IvAdoptedPart represents an Inventor part occurrence in Intent. Every new instance of this design creates a new occurrence in the parent Inventor assembly file. Typically you do not use this design directly. Instead, when you adopt an Inventor part file, the Adopt Wizard creates a new design, which inherits from IvAdoptedPart. Factory and member files: IvAdoptedPart automatically makes a copy of the factory file, and reparameterizes the copy as necessary. These copies are called member files. Intent automatically examines the parameter values and creates appropriate member files when necessary. It reuses the same member file whenever it sees the same set of parameter values. Intent creates a new member file when it sees a set of parameter values that has not been encountered before. Member files are typically stored in the "Member Files" folder in your project folder.
IvAdoptedpartModifier
IvCommonOccurrenceMixin
IvComponentMixin
BaseInventorMixin
Basepart
| Name | Type | Description |
|---|---|---|
| factoryFileName | string | Name of the adopted Inventor part. |
| iProperties | list | Nested list with user defined attributes (iproperties). |
| factoryFileDirectory | string | Directory path to the adopted Inventor part. |
| grounded? | boolean | Specifies whether or not the Inventor occurrence is grounded. |
| inventorFileName | string | Inventor file name. |
| reportModelingErrors? | boolean | Specifies whether Inventor errors during modeling are reported as Intent errors. |
| materialName | string | Name of the material ? must pre-exist as an Inventor material. Material is considered like a parameter in terms of generating member files. |
| color | string | Color (render style) of the Inventor occurrence. |
| DisableMemberPartEditing? | boolean | Controls whether member files can be edited with ordinary Inventor commands. The default is True (files cannot be edited with ordinary commands). |
| suppressedFeatures | list | List of features to actively suppress. Features not explicitly listed in either suppressedFeatures or unsuppressedFeatures are simply left alone. The Adopt command does not do anything with these parameters. |
| unsuppressedFeatures | list | List of features to actively unsuppress. Features not explicitly listed in either suppressedFeatures or unsuppressedFeatures are simply left alone. The Adopt command does not do anything with these parameters. |
| isRef? | boolean | If supplied as True , specifies that no occurrence should be created. |
| NameFeatureGeometry? | boolean | This is a Lookup parameter. Is set to True , then all part level feature geometry (edges, vertices, and faces) will be named. Default is False . To re-enable Part Feature Naming, please set the Rule NameFeatureGeometry? As Boolean = True on the appropriate level of the Intent assembly (for example, on the Root) |
| overrideOpacity | number | Number from 0 to 1 (0 is fully transparent), or NoValue (which is a default meaning 'no override') |
| UseFactoryPartNumber? | boolean | (Default is False ). If set to True , the Inventor's Part Number iProperty in the member file is the same is in factory file. |
| IgnoreInventorVersion | boolean | (Default is
False
). If set to
True
, the Inventor major version does not contribute to the part file signature. Warning: User should be aware of consequences of setting this Parameter to True . For example, in some cases there may be an attempt to open the file with the older version of Inventor. |
| IgnoreFactoryFileName | boolean | (Default is
False
). If set to
True
, the factory file name does not contribute to the part file signature. Warning: User should be aware of consequences of setting this Parameter to True . |
| IgnoreUnits | boolean | (Default is
False
). If set to
True
, the Intent Projects units do not contribute to the part file signature. Warning: User should be aware of consequences of setting this Parameter to True . For example, there will not be difference in the file name prepared for mm and in units |
| IgnoreModificationTime | boolean | (Default is
False
). If set to
True
, the factory file modification time does not contribute to the part file signature. Warning: User should be aware of consequences of setting this Parameter to True . For example, the previously created member files will not be updated after changes in the factory files. The user is expected to clean the "Member Files" folder manually. |
| Name | Type | Description |
|---|---|---|
| cacheFileDirectory | string | Absolute path to member file directory ("cache"). |
| cacheFileName | string | File name of the member file which was instantiated as an occurrence. |
| memberPathname | string | Specifies the file name (full absolute path) to be used when a new member file is created -- and ONLY then. Contrast this with the 'cacheFileName' rule . You can override this rule in your designs to use a different file-naming scheme, instead of Intent's default GUID-based scheme. Your naming scheme must provide a unique file name for each unique set of parameters (and material, etc.) See the implementation for full details. |
| PartNumber | string | Returns the Part Number as read from the document. The part number is set only on signature generation time of the document. It is not possible to have 2 member files that differ only by their Part Numbers . The existing assembly documents will not have their part numbers updated. |
customProperty( propName As String ) As Any
Retrieves value of user defined property by property name. inventorParamValue( paramName As String, _
Optional units As String = "databaseExceptLengthAndAngle" ) As Number
Retrieves value of Inventor parameter in member file; typically used for Inventor parameters that were NOT adopted, but which are driven by the adopted parameters. The possible values for the units parameter are: "databaseExceptLengthAndAngle" - Default. Value returned in project units for length parameters, in degrees for angle parameters, and in Inventor database units for all other parameters. "database" - Value always returned in Inventor database units. Specific units - Value returned in specified units, which must be compatible with the parameter type. inventorParamValueAsString( paramName As String, _
Optional units As String = "InventorParamUnits" ) As String
Retrieves value of Inventor parameter in member file, as a
string
consisting of numeric value and units. The possible values for the units parameter are: "InventorParamUnits" - Default. String returned uses units associated with parameter in Inventor. "database" - String returned uses Inventor database units. Specific units - String returned uses specified units, which must be compatible with the parameter type. GetNewPartNumber( docHandle As String ) As String
Used to return the value of the
Part Number
. May be overridden in user code. docHandle represents the Part Document that was just created. The default implementation returns the value from the {"Part number", "PN"} sublist in the iProperty rule. If no value exists, the file name (without extension) contained in $path is returned.