ComponentAssembly Class¶
-
class
NXOpen.Assemblies.
ComponentAssembly
¶ Bases:
NXOpen.NXObject
Represents the set of :py:class:`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 callingNXOpen.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()
New in version NX3.0.0.
Properties¶
Property | Description |
---|---|
ActiveArrangement | Returns or sets the currently active NXOpen.Assemblies.Arrangement for this ComponentAssembly |
IsOccurrence | Returns whether this object is an occurrence or not. |
JournalIdentifier | Returns the identifier that would be recorded in a journal for this object. |
Name | Returns the custom name of the object. |
OwningComponent | Returns the owning component, if this object is an occurrence. |
OwningPart | Returns the owning part of this object |
Positioner | Returns the component positioner for this assembly. |
Prototype | Returns the prototype of this object if it is an occurrence. |
RootComponent |
|
Tag | Returns the Tag for this object. |
Arrangements |
|
Explosions |
|
ComponentPatterns |
|
Subsets |
|
ClearanceSets |
|
OrdersSet |
|
Methods¶
Method | Description |
---|---|
AddComponent | Creates a new NXOpen.Assemblies.Component in this assembly, based on an existing part file. |
AddMasterPartComponent | Creates a new NXOpen.Assemblies.Component in this assembly as master part. |
AddPendingComponent | Add a pending NXOpen.Assemblies.Component in this assembly. |
ChangeByName | Changes the current NXOpen.Assemblies.Arrangement of the given NXOpen.Assemblies.Component`s to the :py:class:`NXOpen.Assemblies.Arrangement with the given name. |
CheckinComponents | Checks in array of components as per the option NXOpen.Assemblies.ComponentAssemblyCheckinCheckoutOption . |
CheckinWorkset | Checks in workset. |
CheckoutAllModifiedObjects | Checks out all modified objects in the current session. |
CheckoutComponents | Checks out array of components as per the option NXOpen.Assemblies.ComponentAssemblyCheckinCheckoutOption . |
CheckoutWorkset | Checks out workset. |
CloseComponents | Given an array of components, close the components. |
ConvertRememberedMcs | Converts all remembered mating constraints in the part of this assembly to remembered assembly constraints |
CopyComponents | Given an array of components, creates copies of the components such that each copy is created under the parent assembly of the original component. |
CreateAttributeIterator | Create an attribute iterator @return A new attribute iterator object |
CreateComponentPatternBuilder | Creates a NXOpen.Assemblies.ComponentPatternBuilder object This can be used to create or edit a component pattern. |
CreateConstraintGroupBuilder | Creates a NXOpen.Positioning.ComponentConstraintGroupBuilder object. |
CreateMatingConverter | Creates a NXOpen.Positioning.MatingConverter object for this assembly. |
DeleteAllAttributesByType | Deletes all attributes of a specific type. |
DeleteAttributeByTypeAndTitle | Deletes an attribute by type and title. |
DeleteMatingConditions | Delete all the mating conditions in this assembly. |
DeleteUserAttribute | Deletes the first attribute encountered with the given Type, Title. |
DeleteUserAttributes | Deletes the attributes on the object, if any, that satisfy the given iterator |
FindObject | Finds the NXOpen.NXObject with the given identifier as recorded in a journal. |
GetActiveOrder | Returns the active order in the part @return |
GetAsRequiredQuantity | Gets the as-required quantity on this component. |
GetAttributeTitlesByType | Gets all the attribute titles of a specific type. |
GetBooleanUserAttribute | Gets a boolean attribute by Title and array Index. |
GetCheckedoutStatusOfObjects | Returns the checkedout status (checkedout/non checkedout) of all the objects open in NX. |
GetComponentOrders | Returns all :py:class:`NXOpen.Assemblies.ComponentOrder`s available in the part |
GetComponentQuantityType | Gets the quantity type of the components. |
GetComputationalTimeUserAttribute | Gets a time attribute by Title and array Index. |
GetIntegerAttribute | Gets an integer attribute by title. |
GetIntegerQuantity | Gets the value of the integer quantity of component. |
GetIntegerUserAttribute | Gets an integer attribute by Title and array Index. |
GetNextUserAttribute | Gets the next attribute encountered on the object, if any, that satisfies the given iterator. |
GetNonGeometricState | Gets the component state as Geometric or Non-Geometric. |
GetRealAttribute | Gets a real attribute by title. |
GetRealQuantity | Gets the value of real quantity and corresponding units on this component. |
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. |
GetStringAttribute | Gets a string attribute value by title. |
GetStringUserAttribute | Gets a string attribute by Title and array Index. |
GetSuppressedState | Gets the suppression state of the component in its controlling arrangement @return The suppressed state |
GetSuppressionExpression | Gets the expression controlling the suppression of the component in its controlling arrangement @return The suppression expression. |
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, that satisfy the given iterator. |
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, if any, that satisfy the given iterator. |
GetUserAttributesAsStrings | Gets all the attributes that have been set on the given object. |
HasUserAttribute | Determines if an attribute exists on the object, that satisfies the given iterator @return |
MapComponentFromParent | Maps a component in a parent assembly onto a corresponding component in this assembly. |
MapComponentsFromSubassembly | Maps a component in a subassembly onto the corresponding components in this parent assembly. |
MoveComponent | Moves a component by specifying a translation and rotation. |
MoveToPendingComponent | Move a NXOpen.Assemblies.Component in this assembly to a pending list. |
OpenComponents | Given an array of components, open the components using the open_option. |
Prints a representation of this object to the system log file. | |
ReleaseSuppression | Release control of the suppression state of an array of components. |
RemoveComponent | Removes a component from this assemebly. |
ReorderChildrenOfParent | Assigns a new order to immediate children NXOpen.Assemblies.Component`s of parent :py:class:`NXOpen.Assemblies.Component . |
ReorderComponents | Reorders the array of NXOpen.Assemblies.Component`s before or after the target :py:class:`NXOpen.Assemblies.Component . |
ReplaceReferenceSet | Replaces the reference set used by a component. |
ReplaceReferenceSetInOwners | Sets the reference set used to represent each component in an array. |
RestructureComponents | Given an array of components and a specified parent this function will transfer the given components to the parent. |
SetAsRequiredQuantity | Sets the as-required quantity on this component. |
SetAttribute | Creates or modifies an integer attribute. |
SetBooleanUserAttribute | Creates or modifies a boolean attribute with the option to update or not. |
SetDefault | Set the default NXOpen.Assemblies.Arrangement for the given NXOpen.Assemblies.ComponentAssembly . |
SetEmptyRefset | Convenience method for setting the reference set used to represent a component to be empty |
SetEntirePartRefset | Convenience method for setting the reference set used to represent a component to be the entire part. |
SetIntegerQuantity | Sets the integer quantity on this component. |
SetName | Sets the custom name of the object. |
SetNonGeometricState | Sets the component state to Geometric or Non-Geometric. |
SetRealQuantity | Sets the real quantity and corresponding units on this component. |
SetReferenceAttribute | Creates or modifies a string attribute which uses a reference string. |
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. |
SubstituteComponent | Substitutes an old component with a new component. |
SuppressComponents | Suppresses an array of components @return list of errors encountered during the suppress |
UnsuppressComponents | Unsuppresses an array of components in this ComponentAssembly @return list of errors encountered during the unsuppress |
Enumerations¶
ComponentAssemblyCheckinCheckoutOption Enumeration | Check in and Check out options for components |
ComponentAssemblyCloseModified Enumeration | Indicates how close component should handle component parts when they are modified |
ComponentAssemblyOpenComponentStatus Enumeration | Open Component Status |
ComponentAssemblyOpenOption Enumeration | Open options for open_components |
ComponentAssemblyOrderTargetLocation Enumeration | Option controls whether reordered NXOpen.Assemblies.Component`s are placed before or after the target :py:class:`NXOpen.Assemblies.Component |
ComponentAssemblySubstitutionMode Enumeration | Defines how a component substitution operation is performed. |
ComponentAssemblySuppressedState Enumeration | Defines the component supression states. |
Property Detail¶
ActiveArrangement¶
-
ComponentAssembly.
ActiveArrangement
¶ Returns or sets the currently active
NXOpen.Assemblies.Arrangement
for this ComponentAssembly-------------------------------------
Getter Method
Signature
ActiveArrangement()
Returns: The NXOpen.Assemblies.Arrangement
that is currently activeReturn type: NXOpen.Assemblies.Arrangement
New in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------
Setter Method
Signature
ActiveArrangement(newArrangement)
Parameters: newArrangement ( NXOpen.Assemblies.Arrangement
) – The new activeNXOpen.Assemblies.Arrangement
. This Arrangement must be defined in this ComponentAssembly.New in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
IsOccurrence¶
-
ComponentAssembly.
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¶
-
ComponentAssembly.
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¶
-
ComponentAssembly.
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¶
-
ComponentAssembly.
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¶
-
ComponentAssembly.
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.
Positioner¶
-
ComponentAssembly.
Positioner
¶ Returns the component positioner for this assembly.
The positioner manages the component constraints.
-------------------------------------
Getter Method
Signature
Positioner()
Returns: Return type: NXOpen.Positioning.ComponentPositioner
New in version NX4.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
Prototype¶
-
ComponentAssembly.
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.
RootComponent¶
-
ComponentAssembly.
RootComponent
¶ 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 callingNXOpen.Assemblies.ComponentAssembly.AddComponent()
.Note that this will be None if there are no components in the tree. (I.e. if the part that owns this ComponentAssembly is a piece part.)
-------------------------------------
Getter Method
Signature
RootComponent()
Returns: The NXOpen.Assemblies.Component
at the root of this ComponentAssembly’s treeReturn type: NXOpen.Assemblies.Component
New in version NX3.0.0.
License requirements: None.
Arrangements¶
-
ComponentAssembly.
Arrangements
¶ The collection of :py:class:`NXOpen.Assemblies.Arrangement`s defined in the ComponentAssembly
Signature
Arrangements()
New in version NX3.0.0.
Returns: Return type: NXOpen.Assemblies.ArrangementCollection
Explosions¶
-
ComponentAssembly.
Explosions
¶ The collection of :py:class:`NXOpen.Assemblies.Explosion`s defined in the ComponentAssembly
Signature
Explosions()
New in version NX3.0.0.
Returns: Return type: NXOpen.Assemblies.ExplosionCollection
ComponentPatterns¶
-
ComponentAssembly.
ComponentPatterns
¶ The collection of
NXOpen.Assemblies.ComponentPattern
defined in the ComponentAssemblySignature
ComponentPatterns()
New in version NX9.0.0.
Returns: Return type: NXOpen.Assemblies.ComponentPatternCollection
Subsets¶
-
ComponentAssembly.
Subsets
¶ The collection of :py:class:`NXOpen.Assemblies.Subset`s defined in the ComponentAssembly
Signature
Subsets()
New in version NX8.5.0.
Returns: Return type: NXOpen.Assemblies.SubsetCollection
ClearanceSets¶
-
ComponentAssembly.
ClearanceSets
¶ The collection of :py:class:`NXOpen.Assemblies.ClearanceSet`s defined in the ComponentAssembly
Signature
ClearanceSets()
New in version NX9.0.0.
Returns: Return type: NXOpen.Assemblies.ClearanceSetCollection
OrdersSet¶
-
ComponentAssembly.
OrdersSet
¶ The collection of :py:class:`NXOpen.Assemblies.Order`s defined in the ComponentAssembly
Signature
OrdersSet()
New in version NX9.0.0.
Returns: Return type: NXOpen.Assemblies.OrderCollection
Method Detail¶
AddComponent¶
-
ComponentAssembly.
AddComponent
¶ Overloaded method AddComponent
AddComponent(partToAdd, referenceSetName, componentName, basePoint, orientation, layer)
AddComponent(partToAdd, referenceSetName, componentName, basePoint, orientation, layer, uomAsNgc)
AddComponent(partToAdd, referenceSetName, componentName, basePoint, orientation, layer)
-------------------------------------
Creates a new
NXOpen.Assemblies.Component
in this assembly, based on an existing part file.Signature
AddComponent(partToAdd, referenceSetName, componentName, basePoint, orientation, layer)
Parameters: - partToAdd (str) – The part that defines the new component
- referenceSetName (str) – The name of the reference set used to represent the new component
- componentName (str) – The name of the new component
- basePoint (
NXOpen.Point3d
) – Location of the new component - orientation (
NXOpen.Matrix3x3
) – Orientation matrix for the new component, in column order. - layer (int) – 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.
Returns: a tuple
Return type: A tuple consisting of (component, loadStatus). component is a
NXOpen.Assemblies.Component
. The new Component loadStatus is aNXOpen.PartLoadStatus
. Result of loading the part_to_addNew in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------
Creates a new
NXOpen.Assemblies.Component
in this assembly, based on an existing part file.Signature
AddComponent(partToAdd, referenceSetName, componentName, basePoint, orientation, layer, uomAsNgc)
Parameters: - partToAdd (str) – The part that defines the new component
- referenceSetName (str) – The name of the reference set used to represent the new component
- componentName (str) – The name of the new component
- basePoint (
NXOpen.Point3d
) – Location of the new component - orientation (
NXOpen.Matrix3x3
) – Orientation matrix for the new component, in column order. - layer (int) – 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 (bool) – Whether to set to non-geometric if with unit-of-measure
Returns: a tuple
Return type: A tuple consisting of (component, loadStatus). component is a
NXOpen.Assemblies.Component
. The new Component loadStatus is aNXOpen.PartLoadStatus
. Result of loading the part_to_addNew in version NX6.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------
Creates a new
NXOpen.Assemblies.Component
in this assembly, based on an existing part file.Signature
AddComponent(partToAdd, referenceSetName, componentName, basePoint, orientation, layer)
Parameters: - partToAdd (
NXOpen.BasePart
) – The part that defines the new component - referenceSetName (str) – The name of the reference set used to represent the new component
- componentName (str) – The name of the new component
- basePoint (
NXOpen.Point3d
) – Location of the new component - orientation (
NXOpen.Matrix3x3
) – Orientation matrix for the new component, in column order. - layer (int) – 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.
Returns: a tuple
Return type: A tuple consisting of (component, loadStatus). component is a
NXOpen.Assemblies.Component
. The new Component loadStatus is aNXOpen.PartLoadStatus
. Result of loading the part_to_addNew in version NX4.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------
AddMasterPartComponent¶
-
ComponentAssembly.
AddMasterPartComponent
¶ Overloaded method AddMasterPartComponent
AddMasterPartComponent(partToAdd, referenceSetName, componentName, basePoint, orientation, layer)
AddMasterPartComponent(partToAdd, referenceSetName, componentName, basePoint, orientation, layer)
-------------------------------------
Creates a new
NXOpen.Assemblies.Component
in this assembly as master part.Signature
AddMasterPartComponent(partToAdd, referenceSetName, componentName, basePoint, orientation, layer)
Parameters: - partToAdd (str) – The part that defines the new component
- referenceSetName (str) – The name of the reference set used to represent the new component
- componentName (str) – The name of the new component
- basePoint (
NXOpen.Point3d
) – Location of the new component - orientation (
NXOpen.Matrix3x3
) – Orientation matrix for the new component, in column order. - layer (int) – 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.
Returns: a tuple
Return type: A tuple consisting of (component, loadStatus). component is a
NXOpen.Assemblies.Component
. The new Component loadStatus is aNXOpen.PartLoadStatus
. Result of loading the part_to_addNew in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------
Creates a new
NXOpen.Assemblies.Component
in this assembly as master part.Signature
AddMasterPartComponent(partToAdd, referenceSetName, componentName, basePoint, orientation, layer)
Parameters: - partToAdd (
NXOpen.Part
) – The part that defines the new component - referenceSetName (str) – The name of the reference set used to represent the new component
- componentName (str) – The name of the new component
- basePoint (
NXOpen.Point3d
) – Location of the new component - orientation (
NXOpen.Matrix3x3
) – Orientation matrix for the new component, in column order. - layer (int) – 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.
Returns: a tuple
Return type: A tuple consisting of (component, loadStatus). component is a
NXOpen.Assemblies.Component
. The new Component loadStatus is aNXOpen.PartLoadStatus
. Result of loading the part_to_addNew in version NX4.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------
AddPendingComponent¶
-
ComponentAssembly.
AddPendingComponent
¶ Add a pending
NXOpen.Assemblies.Component
in this assembly.Signature
AddPendingComponent(partToAdd, pendingComponent, referenceSetName, componentName, basePoint, orientation, layer, uomAsNgc)
Parameters: - partToAdd (str) – The part that defines the new component
- pendingComponent (
NXOpen.NXObject
) – component to add - referenceSetName (str) – The name of the reference set used to represent the new component
- componentName (str) – The name of the new component
- basePoint (
NXOpen.Point3d
) – Location of the new component - orientation (
NXOpen.Matrix3x3
) – Orientation matrix for the new component, in column order. - layer (int) – 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 (bool) – Whether to set to non-geometric if with unit-of-measure
Returns: Result of loading the
part_to_add :rtype:
NXOpen.PartLoadStatus
New in version NX8.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
ChangeByName¶
-
ComponentAssembly.
ChangeByName
¶ Changes the current
NXOpen.Assemblies.Arrangement
of the givenNXOpen.Assemblies.Component`s to the :py:class:`NXOpen.Assemblies.Arrangement
with the given name.Signature
ChangeByName(name, partOccs)
Parameters: - name (str) – The name of arrangement to change to
- partOccs (list of
NXOpen.Assemblies.Component
) – The :py:class:`NXOpen.Assemblies.Component`s to be modified
New in version NX7.5.2.
License requirements: assemblies (“ASSEMBLIES MODULE”)
CheckinComponents¶
-
ComponentAssembly.
CheckinComponents
¶ Checks in array of components as per the option
NXOpen.Assemblies.ComponentAssemblyCheckinCheckoutOption
.Signature
CheckinComponents(partOccs, checkinInputOption)
Parameters: - partOccs (list of
NXOpen.Assemblies.Component
) – Array of components to check in - checkinInputOption (
NXOpen.Assemblies.ComponentAssemblyCheckinCheckoutOption
) – Option that controls what to check in
Returns: Any errors that occurred during the check in
Return type: New in version NX8.5.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
- partOccs (list of
CheckinWorkset¶
-
ComponentAssembly.
CheckinWorkset
¶ Checks in workset.
Signature
CheckinWorkset()
Returns: Any errors that occurred during checking in of workset Return type: NXOpen.ErrorList
New in version NX8.5.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
CheckoutAllModifiedObjects¶
-
ComponentAssembly.
CheckoutAllModifiedObjects
¶ Checks out all modified objects in the current session.
checkedOutObjects collection will be type of
NXOpen.BasePart
orNXOpen.PDM.DesignElementRevision
Signature
CheckoutAllModifiedObjects()
Returns: a tuple Return type: A tuple consisting of (errorList, checkedOutObjects). errorList is a NXOpen.ErrorList
. Any errors that occurred during checking out of objects checkedOutObjects is a list ofNXOpen.NXObject
. Array of NXObjects checked outNew in version NX8.5.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
CheckoutComponents¶
-
ComponentAssembly.
CheckoutComponents
¶ Checks out array of components as per the option
NXOpen.Assemblies.ComponentAssemblyCheckinCheckoutOption
.Signature
CheckoutComponents(partOccs, checkoutInputOption)
Parameters: - partOccs (list of
NXOpen.Assemblies.Component
) – Array of components to check out - checkoutInputOption (
NXOpen.Assemblies.ComponentAssemblyCheckinCheckoutOption
) – Option that controls what to check out
Returns: Any errors that occurred during the check out
Return type: New in version NX8.5.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
- partOccs (list of
CheckoutWorkset¶
-
ComponentAssembly.
CheckoutWorkset
¶ Checks out workset.
Signature
CheckoutWorkset()
Returns: Any errors that occurred during checking out of workset Return type: NXOpen.ErrorList
New in version NX8.5.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
CloseComponents¶
-
ComponentAssembly.
CloseComponents
¶ 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.
Signature
CloseComponents(componentsToClose, wholeTree, closeModified)
Parameters: - componentsToClose (list of
NXOpen.Assemblies.Component
) – Array of components to close - wholeTree (
NXOpen.BasePartCloseWholeTree
) – If true, unloads all components of the part. If false, unloads only the top-level part - closeModified (
NXOpen.Assemblies.ComponentAssemblyCloseModified
) – Behavior of close if component parts are modified.
Returns: Close status for the parts
Return type: New in version NX6.0.1.
License requirements: None.
- componentsToClose (list of
ConvertRememberedMcs¶
-
ComponentAssembly.
ConvertRememberedMcs
¶ Converts all remembered mating constraints in the part of this assembly to remembered assembly constraints
Signature
ConvertRememberedMcs()
New in version NX7.5.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
CopyComponents¶
-
ComponentAssembly.
CopyComponents
¶ 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.
Signature
CopyComponents(components)
Parameters: components (list of NXOpen.Assemblies.Component
) – Components to be copied.Returns: The newly created copies. Return type: list of NXOpen.Assemblies.Component
New in version NX6.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
CreateComponentPatternBuilder¶
-
ComponentAssembly.
CreateComponentPatternBuilder
¶ Creates a
NXOpen.Assemblies.ComponentPatternBuilder
object This can be used to create or edit a component pattern.Signature
CreateComponentPatternBuilder(compPattern)
Parameters: compPattern ( NXOpen.Assemblies.ComponentPattern
) – The pattern definition object will be used in editReturns: Return type: NXOpen.Assemblies.ComponentPatternBuilder
New in version NX9.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
CreateConstraintGroupBuilder¶
-
ComponentAssembly.
CreateConstraintGroupBuilder
¶ 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 None the displayed constraints used are in the same part as the member constraints.
Signature
CreateConstraintGroupBuilder(group, contextComponent)
Parameters: - group (
NXOpen.Positioning.ComponentConstraintGroup
) – Group to be edited, if None then a new group is created - contextComponent (
NXOpen.Assemblies.Component
) – Context component, can be None
Returns: Return type: New in version NX8.0.1.
License requirements: assemblies (“ASSEMBLIES MODULE”)
- group (
CreateMatingConverter¶
-
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.
Signature
CreateMatingConverter()
Returns: The new Mating Converter Return type: NXOpen.Positioning.MatingConverter
New in version NX5.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
DeleteMatingConditions¶
-
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.
Signature
DeleteMatingConditions()
New in version NX7.5.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
FindObject¶
-
ComponentAssembly.
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.
GetActiveOrder¶
-
ComponentAssembly.
GetActiveOrder
¶ Returns the active order in the part
Signature
GetActiveOrder()
Returns: Return type: NXOpen.Assemblies.Order
New in version NX10.0.3.
License requirements: assemblies (“ASSEMBLIES MODULE”)
GetAsRequiredQuantity¶
-
ComponentAssembly.
GetAsRequiredQuantity
¶ Gets the as-required quantity on this component.
Signature
GetAsRequiredQuantity(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to edit. Must be directly owned by this assembly.Returns: As-Required string “A/R” Return type: str New in version NX6.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
GetCheckedoutStatusOfObjects¶
-
ComponentAssembly.
GetCheckedoutStatusOfObjects
¶ Returns the checkedout status (checkedout/non checkedout) of all the objects open in NX.
Signature
GetCheckedoutStatusOfObjects()
Returns: a tuple Return type: A tuple consisting of (checkedOutObjects, uncheckedOutObjects). checkedOutObjects is a list of NXOpen.NXObject
. Array of NXObjects which are open in session and checked out uncheckedOutObjects is a list ofNXOpen.NXObject
. Array of NXObjects which are open in session but not checkoutNew in version NX8.5.0.
License requirements: None.
GetComponentOrders¶
-
ComponentAssembly.
GetComponentOrders
¶ Returns all :py:class:`NXOpen.Assemblies.ComponentOrder`s available in the part
Signature
GetComponentOrders()
Returns: Returns array of :py:class:`NXOpen.Assemblies.ComponentOrder`s in part Return type: list of NXOpen.Assemblies.ComponentOrder
New in version NX9.0.0.
License requirements: None.
GetComponentQuantityType¶
-
ComponentAssembly.
GetComponentQuantityType
¶ Gets the quantity type of the components.
Returns
NXOpen.Assemblies.ComponentQuantity
.Signature
GetComponentQuantityType(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to query. Must be directly owned by this assembly.Returns: Quantity type an enumeration value Return type: NXOpen.Assemblies.ComponentQuantity
New in version NX6.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
GetIntegerQuantity¶
-
ComponentAssembly.
GetIntegerQuantity
¶ Gets the value of the integer quantity of component.
Signature
GetIntegerQuantity(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to query. Must be directly owned by this assembly.Returns: Integer quantity value Return type: int New in version NX6.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
GetNonGeometricState¶
-
ComponentAssembly.
GetNonGeometricState
¶ Gets the component state as Geometric or Non-Geometric.
Signature
GetNonGeometricState(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to query. Must be directly owned by this assembly.Returns: True if the component is non-geometric, false otherwise Return type: bool New in version NX6.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
GetRealQuantity¶
-
ComponentAssembly.
GetRealQuantity
¶ Gets the value of real quantity and corresponding units on this component.
Signature
GetRealQuantity(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to query. Must be directly owned by this assembly.Returns: a tuple Return type: A tuple consisting of (realQuantity, units). realQuantity is a float. Real quantity value units is a str. Units New in version NX6.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
GetSuppressedState¶
-
ComponentAssembly.
GetSuppressedState
¶ Overloaded method GetSuppressedState
GetSuppressedState(component)
GetSuppressedState(component, arrangement)
-------------------------------------
Gets the suppression state of the component in its controlling arrangement
Signature
GetSuppressedState(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to query.Returns: a tuple Return type: A tuple consisting of (suppressedState, controlled). suppressedState is a NXOpen.Assemblies.ComponentAssemblySuppressedState
. The suppressed state controlled is a bool. Is the suppression state controlled at the level of arrangement?New in version NX6.0.4.
License requirements: None.
-------------------------------------
Gets the suppression state of the component in the given arrangement.
Signature
GetSuppressedState(component, arrangement)
Parameters: - component (
NXOpen.Assemblies.Component
) – The component to query. - arrangement (
NXOpen.Assemblies.Arrangement
) – Arrangements in which components should be suppressed.
Returns: a tuple
Return type: A tuple consisting of (suppressedState, controlled). suppressedState is a
NXOpen.Assemblies.ComponentAssemblySuppressedState
. The suppressed state controlled is a bool. Is the suppression state controlled at the level of arrangement?New in version NX6.0.4.
License requirements: None.
-------------------------------------
GetSuppressionExpression¶
-
ComponentAssembly.
GetSuppressionExpression
¶ Overloaded method GetSuppressionExpression
GetSuppressionExpression(component)
GetSuppressionExpression(component, arrangement)
-------------------------------------
Gets the expression controlling the suppression of the component in its controlling arrangement
Signature
GetSuppressionExpression(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to query.Returns: The suppression expression. Return type: NXOpen.Expression
New in version NX6.0.4.
License requirements: None.
-------------------------------------
Gets the expression controlling the suppression of the component in the given arrangment
Signature
GetSuppressionExpression(component, arrangement)
Parameters: - component (
NXOpen.Assemblies.Component
) – The component to query. - arrangement (
NXOpen.Assemblies.Arrangement
) – The arrangement in which to query the suppressed state
Returns: The suppression expression.
Return type: New in version NX6.0.4.
License requirements: None.
-------------------------------------
MapComponentFromParent¶
-
ComponentAssembly.
MapComponentFromParent
¶ Maps a component in a parent assembly onto a corresponding component in this assembly.
For example, given an Axle assembly: <code>
Axle / / Left Right Wheel Wheel
</code> and a Car assembly containing two Axle components: <code>
Car _______ |_______ / / Front Rear Axle Axle / / / / Front Left Front Right Rear Left Rear Right Wheel Wheel Wheel Wheel
</code>
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.
Signature
MapComponentFromParent(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to map. This should be defined in the tree of a parent assembly which contains this assembly.Returns: The mapped component. This will be defined in the component tree of this assembly parameter.
Return type: NXOpen.Assemblies.Component
New in version NX3.0.0.
License requirements: None.
MapComponentsFromSubassembly¶
-
ComponentAssembly.
MapComponentsFromSubassembly
¶ Maps a component in a subassembly onto the corresponding components in this parent assembly.
For example, given an Axle assembly: <code>
Axle / / Left Right Wheel Wheel
</code> and a Car assembly containing two Axle components: <code>
Car _______ |_______ / / Front Rear Axle Axle / / / / Front Left Front Right Rear Left Rear Right Wheel Wheel Wheel Wheel
</code>
then calling Car.MapComponentsFromSubassembly on Left Wheel will return Front Left Wheel and Rear Left Wheel. See also
NXOpen.Assemblies.ComponentAssembly.MapComponentFromParent()
.Signature
MapComponentsFromSubassembly(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to map. This must be defined in a subassembly of this assembly.Returns: The mapped components. Return type: list of NXOpen.Assemblies.Component
New in version NX3.0.0.
License requirements: None.
MoveComponent¶
-
ComponentAssembly.
MoveComponent
¶ 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.
Signature
MoveComponent(component, translation, rotation)
Parameters: - component (
NXOpen.Assemblies.Component
) – The component to edit. Must be directly owned by this assembly - translation (
NXOpen.Vector3d
) – The translation delta - rotation (
NXOpen.Matrix3x3
) – The rotation delta, in column order.
New in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
- component (
MoveToPendingComponent¶
-
ComponentAssembly.
MoveToPendingComponent
¶ 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.Signature
MoveToPendingComponent(component)
Parameters: component ( NXOpen.NXObject
) – component to move to pending listNew in version NX10.0.2.
License requirements: assemblies (“ASSEMBLIES MODULE”)
OpenComponents¶
-
ComponentAssembly.
OpenComponents
¶ Given an array of components, open the components using the open_option.
Signature
OpenComponents(openOption, componentsToOpen)
Parameters: - openOption (
NXOpen.Assemblies.ComponentAssemblyOpenOption
) – The option that controls the open operation - componentsToOpen (list of
NXOpen.Assemblies.Component
) – Array of components to open
Returns: a tuple
Return type: A tuple consisting of (loadStatus, openStatus). loadStatus is a
NXOpen.PartLoadStatus
. If any components could not be loaded, this object contains the error information. openStatus is a list ofNXOpen.Assemblies.ComponentAssemblyOpenComponentStatus
. Shows the status of the objects in an indexed array according to if they could be openedNew in version NX6.0.1.
License requirements: None.
- openOption (
Print¶
-
ComponentAssembly.
Print
¶ Prints a representation of this object to the system log file.
Signature
Print()
New in version NX3.0.0.
License requirements: None.
ReleaseSuppression¶
-
ComponentAssembly.
ReleaseSuppression
¶ Overloaded method ReleaseSuppression
ReleaseSuppression(components, arrangements)
ReleaseSuppression(components)
-------------------------------------
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.)
Signature
ReleaseSuppression(components, arrangements)
Parameters: - components (list of
NXOpen.Assemblies.Component
) – :py:class:`NXOpen.Assemblies.Component`s to be released - arrangements (list of
NXOpen.Assemblies.Arrangement
) – Arrangements in which components should be released. These arrangements must be defined in this ComponentAssembly
Returns: list of errors encountered during the release
Return type: New in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------
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.
Signature
ReleaseSuppression(components)
Parameters: components (list of NXOpen.Assemblies.Component
) – :py:class:`NXOpen.Assemblies.Component`s to be releasedReturns: list of errors encountered during the release Return type: NXOpen.ErrorList
New in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------
RemoveComponent¶
-
ComponentAssembly.
RemoveComponent
¶ Removes a component from this assemebly.
Signature
RemoveComponent(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to remove. Must be directly owned by this assembly.New in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
ReorderChildrenOfParent¶
-
ComponentAssembly.
ReorderChildrenOfParent
¶ Assigns a new order to immediate children
NXOpen.Assemblies.Component`s of parent :py:class:`NXOpen.Assemblies.Component
.Signature
ReorderChildrenOfParent(order, parentComponent, componentsToReorder)
Parameters: - order (
NXOpen.Assemblies.ComponentOrder
) –NXOpen.Assemblies.ComponentOrder
in which children are reordered - parentComponent (
NXOpen.Assemblies.Component
) – Parent component whose children are reordered - componentsToReorder (list of
NXOpen.Assemblies.Component
) – Array of children components in new order
New in version NX9.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
- order (
ReorderComponents¶
-
ComponentAssembly.
ReorderComponents
¶ Reorders the array of
NXOpen.Assemblies.Component`s before or after the target :py:class:`NXOpen.Assemblies.Component
.NXOpen.Assemblies.Component`s to reorder and the target :py:class:`NXOpen.Assemblies.Component
should be children of the same immediate parent.Signature
ReorderComponents(order, componentsToReorder, targetComponent, beforeOrAfter)
Parameters: - order (
NXOpen.Assemblies.ComponentOrder
) –NXOpen.Assemblies.ComponentOrder
in which components are reordered - componentsToReorder (list of
NXOpen.Assemblies.Component
) – Array of components to be reordered - targetComponent (
NXOpen.Assemblies.Component
) – Components are moved before or after this component - beforeOrAfter (
NXOpen.Assemblies.ComponentAssemblyOrderTargetLocation
) – Whether to move components before or after the target component
New in version NX9.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
- order (
ReplaceReferenceSet¶
-
ComponentAssembly.
ReplaceReferenceSet
¶ 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()
orNXOpen.Assemblies.Component.EntirePartRefsetName()
.Signature
ReplaceReferenceSet(component, newReferenceSet)
Parameters: - component (
NXOpen.Assemblies.Component
) – The component to edit. Must be directly owned by this assembly. - newReferenceSet (str) – The name of the new reference set
New in version NX3.0.0.
License requirements: None.
- component (
ReplaceReferenceSetInOwners¶
-
ComponentAssembly.
ReplaceReferenceSetInOwners
¶ Sets the reference set used to represent each component in an array.
This is the equivalent of calling: <code> NXOpen.Assemblies.Component.DirectOwner:py:meth:NXOpen.Assemblies.Component.DirectOwner </code> <code> NXOpen.Assemblies.ComponentAssembly.ReplaceReferenceSet:py:meth:NXOpen.Assemblies.ComponentAssembly.ReplaceReferenceSet </code>
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()
orNXOpen.Assemblies.Component.EntirePartRefsetName()
.Signature
ReplaceReferenceSetInOwners(newReferenceSet, components)
Parameters: - newReferenceSet (str) – The name of the new reference set
- components (list of
NXOpen.Assemblies.Component
) – Components to be edited. Each component will have its reference set updated in its owning assembly.
Returns: list of errors encountered during the edit
Return type: New in version NX3.0.0.
License requirements: None.
RestructureComponents¶
-
ComponentAssembly.
RestructureComponents
¶ 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
Signature
RestructureComponents(origComponents, newParentComponent, deleteFlag)
Parameters: - origComponents (list of
NXOpen.Assemblies.Component
) – Array of components to be restructured - newParentComponent (
NXOpen.Assemblies.Component
) – Destination for restructure - deleteFlag (bool) – Flag to delete original components
Returns: a tuple
Return type: A tuple consisting of (newComponents, errorList). newComponents is a list of
NXOpen.Assemblies.Component
. Restructured components errorList is aNXOpen.ErrorList
. Any errors that occurred during the restructureNew in version NX6.0.1.
License requirements: assemblies (“ASSEMBLIES MODULE”)
- origComponents (list of
SetAsRequiredQuantity¶
-
ComponentAssembly.
SetAsRequiredQuantity
¶ Sets the as-required quantity on this component.
Signature
SetAsRequiredQuantity(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to edit. Must be directly owned by this assembly.New in version NX6.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
SetDefault¶
-
ComponentAssembly.
SetDefault
¶ Set the default
NXOpen.Assemblies.Arrangement
for the givenNXOpen.Assemblies.ComponentAssembly
.Signature
SetDefault(arrangement)
Parameters: arrangement ( NXOpen.Assemblies.Arrangement
) – The new defaultNXOpen.Assemblies.Arrangement
.New in version NX7.5.2.
License requirements: assemblies (“ASSEMBLIES MODULE”)
SetEmptyRefset¶
-
ComponentAssembly.
SetEmptyRefset
¶ Convenience method for setting the reference set used to represent a component to be empty
Signature
SetEmptyRefset(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to edit. Must be directly owned by this assembly.New in version NX3.0.0.
License requirements: None.
SetEntirePartRefset¶
-
ComponentAssembly.
SetEntirePartRefset
¶ Convenience method for setting the reference set used to represent a component to be the entire part.
Signature
SetEntirePartRefset(component)
Parameters: component ( NXOpen.Assemblies.Component
) – The component to edit. Must be directly owned by this assembly.New in version NX3.0.0.
License requirements: None.
SetIntegerQuantity¶
-
ComponentAssembly.
SetIntegerQuantity
¶ Sets the integer quantity on this component.
Signature
SetIntegerQuantity(component, integerQuantity)
Parameters: - component (
NXOpen.Assemblies.Component
) – The component to edit. Must be directly owned by this assembly. - integerQuantity (int) – Integer quantity value
New in version NX6.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
- component (
SetName¶
-
ComponentAssembly.
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.
SetNonGeometricState¶
-
ComponentAssembly.
SetNonGeometricState
¶ Sets the component state to Geometric or Non-Geometric.
Component which are made non-geometric are undrawn from graphics area.
Signature
SetNonGeometricState(component, nonGeometricState)
Parameters: - component (
NXOpen.Assemblies.Component
) – The component to edit. Must be directly owned by this assembly. - nonGeometricState (bool) – True to make component non-geometric, false otherwise
New in version NX6.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
- component (
SetRealQuantity¶
-
ComponentAssembly.
SetRealQuantity
¶ Sets the real quantity and corresponding units on this component.
Signature
SetRealQuantity(component, realQuantity, quantityUnits)
Parameters: - component (
NXOpen.Assemblies.Component
) – The component to edit. Must be directly owned by this assembly. - realQuantity (float) – Real quantity value
- quantityUnits (str) – Units
New in version NX6.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
- component (
SubstituteComponent¶
-
ComponentAssembly.
SubstituteComponent
¶ 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.
Signature
SubstituteComponent(component, part, newName, referenceSet, layer, mode)
Parameters: - component (
NXOpen.Assemblies.Component
) – The old component to be substituted. - part (
NXOpen.BasePart
) – The new part - newName (str) – The name for the new component
- referenceSet (str) – The name of the reference set for the new component
- layer (int) – 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 (
NXOpen.Assemblies.ComponentAssemblySubstitutionMode
) – Defines the substitution mode
Returns: The new Component that replaces the old one.
Return type: New in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
- component (
SuppressComponents¶
-
ComponentAssembly.
SuppressComponents
¶ Overloaded method SuppressComponents
SuppressComponents(components, arrangements)
SuppressComponents(components)
SuppressComponents(components, arrangements, expression)
-------------------------------------
Suppresses an array of components
Signature
SuppressComponents(components, arrangements)
Parameters: - components (list of
NXOpen.Assemblies.Component
) – :py:class:`NXOpen.Assemblies.Component`s to be suppressed - arrangements (list of
NXOpen.Assemblies.Arrangement
) – Arrangements in which components should be suppressed. These arrangements must be defined in this ComponentAssembly
Returns: list of errors encountered during the suppress
Return type: New in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------
Suppresses an array of components in all
NXOpen.Assemblies.Arrangement
s in this ComponentAssemblySignature
SuppressComponents(components)
Parameters: components (list of NXOpen.Assemblies.Component
) – :py:class:`NXOpen.Assemblies.Component`s to be suppressedReturns: list of errors encountered during the suppress Return type: NXOpen.ErrorList
New in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------
Suppresses an array of components in all
NXOpen.Assemblies.Arrangement
s in this ComponentAssemblySignature
SuppressComponents(components, arrangements, expression)
Parameters: - components (list of
NXOpen.Assemblies.Component
) – :py:class:`NXOpen.Assemblies.Component`s to be suppressed - arrangements (list of
NXOpen.Assemblies.Arrangement
) – Arrangements in which components should be unsuppressed - expression (str) – Suppress components if expression evalutes zero else unsuppress components
Returns: list of errors encountered during the suppress
Return type: New in version NX5.0.1.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------
UnsuppressComponents¶
-
ComponentAssembly.
UnsuppressComponents
¶ Overloaded method UnsuppressComponents
UnsuppressComponents(components, arrangements)
UnsuppressComponents(components)
-------------------------------------
Unsuppresses an array of components in this ComponentAssembly
Signature
UnsuppressComponents(components, arrangements)
Parameters: - components (list of
NXOpen.Assemblies.Component
) – :py:class:`NXOpen.Assemblies.Component`s to be unsuppressed - arrangements (list of
NXOpen.Assemblies.Arrangement
) – Arrangements in which components should be unsuppressed. These arrangements must be defined in this ComponentAssembly
Returns: list of errors encountered during the unsuppress
Return type: New in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------
Unsuppresses an array of components in all
NXOpen.Assemblies.Arrangement
s in this ComponentAssemblySignature
UnsuppressComponents(components)
Parameters: components (list of NXOpen.Assemblies.Component
) – :py:class:`NXOpen.Assemblies.Component`s to be unsuppressedReturns: list of errors encountered during the unsuppress Return type: NXOpen.ErrorList
New in version NX3.0.0.
License requirements: assemblies (“ASSEMBLIES MODULE”)
-------------------------------------