References Repeatedly Lost

[OshanaHaydn]

Hi Fusion people 🙂

I have an issue where my references for items way back in the timeline have started to break without being touched. I have been back in time a many, many times and fixed all the issues, taking numerous entire days, but they keep reoccurring. I recompute regularly, and the design is clean until I close and reopen and THEN recompute, at which point it's semi-reliable to reproduce the warnings. Something definitely happens on the journey through the cloud...

It's a yellow warning or three that, only when fixed (usually just by opening and pressing okay) leads to cascading cataclysmic failures that take a day to get through. In the screenshot case the geometry is the offset inside surface of a helmet, so quite parametrically complex, but the operation itself is a simple loft between two surfaces which computed instantly. 

I'm guessing this is an edge naming issue. Does Fusion rename edges in some way/at certain points that I could work to prevent to ensure the edge names are stable?

Alternatively, this design is around 1000 operations now, going on for 1500 potentially. Is this just to big of a file for Fusion? Is it better to split components out into separate designs or covert to direct at this point?

Or do I just live with yellow warnings in my timeline?

Please help, debugging is taking over my entire life!

[TrippyLighting]

Can you share that design?

[OshanaHaydn]

I have messaged privately with the file, I can't share it publicly but obviously please feel free to post the solution here.

Thanks a million.

[TrippyLighting]

I've looked at it and experienced the same thing: after a compute-all, a couple of lofts are complaining. I cannot determine a definitive cause other than that Fusion sometimes seems to lose previous selections or selects "something" adjacent.

I won't have time to investigate this further as I am heading into an intense work week with a deadline.

I am tagging @Phil.E  

[OshanaHaydn]

Really appreciate the assist, thank you!

I have meanwhile decided to leave my computer on for the rest of eternity as a workaround 🙂

[Phil.E]

Please confirm, this is happening with one design? If so, when was the design started (what build/timeframe) would be important, as well as having the file to debug. 

[OshanaHaydn]

Hi Phil.

One design, yes.

So...when was it started is an interesting question 😞 I would guess early to mid 2023. I had another issue in September which I had thought was unrelated. Since then all my pre-September designs have for some reason been dated between 18 and 25 March (screenshot attached).

To summarize, it was an account upgrade and change to company email address which didn't go smoothly, and I lost work. I also had a forum engagement then, and perhaps the details are relevant.

https://forums.autodesk.com/t5/installation-licensing/lost-work-done-since-upgrading-from-trial/m-p/...

I am not sure whether the first warnings are in post- or pre-account-transfer operations. I think pre- but same ballpark.

I have sent the file in a private message.

Again, thanks a million for the assist!

[Phil.E · Accepted solution]

The account issue has nothing to do with the parametric history or geometry references of a design. I'll check out the link, thanks for that, and get back to you.

I see the same thing that @TrippyLighting sees. However, this model is too complex for me to figure out anything about it related to references. I just don't have a couple weeks to sort it out.

Have you considered stabilizing it and then creating DM features for some of the parts that are "set in stone"? If you no longer need to edit a parametric feature, and that feature keeps getting an error, right click on it and use convert to DM feature. That removes the parametric references. Sometimes this can help to simplify a design like this and avoid errors from compute. 

[OshanaHaydn]

Hi Phil.

The part is dependent.  I considered allowing the warnings to remain, but it feels like a sword of Damocles.

If you think it's not a file corruption issue and is workable-through, I will go back and have another look, restarting Fusion each time.

If I find a solution I'll post it here in case it's of interest.

Cheers, thanks for getting back to me so quickly. Have a great week.

Haydn

[Phil.E]

Thanks. Just to be sure I understand, you are still editing from time to time the geometry that is projected into the loft-sketches that are losing these references? 

[OshanaHaydn]

Hi Phil.

The idea was to lay up the outside surface, physically test and adjust materials, measure thickness and corners, then go back to adjust the internal surface in Fusion, so it would be super helpful to keep it parametric, else I'll have to face the tolerances some other way.

The sketch geometry involved here is for the cutting tool, which created the loft edges by cutting surfaces. Basically it's a "thicken" workaround, lofting offset surfaces together and then boundary filling.  

If it's the sketch, do you think that if I retry building a detailed parametric constraint system for the loft profile cutting tools, this might help? It's fairly non-parametric to be honest. I tried locking it all down once with arbitrary constraints, but the error recurred so I removed them...maybe they weren't good enough...

Thanks again for the assist.

[Phil.E]

If the source of the projected geometry in the sketches that turn yellow must be constantly edited, and it causes problems downstream, then your only choice is to try another method to deal with these changes.

I would just avoid associative sketch projections. Manually update all downstream sketches/features that depend on the stuff you are editing. Is this a perpetual design, like are you ever going to finish it? Perhaps making an entirely new design would be the best route if you plan to work with this for another year or two.

[OshanaHaydn]

It's not sketch projections that are bugging out, it's the lofts. The sketch curves aren't associative, they're just arbitrary arcs cutting offset form faces. It's the loft that connects two of these edges that fails. The weird thing is they recompute fine after I fix them, it's just the journey through the cloud that annoys them. And even that never used to happen. They must be soooo close...

Yes was once perpetual part-time, first-time designing for me, but now it's being funded and I have a December deadline. Needs to be good enough to prototype, which is why I'm thinking to run with the Yellows. 4th generation but you still see fingerprints of CAD ideation... new products are hard!

[steve3957T · Accepted solution]

I have have a very similar issue with one my files.  Recomputing with the file open and everything is fine, but closing and opening causes massive failures.  I pinned mine down to a "split" feature that will not remember selections.  I had used "split body" and made multiple selections to use as a splitting tool.  If you do this, and edit the spit body feature later, fusion forgets all the selections.  It will work ok just doing a recompute, but closing and opening would sometimes make it forget the selection as well.  

Not sure if this is what is happening to yours, but maybe something to look for.  It looks like you have a lot of splits in your timeline.

[OshanaHaydn]

Hi Steve!

Thanks for this, you weren't far off. I have solved my problem to a degree, but honestly not sure quite what it was. The meta problem was that there were two "real" errors on the profile surfaces of the same loft, each a step or two removed from the yellow error itself, and so whatever I fixed when trying to isolate it didn't help.

One I understand, which your suggestion points to, which was I was lofting from an edge of a surface that was itself lofted from another surface that had sneakily stitched itself without my noticing or giving any error. Solved by reworking with precision tools i.e. cutting out a strip and lofting across it.

Second profile was an offset of a loft between two organic t-splines. It seemed fine, I'd already worked out any possible intersections and the offset was on the outside of a corner, not tight at all, but obviously it had some gremlin from the 11th dimension. What I ended up doing was very messy and tedious: slicing it (and its adjoining profiles) up and lofting off it until I found the section that was complaining (saving, restarting and recomputing each time) and then reconstructing that surface using rails manually approximated on projections from from the failing part (urgh). Now I have is a slightly wonky part but since it's composite, the outside surface matters most, and it's just a prototype...and it isn't broken. I don't drink currently but I had a beer when I fixed this.

A suggestion to @Phil.E and the Fusion team: Perhaps look at getting recompute to do what the journey through the cloud does? Even if it takes a bit longer. Recomputing currently only has a chance of working.

Thanks again everyone for your time helping me on this.

[Phil.E]

Sorry it took so long to respond again.

A developer is happy to look at the design. Can you please share a link to it? or email me at phil dot eichmiller at autodesk dot com with the link or file?

[OshanaHaydn]

Hi Phil.

Thanks for the revert.

I've moved past this point now and am not looking to improve the solution further. I'd be happy to try to reproduce the error back at that version and send it through if it would be useful for you guys, but I don't actually need an assist anymore.

Please let me know.

Kind regards,

Haydn

[Phil.E]

Okay, thanks for letting me know. Good luck with the project!