Fusion360 crashed but still open & opinions on my workflow

[Anonymous]

Hi all,

as you know I'me very new to F360 and I've experienced some software freezes.

I've finished the ring at the link: https://a360.co/2MVZ67b (not mine, but just to practice with some object easy to do) and, if you open it and try to edit the first feature (extrusion, for example, from 3,5mm to 3mm), F360 will freeze and you will need to terminate it... sometimes it reboots windows after the blue screen. Any idea?

Anyway, please have a look at my workflow and tell my about it...

Thanks a lot

Marco

[GRSnyder]

It doesn't crash for me, but I can confirm that it seems to go into some kind of infinite loop that requires termination. This is on macOS Catalina.

Your construction looks fine to me, except that you've used Move and Capture Position a couple of times. Better to make the setting a component of its own and use joints between components to set the positions. I suspect that if you did this, Fusion wouldn't be freezing. (Not that that's an excuse; it should never freeze this way.)

[jeff_strater]

thanks for sharing the model.  I can verify that if you change the first extrude to 3, it does cause a hang.  It appears to happen in this fillet:

I'll have the modeling kernel team take a look at it

[Anonymous]

Thanks GRSnyder,

so for the setting, you say to make a component and use the joints, but once I've ended the rough modeling, have I to turn it back a body to combine with the ring?

When in modeling, I don't know exactly where and when I would put a body since I can see the global object.

Thanks

Marco

[Anonymous]

Thanks, Jeff.

Let me know, please.

Marco

[jeff_strater]

@Anonymous - I was off by one fillet.  It is actually the one before that that seems to be the cause of the hang:

If you look at the geometry after the edit to 3 mm, but before that fillet, it looks like this:

You can see that the small spheres here now interact with the side face that did not at 3.5mm.  My guess is that is why the fillet hangs.  My guess is that it will eventually fail (I'm about to test that theory by starting it, and going home for the night).  But, if you want to make your design totally parametric, my guess is that you want to change the size of those spheres (I notice that the ones on the other side are missing) based on that parameter.  Regardless, though, Fusion should not hang.  

I've sent this off to the kernel team for comment.  I'll respond when I know what they have to say

[Anonymous]

Jeff,

thanks.

Having it completely paramentric would be a great goal form because of the different size of the finger.

Let me know.

Thanks

Marco

[jeff_strater · Accepted solution]

sorry for the delay.  Making a design fully parametric is a challenging task, and takes some planning.  The first thing you need to think about is:  What aspects of my design do I want to be changeable.  You can try to make every single dimension editable, but in my experience, that is extremely challenging.  So, instead, you want to try to identify a couple of critical dimension that you will want to change.  In this case, I would think that the size of the outer band of the ring would be the most important dimension to be changed, since that's what affects the ring size.  So, I would make that diameter a user parameter from the start.  Then, as you build your design, stop frequently and try out various values, to see how your design reacts to those changes.  You also need to think about what is a "reasonable value" for each critical dimension.  For instance, in this ring design, it probably doesn't make sense for the outer diameter to be 2 mm, or, say, larger than 40 mm.  So, keep that in mind when "testing" your design.

Looking at that, in this ring design, if I change the diameter from 18 to 20:

Then, step through the design, it goes OK, until I hit the hole feature Hole1.  This feature fails.  So, you'd need to go back and figure out how to make this hole feature more robust.

Back to the original change that prompted this post:  This change is actually to the width of the band.  So, first, is that a reasonable dimension to want to change?  If so, what ranges are valid?  In that change, you went from 3.5mm to 3mm.  Where the problems start is with the small retaining features that start in sketch5:

in that sketch, the circles are not positioned parametrically, nor are they sized relative to the overall width.  So, you'd probably need to change that sketch to be dependent on the band width for size and position.

And so on...  One thing, in this particular design, the number of small stones is constant.  Is that your design intent?  Or, do you want the number to change as the overall diameter changes?  That, itself, is a bit of a challenge.  But, something to consider.

Hope this helps to shed some light on the topic you asked about.

[Anonymous]

Jeff,

what a complete explanation!!!😎 WOW!

Thanks a lot.

Many  many digital jewelers work with Rhino3d wich is not completely parametric (please note "completely"); starting from an initial model and keeping the curves used to generate the solids, they can turn back the history by hands rebuilding the model step by step... this is a very time consuming way to operate but you're right when you write that I can choose some dimensions that change and replace the old values with a new one with in mind the dependencies between that value and the other (the small spheres are not positioned parametrically).

This way, with some changes, it's possible to achieve the result without have to rebuild all the model.

However, I think Rhino3d is still more complete than F360 in the way it manages curves and surfaces.

I'm now trying to recreate a rhino3d workflow using F360 to undestand where exactly they are different.

If you're interested in, I can keep you updated.

Thanks a lot for all!

Marco

[jeff_strater]

Thanks, @Anonymous - glad that it could help, even if it is not complete.  Yes, I am interested in your progress on the Rhino workflow.  I suspect you will get frustrated, because the two tools are very different (Fusion tends to be more "solid focused", while Rhino is more "surface focused"), and we don't claim to be a replacement for Rhino.  But, there are probably some jewelry projects which you can use Fusion to design, once you understand and embrace the parametric solid modeling workflow.  You will certainly be able to make your designs much more customizable, if you follow those guidelines for making your design parametric.