iPart: sketch not remaining on work plane

[foolishgrunt]

I have a multi-body iPart factory that I'm using as a workshop for designing many sheet metal parts. As I switch to a different member, some of my work features are formulated to change positions. One of my sheet metal faces is set to reside on one such work plane, as seen here (with the work place highlighted):

When I switch to a different member, the positioning of the work plane changes appropriately, but the sheet metal face does not:

This of course creates a cascade of other errors with other features dependent on the face in question. I can correct all these issues by simply redefining the sketch back onto the work plane, but I have to do this manually each time I change members. The upshot of this is that I cannot generate all of the iPart member files with a single click: I instead have to generate, switch to another member from the table, redefine the sketch, generate, and so on. This becomes very tedious when I have 20 different members to generate.

Adding to my consternation is the fact that I have another (very similar) iPart factory that does not have this issue: every time I switch members, the work plane and the sketch move in tandem. Does anybody have any insight as to why this particular sketch does not remain on the work plane as it moves? Why does it need to be redefined every time?

[johnsonshiue]

Hi! The behavior looks like a bug. Please share the iPart factory file here or send it to me directly (johnson.shiue@autodesk.com).

Many thanks!

[johnsonshiue · Accepted solution]

Hi Andy,

Many thanks for sending me the file! I believe this is a bug in the compute sequence. For some reason, the sketch lacks another update after the Bulkhead Plane is changed. It should always be up-to-date. Interestingly, if you do Rebuild All after activating the member, the Face feature will move correctly.

Normally, I would not suggest you use iLogic rule in an iPart, since it would interfere with how iPart compute works (two drivers in a car). But, in this case, the easiest thing to avoid the issue is to add a simple iLogic rule (ThisDoc.Document.Rebuild()), triggered by any geometric change. Please take a look at attached part and see if it works better.

I notice that you are still using Inventor 2019 RTM build. Please install 2019.4 update followed by 2019.4.5 update.

Thanks again!

[foolishgrunt]

Thank you for your help! Using the iLogic workaround you suggested, the part does update upon switching members, though the process does take longer than it did before inserting the rebuild operation. But the important point is that I can once again generate all members in a single operation, so I will be using this workaround until such a time that the bug is fixed and/or I can upgrade to that version. 🙂