topic Re: Fillet in Sketch alters diminsions of rectangle in Fusion Design, Validate & Document Forum

Fillet in Sketch alters diminsions of rectangle

Anonymous — Thu, 07 Jul 2016 18:25:33 GMT

I've got a sketch where attempting to round corners changes the width of the rectangle used to create it. It's the HiTEC HS-5035HD sketch in this design: http://a360.co/29tJRzb

This screencast shows the issue:

I think its because of to all constraints in the sketch but it sure looks like a bug to me. I do find it some what challenging using constraints to line up sketch elements. In this case I was working from an actual part taking measurements from the part as I went along. The sketch really doesn't need all the constraints but it's the only way I know to line up features.

I'm going to remove most or all of the constraints and try again.

-Dave

Re: Fillet in Sketch alters diminsions of rectangle

Anonymous — Thu, 07 Jul 2016 18:42:51 GMT

This version has some constraints removed and the problem goes away: http://a360.co/29tJRzb
The original with the constraints intact (problem still exists) is here: http://a360.co/29lhvnb

This may or may not be a constraint related bug with fillet. If it isn't a bug please indicate which constraints were causing the problem and how I would have discovered it.
Thanks.

Re: Fillet in Sketch alters diminsions of rectangle

TheCADWhisperer — Thu, 07 Jul 2016 19:15:08 GMT

~~Dimension to lines rather than to endpoints and you will generally not lose dimensions when adding a sketch fillet.~~

~~use CenterPoint rectangle~~

add Fillets as features rather than in sketch.

Edit:

Well I experimented a bit more and this one is poorly behaved.

I might do a couple of more simple sketches or use fillet features.

Re: Fillet in Sketch alters diminsions of rectangle

Anonymous — Thu, 07 Jul 2016 19:48:46 GMT

The sketch is a top view of a servo. I'm making adapters for different sized servos so I want all the sketches to be aligned on the drive shaft center. I did that by projecting the drive from the standard servo on to this sketch and then creating the rest of the view from that reference point.

That combined with the restricted ability to get reliable caliper measurements from the original (It's hard to use calipers to measure from a projected plane) made the sketch method a little unorthodox but not that crazy. I did not intentionally dimension from an endpoint.

As far as adding fillets as features instead of on the sketch, that seems like working around an issue to me. The part I'm making fills in the difference (more or less) between two servo cases. I may be missing something but It appears that fillets on sketches have to be done one at a time. I couldn't figure out how to select a bunch of corners and round them. That and it didn't remember the prior fillet amount so I kept having to enter the radius - annoying.

Maybe the fillet function in sketches could use some work. If you know of a way I've missed, I'd love to learn it.

Thanks for the response.

Re: Fillet in Sketch alters diminsions of rectangle

TrippyLighting — Fri, 08 Jul 2016 00:23:44 GMT

@Anonymous wrote:

As far as adding fillets as features instead of on the sketch, that seems like working around an issue to me.

That's been a recommended CAD practice since I've worked with 3D CAD which is almost 2 decades.

However, the sketch engine can use improvements and it's being worked on heavily 😉

Looking at your sketch Fusion should actually throw a warning that it cannot fillet that edge, because it really cannot.

The horizontal line has a midpoint constraint to the vertical, fully constrained construction line.

The horizontal line is also horizontally fully constrained as it has been dimensioned.

When you apply a radius to the corner either the dimension has to go so the midpoint constraint to that now shorter horizontal line can be maintained, or it maintains the dimension and will throw a warning.

Even when you remove the midpoint constraint Fusion 360 will remove the dimensioning as the dimensioning is applied to the horizontal line and not between the two vertical lines.

I would definitely consider this a bug.!

Re: Fillet in Sketch alters diminsions of rectangle

TrippyLighting — Fri, 08 Jul 2016 00:51:44 GMT

I've created a screencast on a much simpler sketch and was able to reproduce this undesirable behavior.

While these fillets are probably better applied as solid features, it's not and excuse for the sketch fillet not to work!

Re: Fillet in Sketch alters diminsions of rectangle

Anonymous — Fri, 08 Jul 2016 01:52:43 GMT

Thanks for figuring out the constraint tangle. The fillet changes both the length and when performed one end at a time (the only way possible) the midpoint when only one side is rounded.

It should throw a constraint warning.

Re: Fillet in Sketch alters diminsions of rectangle

innovatenate — Fri, 08 Jul 2016 04:47:54 GMT

Thanks for reporting this! I will get this one logged with development. I've seen similar sample with symmetric constraints, but its always good to have more tests!

Re: Fillet in Sketch alters diminsions of rectangle

innovatenate — Fri, 08 Jul 2016 21:13:34 GMT

I have the report logged under reference ID FUS-25958.

Thanks again for reporting this!

Re: Fillet in Sketch alters diminsions of rectangle

Anonymous — Thu, 29 Jun 2017 20:06:29 GMT

It's been a year already and I'm still having this problem. Creating a Centered Rectangle and adding Fillets to the sketch break all constrains and the rectangles its not centered and fixed anymore. Adding Fillets at extruding time simply does not worked when you are designing a refrigerator wire rack using the Pipe tool.

Does anyone here has a remedy for this?

Re: Fillet in Sketch alters diminsions of rectangle

cekuhnen — Sun, 02 Jul 2017 00:46:52 GMT

@Anonymous

By logic the rectangle center constraint breaks when filleting the edges

so you can just add new dimension constraints to maintain thensketch being centered - pretty easy.

i cannot understand your fillet in model space is not a workable option for you

can you explain this more ?

Re: Fillet in Sketch alters diminsions of rectangle

TheCADWhisperer — Sun, 02 Jul 2017 16:08:36 GMT

@cekuhnen wrote:

...

i cannot understand your fillet in model space is not a workable option for you

can you explain this more ?

I created a video to illustrate the issue - while it is being processed - I recommend going back are carefully reading the problem description as outlined in Post #10.

Re: Fillet in Sketch alters diminsions of rectangle

TheCADWhisperer — Sun, 02 Jul 2017 16:26:00 GMT

Here is the video that I think illustrates two issues - logic of maintaining centerpoint design intent and why sometimes sketch fillets are, of course, required or at least the most efficient technique of creating particular geometries.

Interestingly, in the process of creating this video - I discovered other inconsistent behavior in Fusion - another video to illustrate that behavior to follow in a few minutes.

Re: Fillet in Sketch alters diminsions of rectangle

cekuhnen — Sun, 02 Jul 2017 16:48:38 GMT

@TheCADWhisperer@Anonymous@innovatenate @TrippyLighting

Hmm works quite normal. I am 1000% sure SW adds constraints when you add the fillets in the sketch.

There are two ways to after adding the fillets in Fusion to fully constrain the sketch to the sketch center too.

A: via inner half dimensions and not using the diagonal lines

B: vert hori constraints of diagonal endpoints to the fillet end points

C: Add a Point mid onto a line and add a hori vert constraint of that point to the sketch center

I prefer version A or C as it is radically lighter using less constraints

https://forums.autodesk.com/t5/fusion-360-design-validate/create-component-preserving-history/td-p/7198374

Re: Fillet in Sketch alters diminsions of rectangle

TheCADWhisperer — Sun, 02 Jul 2017 16:57:53 GMT

Well as a Fusion neophyte I messed up a couple of times in the following video and was tempted to do the recording over lest my message gets lost in the fumbling - but then it occurred to me that the issues a beginner encounters can be more instructive than watching a pro who avoids the issues based on prior experience without even thinking about them anymore.

So here it is

Re: Fillet in Sketch alters diminsions of rectangle

Scoox — Fri, 10 Nov 2017 16:23:21 GMT

Same problems here. Also, in his last video here TheCADWhisperer highlights a separate problem which is that after you select a command from one of the menus (Fillet in this case), Fusion 360 requires users to click in the Fusion 360 window to focus it again. Is as if the menu were a separate window that steals focus and focus doesn't return to the main window once the menu closes.

Re: Fillet in Sketch alters diminsions of rectangle

marc.e.lefevre — Mon, 16 Jul 2018 17:43:08 GMT

I have into this as well running 2.0.4279 so it obviously has not been fixed. After the fillets are placed and I change one of the dimensions of the rectangle, only one side of the rectangle moves to accommodate the dimension change. The diagonal construction lines that were created when the original center rectangle was created stay in place and the rectangle moves away from them. The constraints for the fillets are visible (tangents) but there are no constraints shown at the corners.

I'm new to Fusion 360 coming from OpenSCAD so not much is intuitive to me at this point. I, like others, have to add this to my list of scenarios to avoid. Filetting in 3D space works fine.

Re: Fillet in Sketch alters diminsions of rectangle

TrippyLighting — Mon, 16 Jul 2018 17:50:49 GMT

@marc.e.lefevre wrote:

Filetting in 3D space works fine.

Right! That's why fillets don't usually belong in sketches. In fact I personally keep all features out of sketches that I can use solid modeling features for. Not only is that usually much faster to sketch and model, it is also harder to break the design history.

Re: Fillet in Sketch alters diminsions of rectangle

TheCADWhisperer — Mon, 16 Jul 2018 17:51:28 GMT

Yep, here it is a year later and the same issue occurred in a sketch I did just a bit ago.

Design Differently!

Re: Fillet in Sketch alters diminsions of rectangle

TheCADWhisperer — Mon, 16 Jul 2018 17:58:46 GMT

@TrippyLighting wrote:
….That's why fillets don't usually belong in sketches. ...

While I agree that fillets usually should be done as placed features rather than as sketch entities - there cases where it makes sense to place in the sketch.

This should work.

It does work in Autodesk Inventor Professional.

Perhaps the Fusion developers should "walk across the hall" and ask how it is done.

Design Differently!