Calling a specific part in an assembly through a macro
You can always get reference to desired parameter by its name using Item property of the Parameters collection.
Parameters.Item( Index As Variant ) As Parameter
| Index |
Input Variant value that specifies the object to return. This can be either a numeric value indicating the index of the item in the collection or it can be a string indicating the parameter name.
|
You should use the name you see in the Inventor parameters editor in UI, e.g. "d7".
It is good idea to give parameters more meaningful names.
Cheers,
Vladimir Ananyev
Developer Technical Services
Autodesk Developer Network
When you work in an assembly context access to parts parameters become slightly more complicated.
Assembly document has a collection of references to all its components. They can be parts or subassemblies.
Component is represented by ComponentOccurrence object in the Inventor API. If component is a part then property ComponentOccurrence.Definition returns PartComponentDefinition object that allows you to get references to all part parameters.
Private Sub Test_Occurrences()
Dim oAssyDoc As AssemblyDocument
Set oAssyDoc = ThisApplication.ActiveDocument
Dim oAssyDef As AssemblyComponentDefinition
Set oAssyDef = oAssyDoc.ComponentDefinition
'process all subassemblies
Dim oOcc As ComponentOccurrence
'access to component by its name (as it is shown in browser)
Set oOcc = oAssyDef.Occurrences.ItemByName("LD-049:1")
If oOcc.Definition.Type = kPartComponentDefinitionObject Then
'reference to Component Definition
Dim oDef As PartComponentDefinition
Set oDef = oOcc.Definition
'reference to part document
Dim oDoc As PartDocument
Set oDoc = oDef.Document
'reference to parameters
Dim oPars As Inventor.Parameters
Set oPars = oDef.Parameters
Dim oPar As Inventor.Parameter
Set oPar = oPars.Item("d7")
Debug.Print oPar.Expression
oPar.Expression = "50 mm"
'update & save changes
oDoc.Update
oDoc.Save
End If
End Sub
See also overview "Building an Assembly" in the Inventor API Help.
Cheers,
Vladimir Ananyev
Developer Technical Services
Autodesk Developer Network
Edit: I see you have some code now to work with (added while i was typing my reply) so therefore some of my reply is now irrelevant. I will however leave it in case any of It is of use...
Hi VS,
i am not at my computer at the moment but I will give you some code tomorrow that you can edit to get what you want.
if I understand you right then your immediate challenge is that you just need to find the property set / collection set, that the referenced file descriptor resides in, to then allocate the referenced file to your variable.
One of the biggest breakthroughs i had when staritng out was to understand that one easy way of finding a specific property set is to use the debug functions in the code window, to step one line at a time while you observe your Locals window. In there you can burrow down into the object variable, in this case your assembly document is the uppermost object, then just expand likey candidates within that object to see various types of collection sets or property sets to see what the appropriate category names are for you to transverse or choose specific items from within.
another handy tip, you may now this but if you find a function, property set or method that you wish to understand further is to type it into your code, then highlight the word then hit F1 to bring up the API supporting documentation. It's will then provide examples of the concept, that you can then work out to your own requirements.
i hope this helps.
best regards,
- Mark
(Kudo or Tag if helpful - in case it also helps others)
PDSU 2020 Windows 10, 64bit.
- Mark
(Kudo or Tag if helpful - in case it also helps others)
PDSU 2020 Windows 10, 64bit.