Autodesk Inventor iPart Best Practices

Autodesk Inventor iPart Help Tool Tip

Have you ever wondered if there is a right way to manage your iParts? Do you often suffer with iPart members not generating how you would expect them to? Or regenerating the members results in broken links within your designs? Are you happy with the way your iPart member folders are named? If you are wondering what the answer is to any of these questions then read on.

Controlling folder names and filenames

Setup your iPart following standard steps, which can be found here in the Inventor Help file.

Tip: Make sure you don’t use any special characters in the Member name or Filename columns within your iPart Table. It can create undesirable file naming problems, or errors appearing when switching between different iPart members.
Autodesk Inventor iPart Member Folder Name

Then rename the top browser node (highlighted above), type in the name of the folder you would like the iPart members to be saved to.
Autodesk Inventor iPart Member Folder Name Examples

Just remember the Top Browser Node (Green Rectangle), ISN’T the filename. This is just a workaround to control the name of the folder the iPart Members get published/generated/saved to.

Autodesk Inventor iPart Filename
The actual file name can be found in the iProperties dialog if you need it, shown above.

Autodesk Inventor iPart Filename Column
The filename of your iPart members is controlled in the iPart table, by setting the column you want to become the filename. By default this is the Member name column, shown above.

Generating Members

Rule number 1, NEVER delete the iPart members from their folder once they are in use within designs or iAssemblies. You will break association and potentially cause yourself A LOT of rework.
Rule number 2, DON’T assume all the members are regenerated. I experienced far too many occasions where a number of the members haven’t regenerated, post factory edits, when I was expecting them to. I found a failsafe though, if you change the value of a property in the factory, they regenerate without fail every time.
While this guide focuses on first time creation, it’s important to build in stability for future edits you will almost certainly have to perform. For this reason, its good practice to test applying some changes to your factories and make sure they translate into your members as expected. An even more thorough test would be to have the first version of members constrained in an assembly. That way when you regenerate the members you will be able to see if constraint errors occur, and tend to them immediately rather than after the iPart Factory has gone into ‘production’.
Autodesk Inventor iPart Factory Generator Custom iProperty
  • Create or Modify a custom iProperty called ‘Gen’
    as shown in the image above. This will force each iPart Member in the table to
    be regenerated.

Autodesk Inventor iPart Rebuild All
  • From the manage tab, Update the Mass, then
    Rebuild All. DON’T forget this, you may regret it later.
  • Save your file.

Autodesk Inventor Generate iPart Members
  • Highlight ALL the Members in the Inventor
    Browser, then select Generate Files from the context menu.
  • Switch to Windows Explorer and browse to the
    OldVersions folder found in the iPart Member folder (shown above).
  • You should see the same number of OldVersions
    files, as there were Members highlighted in the Inventor Browser.

  • You should also check the Date Modified
    properties of the files, to make sure they were generated within the expected
    timeframe.

You should now test your iPart Factory, by opening a new
assembly, and placing the Factory. If everything has worked you will be able to
place one of each of the members.

Autodesk Vault Check In

Autodesk Inventor iPart Vault Check In
  1. Switch to the Vault browser
  2. Highlight the iPart Factory, make sure you
    expand at least one Member to get to it

  3. Check In from the context menu

  4. Add a comment to describe this version of the
    files

  5. Click Ok.

Congratulations, you have successfully created, published
and Checked In an iPart Factory and its Members to Vault.
Now, the next step is to get your head around Autodesk Inventor iAssembly Best Practices.
Thanks for reading! If you have any questions, or require clarification just fire away in the comments below.

Leave a reply