
Changes the current NXOpen.Assemblies.Arrangement of the given NXOpen.Assemblies.Component s to the NXOpen.Assemblies.Arrangement with the given name. More... | |
unsafe void | SetDefault (NXOpen.Assemblies.Arrangement arrangement) |
Set the default NXOpen.Assemblies.Arrangement for the given NXOpen.Assemblies.ComponentAssembly . More... | |
unsafe NXOpen.ErrorList | SuppressComponents (NXOpen.Assemblies.Component[] components, NXOpen.Assemblies.Arrangement[] arrangements) |
Suppresses an array of components More... | |
unsafe NXOpen.ErrorList | SuppressComponents (NXOpen.Assemblies.Component[] components) |
Suppresses an array of components in all NXOpen.Assemblies.Arrangement s in this ComponentAssembly More... | |
unsafe NXOpen.ErrorList | SuppressComponents (NXOpen.Assemblies.Component[] components, NXOpen.Assemblies.Arrangement[] arrangements, string expression) |
Suppresses an array of components in all NXOpen.Assemblies.Arrangement s in this ComponentAssembly More... | |
unsafe NXOpen.ErrorList | UnsuppressComponents (NXOpen.Assemblies.Component[] components, NXOpen.Assemblies.Arrangement[] arrangements) |
Unsuppresses an array of components in this ComponentAssembly More... | |
unsafe NXOpen.ErrorList | UnsuppressComponents (NXOpen.Assemblies.Component[] components) |
Unsuppresses an array of components in all NXOpen.Assemblies.Arrangement s in this ComponentAssembly More... | |
unsafe NXOpen.ErrorList | ReleaseSuppression (NXOpen.Assemblies.Component[] components, NXOpen.Assemblies.Arrangement[] arrangements) |
Release control of the suppression state of an array of components. More... | |
unsafe NXOpen.ErrorList | ReleaseSuppression (NXOpen.Assemblies.Component[] components) |
Release control of the suppression state of an array of components. More... | |
unsafe void | SetEntirePartRefset (NXOpen.Assemblies.Component component) |
Convenience method for setting the reference set used to represent a component to be the entire part. More... | |
unsafe void | SetEmptyRefset (NXOpen.Assemblies.Component component) |
Convenience method for setting the reference set used to represent a component to be empty More... | |
unsafe NXOpen.ErrorList | ReplaceReferenceSetInOwners (string newReferenceSet, NXOpen.Assemblies.Component[] components) |
Sets the reference set used to represent each component in an array. More... | |
unsafe void | ReplaceReferenceSet (NXOpen.Assemblies.Component component, string newReferenceSet) |
Replaces the reference set used by a component. More... | |
unsafe void | MoveComponent (NXOpen.Assemblies.Component component, NXOpen.Vector3d translation, NXOpen.Matrix3x3 rotation) |
Moves a component by specifying a translation and rotation. More... | |
unsafe NXOpen.Positioning.MatingConverter | CreateMatingConverter () |
Creates a NXOpen.Positioning.MatingConverter object for this assembly. More... | |
unsafe void | DeleteMatingConditions () |
Delete all the mating conditions in this assembly. More... | |
unsafe void | ConvertRememberedMcs () |
Converts all remembered mating constraints in the part of this assembly to remembered assembly constraints More... | |
unsafe void | SetNonGeometricState (NXOpen.Assemblies.Component component, bool nonGeometricState) |
Sets the component state to Geometric or Non-Geometric. More... | |
unsafe bool | GetNonGeometricState (NXOpen.Assemblies.Component component) |
Gets the component state as Geometric or Non-Geometric. More... | |
unsafe NXOpen.Assemblies.ComponentQuantity | GetComponentQuantityType (NXOpen.Assemblies.Component component) |
Gets the quantity type of the components. More... | |
unsafe void | SetIntegerQuantity (NXOpen.Assemblies.Component component, int integerQuantity) |
Sets the integer quantity on this component. More... | |
unsafe int | GetIntegerQuantity (NXOpen.Assemblies.Component component) |
Gets the value of the integer quantity of component. More... | |
unsafe void | SetRealQuantity (NXOpen.Assemblies.Component component, double realQuantity, string quantityUnits) |
Sets the real quantity and corresponding units on this component. More... | |
unsafe double | GetRealQuantity (NXOpen.Assemblies.Component component, out string units) |
Gets the value of real quantity and corresponding units on this component. More... | |
unsafe void | SetAsRequiredQuantity (NXOpen.Assemblies.Component component) |
Sets the as-required quantity on this component. More... | |
unsafe string | GetAsRequiredQuantity (NXOpen.Assemblies.Component component) |
Gets the as-required quantity on this component. More... | |
unsafe NXOpen.Assemblies.Component[] | CopyComponents (NXOpen.Assemblies.Component[] components) |
Given an array of components, creates copies of the components such that each copy is created under the parent assembly of the original component. More... | |
unsafe void | RestructureComponents (NXOpen.Assemblies.Component[] origComponents, NXOpen.Assemblies.Component newParentComponent, bool deleteFlag, out NXOpen.Assemblies.Component[] newComponents, out NXOpen.ErrorList errorList) |
Given an array of components and a specified parent this function will transfer the given components to the parent. More... | |
unsafe NXOpen.PartLoadStatus | OpenComponents (NXOpen.Assemblies.ComponentAssembly.OpenOption openOption, NXOpen.Assemblies.Component[] componentsToOpen, out NXOpen.Assemblies.ComponentAssembly.OpenComponentStatus[] openStatus) |
Given an array of components, open the components using the open_option. More... | |
unsafe NXOpen.PartCloseStatus | CloseComponents (NXOpen.Assemblies.Component[] componentsToClose, NXOpen.BasePart.CloseWholeTree wholeTree, NXOpen.Assemblies.ComponentAssembly.CloseModified closeModified) |
Given an array of components, close the components. More... | |
unsafe NXOpen.Expression | GetSuppressionExpression (NXOpen.Assemblies.Component component) |
Gets the expression controlling the suppression of the component in its controlling arrangement More... | |
unsafe NXOpen.Expression | GetSuppressionExpression (NXOpen.Assemblies.Component component, NXOpen.Assemblies.Arrangement arrangement) |
Gets the expression controlling the suppression of the component in the given arrangment More... | |
unsafe NXOpen.Assemblies.ComponentAssembly.SuppressedState | GetSuppressedState (NXOpen.Assemblies.Component component, out bool controlled) |
Gets the suppression state of the component in its controlling arrangement More... | |
unsafe NXOpen.Assemblies.ComponentAssembly.SuppressedState | GetSuppressedState (NXOpen.Assemblies.Component component, NXOpen.Assemblies.Arrangement arrangement, out bool controlled) |
Gets the suppression state of the component in the given arrangement. More... | |
unsafe NXOpen.Assemblies.ComponentPatternBuilder | CreateComponentPatternBuilder (NXOpen.Assemblies.ComponentPattern compPattern) |
Creates a NXOpen.Assemblies.ComponentPatternBuilder object This can be used to create or edit a component pattern. More... | |
unsafe NXOpen.PartLoadStatus | AddPendingComponent (string partToAdd, NXOpen.NXObject pendingComponent, string referenceSetName, string componentName, NXOpen.Point3d basePoint, NXOpen.Matrix3x3 orientation, int layer, bool uomAsNgc) |
Add a pending NXOpen.Assemblies.Component in this assembly. More... | |
unsafe NXOpen.Positioning.ComponentConstraintGroupBuilder | CreateConstraintGroupBuilder (NXOpen.Positioning.ComponentConstraintGroup group, NXOpen.Assemblies.Component contextComponent) |
Creates a NXOpen.Positioning.ComponentConstraintGroupBuilder object. More... | |
unsafe NXOpen.ErrorList | CheckinComponents (NXOpen.Assemblies.Component[] partOccs, NXOpen.Assemblies.ComponentAssembly.CheckinCheckoutOption checkinInputOption) |
Checks in array of components as per the option NXOpen.Assemblies.ComponentAssembly.CheckinCheckoutOption . More... | |
unsafe NXOpen.ErrorList | CheckoutComponents (NXOpen.Assemblies.Component[] partOccs, NXOpen.Assemblies.ComponentAssembly.CheckinCheckoutOption checkoutInputOption) |
Checks out array of components as per the option NXOpen.Assemblies.ComponentAssembly.CheckinCheckoutOption . More... | |
unsafe NXOpen.ErrorList | CheckoutWorkset () |
Checks out workset. More... | |
unsafe NXOpen.ErrorList | CheckinWorkset () |
Checks in workset. More... | |
unsafe NXOpen.ErrorList | CheckoutAllModifiedObjects (out NXOpen.NXObject[] checkedOutObjects) |
Checks out all modified objects in the current session. More... | |
unsafe void | GetCheckedoutStatusOfObjects (out NXOpen.NXObject[] checkedOutObjects, out NXOpen.NXObject[] uncheckedOutObjects) |
Returns the checkedout status (checkedout/non checkedout) of all the objects open in NX. More... | |
unsafe void | ReorderComponents (NXOpen.Assemblies.ComponentOrder order, NXOpen.Assemblies.Component[] componentsToReorder, NXOpen.Assemblies.Component targetComponent, NXOpen.Assemblies.ComponentAssembly.OrderTargetLocation beforeOrAfter) |
Reorders the array of NXOpen.Assemblies.Component s before or after the target NXOpen.Assemblies.Component . More... | |
unsafe void | ReorderChildrenOfParent (NXOpen.Assemblies.ComponentOrder order, NXOpen.Assemblies.Component parentComponent, NXOpen.Assemblies.Component[] componentsToReorder) |
Assigns a new order to immediate children NXOpen.Assemblies.Component s of parent NXOpen.Assemblies.Component . More... | |
unsafe void | GetComponentOrders (out NXOpen.Assemblies.ComponentOrder[] orders) |
Returns all NXOpen.Assemblies.ComponentOrder s available in the part More... | |
unsafe void | MoveToPendingComponent (NXOpen.NXObject component) |
Move a NXOpen.Assemblies.Component in this assembly to a pending list. More... | |
unsafe NXOpen.Assemblies.Order | GetActiveOrder () |
Returns the active order in the part More... | |
unsafe NXOpen.ErrorList | CreateIsolateViewWithComponents (NXOpen.Assemblies.Component[] components, out NXOpen.View view) |
Creates a temporary NXOpen.View and shows array of components in it and treats this as Isolate view till it gets undisplayed. More... | |
unsafe NXOpen.ErrorList | ShowComponentsInIsolateView (NXOpen.Assemblies.Component[] components, out NXOpen.View view) |
Shows array of components in Isolate view NXOpen.View . More... | |
unsafe NXOpen.ErrorList | HideComponentsInIsolateView (NXOpen.Assemblies.Component[] components, out NXOpen.View view) |
Hides array of components in Isolate view NXOpen.View . More... | |
Public Member Functions inherited from NXOpen.NXObject | |
unsafe void | SetUserAttribute (NXOpen.NXObject.AttributeInformation info, NXOpen.Update.Option option) |
Creates or modifies an attribute with the option to update or not. More... | |
unsafe void | SetUserAttribute (string title, int index, int value, NXOpen.Update.Option option) |
Creates or modifies an integer attribute with the option to update or not. More... | |
unsafe void | SetUserAttribute (string title, int index, double value, NXOpen.Update.Option option) |
Creates or modifies a real attribute with the option to update or not. More... | |
unsafe void | SetUserAttribute (string title, int index, string value, NXOpen.Update.Option option) |
Creates or modifies a string attribute with the option to update or not. More... | |
unsafe void | SetUserAttribute (string title, int index, NXOpen.Update.Option option) |
Creates or modifies a null attribute with the option to update or not. More... | |
unsafe void | SetTimeUserAttribute (string title, int index, string value, NXOpen.Update.Option option) |
Creates or modifies a time attribute with the option to update or not. More... | |
unsafe void | SetTimeUserAttribute (string title, int index, NXOpen.NXObject.ComputationalTime value, NXOpen.Update.Option option) |
Creates or modifies a time attribute with the option to update or not. More... | |
unsafe void | SetBooleanUserAttribute (string title, int index, bool value, NXOpen.Update.Option option) |
Creates or modifies a boolean attribute with the option to update or not. More... | |
unsafe NXOpen.AttributeIterator | CreateAttributeIterator () |
Create an attribute iterator More... | |
unsafe bool | HasUserAttribute (NXOpen.AttributeIterator iterator) |
Determines if an attribute exists on the object, that satisfies the given iterator More... | |
unsafe bool | HasUserAttribute (string title, NXOpen.NXObject.AttributeType type, int index) |
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. More... | |
unsafe int | GetUserAttributeCount (NXOpen.AttributeIterator iterator) |
Gets the count of set attributes on the object, if any, that satisfy the given iterator. More... | |
unsafe int | GetUserAttributeCount (NXOpen.AttributeIterator iterator, bool countArrayAsOneAttribute) |
Gets the count of set attributes on the object, if any, that satisfy the given iterator. More... | |
unsafe int | GetUserAttributeCount (NXOpen.NXObject.AttributeType type) |
Gets the count of set attributes on the object, if any, of the given type. More... | |
unsafe int | GetUserAttributeCount (NXOpen.NXObject.AttributeType type, bool includeUnset, bool countArrayAsOneAttribute) |
Gets the count of attributes on the object, if any, of the given type. More... | |
unsafe int | GetUserAttributeSize (string title, NXOpen.NXObject.AttributeType type) |
Gets the size of the first attribute encountered on the object, if any, with a given Title and Type. More... | |
unsafe bool | GetNextUserAttribute (NXOpen.AttributeIterator iterator, out NXOpen.NXObject.AttributeInformation info) |
Gets the next attribute encountered on the object, if any, that satisfies the given iterator. More... | |
unsafe NXOpen.NXObject.AttributeInformation | GetUserAttribute (string title, NXOpen.NXObject.AttributeType type, int index) |
Gets the first attribute encountered on the object, if any, with a given Title, Type and array Index. More... | |
unsafe bool | GetBooleanUserAttribute (string title, int index) |
Gets a boolean attribute by Title and array Index. More... | |
unsafe int | GetIntegerUserAttribute (string title, int index) |
Gets an integer attribute by Title and array Index. More... | |
unsafe double | GetRealUserAttribute (string title, int index) |
Gets a real attribute by Title and array Index. More... | |
unsafe string | GetStringUserAttribute (string title, int index) |
Gets a string attribute by Title and array Index. More... | |
unsafe string | GetTimeUserAttribute (string title, int index) |
Gets a time attribute by Title and array Index. More... | |
unsafe NXOpen.NXObject.ComputationalTime | GetComputationalTimeUserAttribute (string title, int index) |
Gets a time attribute by Title and array Index. More... | |
unsafe NXOpen.NXObject.AttributeInformation[] | GetUserAttributes (NXOpen.AttributeIterator iterator) |
Gets all the attributes that have been set on the given object, if any, that satisfy the given iterator. More... | |
unsafe NXOpen.NXObject.AttributeInformation[] | GetUserAttributes () |
Gets all the attributes that have been set on the given object. More... | |
unsafe NXOpen.NXObject.AttributeInformation[] | GetUserAttributes (bool includeUnset) |
Gets all the attributes of the given object. More... | |
unsafe string | GetUserAttributeAsString (string title, NXOpen.NXObject.AttributeType type, int index) |
Gets the first attribute encountered on the object, if any, with a given title, type and array index. More... | |
unsafe void | DeleteUserAttributes (NXOpen.AttributeIterator iterator, NXOpen.Update.Option option) |
Deletes the attributes on the object, if any, that satisfy the given iterator More... | |
unsafe void | DeleteUserAttribute (NXOpen.NXObject.AttributeType type, string title, bool deleteEntireArray, NXOpen.Update.Option option) |
Deletes the first attribute encountered with the given Type, Title. More... | |
unsafe void | DeleteUserAttributes (NXOpen.NXObject.AttributeType type, NXOpen.Update.Option option) |
Deletes the attributes encountered with the given Type with option to update or not. More... | |
unsafe void | SetUserAttributeLock (string title, NXOpen.NXObject.AttributeType type, bool @lock) |
Lock or unlock the given attribute. More... | |
unsafe bool | GetUserAttributeLock (string title, NXOpen.NXObject.AttributeType type) |
Determine the lock of the given attribute. More... | |
unsafe NXOpen.NXObject[] | GetUserAttributeSourceObjects () |
Returns an array of objects from which this object presents attributes. More... | |
unsafe void | SetPdmReferenceAttribute (string attributeTitle, string attributeValue) |
Sets the value of PDM Reference attribute on the object. More... | |
unsafe string | GetPdmReferenceAttributeValue (string attributeTitle) |
Gets the value of PDM Reference attribute for given object. More... | |
unsafe NXOpen.NXObject.AttributeInformation[] | GetUserAttribute (string title, bool includeUnset, bool addStringValues, NXOpen.NXObject.AttributeType type) |
Gets the first attribute (or attribute array) encountered on the object, if any, with a given Title and Type. More... | |
unsafe NXOpen.NXObject.AttributeInformation[] | GetUserAttributes (bool includeUnset, bool addStringValues) |
Gets all the attributes of the given object. More... | |
unsafe void | DeleteAllAttributesByType (NXOpen.NXObject.AttributeType type) |
Deletes all attributes of a specific type. More... | |
unsafe void | DeleteAllAttributesByType (NXOpen.NXObject.AttributeType type, NXOpen.Update.Option option) |
Deletes all attributes of a specific type with the option to update or not. More... | |
unsafe void | SetAttribute (string title, int value) |
Creates or modifies an integer attribute. More... | |
unsafe void | SetAttribute (string title, int value, NXOpen.Update.Option option) |
Creates or modifies an integer attribute with the option to update or not. More... | |
unsafe void | SetAttribute (string title, double value) |
Creates or modifies a real attribute. More... | |
unsafe void | SetAttribute (string title, double value, NXOpen.Update.Option option) |
Creates or modifies a real attribute with the option to update or not. More... | |
unsafe void | SetAttribute (string title, string value) |
Creates or modifies a string attribute. More... | |
unsafe void | SetAttribute (string title, string value, NXOpen.Update.Option option) |
Creates or modifies a string attribute with the option to update or not. More... | |
unsafe void | SetAttribute (string title) |
Creates or modifies a null attribute which is an attribute with a title and no value. More... | |
unsafe void | SetAttribute (string title, NXOpen.Update.Option option) |
Creates or modifies a null attribute with the option to update or not. More... | |
unsafe void | SetTimeAttribute (string title, string value) |
Creates or modifies a time attribute. More... | |
unsafe void | SetTimeAttribute (string title, string value, NXOpen.Update.Option option) |
Creates or modifies a time attribute with the option to update or not. More... | |
unsafe int | GetIntegerAttribute (string title) |
Gets an integer attribute by title. More... | |
unsafe double | GetRealAttribute (string title) |
Gets a real attribute by title. More... | |
unsafe string | GetStringAttribute (string title) |
Gets a string attribute value by title. More... | |
unsafe string | GetTimeAttribute (NXOpen.NXObject.DateAndTimeFormat format, string title) |
Gets a time attribute by title. More... | |
unsafe string | GetReferenceAttribute (string title) |
Gets the reference string (not the calculated value) of a string attribute that uses a reference string. More... | |
unsafe void | DeleteAttributeByTypeAndTitle (NXOpen.NXObject.AttributeType type, string title) |
Deletes an attribute by type and title. More... | |
unsafe void | DeleteAttributeByTypeAndTitle (NXOpen.NXObject.AttributeType type, string title, NXOpen.Update.Option option) |
Deletes an attribute by type and title with the option to update or not. More... | |
unsafe void | SetReferenceAttribute (string title, string value) |
Creates or modifies a string attribute which uses a reference string. More... | |
unsafe void | SetReferenceAttribute (string title, string value, NXOpen.Update.Option option) |
Creates or modifies a string attribute which uses a reference string, with the option to update or not. More... | |
unsafe NXOpen.NXObject.AttributeInformation[] | GetAttributeTitlesByType (NXOpen.NXObject.AttributeType type) |
Gets all the attribute titles of a specific type. More... | |
unsafe string[] | GetUserAttributesAsStrings () |
Gets all the attributes that have been set on the given object. More... | |
unsafe NXOpen.INXObject | FindObject (string journalIdentifier) |
Finds the NXOpen.NXObject with the given identifier as recorded in a journal. More... | |
unsafe void | Print () |
Prints a representation of this object to the system log file. More... | |
unsafe void | SetName (string name) |
Sets the custom name of the object. More... | |
Properties | |
NXOpen.Assemblies.ArrangementCollection | Arrangements [get] |
The collection of NXOpen.Assemblies.Arrangement s defined in the ComponentAssembly More... | |
NXOpen.Assemblies.ExplosionCollection | Explosions [get] |
The collection of NXOpen.Assemblies.Explosion s defined in the ComponentAssembly More... | |
NXOpen.Assemblies.DrawingExplosionCollection | DrawingExplosions [get] |
The collection of NXOpen.Assemblies.DrawingExplosion s defined in the ComponentAssembly More... | |
NXOpen.Assemblies.ComponentPatternCollection | ComponentPatterns [get] |
The collection of NXOpen.Assemblies.ComponentPattern defined in the ComponentAssembly More... | |
NXOpen.Assemblies.SubsetCollection | Subsets [get] |
The collection of NXOpen.Assemblies.Subset s defined in the ComponentAssembly More... | |
NXOpen.Assemblies.ClearanceSetCollection | ClearanceSets [get] |
The collection of NXOpen.Assemblies.ClearanceSet s defined in the ComponentAssembly More... | |
NXOpen.Assemblies.OrderCollection | OrdersSet [get] |
The collection of NXOpen.Assemblies.Order s defined in the ComponentAssembly More... | |
unsafe NXOpen.Assemblies.Arrangement | ActiveArrangement [get, set] |
Returns or sets the currently active NXOpen.Assemblies.Arrangement for this ComponentAssembly More... | |
unsafe NXOpen.Positioning.ComponentPositioner | Positioner [get] |
Returns the component positioner for this assembly. More... | |
unsafe NXOpen.Assemblies.Component | RootComponent [get] |
Returns the top-level component, i.e. More... | |
Properties inherited from NXOpen.NXObject | |
unsafe bool | IsOccurrence [get] |
Returns whether this object is an occurrence or not. More... | |
unsafe string | JournalIdentifier [get] |
Returns the identifier that would be recorded in a journal for this object. More... | |
unsafe string | Name [get] |
Returns the custom name of the object. More... | |
unsafe NXOpen.Assemblies.Component | OwningComponent [get] |
Returns the owning component, if this object is an occurrence. More... | |
unsafe NXOpen.BasePart | OwningPart [get] |
Returns the owning part of this object More... | |
unsafe NXOpen.INXObject | Prototype [get] |
Returns the prototype of this object if it is an occurrence. More... | |
Properties inherited from NXOpen.INXObject | |
bool | IsOccurrence [get] |
Returns whether this object is an occurrence or not. More... | |
string | JournalIdentifier [get] |
Returns the identifier that would be recorded in a journal for this object. More... | |
string | Name [get] |
Returns the custom name of the object. More... | |
NXOpen.Assemblies.Component | OwningComponent [get] |
Returns the owning component, if this object is an occurrence. More... | |
NXOpen.BasePart | OwningPart [get] |
Returns the owning part of this object More... | |
NXOpen.INXObject | Prototype [get] |
Returns the prototype of this object if it is an occurrence. More... | |
Represents the set of NXOpen.Assemblies.Component s that make up an assembly.
Components are arranged in a tree structure, with a single component at the root. (See NXOpen.Assemblies.ComponentAssembly.RootComponent .) The components directly below the root are added to this assembly by calling NXOpen.Assemblies.ComponentAssembly.AddComponent . These "Top Level" components are said to be owned directly by this assembly. Top Level components may themselves have subcomponents.
Certain methods in this class will only operate on Top Level components. For example, NXOpen.Assemblies.ComponentAssembly.MoveComponent will throw an exception if the input component is not owned directly by this assembly.
Note, however, that input components will be mapped onto the correct component in the assembly. See NXOpen.Assemblies.ComponentAssembly.MapComponentFromParent .
For any methods that specify a component's position, the orientation matrix is in column order. The first column of the matrix specifies the X axis, the second the Y axis, and the third the Z axis.
To obtain an instance of this class, use NXOpen.BasePart.ComponentAssembly
Created in NX3.0.0
Check in and Check out options for components
Open options for open_components
Option controls whether reordered NXOpen.Assemblies.Component s are placed before or after the target NXOpen.Assemblies.Component
Enumerator | |
---|---|
PlaceBefore |
Move reordered NXOpen.Assemblies.Component s before the target NXOpen.Assemblies.Component |
PlaceAfter |
Move reordered NXOpen.Assemblies.Component s after the target NXOpen.Assemblies.Component |
Defines how a component substitution operation is performed.
unsafe NXOpen.Assemblies.Component NXOpen.Assemblies.ComponentAssembly.AddComponent | ( | string | partToAdd, |
string | referenceSetName, | ||
string | componentName, | ||
NXOpen.Point3d | basePoint, | ||
NXOpen.Matrix3x3 | orientation, | ||
int | layer, | ||
out NXOpen.PartLoadStatus | loadStatus | ||
) |
Creates a new NXOpen.Assemblies.Component in this assembly, based on an existing part file.
Created in NX3.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
partToAdd | The part that defines the new component |
referenceSetName | The name of the reference set used to represent the new component |
componentName | The name of the new component |
basePoint | Location of the new component |
orientation | Orientation matrix for the new component, in column order. |
layer | The layer to place the new component on -1 means use the original layers defined in the component. 0 means use the work layer. 1-256 means use the specified layer. |
loadStatus | Result of loading the part_to_add |
unsafe NXOpen.Assemblies.Component NXOpen.Assemblies.ComponentAssembly.AddComponent | ( | string | partToAdd, |
string | referenceSetName, | ||
string | componentName, | ||
NXOpen.Point3d | basePoint, | ||
NXOpen.Matrix3x3 | orientation, | ||
int | layer, | ||
out NXOpen.PartLoadStatus | loadStatus, | ||
bool | uomAsNgc | ||
) |
Creates a new NXOpen.Assemblies.Component in this assembly, based on an existing part file.
Created in NX6.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
partToAdd | The part that defines the new component |
referenceSetName | The name of the reference set used to represent the new component |
componentName | The name of the new component |
basePoint | Location of the new component |
orientation | Orientation matrix for the new component, in column order. |
layer | The layer to place the new component on -1 means use the original layers defined in the component. 0 means use the work layer. 1-256 means use the specified layer. |
loadStatus | Result of loading the part_to_add |
uomAsNgc | Whether to set to non-geometric if with unit-of-measure |
unsafe NXOpen.Assemblies.Component NXOpen.Assemblies.ComponentAssembly.AddComponent | ( | NXOpen.BasePart | partToAdd, |
string | referenceSetName, | ||
string | componentName, | ||
NXOpen.Point3d | basePoint, | ||
NXOpen.Matrix3x3 | orientation, | ||
int | layer, | ||
out NXOpen.PartLoadStatus | loadStatus | ||
) |
Creates a new NXOpen.Assemblies.Component in this assembly, based on an existing part file.
Created in NX4.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
partToAdd | The part that defines the new component |
referenceSetName | The name of the reference set used to represent the new component |
componentName | The name of the new component |
basePoint | Location of the new component |
orientation | Orientation matrix for the new component, in column order. |
layer | The layer to place the new component on -1 means use the original layers defined in the component. 0 means use the work layer. 1-256 means use the specified layer. |
loadStatus | Result of loading the part_to_add |
unsafe void NXOpen.Assemblies.ComponentAssembly.AddComponents | ( | NXOpen.Part[] | partsToAdd, |
NXOpen.Point3d | point, | ||
NXOpen.Matrix3x3 | orientation, | ||
int | layer, | ||
string | referenceSetName, | ||
int | count, | ||
bool | scatter, | ||
out NXOpen.Assemblies.Component[] | components | ||
) |
Creates new NXOpen.Assemblies.Component in this assembly, based on existing part files.
Created in NX12.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
partsToAdd | The parts that define new components |
point | Location of the new component |
orientation | Orientation matrix for the new component, in column order. |
layer | The layer to place the new component on -1 means use the original layers defined in the component. 0 means use the work layer. 1-256 means use the specified layer. |
referenceSetName | The name of the reference set used to represent the new component |
count | number of times each part to be added as component in parent part |
scatter | Scatter the multiple components around the specified location |
components | The array of components added to the parent part |
unsafe NXOpen.Assemblies.Component NXOpen.Assemblies.ComponentAssembly.AddMasterPartComponent | ( | string | partToAdd, |
string | referenceSetName, | ||
string | componentName, | ||
NXOpen.Point3d | basePoint, | ||
NXOpen.Matrix3x3 | orientation, | ||
int | layer, | ||
out NXOpen.PartLoadStatus | loadStatus | ||
) |
Creates a new NXOpen.Assemblies.Component in this assembly as master part.
Created in NX3.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
partToAdd | The part that defines the new component |
referenceSetName | The name of the reference set used to represent the new component |
componentName | The name of the new component |
basePoint | Location of the new component |
orientation | Orientation matrix for the new component, in column order. |
layer | The layer to place the new component on -1 means use the original layers defined in the component. 0 means use the work layer. 1-256 means use the specified layer. |
loadStatus | Result of loading the part_to_add |
unsafe NXOpen.Assemblies.Component NXOpen.Assemblies.ComponentAssembly.AddMasterPartComponent | ( | NXOpen.Part | partToAdd, |
string | referenceSetName, | ||
string | componentName, | ||
NXOpen.Point3d | basePoint, | ||
NXOpen.Matrix3x3 | orientation, | ||
int | layer, | ||
out NXOpen.PartLoadStatus | loadStatus | ||
) |
Creates a new NXOpen.Assemblies.Component in this assembly as master part.
Created in NX4.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
partToAdd | The part that defines the new component |
referenceSetName | The name of the reference set used to represent the new component |
componentName | The name of the new component |
basePoint | Location of the new component |
orientation | Orientation matrix for the new component, in column order. |
layer | The layer to place the new component on -1 means use the original layers defined in the component. 0 means use the work layer. 1-256 means use the specified layer. |
loadStatus | Result of loading the part_to_add |
unsafe NXOpen.PartLoadStatus NXOpen.Assemblies.ComponentAssembly.AddPendingComponent | ( | string | partToAdd, |
NXOpen.NXObject | pendingComponent, | ||
string | referenceSetName, | ||
string | componentName, | ||
NXOpen.Point3d | basePoint, | ||
NXOpen.Matrix3x3 | orientation, | ||
int | layer, | ||
bool | uomAsNgc | ||
) |
Add a pending NXOpen.Assemblies.Component in this assembly.
Created in NX8.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
partToAdd | The part that defines the new component |
pendingComponent | component to add |
referenceSetName | The name of the reference set used to represent the new component |
componentName | The name of the new component |
basePoint | Location of the new component |
orientation | Orientation matrix for the new component, in column order. |
layer | The layer to place the new component on -1 means use the original layers defined in the component. 0 means use the work layer. 1-256 means use the specified layer. |
uomAsNgc | Whether to set to non-geometric if with unit-of-measure |
unsafe void NXOpen.Assemblies.ComponentAssembly.ChangeByName | ( | string | name, |
NXOpen.Assemblies.Component[] | partOccs | ||
) |
Changes the current NXOpen.Assemblies.Arrangement of the given NXOpen.Assemblies.Component s to the NXOpen.Assemblies.Arrangement with the given name.
Created in NX7.5.2
License requirements: assemblies ("ASSEMBLIES MODULE")
name | The name of arrangement to change to |
partOccs | The NXOpen.Assemblies.Component s to be modified |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.CheckinComponents | ( | NXOpen.Assemblies.Component[] | partOccs, |
NXOpen.Assemblies.ComponentAssembly.CheckinCheckoutOption | checkinInputOption | ||
) |
Checks in array of components as per the option NXOpen.Assemblies.ComponentAssembly.CheckinCheckoutOption .
Created in NX8.5.0
License requirements: assemblies ("ASSEMBLIES MODULE")
partOccs | Array of components to check in |
checkinInputOption | Option that controls what to check in |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.CheckinWorkset | ( | ) |
Checks in workset.
Created in NX8.5.0
License requirements: assemblies ("ASSEMBLIES MODULE")
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.CheckoutAllModifiedObjects | ( | out NXOpen.NXObject[] | checkedOutObjects | ) |
Checks out all modified objects in the current session.
checkedOutObjects collection will be type of NXOpen.BasePart or NXOpen.PDM.DesignElementRevision
Created in NX8.5.0
License requirements: assemblies ("ASSEMBLIES MODULE")
checkedOutObjects | Array of NXObjects checked out |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.CheckoutComponents | ( | NXOpen.Assemblies.Component[] | partOccs, |
NXOpen.Assemblies.ComponentAssembly.CheckinCheckoutOption | checkoutInputOption | ||
) |
Checks out array of components as per the option NXOpen.Assemblies.ComponentAssembly.CheckinCheckoutOption .
Created in NX8.5.0
License requirements: assemblies ("ASSEMBLIES MODULE")
partOccs | Array of components to check out |
checkoutInputOption | Option that controls what to check out |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.CheckoutWorkset | ( | ) |
Checks out workset.
Created in NX8.5.0
License requirements: assemblies ("ASSEMBLIES MODULE")
unsafe NXOpen.PartCloseStatus NXOpen.Assemblies.ComponentAssembly.CloseComponents | ( | NXOpen.Assemblies.Component[] | componentsToClose, |
NXOpen.BasePart.CloseWholeTree | wholeTree, | ||
NXOpen.Assemblies.ComponentAssembly.CloseModified | closeModified | ||
) |
Given an array of components, close the components.
This close of the components will check for different reasons that the part cannot be closed. The reasons will be returned in the PartCloseStatus object.
Created in NX6.0.1
License requirements: None.
componentsToClose | Array of components to close |
wholeTree | If true, unloads all components of the part. If false, unloads only the top-level part |
closeModified | Behavior of close if component parts are modified. |
unsafe void NXOpen.Assemblies.ComponentAssembly.ConvertRememberedMcs | ( | ) |
Converts all remembered mating constraints in the part of this assembly to remembered assembly constraints
Created in NX7.5.0
License requirements: assemblies ("ASSEMBLIES MODULE")
unsafe NXOpen.Assemblies.Component [] NXOpen.Assemblies.ComponentAssembly.CopyComponents | ( | NXOpen.Assemblies.Component[] | components | ) |
Given an array of components, creates copies of the components such that each copy is created under the parent assembly of the original component.
The original components do not need to be under the same parent assembly as each other.
The number of new components may be different from the original number of components if problems occurred during the copy.
Created in NX6.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
components | Components to be copied. |
unsafe NXOpen.Assemblies.ComponentPatternBuilder NXOpen.Assemblies.ComponentAssembly.CreateComponentPatternBuilder | ( | NXOpen.Assemblies.ComponentPattern | compPattern | ) |
Creates a NXOpen.Assemblies.ComponentPatternBuilder object This can be used to create or edit a component pattern.
Created in NX9.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
compPattern | The pattern definition object will be used in edit |
unsafe NXOpen.Positioning.ComponentConstraintGroupBuilder NXOpen.Assemblies.ComponentAssembly.CreateConstraintGroupBuilder | ( | NXOpen.Positioning.ComponentConstraintGroup | group, |
NXOpen.Assemblies.Component | contextComponent | ||
) |
Creates a NXOpen.Positioning.ComponentConstraintGroupBuilder object.
This can be used to create a constraint group or edit an existing constraint group. The context component decides which displayed constraints are to be used from the member constraints of an existing constraint group. If the context component is a null reference (Nothing in Visual Basic) the displayed constraints used are in the same part as the member constraints.
Created in NX8.0.1
License requirements: assemblies ("ASSEMBLIES MODULE")
group | Group to be edited, if a null reference (Nothing in Visual Basic) then a new group is created |
contextComponent | Context component, can be a null reference (Nothing in Visual Basic) |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.CreateIsolateViewWithComponents | ( | NXOpen.Assemblies.Component[] | components, |
out NXOpen.View | view | ||
) |
Creates a temporary NXOpen.View and shows array of components in it and treats this as Isolate view till it gets undisplayed.
Only one Isolate view can be created for the assembly. Returns NXOpen.View which is treated as Isolate View.
Created in NX11.0.1
License requirements: gateway ("UG GATEWAY")
components | Array of components to be shown in isolate view |
view | Return the isolate view |
unsafe NXOpen.Positioning.MatingConverter NXOpen.Assemblies.ComponentAssembly.CreateMatingConverter | ( | ) |
Creates a NXOpen.Positioning.MatingConverter object for this assembly.
This can be used to convert Mating Conditions in this part and in its child components to Assembly Constraints. Note that this part need not be the work part for this.
Created in NX5.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
unsafe void NXOpen.Assemblies.ComponentAssembly.DeleteMatingConditions | ( | ) |
Delete all the mating conditions in this assembly.
This can be used before creating assembly constraints in the assembly, if the mating conditions are not being converted. Component-component mating conditions and inherited mating conditions are not deleted. Update should be called afterwards.
Created in NX7.5.0
License requirements: assemblies ("ASSEMBLIES MODULE")
unsafe NXOpen.Assemblies.Order NXOpen.Assemblies.ComponentAssembly.GetActiveOrder | ( | ) |
Returns the active order in the part
Created in NX10.0.3
License requirements: assemblies ("ASSEMBLIES MODULE")
unsafe string NXOpen.Assemblies.ComponentAssembly.GetAsRequiredQuantity | ( | NXOpen.Assemblies.Component | component | ) |
Gets the as-required quantity on this component.
Created in NX6.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
component | The component to edit. Must be directly owned by this assembly. |
unsafe void NXOpen.Assemblies.ComponentAssembly.GetCheckedoutStatusOfObjects | ( | out NXOpen.NXObject[] | checkedOutObjects, |
out NXOpen.NXObject[] | uncheckedOutObjects | ||
) |
Returns the checkedout status (checkedout/non checkedout) of all the objects open in NX.
Created in NX8.5.0
License requirements: None.
checkedOutObjects | Array of NXObjects which are open in session and checked out |
uncheckedOutObjects | Array of NXObjects which are open in session but not checkout |
unsafe void NXOpen.Assemblies.ComponentAssembly.GetComponentOrders | ( | out NXOpen.Assemblies.ComponentOrder[] | orders | ) |
Returns all NXOpen.Assemblies.ComponentOrder s available in the part
Created in NX9.0.0
License requirements: None.
orders | Returns array of NXOpen.Assemblies.ComponentOrder s in part |
unsafe NXOpen.Assemblies.ComponentQuantity NXOpen.Assemblies.ComponentAssembly.GetComponentQuantityType | ( | NXOpen.Assemblies.Component | component | ) |
Gets the quantity type of the components.
Returns NXOpen.Assemblies.ComponentQuantity .
Created in NX6.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
component | The component to query. Must be directly owned by this assembly. |
unsafe int NXOpen.Assemblies.ComponentAssembly.GetIntegerQuantity | ( | NXOpen.Assemblies.Component | component | ) |
Gets the value of the integer quantity of component.
Created in NX6.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
component | The component to query. Must be directly owned by this assembly. |
unsafe bool NXOpen.Assemblies.ComponentAssembly.GetNonGeometricState | ( | NXOpen.Assemblies.Component | component | ) |
Gets the component state as Geometric or Non-Geometric.
Created in NX6.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
component | The component to query. Must be directly owned by this assembly. |
unsafe double NXOpen.Assemblies.ComponentAssembly.GetRealQuantity | ( | NXOpen.Assemblies.Component | component, |
out string | units | ||
) |
Gets the value of real quantity and corresponding units on this component.
Created in NX6.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
component | The component to query. Must be directly owned by this assembly. |
units | Units |
unsafe NXOpen.Assemblies.ComponentAssembly.SuppressedState NXOpen.Assemblies.ComponentAssembly.GetSuppressedState | ( | NXOpen.Assemblies.Component | component, |
out bool | controlled | ||
) |
Gets the suppression state of the component in its controlling arrangement
Created in NX6.0.4
License requirements: None.
component | The component to query. |
controlled | Is the suppression state controlled at the level of arrangement? |
unsafe NXOpen.Assemblies.ComponentAssembly.SuppressedState NXOpen.Assemblies.ComponentAssembly.GetSuppressedState | ( | NXOpen.Assemblies.Component | component, |
NXOpen.Assemblies.Arrangement | arrangement, | ||
out bool | controlled | ||
) |
Gets the suppression state of the component in the given arrangement.
Created in NX6.0.4
License requirements: None.
component | The component to query. |
arrangement | Arrangements in which components should be suppressed. |
controlled | Is the suppression state controlled at the level of arrangement? |
unsafe NXOpen.Expression NXOpen.Assemblies.ComponentAssembly.GetSuppressionExpression | ( | NXOpen.Assemblies.Component | component | ) |
Gets the expression controlling the suppression of the component in its controlling arrangement
Created in NX6.0.4
License requirements: None.
component | The component to query. |
unsafe NXOpen.Expression NXOpen.Assemblies.ComponentAssembly.GetSuppressionExpression | ( | NXOpen.Assemblies.Component | component, |
NXOpen.Assemblies.Arrangement | arrangement | ||
) |
Gets the expression controlling the suppression of the component in the given arrangment
Created in NX6.0.4
License requirements: None.
component | The component to query. |
arrangement | The arrangement in which to query the suppressed state |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.HideComponentsInIsolateView | ( | NXOpen.Assemblies.Component[] | components, |
out NXOpen.View | view | ||
) |
Hides array of components in Isolate view NXOpen.View .
If Isolate view doesn't exist then this API doesn't do anything. Returns NXOpen.View which is treated as Isolate View.
Created in NX11.0.1
License requirements: gateway ("UG GATEWAY")
components | Array of components to be shown in isolate view |
view | Return the isolate view |
unsafe NXOpen.Assemblies.Component NXOpen.Assemblies.ComponentAssembly.InsertProduct | ( | NXOpen.Part | productPart, |
int | layer, | ||
out NXOpen.PartLoadStatus | loadStatus | ||
) |
Adds a product into workset part at identity location.
Created in NX12.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
productPart | The product being added to the workset |
layer | The layer to place the new component on -1 means use the original layers defined in the component. 0 means use the work layer. 1-256 means use the specified layer. |
loadStatus | Result of loading the part_to_add |
unsafe NXOpen.Assemblies.Component NXOpen.Assemblies.ComponentAssembly.MapComponentFromParent | ( | NXOpen.Assemblies.Component | component | ) |
Maps a component in a parent assembly onto a corresponding component in this assembly.
For example, given an Axle assembly:
and a Car assembly containing two Axle components:
then calling Axle.MapComponentFromParent with the Front Left Wheel component will return the Left Wheel component. Note that calling Car.MapComponentFromParent on Left Wheel will not work. See NXOpen.Assemblies.ComponentAssembly.MapComponentsFromSubassembly .
Calling Axle.MapComponent with the Left Wheel component will simply return Left Wheel, i.e. it is a null operation.
Note that calling this method may load additional assembly data from the Axle part.
Created in NX3.0.0
License requirements: None.
component | The component to map. This should be defined in the tree of a parent assembly which contains this assembly. |
unsafe NXOpen.Assemblies.Component [] NXOpen.Assemblies.ComponentAssembly.MapComponentsFromSubassembly | ( | NXOpen.Assemblies.Component | component | ) |
Maps a component in a subassembly onto the corresponding components in this parent assembly.
For example, given an Axle assembly:
and a Car assembly containing two Axle components:
then calling Car.MapComponentsFromSubassembly on Left Wheel will return Front Left Wheel and Rear Left Wheel. See also NXOpen.Assemblies.ComponentAssembly.MapComponentFromParent .
Created in NX3.0.0
License requirements: None.
component | The component to map. This must be defined in a subassembly of this assembly. |
unsafe void NXOpen.Assemblies.ComponentAssembly.MoveComponent | ( | NXOpen.Assemblies.Component | component, |
NXOpen.Vector3d | translation, | ||
NXOpen.Matrix3x3 | rotation | ||
) |
Moves a component by specifying a translation and rotation.
Note that these are specified in the coordinates of this assembly, which are not necessarily the coordinates of the displayed part. Note that the rotation matrix is expected to be stored in a column order fashion.
Created in NX3.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
component | The component to edit. Must be directly owned by this assembly |
translation | The translation delta |
rotation | The rotation delta, in column order. |
unsafe void NXOpen.Assemblies.ComponentAssembly.MoveToPendingComponent | ( | NXOpen.NXObject | component | ) |
Move a NXOpen.Assemblies.Component in this assembly to a pending list.
The NXOpen.Assemblies.Component should be previously in the pending list and just got added into the assembly.
Created in NX10.0.2
License requirements: assemblies ("ASSEMBLIES MODULE")
component | component to move to pending list |
unsafe NXOpen.PartLoadStatus NXOpen.Assemblies.ComponentAssembly.OpenComponents | ( | NXOpen.Assemblies.ComponentAssembly.OpenOption | openOption, |
NXOpen.Assemblies.Component[] | componentsToOpen, | ||
out NXOpen.Assemblies.ComponentAssembly.OpenComponentStatus[] | openStatus | ||
) |
Given an array of components, open the components using the open_option.
Created in NX6.0.1
License requirements: None.
openOption | The option that controls the open operation |
componentsToOpen | Array of components to open |
openStatus | Shows the status of the objects in an indexed array according to if they could be opened |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.ReleaseSuppression | ( | NXOpen.Assemblies.Component[] | components, |
NXOpen.Assemblies.Arrangement[] | arrangements | ||
) |
Release control of the suppression state of an array of components.
The components will no longer have their suppression state controlled by the given arrangements. (Note that it is not an error if the given arrangements do not control the components.)
Created in NX3.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
components | NXOpen.Assemblies.Component s to be released |
arrangements | Arrangements in which components should be released. These arrangements must be defined in this ComponentAssembly |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.ReleaseSuppression | ( | NXOpen.Assemblies.Component[] | components | ) |
Release control of the suppression state of an array of components.
The components will no longer have their suppression state controlled by any of the arrangements in the ComponentAssembly.
Created in NX3.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
components | NXOpen.Assemblies.Component s to be released |
unsafe void NXOpen.Assemblies.ComponentAssembly.RemoveComponent | ( | NXOpen.Assemblies.Component | component | ) |
Removes a component from this assemebly.
Created in NX3.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
component | The component to remove. Must be directly owned by this assembly. |
unsafe void NXOpen.Assemblies.ComponentAssembly.ReorderChildrenOfParent | ( | NXOpen.Assemblies.ComponentOrder | order, |
NXOpen.Assemblies.Component | parentComponent, | ||
NXOpen.Assemblies.Component[] | componentsToReorder | ||
) |
Assigns a new order to immediate children NXOpen.Assemblies.Component s of parent NXOpen.Assemblies.Component .
Created in NX9.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
order | NXOpen.Assemblies.ComponentOrder in which children are reordered |
parentComponent | Parent component whose children are reordered |
componentsToReorder | Array of children components in new order |
unsafe void NXOpen.Assemblies.ComponentAssembly.ReorderComponents | ( | NXOpen.Assemblies.ComponentOrder | order, |
NXOpen.Assemblies.Component[] | componentsToReorder, | ||
NXOpen.Assemblies.Component | targetComponent, | ||
NXOpen.Assemblies.ComponentAssembly.OrderTargetLocation | beforeOrAfter | ||
) |
Reorders the array of NXOpen.Assemblies.Component s before or after the target NXOpen.Assemblies.Component .
NXOpen.Assemblies.Component s to reorder and the target NXOpen.Assemblies.Component should be children of the same immediate parent.
Created in NX9.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
order | NXOpen.Assemblies.ComponentOrder in which components are reordered |
componentsToReorder | Array of components to be reordered |
targetComponent | Components are moved before or after this component |
beforeOrAfter | Whether to move components before or after the target component |
unsafe void NXOpen.Assemblies.ComponentAssembly.ReplaceReferenceSet | ( | NXOpen.Assemblies.Component | component, |
string | newReferenceSet | ||
) |
Replaces the reference set used by a component.
Note that the names of the default reference sets Empty and Entire Part can be obtained from NXOpen.Assemblies.Component.EmptyPartRefsetName or NXOpen.Assemblies.Component.EntirePartRefsetName .
Created in NX3.0.0
License requirements: None.
component | The component to edit. Must be directly owned by this assembly. |
newReferenceSet | The name of the new reference set |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.ReplaceReferenceSetInOwners | ( | string | newReferenceSet, |
NXOpen.Assemblies.Component[] | components | ||
) |
Sets the reference set used to represent each component in an array.
This is the equivalent of calling:
on each component in the array. However, this method will ensure that the reference set operations are carried out in the correct order, so that any effects caused by a parent's reference set change will be correctly reflected in the children. If changing reference set on components at various levels in the assembly, use this method.
Note that the names of the default reference sets Empty and Entire Part can be obtained from NXOpen.Assemblies.Component.EmptyPartRefsetName or NXOpen.Assemblies.Component.EntirePartRefsetName .
Created in NX3.0.0
License requirements: None.
newReferenceSet | The name of the new reference set |
components | Components to be edited. Each component will have its reference set updated in its owning assembly. |
unsafe void NXOpen.Assemblies.ComponentAssembly.RestructureComponents | ( | NXOpen.Assemblies.Component[] | origComponents, |
NXOpen.Assemblies.Component | newParentComponent, | ||
bool | deleteFlag, | ||
out NXOpen.Assemblies.Component[] | newComponents, | ||
out NXOpen.ErrorList | errorList | ||
) |
Given an array of components and a specified parent this function will transfer the given components to the parent.
The original components do not need to be under the same parent assembly as each other.
The number of new components may be different from the original number of components if problems occurred during the transfer
Created in NX6.0.1
License requirements: assemblies ("ASSEMBLIES MODULE")
origComponents | Array of components to be restructured |
newParentComponent | Destination for restructure |
deleteFlag | Flag to delete original components |
newComponents | Restructured components |
errorList | Any errors that occurred during the restructure |
unsafe void NXOpen.Assemblies.ComponentAssembly.SetAsRequiredQuantity | ( | NXOpen.Assemblies.Component | component | ) |
Sets the as-required quantity on this component.
Created in NX6.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
component | The component to edit. Must be directly owned by this assembly. |
unsafe void NXOpen.Assemblies.ComponentAssembly.SetDefault | ( | NXOpen.Assemblies.Arrangement | arrangement | ) |
Set the default NXOpen.Assemblies.Arrangement for the given NXOpen.Assemblies.ComponentAssembly .
Created in NX7.5.2
License requirements: assemblies ("ASSEMBLIES MODULE")
arrangement | The new default NXOpen.Assemblies.Arrangement . |
unsafe void NXOpen.Assemblies.ComponentAssembly.SetEmptyRefset | ( | NXOpen.Assemblies.Component | component | ) |
Convenience method for setting the reference set used to represent a component to be empty
Created in NX3.0.0
License requirements: None.
component | The component to edit. Must be directly owned by this assembly. |
unsafe void NXOpen.Assemblies.ComponentAssembly.SetEntirePartRefset | ( | NXOpen.Assemblies.Component | component | ) |
Convenience method for setting the reference set used to represent a component to be the entire part.
Created in NX3.0.0
License requirements: None.
component | The component to edit. Must be directly owned by this assembly. |
unsafe void NXOpen.Assemblies.ComponentAssembly.SetIntegerQuantity | ( | NXOpen.Assemblies.Component | component, |
int | integerQuantity | ||
) |
Sets the integer quantity on this component.
Created in NX6.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
component | The component to edit. Must be directly owned by this assembly. |
integerQuantity | Integer quantity value |
unsafe void NXOpen.Assemblies.ComponentAssembly.SetNonGeometricState | ( | NXOpen.Assemblies.Component | component, |
bool | nonGeometricState | ||
) |
Sets the component state to Geometric or Non-Geometric.
Component which are made non-geometric are undrawn from graphics area.
Created in NX6.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
component | The component to edit. Must be directly owned by this assembly. |
nonGeometricState | True to make component non-geometric, false otherwise |
unsafe void NXOpen.Assemblies.ComponentAssembly.SetRealQuantity | ( | NXOpen.Assemblies.Component | component, |
double | realQuantity, | ||
string | quantityUnits | ||
) |
Sets the real quantity and corresponding units on this component.
Created in NX6.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
component | The component to edit. Must be directly owned by this assembly. |
realQuantity | Real quantity value |
quantityUnits | Units |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.ShowComponentsInIsolateView | ( | NXOpen.Assemblies.Component[] | components, |
out NXOpen.View | view | ||
) |
Shows array of components in Isolate view NXOpen.View .
If Isolate view doesn't exist then this API doesn't do anything. Returns NXOpen.View which is treated as Isolate View.
Created in NX11.0.1
License requirements: gateway ("UG GATEWAY")
components | Array of components to be shown in isolate view |
view | Return the isolate view |
unsafe NXOpen.Assemblies.Component NXOpen.Assemblies.ComponentAssembly.SubstituteComponent | ( | NXOpen.Assemblies.Component | component, |
NXOpen.BasePart | part, | ||
string | newName, | ||
string | referenceSet, | ||
int | layer, | ||
NXOpen.Assemblies.ComponentAssembly.SubstitutionMode | mode | ||
) |
Substitutes an old component with a new component.
The new component represents a new part, but will be placed in the same location as the original.
Created in NX3.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
component | The old component to be substituted. |
part | The new part |
newName | The name for the new component |
referenceSet | The name of the reference set for the new component |
layer | The layer for the new component -1 means use the original layers defined in the component. 0 means use the work layer 1-256 means use the specified layer. |
mode | Defines the substitution mode |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.SuppressComponents | ( | NXOpen.Assemblies.Component[] | components, |
NXOpen.Assemblies.Arrangement[] | arrangements | ||
) |
Suppresses an array of components
Created in NX3.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
components | NXOpen.Assemblies.Component s to be suppressed |
arrangements | Arrangements in which components should be suppressed. These arrangements must be defined in this ComponentAssembly |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.SuppressComponents | ( | NXOpen.Assemblies.Component[] | components | ) |
Suppresses an array of components in all NXOpen.Assemblies.Arrangement s in this ComponentAssembly
Created in NX3.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
components | NXOpen.Assemblies.Component s to be suppressed |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.SuppressComponents | ( | NXOpen.Assemblies.Component[] | components, |
NXOpen.Assemblies.Arrangement[] | arrangements, | ||
string | expression | ||
) |
Suppresses an array of components in all NXOpen.Assemblies.Arrangement s in this ComponentAssembly
Created in NX5.0.1
License requirements: assemblies ("ASSEMBLIES MODULE")
components | NXOpen.Assemblies.Component s to be suppressed |
arrangements | Arrangements in which components should be unsuppressed |
expression | Suppress components if expression evalutes zero else unsuppress components |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.UnsuppressComponents | ( | NXOpen.Assemblies.Component[] | components, |
NXOpen.Assemblies.Arrangement[] | arrangements | ||
) |
Unsuppresses an array of components in this ComponentAssembly
Created in NX3.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
components | NXOpen.Assemblies.Component s to be unsuppressed |
arrangements | Arrangements in which components should be unsuppressed. These arrangements must be defined in this ComponentAssembly |
unsafe NXOpen.ErrorList NXOpen.Assemblies.ComponentAssembly.UnsuppressComponents | ( | NXOpen.Assemblies.Component[] | components | ) |
Unsuppresses an array of components in all NXOpen.Assemblies.Arrangement s in this ComponentAssembly
Created in NX3.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
components | NXOpen.Assemblies.Component s to be unsuppressed |
|
getset |
Returns or sets the currently active NXOpen.Assemblies.Arrangement for this ComponentAssembly
Created in NX3.0.0
License requirements to get this property: assemblies ("ASSEMBLIES MODULE")
License requirements to set this property: assemblies ("ASSEMBLIES MODULE")
|
get |
The collection of NXOpen.Assemblies.Arrangement s defined in the ComponentAssembly
Created in NX3.0.0
|
get |
The collection of NXOpen.Assemblies.ClearanceSet s defined in the ComponentAssembly
Created in NX9.0.0
|
get |
The collection of NXOpen.Assemblies.ComponentPattern defined in the ComponentAssembly
Created in NX9.0.0
|
get |
The collection of NXOpen.Assemblies.DrawingExplosion s defined in the ComponentAssembly
Created in NX12.0.0
|
get |
The collection of NXOpen.Assemblies.Explosion s defined in the ComponentAssembly
Created in NX3.0.0
|
get |
The collection of NXOpen.Assemblies.Order s defined in the ComponentAssembly
Created in NX9.0.0
|
get |
Returns the component positioner for this assembly.
The positioner manages the component constraints.
Created in NX4.0.0
License requirements: assemblies ("ASSEMBLIES MODULE")
|
get |
Returns the top-level component, i.e.
the component at the root of the component tree.
This component corresponds to the part that owns this NXOpen.Assemblies.ComponentAssembly . The components below this will correspond to parts added by calling NXOpen.Assemblies.ComponentAssembly.AddComponent .
Note that this will be a null reference (Nothing in Visual Basic) if there are no components in the tree. (I.e. if the part that owns this ComponentAssembly is a piece part.)
Created in NX3.0.0
License requirements: None.
|
get |
The collection of NXOpen.Assemblies.Subset s defined in the ComponentAssembly
Created in NX8.5.0