Sketch Fillet option, but no chamfer?

[LibertyMachine]

Doing a quick sketch, I see there is an option to put a fillet of any size on the corners of the sketch. No option for chamfer though, or is it hidden?

[jeff_strater · Accepted solution]

No, there is currently no Sketch Chamfer command.  Sounds like an good candidate for the Fusion Idea Station.

Jeff Strater (Fusion development)

[Anonymous]

Hi Jeff,

Any progress on this or has it been rejected?

Thanks,

Matthew

[jeff_strater]

Neither.  It's still hanging around, but has not risen to the top of the priority stack just yet.  I found several IdeaStation entries for this (that probably need to be merged):

• chamfer-in-sketching
• chamfer-in-sketch-tool-and-sketch-tool-in-drawing-mode
• adding-chamfer-option-to-sketch-toolbox
• please-provide-chamfer-command-in-sketcher-environment

[Anonymous]

Hmm... No chamfer while sketching?! At least it looks strange for a guy with solidworks background.

[geraldft]

It looks strange to anyone...  quite a random and annoying exclusion, which does limit how you do things.  Unless you manually draw the chamfer - tedious...

[Anonymous]

It would be very nice to have a chamfer tool in Sketch

[TrippyLighting]

I wonder why this is requested. What makes this a necessity as opposed to using the solid modeling chamfer tool ?

[geraldft]

It's a convenience and it suits the way a lot of people like to work.  Also it's not just for making little narrow chamfers on an edge.  It would be a quicker way of making custom shapes - like take a basic rectangle and make a 5th side.   BTW why not also ask - why is there a filet in sketch?  Is that a necessity?

[LibertyMachine]

As @geraldft mentioned, it goes beyond small edge breaks. It's a function that is common in other software packages (Solidworks, Esprit, Autocad). It might be preferable to actually draw the part with the correct features in the sketch and then do an extrude. Drawing them manually is tedious.

One example, although one that does not really apply to me. Cabinetry work. Raised panel doors might have corners that terminate in a nice large 45. You aren't going to get that with the Chamfer button in the solid model side (not at the rate that it's been failing anyways..) So, sketch it and extrude it.

[JDMather]

---

@TrippyLighting wrote:

I wonder why this is requested. What makes this a necessity as opposed to using the solid modeling chamfer tool ?

---

Here you go.  

Have fun modeling!

Hmmm, that one might be is too easy to do either way.  I'll try to find a better example.

[LibertyMachine]

@JDMather not an overly difficult part, to be sure. But, it does convey the sentiment I think.

My scenario involves industrial design and mating components, whether that is raw stock and fixtures, or machined components and vise jaws/fixtures. I find I often have the need for a chamfer inside the sketch environment, so I either draw it out manually (yuck) or make it square corner and add chamfers in the model space. Goes back to "why is there fillet" in the sketch space.

-EDIT- I think the thing to keep in mind is this; most anyone on these forums with a 10, 11 or 12 next to their user name probably has a rather advanced understanding of work flows in Fusion. Model tools present different solutions, as do sketch. When I initially posted this question  back in March of 2016, I was very comfortable with the CAM side, but still learning the ropes on the modeling side. All the CAD/CAM tools I had used up until that point had a fillet/chamfer option in the sketch workspace. Right or wrong, that was my experience. I was just looking for the same flow, and wondering why it did not exist

[TrippyLighting]

---

@LibertyMachine wrote: 

-EDIT- I think the thing to keep in mind is this; most anyone on these forums with a 10, 11 or 12 next to their user name probably has a rather advanced understanding of work flows in Fusion. Model tools present different solutions, as do sketch. 

---

Thank you!

Until you wrote that I had considered abandoning this thread.

The reason I asked the question is two fold:

1. You are a CAM guy and I while I am noob in the CAM space I've been through enough threads and the occasional CAM tutorial to know that sometimes sketches and other modeling techniques are used to help create specific tool paths. I was wondering if that might be the case here.
   
   
2. Of course I am aware that sometimes a fillet or a chamfer are needed in the sketch in order to model specific geometry. Obviously that can be already be achieved with the existing tools. The question then is how frequent does that need arise and if that justifies having a specific convenience function implemented.
   
   

When I look through the "what's new" blog that is issued along with a new update I often feel it's a strange mixture. A slightly new UI is implemented that wastes a few pixels and people that appear to attempt DAD & 3D modeling on a cell phone get upset and color choices get discussed at length.

I can almost guarantee that one of the next updates addresses one of these almost completely irrelevant things. Yet, the bugs that I report - the last 2 updates were terrible - and that hinder not only my workflows don't seem to get fixed and neither do my Ideas get traction because the idea station also is mostly frequented by too many people with too little experience in Fusion 360 and CAD in general.

Given that I don't see the ROI ( so to speak) it makes me question why I am still spending so much time here on the forum and whether it's time to move on. 

[JDMather]

OK, I couldn't recall why that part made a good example until I started looking at some of my other examples (from a paper that I wrote 11-12 yrs ago).

This is particularly related to cast or molded parts with Face Draft.

I have long promoted using Feature Fillets and Chamfers rather than sketch fillets and chamfers when possible and practical.  

But back in 2006 and 2007 I also demonstrated at AU that sometimes it is necessary to use sketch fillets and chamfers to achieve desired Design Intent.  I doubt that I was the first one to recognize this as if I recall correctly I "borrowed" this part from a book by Dan Banach and Travis Jones.

A Feature Chamfer results in parallel sides to the feature, while a sketch chamfer results in angled sides that would progress to a pyramid (hmmm, I should have used a simple box shape with face draft to illustrate this).  The same is true for Feature Fillets vs sketch fillets and Face Draft.  One results in parallel "cylindrical" face while the other results in a conic face.

So Design Intent sometimes drives a need for Sketch Fillets and Chamfers rather than Place Features.

(The two chamfers in image below look like different sizes because of screen capture zoom, but they are both 15mm x 45° as from the drawing I posted earlier - one is result after taper extrude of sketch with chamfer, the other is result of adding chamfer feature after taper extrude.)

[Anonymous]

I've just tried to draw a certain rail curve in sketch mode, but wondered where the chamfer tool is. Came across this thread... Still no chamfer tool in sketcher? Can't belief this. 😕

Sure, you could always draw your chamfers yourself anyways, but still...

[geraldft]

It seems almost like random belligerence to leave it out.  Just because you can overcome the lack by using other techniques is not a sound argument in itself.  It has other basic tools like fillet which are replicated in both sketch and modelling, why pick on this one?  I occasionally design electrical panels with cutouts to to fit various kinds of switches.  I'd much prefer to draw the chamfers at the sketch level.  

[jeff_strater]

@geraldft - I can assure you it is not "belligerence".  It is simply a matter of priority.  It is a perfectly valid request to expect that Fusion supports sketch chamfer.  And it will, eventually.  But, the fact is that not that many people have asked for this, and we have a limited development team, so we've invested in higher-priority requests for now. Hope you understand.

[geraldft]

Jeff.  It is reassuring the team is aware of it.  The thing that surprises me is that this is such a basic tool, I'd have expected it to be there from the start, way before all the more esoteric features?  And when drawing attention to this, some responses imply that we are just using Fusion the wrong way.  Anyway - I look forward to to seeing it one day in the not too distant future?  My vote is to please bump it up the queue...

[HughesTooling]

Just want to add some thoughts on this and how a chamfer sketch tool will work in with a sketch solver like Fusion uses. I have a couple other solid modelers and used solid moders for about 20 years and in that time I've never used the chamfer sketch tool. Both of the other programs do have chamfer tools, one just adds a chamfer totally unconstrained the other adds dimensions but creates a very inefficient sketch.

Here's the example, note if you want to change the chamfer you'd need to edit each dimension and link them to a single parameter or waste a lot of time editing each one.

Here's what I'd create in Fusion and only took a few seconds more but far easier to edit and work with. To fix the sketch above from the other program would have taken more time than creating the Fusion sketch.

I guess with some planning the Fusion team might be able to come up with something that works as well as the fillet tool where the tool links all the fillets you create. If not I guess just adding the chamfer totally unconstrained would be better than the example above from the other program.

Mark

[LibertyMachine]

I do regret starting this thread. As stated much earlier in the discussion; my reason for asking was simply out of "the software I came from had this option, where is it in Fusion". After using Fusion now for several years, I can honestly say I haven't found a solid need for it, at least not enough for me to continue asking for it. I just needed to change my mindset and workflow a little. Not a terribly difficult thing, just requires a bit of humility and open mindedness. There are certainly other issues I'd like to see addressed before this is considered.