Updating part file parameters with Python

[20854706]

Dear forum users,

Is there a way to use Python to update certain parameters within a part file in Inventor? I've searched the forum, and the closest I could come to a solution is a post about adding missing parameters, which is not what I want to do. 

Any help would be extremely helpful.

Kind regards 

[JelteDeJong]

this rule will update a parameter

import win32com.client
from win32com.client import gencache, Dispatch, constants, DispatchEx

ThisApplication = win32com.client.Dispatch('Inventor.Application')
ThisApplication.Visible = True
CastTo = gencache.EnsureModule('{D98A091D-3A0F-4C3E-B36E-61F62068D488}', 0, 1, 0)
ThisApplication = CastTo.Application(ThisApplication)

oDoc = ThisApplication.ActiveDocument
oDoc = CastTo.PartDocument(oDoc)

params = oDoc.ComponentDefinition.Parameters

parameter1 = params.Item("MyParameterName")
print("number of Parameters: ",parameter1.Value)

parameter1.Value = 2.0
print("number of Parameters: ",parameter1.Value)

[20854706]

@JelteDeJong Thank you for your reply. It works! Although, while the parameter updates, the part does not. Is there a way to force the update rather than manually clicking on the "Update" button on the Manage tab? 

My goal is to update the whole part with the new values, then export it as a .stl file after all the updates have happened. 

Is it possible to make this all automatic? 

[JelteDeJong]

you can try:

oDoc.Update()
oDoc.Update2()

[20854706]

@JelteDeJong Thank you again for the quick reply. The first line worked!
The last thing that I'm struggling with is exporting the file after I made the updates to the parameters. Is there a possible way of doing this?

[JelteDeJong]

what do you mean by exporting? do you want to create dxf's or pdf's?

[20854706]

@JelteDeJong, I want to export the part as a .stl file type.

[JelteDeJong · Accepted solution]

try this:

newFileName = "d:\\temp\\test.stl"
oDoc.SaveAs(newFileName, True)

[20854706]

Thank you very much! You've been a great help!