Save As autosaved my current version.

[weshowe]

I uncovered a problem when I changed two dimensions on a sketch. Summarizing the issue, this sketch drove a revolve, which was combined with a cylinder. That worked. Moving forward in the timeline, a third body was used to cut this combined body. That did not work right... the cut was made, but the body was split back into the two original bodies (both were cut, and also separated).

So I decided to use Save As to save this broken version and planned to abandon the changes to keep my previous version. Fusion saved all my changes, closed the working file and made a new file. This is so wrong in so many ways as a program behavior. It is not helpful. It should have left the unsaved edited file open and made a new file like I wanted. Now I can't revert and try something different, I have two broken files.

I am attaching this broken version so you can look at it and find out why the edit sketch broke the second combine operation. But I want you to know I am not at all happy with the file management issue either.

[TrippyLighting]

In the data panel you can promote a previous version of your file to be the current one. then you have the working version back.

[weshowe]

TYVM. Now I have my old file back. That is not so intuitive, but it solves part of my issue.

I still think the Save As is wrong headed. I know if you try to close an unsaved file, you get a warning, and I often close the panel and abandon the changes as a sort of mass-undo. I did not expect Save As to follow a different type of behavior.

As for the attached file, I believe it needs attention. My original version, prior to editing the sketch, was fine. I think I can even use this broken file by combining the parts outside Fusion after exporting them as STL. Autodesk will never conquer the mountain until problems like this can be sorted out.

 - Wes

[TrippyLighting · Accepted solution]

It's less the file that needs attention but your design style 😉

What body gets cut by which loft is controlled imlpicitely by the visibility state of the bodies involved.

This is problematic because object visibility is not being kept track of in the timeline. Once the design is created it is hard to recreate what bodies were visible when the combine operations happened. This is likely the reason why the file appears to be broken. 

This can be entirely avoided by working with components and that is best done by following Fusion 360's R.U.L.E #1: Before doing anything, create a component and make sure it's activated.

I won't go into details here, but if you search the forum for R.U.L.E #1 you'll get plenty of hits that will explain the advantages of that approach.

I've attached a file that shows the same design as your, but is much more parametric. The sketch for the plug profile is only present in the first component. If it's changed there, the profiles of the other two plugs will also change. This is achieved by creating two additional empty components in addition to the first one with the completed plug. Then the body from the first plug is copy/pasted into these components.

After the "raw" body has been copied the loft-cut sketches are added to each component and the loft-cuts are created.

It is important to activate a component before adding "stuff" to it.

[weshowe]

OK. I concede you are right. 🙂

I did use visibility to  keep the parts pieces separate. Perhaps my n00b experience will remain of some value as a lesson on what beginners will do.

Oh, and TY for going the extra mile and fixing this. On that, I have a question. It is obvious you got the parts from my original file, and I wonder how. Was it a cut-and-paste from one project to another (does that work)? Or if not, what method did you use (so I can learn it, I don't [think] I need detailed step-by-step on this)?

Knowing a why this happened helps a lot. The whole parametric method appeals to me greatly, it's like writing source code and getting it compiled, only I'm making hardware instead of software!

  - Wes

[TrippyLighting · Accepted solution]

I did not use any of the stuff in your original file other than copying the few text strings for the sketch names.

The few sketches were quick work. I do wish there would be a quick and convenient way to copy/paste a sketch from one project to another but there is not.

If a sketch includes more work, you can create a component from it, export the component and then import that component into a new design, but that is only worth the trouble if the sketch is more complex than a rectangle 😉

[weshowe]

Thanks for the answer and the advice.

I did notice that each component has it's own timeline, and the default component at the top has all of them. So I see that is the method that isolates the operations from affecting other portions of the file.

 - Wes