How do I edit a sketch fillet?

julian_foster

You can change the radius of the arc of a fillet but it doesn't respond as a fillet it actually moves the connecting lines to a new position based on the original fillets centre point. Anyone know what I'm doing wrong, presumably its something to do with the constraints?

3dcad

Can you post some picture on your situation or share your model?

It works ok for me, just double click the R value and set new value. 

If your lines are not in 90 deg, then it needs to move a line to keep fillet in tangent for both lines when changing the radius.

julian_foster

@3dcad - Thanks for your reply.

Can you confirm that this doesn't work if the lines you are applying to are not at 90deg? If this is the case it is definitely a bug.

A fillet should never move a line it is based on regardless of angle, it should recalculate a new centre point based only on tangental constraints.
Thanks for looking into this for me though, the solution may be to constrain the lines completely before applying a fillet but this could become quite annoying I think!

paul_chastell

Let me explain a bit about how a sketch is represented and how Onshape deals with changes, which is my long-winded way of saying "sorry, the sketch isn't built that way".

A sketch is a collection of geometry and a collection of constraints that determine relations between those geometries. There is no history. When a dimension is changed we solve the sketch to meet that new value, plus all the other constraints that exist, all at once. When we do this we try to make the smallest possible change to the sketch.

When a fillet operation makes a fillet it doesn't add a historical feature in any way because sketches have no history. The sketch doesn't even remember that the arc is a fillet. Rather the fillet command is a shortcut for "separate the lines; create an arc; join it to the lines; make it tangent to both; add a radius dimension".

So now when you change that dimension we get a solution for that change, but in the absence of other constraints there's no specific way in which it will change. Specifically, while I understand your desire to have the lines remain where they are, there's no easy way for Onshape to ensure that.

We could try to special case various behaviors when we see stuff that looks like a fillet but because the solver solves everything at once such special case code invariably leads to problems in other cases and inconsistent behavior.

3dcad

@Paul Chastell Thanks for explaining how sketches actually work.

It's good to know that tools like fillet or rectangle is just shortcut to create the geometry and add certain constraints. So if you need to modify, just remove constraints and make changes as you like.

julian_foster

Thanks Paul, explanation much appreciated. It is a shame about lack of history in the sketch though as its such a promising product and I'm really keen to give it a go, I realise it is early days though and very impressive despite this. Unfortunately the model I was using as a test was entirely based on a sweep so of course being able to adjust the curves of the path accurately is fundamental.

andrew_troup

Paul Chastell said:

...... while I understand your desire to have the lines remain where they are, there's no easy way to ensure that .....

(Andrew Troup wrote, seemingly unable to append this under the quote frame where it belongs:)
Could he not simply select all the lines and temporarily apply a 'fix' relation to all at once?

3dcad

Andrew_Troup said:

(Andrew Troup wrote, seemingly unable to append this under the quote frame where it belongs:)
Could he not simply select all the lines and temporarily apply a 'fix' relation to all at once?

Offtopic - @Andrew_Troup  You need to use 'Toggle HTML view (</>)' and write a letter after code "</blockquote>" then switch back to normal view and replace the letter with your text. 

andrew_troup

Thanks, 3dcad. Not being an html native, I never thought of that. 

paul_chastell

Yup. Correct Andrew_Troup. I meant that there is no easy way for Onshape to do it without complicating other cases. I rewrote history to reflect that.

julian_foster, if you set up the relations you need then the sketch ought to behave as you want on changes. If those lines are meant to remain where they are the typical workflow is to capture that intent in dimensions or constraints, usually with constraints to outside of the sketch, e.g. to the origin, reference planes or part geometry, and then they will stay where you mean them to be and other stuff, e.g. the fillet, will change to your driving constraints. In addition if that defining geometry ever moves your sketch will update based on the constraints you provided. Andrew's solution is the simplest of those, by fixing you are saying "these lines are where I want them to be and they should never, ever move". And they won't.

julian_foster

Thanks Paul, Yes I mentioned this process in my original thoughts, the only issue is that it starts to infringe on the speed of workflow when creating conceptual models that change frequently during creation.

Realistically I imagine most users only want a line to move or change when they decide anyway, in which case having a default lock for every line would make sense and the lock is released by specific operations in specific ways - i.e. editing a fillet keeps the line in place but allows changes to its length (or trims it according to the resulting fillet) whereas changing the length of line A would allow the line it is joined to B to change its position but not length. I am sure this functionality is not trivial to implement but is the sort of intuitive response I would like to see in a sketch adjustment. I used Alibre (now Geomagic) for a few years and it behaved this way if I remember. Thanks for your explanations though I am still keen to see how OnShape develops!

paul_chastell

3dcad: Yes, indeed. You could even use sketch pattern as a cheap copy/paste in the sketch by patterning and then deleting the pattern constraint.

andrew_troup

3dcad said:

@Paul Chastell Thanks for explaining how sketches actually work.

It's good to know .....

Indeed! That sort of glimpse behind the curtain is immensely helpful in all sorts of ways.  

Onshape makes a simplifying virtue of the fact that surface extrudes are almost the same thing as solid extrudes (I say this because solid modellers are just surface modellers with 'extra benefits') and is not afraid to call a Boolean what it is.

I personally think other packages keep us rather more "arms-length" from the fundamentals, and it makes it a lot harder to troubleshoot when things do not behave as we need. 

I'm just going to fire up Solidworks (albeit not the latest version) to check how it handles sketch fillets to unconstrained lines. Out of habit, I hardly ever apply them that way, I prefer my pasta in a bowl!

andrew_troup

Hmmm: Sldwks 2009 behaves much the same as OnS, when an existing fillet is edited to a new radius when the lines are unconstrained. Not surprising given that they share the same basic solver, AFAIK.

However, both packages "play nice" when each fillet is initially added, presumably because at THAT stage, it is clear that the desired result is a fillet, not just a tangential arc. So another, more elegant workaround for the OP's specific issue, is to delete the wrong-sized fillet and create a new one, which can then be tweaked to the desired size without moving the unconstrained lines.

The more I think about this, the more I understand and support what @Paul Chastell  says. A sketch should always behave in a WYSYWIG way. There should not be hidden legacy behaviour, where apparently identical geometry, with identical constraints when audited, behaves differently depending on how it was created. (ie "history"). It would be almost impossibly hard to come back to later, or make changes to a model created by others.

andrew_troup

It did fleetingly cross my mind that an alternative would be for OnS to create a new type of constraint, called a "Fillet" relation.

However this would quickly fight with other relations once other constraints were added, requiring escalating "fixes of fixes". In any case (personal opinion warning!) this would be a bit like taking a baseball bat to a mosquito. I'm not trying to be provocative, but there seem to me a whole bunch of other situations where working with unconstrained geometry goes tits-up in a parametric sketcher, and addressing all these situations with software "features" could quickly turn a useful, plain-walking beast of burden into a temperamental, neurotic show-pony. 

I'm not saying there's not a place for a brain-storming tool of the sort the OP would clearly prefer. (An app for a tablet would be brilliant)

I just think the front end of a rigorous MCAD solid modeller is not that place: the missions are too divergent.

julian_foster

Fair points Andrew - Ultimately in this case, I am probably not using OnShape for its intended purpose. I am still hoping to find that elusive tool that allows creativity to flow until such a point where it can be frozen into a precise model that can have all the details required for manufacture applied with ease! Probably I will come back to OnShape at a later point in the process. Thanks to all who gave input to this question.

andrew_troup

I do think I know what you mean, @julian_foster, about ideation.
 
I'm always striving to team up with my design tools in ways which make them "disappear" from my consciousness, to the maximum extent possible, and UI issues are a biggie for me as a result. 

I want a tool which lets me whip an idea into a finished real world prototype with the minimum fuss, because every road block has the potential to derail the creative flow. But also the process needs (for me, at least) to be both fun and ... somehow graceful. 

Having said that, clunkiness is a problem for me not so much because it's ugly, but because it's distracting.

julian_foster

Well looks like I'm mistaken! I dug out my old Alibre license and attempted the same model / fillet situation and it works exactly like OnShape . I've used so many 3D programs over the years (and been out of the game for 5 years now) I think I was confusing the solidworks type software with the likes of Powernurbs which I frequently used within 3DSmax. So apologies for my ramblings - at least we had a discussion about where we would like OnShape to go in future! ;-)