sketches and bodies are disappearing during edit sketch

[Anonymous]

Greetings,

since the most recent update I have had an issue with sketches (others that I am not editing) and bodies disappearing when I select Edit Sketch. They disappear from both the model view and the browser tree and return as soon as hit Finish Sketch. Makes it kinda hard to sketch when the objects I need to reference vanish.

any thoughts?

regards,

Hanswurst

[jeff_strater]

Hi @Anonymous,

This is a great question.  It is a common question among people who are not familiar with history-based parametric modeling.  The timeline at the bottom of the screen is a historical record of operations that you have done.  When you edit a sketch or a feature, you are really time-traveling back to the point in time when that sketch was first created.  So, yes, everything after that sketch is no longer available.  This is necessary because this style of modeling is associative.  That is, you can have features that depend on sketch geometry, such that, if you edit the sketch, the feature will update.  This results in a dependency from the sketch to the feature.  Parametric modelers such as Fusion then have to prevent you from creating circular dependencies.  So, if you have Sketch1, and an Extrude1 that consumes it, then you create Sketch2 by sketching on a face produced by Extrude1, you have a dependency chain from Sketch1 -> Extrude1 -> Sketch2.  So, you cannot create a dependency from Sketch2 -> Sketch1, or you would have a cycle.  So, when you edit Sketch1, Fusion "rolls back" the timeline to a point before Extrude1 and Sketch2 existed, to prevent these types of cycles from being created.

And yes, this does require you to plan your design a little.   If you need something in SketchB in SketchA, then, it's best to create SketchB before SketchA.  In all the cases that I've seen, there is always an ordering that will satsify all the requirements of building a design.

So:  editing a sketch or a feature is time-travel.  If you remember this, it will make everything easier.

Jeff Strater (Fusion development)

[philQ46VH]

Thanks for the exact answer I was looking for!  I did just realize, at least with sketches, one way around the problem of trying to reference later sketch geometries from earlier sketches, and that is to either copy the earlier geometries to a new later sketch, or copy the later geometries to an earlier sketch.  

And, so you won't have to look this up like I did a few days back, in order to copy sketch geometries between sketches you must first open and edit the sketch, select the items, and hit copy (Cntl/Cmd - C), then open the other sketch and paste them!

[Anonymous]

I have been working on a model of a truck since the last few months.  Today, while I was almost getting done with my project, I saw that Fusion 360 was backing up my data in the background.  While the backup was happening in the background, Sketch#505 was still in edit mode and at the same time, I was turning-off other sketches to simplify my view.

Just as the auto-backup finished, the list of the sketches, components, bodies, etc. froze for a while and came back.  Next, I noticed that more that half of my sketches, bodies and components DISAPPEARED!!!!!  I was working on sketch#505, and now the latest sketch visible is Sketck#251!!!!!!

I just lost a good 15 days of work!  My Manual backup file that is 10 days old has upto Sketch#383!!!!  C'mon Autodesk, why is this happening??? This to really bad, I mean, very very very bad!  I really hope and pray that I get my data back.

[chrisplyler]

If I were you, I would make this complaint in a new thread, instead of posting it within someone else's two-year old thread.

[mikesmail0000]

I hate to necro a post but this came up when I searched for more or less the same thing. I would really appreciate if someone would weigh in on the things below. If they are correct then they would actually solve the above issue. Please keep in mind I'm a newbie but I tend to believe that I have around about the same level of experience as the OP (at the time of the original post).

1. Keep the component you're working on activated so sketches are nested (organized) properly, and

2. Do not extrude while in sketch mode.(<--Edited) Depending on the timeline one or more features may not be visible/selectable while editing a particular sketch but this won't be the case once you leave sketch mode. Finish the sketch and then extrude from the sketch objects. This should avoid the OP's issue entirely (it was my issue until about 30 minutes ago)., and

3. Please weigh in on this: Don't let a fear of creating "too many" sketches influence your design process. Once you've finished creating the extrusions you planned when drawing a particular sketch, be done with it and create a new one. Don't keep going back and updating that sketch as that will cause confusion in the timeline. Obviously, I'm not saying you should redraw a feature, you can still reference prior sketches so there's no need to do so.

Is the above accurate?

Edited to correct error in #2 thank you cadwhisperer!

[TheCADWhisperer]

@mikesmail0000 

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

I think you will make the fastest progression if the experts here take a look at your work.

[mikesmail0000]

There is no file to export as this is a generic question about best practices. I believe I used correct terms for various functions and if so then it should be decipherable. However, if not I would appreciate pointing out where clarification is needed because I likely need to learn the correct terminology

[TheCADWhisperer]

@mikesmail0000 

Thirty years of experience have taught me to observe and comment on geometry, not words.

[mikesmail0000]

You are indeed 'euclidean'! This question however needs Socrates — or Plato I guess since he's the actual source we refer to.

I just read it again and double checked my terminology too and confirmed they were used correctly. There's a bit of text there so is imagine that's a turn off.

I guess I'll try a different tack:

I assert that the three points I listed in my post above are best practices and if they are then I encourage other newbies to consider them as well. If I understand correctly they will respect the timeline. After integrating those practices into my habits I'm no longer experiencing the same frustrations expressed by the OP. 

If I'm wrong, please do correct me for both my and future reader's benefit. Otherwise, said future readers may be misled. However, if those are in fact "best practices" then great!

[TheCADWhisperer]

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@mikesmail0000 wrote:

2. Only extrude while in sketch mode. ... Finish the sketch and then extrude from the sketch objects.

---

@mikesmail0000 

Do you have a concrete example? A file that illustrates this?

[mikesmail0000]

🤦 I do not but the first sentence was the opposite of my intention and so was entirely confusing (sigh). I corrected my post above to say: "Do not extrude while in sketch mode." (emphasis added here, not in previous post)

In regards to creating/providing a file to illustrate, I don't think the timeline differentiates whether the user was in sketch mode (currently editing a sketch) or not when they select then extrude an object, does it? I think it just records an extrusion. That's what #2 is saying, to be in one mode as opposed to the other when extruding an object. After thinking about it more I see your point about how a file is beneficial in posts. I genuinely don't know how to demonstrate what I'm saying. I'm sorry