Having trouble with Fusion in general

[Anonymous]

So I'm having a bit of a workflow crisis with Fusion in general.

If I go top-down and just blast out stuff without a care in the world, it works out okay, but parametric relationships are terrible and none of the parts are drawn 'as manufactured.' This works out OK.

If I go 'bottom-up' and draw really concise 2d sketches I get really slow sketches and Fusion does a terrible job of handling constraints. I can't get a well functioning 2d sketch like is required of you in a program like SolidWorks. Then when I go back to make changes the whole thing explodes.

It seems like I can go willy nilly making random stuff and it works, but it's nothing manufacturable. Or I can go step by step and make something manufacturable but it's impossible to make changes.

I don't know what I'm doing wrong and it's extremely frustrating.

I'm at month 4 with Fusion and still feel like I'm making fun shapes and nothing that's real.

[Anonymous]

Hi Luke, in response to your comments:

"3:50 -- could Fusion team add better selection priority here for the two corner points? let original points take priority over projected points for example"

This does not appear to be a selection priority issue, but rather the vertical sketch being visible interfering with the live editability of the horizontal sketch.

"5:30 -- I strive for as concise a timeline as possible so that I build "editability" (see "drinkability") into my projects... problem is, this can actually cause more issues than it solves. What's the benefit of having this move feature in your Timeline?"

So far I've found it very editable (similar to edible? ) once getting used to it, knowing how corresponding operations/actions are highlighted when clicking elsewhere in workspace, etc.  I find it actually very user friendly and powerful.  Not sure what you mean by drinkability, unless that's similar to edibility .  One reason to have the move feature, is I've found sometimes say for moving components (vs bodies), if the move is not captured in the timeline, the moved component will return to original position upon Compute All command.  Also as said I find it nice to have a fully interactive 'flow of time'.

"https://screencast.autodesk.com/main/details/af2caf41-c290-42d2-9fca-0279ccf8db19"
Yes in my fixed video soon to be uploaded, a part accidentally deleted that further discusses what you showed there.

"7:05 -- how did that dimension appear out of nowhere?"
I took a long time to make that dimension (was getting tired) so for sake of brevity removed that hopefully self explanatory operation

"10:40 -- OK back to the 1 vs 2 jiggle. It seems to me that Fusion is reporting the 2 jiggle simply because your sketch is inside the component that you're jointing to. But I cannot think of any reason why the resilience of the joint would be any different than if you jointed to the base level sketch, since the base level sketch will always drive that projected point. I would assume that this is a case where the 2 jiggle is being shown because the "jiggle engine" isn't smart enough to realize that you're working of geometry projected from the base component sketch."
From my preliminary tests I've found that it is in fact important when moving the components to new location then doing editing/free editing again of vertical faces.  The tangential relationship with respect to the face is maintained from the projected point, but unless that point is in a sketch locked to the object face, I believe the perpendicular spatial relationship is not maintained upon component moves, and the joint depends on this relationship as well.  Also, as stated in the fixed video soon to be uploaded, it appears the larger body does not jiggle because it needs to be moved out of the base component (and if there is a position driving sketch yes that needs to be in same component as body).

"12:10 is a perfect example of why I hate leaving sketches in the base component. This is extremely counter intuitive having your sketches left behind in 3d space. Now go drag those live to adjust your geometry and see how it goes. "
I haven't found any problem with it, but as shown a little later in the video it's optional as there's a perfectly fine alternative. 

Glad to help at all!

[Anonymous]

Luke wrote: "I understand the jiggle better and I see that you are correct. Sorry about the noise. I always forget to check/uncheck the mic button at the end. Wish I could delete audio on the Screencast website..."

That looks like an interesting screencast you did, I will look at it more closely later. 

Jesse

[Anonymous]

Hi Ludo, I found this short video helpful for updating broken references:

https://www.youtube.com/watch?v=Ef1k-uDl3WU

I've found if it's a profile that is changed, it doesn't seem to break say a 3D extrude, likely because there are other sides so the profile internal identifier (probably each feature created has a unique identifier code) does not change, whereas a surface extruded from a line/curve, if that line/curve is deleted and replaced, then the surface extruded from the new line/curve is going to get a new identifier code, so something referencing that new face is going to get broken.

Just my theory 😉

Jesse

[Phil.E]

It's not a theory it's exactly how it works. It's what makes it "parametric"!

I like to use this example with my Inventor students.

When you need to make an edit, you will want desperately to preserve the lines, arcs, faces, etc that already exist. These all have an "address" and a "name".

Imagine if you come home from work to find that the city has demolished your house and built another one exactly like it, right down to the mailbox and furniture. Is it still "your" house? Not really, so you throw an exception: "warning reference is missing".

In this case the offset workplane is really looking for  a very specific reference. Just replacing the line is like building an identical house in place of the one you love and refer to as "home". 🙂

[Anonymous]

Needing a move feature to successfully render after a Compute All sounds like an issue with Fusion being able to calculate, unless your component isn't constrained or you don't have a snapshot recorded. In fact, you shouldn't even get a move feature unless you're moving a body, and I try to get into components ASAP. There seems to be some disagreement even within Fusion team as to whether component before vs component after is a better workflow.

https://screencast.autodesk.com/main/details/08865856-be95-4923-a92e-2a9fb13bfddb

And furthermore, if you EVER want that sketch to be in your component... you have to delete everything in that component, everything that relies on that component, move the sketch, and start again. THAT to me, is indicitive of poor workflow requirements.

Good discussion, I'm learning a lot. 🙂 Will watch the rest of your video now.

[Anonymous]

Here's the fixed version, the added part that was accidentally deleted being from 6:38-7:47.  Remember to increase resolution setting to 720p!

[Anonymous]

Thanks Phil, home is indeed where the heart is 🙂

Mark wrote: "I think the idea of having the Main Assembly as direct then having components as either direct or with history would work quite well."

Hi Mark, I quickly tried this idea but couldn't get it to work.  Although I haven't ran into problems with the timeline yet, perhaps with massive projects it may get somewhat cumbersome.  If you could be sure your idea can work, and basically how you did it, or even a screencast 😉 that would be great.

Jesse

[Anonymous]

Thanks for that screencast Luke, that's useful to know the move tool, along with the 'click and hold' selection of the point beneath the projected point, can move one sketch with the other being visible.

You wrote: "And furthermore, if you EVER want that sketch to be in your component... you have to delete everything in that component, everything that relies on that component, move the sketch, and start again. THAT to me, is indicitive of poor workflow requirements."

I don't know why exactly the moving driving sketches into another component is not allowed, but I have not found it to actually be a big deal.  I've found the easiest thing to do once a component is moved, and if I forgot to have a driving sketch go into that component so therefore it's not going to move also with the component move tool, is for future geometry to just create a new sketch on the relevant (active) component face.  Furthermore, before moving a component, you of course have the option to create a new sketch in the (active) component, and project the relevant features of the driving sketch into the new sketch.  If you want to move/edit these projected features at some point, you can just select them, right click and choose 'break link'.  I've not needed to really do this yet, but I suppose in some situations it could save a little time.  Overall, if can remember to activate components before making sketches, then this whole thing is a moot point, and if forget, there are several good alternatives. 

I'm definitely learning a lot too, especially from your questions!

Jesse

[Anonymous]

Note that in my scenario of projecting features from sketch in 'top level' as you say (good description) into sketch going into a different activated component, here's one beauty of the timeline, is if the component has already been moved, just roll time back to before the snapshot of that move, so that now component is back directly on top of top level sketch of interest to project/copy.  Then roll the time back to present (top level component needs to be active), and our new sketch with projected geometry moves to new position without problem from what I've tried. 

[Anonymous]

Another likely even easier method than projecting from old to new sketch, is first roll time before move snapshot (as in previous scenario) if move has occurred, then simply select and copy relevant old sketch geometry (don't even need to enter old sketch), then paste it in new sketch (which is in proper activated component), and do a quick single point to point move to line up pasted features with original.  Move time back to present day, and done and done.

I can make a vid for any of this stuff for anyone that requests that. 

[Oceanconcepts]

A very interesting discussion. Particularly, for me, concerning the relative usefulness of Direct or History based modeling. 

The kinds of design problems I’m typically working on involve a number of sourced imported components that have fixed designs already, some components that I am designing, and trying to fit it all together into an ergonomic and manufacturable package. And I may chose different sourced components based on what I find when I start putting the puzzle together. Far from being a linear process (EE provides circuit board, I build enclosure) it is iterative and loopy. We’re a small group, we go back and forth with design concerns. 

What I have found in trying to use history early on in this process is that it gets way too messy. I’m moving, tweaking contours speculatively, drawing and deleting, trying to work out optimal relationships between components, to decide if I need to find a lower profile connector for that LCD, which of several possible piezo devices would fit best, asking our engineer if this lens would still be strong enough at 3 mm rather than 4 mm, can I make the circuit board a few mm shorter- the early stages are a jumble. So I find myself spending most of my time- as working out the puzzle is by far the most time consuming aspect- in direct modeling. That may just be me sticking with the familiar. But with history I seem to end up with a timeline that is geologic in scale. Maybe there are better workflows to manage this?

Yet there are times when history would be tremendously beneficial- particularly if it could just exist within specific components. I realize I have not fully explored the potential of the timeline, and this discussion is very helpful. Any workflow that would enable me to say to a particular component “OK, you, now, track your history.” would be very useful. An alternative I have used is to rebuild the design in parametric mode when I have a better idea where I am headed. This discussion is providing some food for thought, thanks to all. 

[jeff_strater]

We do recognize that the "move a sketch into the component that you created from that sketch" is not an ideal workflow, and are in the middle of fixing that.  We got there because we disallowed some other cases (for instance, if the sketch drives two components), and sort of over-generalized it.  But this specific case (one sketch producing one component, drag the sketch into the component) is a very common and useful request, so we do plan to handle that.

Jeff

[Anonymous]

Just want to post this excellent short video if someone hasn't seen it, showing how to 'flatten' features in timeline to DM, while mixing up with other timeline features.

[daniel_lyall]

hope you don't brake it up to much its good to make one thing from one drawing with lots of parts that work together as in the cabint, draw and bookself what are templates I did and posted over on the woodwork post 

[Anonymous]

Another possibility, don't know how much of a practical solution it is or not, but say after making a component with a lot of different timeline features/operations, you can select all those, right click and select Create Group, then you can also right click on that and choose Rename to make a nice informative group label.  At least this may give some structure and also management of large projects. 

Jesse

[daniel_lyall]

you just found another problem a lot of the vids that are gold just get lost I have said before some one needs to go through gaver them all up put them some where with a link or what ever to them with a good name.

a lot of the question people have asked these vids are a good answeer to them 

[Anonymous]

Didn't even know you could do a DM feature in a history document.

So we have:

DM document, DM components
History document, History components
History document, DM Components & History

Now all we need is DM document with History components & DM components.

Or in other words... assembly document with linked components in other files... like every other CAD program 😉

[LMD001]

Hello Jesse,

Thanks for the link!

Most drafting software actually use some form of a database structure, so you are correct that when you change geometry enough, the database often cannot simply replace old with new and breaks.
Like Jeff wrote, the Fusion Team is hard at work to provide feedback on these failures so that is is easier to repair a broken model.
Now sometimes it is just more timesaving to start again than try to fix a model, with me, the second run tends to give shorter timelines ;-).

Best regards,
Ludo

[Anonymous]

I really appreciate all you guys do, and thanks for working on this particular issue.  In teaching empowering software like this to people, a new user will already be juggling so many things in their mind, it's quite easy to forget say creating and activating a component before making a sketch and a driven feature, and then when realizing have to either redo or use alternative editing methods, it can be frustrating, and for new learners, it's great to try to keep frustration as minimal as possible 😉

Jesse

[Anonymous]

Ludo, yes it is very true that the second time around gives much shorter timelines! Sometimes the pursuit of short timelines from the beginning can be frustrating and sometimes it is worth it... Sometimes it's not worth it! Sometimes I just draw the thing and convert it to DM at the end because I don't even want to look at the timeline! LOL