Why can't I add a fillet to this shape?

[Anonymous]

I'm having difficulty adding a fillet around this guitar body shape that I've made available for public download: http://a360.co/1Nk4Ems. No matter what order I try to add fillets to the curves, I get the error "The fillet/chamfer could not be created at the requested size" when I try to add a 4mm fillet to the edge around the back of the guitar. It works OK if I only select the curve and straight line that make up the lower bout and output jack area, put fails if I include the upper bout in the selection set for the fillet. The front side (top in this drawing) will need a roundover too eventually, but it may need special attention around the neck pocket. For now however:

1. What's preventing the operation, and how can I find out the details? Are there detailed logs somewhere, or a way to get more informative error messages?
2. What can I change to make this work? There isn't much room for me to alter the design unless it's in inperceivable ways because it's already the right shape.
3. Is there a way to get a fillet other than the Modify|Fillet tool that might work better?

Thanks,

Michael

[HughesTooling]

I guessing you imported the outline. The problem is down to how smooth the spline is, it will fillet with a 2mm rad but fails with anything bigger. I suggest you try tracing over the outline using Fusion's splines.

I've attached my attempt, I don't use splines for my work and didn't spent much time on it but it will fillet with a rad upto 12mm.

Mark

Edit to load the file use New Design From File on the file menu. Also I'd use Export in the future instead of the download link.

[Anonymous]

Thanks Mark for such a fast reply and for your example. It gives me hope that this will be work out.

I created the sketch using Fusion 360's "ImportSplineCSV" script, with a little tweak so I could import multiple splines into a single sketch. Then I joined the splines together with straight lines to produce a closed curve, and added tangent constraints between each straight line segment and spline so that the curve would be smooth all the way around. I have attached the csv files I used in case they are of interest.

It does look like the splines created within Fusion 360 are smooth at each point. Maybe there's a rounding error or something that makes them not quite smooth when there are lots of points or points that are too close?

An experiment occurs to me: maybe I could break the problematic bits down into separate splines (with tangent relationships between them to keep it smooth) to try to find where the problem lies.

Michael

[HughesTooling · Accepted solution]

After looking at this a bit more perhaps the problem is more down to the spline being too dense. I removed a couple of splines and replaced with arcs and now it works, file attached. If you can I'd try reducing the amount of points.

Mark

[Anonymous]

Thanks again Mark, I'd say you've got this all figured out. It seems like the point density was the issue. I'm looking forward to completing a full model now.

Regards,

Michael

[HughesTooling]

What you need to think about in an area like that, when you add a fillet it's similar to offsetting the curve so the points get pushed together and if the offset is to much the points can cross over. If it was an internal curve rather than external the points get farther apart so there's no problem. 

Mark

[rinMJQG5]

Hi guys,

I have designed an electric guitar and the body is giving me grief. I would like to round the edges (fillet) but I am getting inconsistent results. I finished a version and got it to do a 4mm fillet but the I realised I have to make some serious changes and couldn't get it to fillet on the new version. It wont do the full circumference in one go and  but sometimes it will fillet a small length then it will freak out, the error is:

"Error: The fillet/chamfer could not be created at the requested size. This might be occurring at the ends of the selected edges. Try adjusting the size or using multiple separate operations. Check that the selected edge chain ends at a sensible position, and if not try selecting more edges."

I have made simple squares and circles and can fillet them but thats not what I'm attempting to make. It doesn't matter if I select a short straight section or a tight curve. Once it has freaked out once I have to restart the app as it seems to retain some kind of bad mojo from the errors!  Here is a screenshot.......

[etfrench]

@HughesTooling in post #5 indicates the most likely cause for the failure.  Try filleting small sections at a time to find the problem area.  Attach your file to this thread for more detailed analysis.

[Anonymous]

Thanks for the suggestion but I may have failed to mention that I have done that already. To take it to another level I have to try do it in small sections with varying success and also can only start by adding the smallest fillet possible the slowing increment the fillet till it crashes and go back an increment. Sometimes I can add a fillet to a particular section and other times (after reverting back to a previous state), I can't. The sections aren't tiny as can bee seen from the screenshot. I'm sure there is a logic reason but it doesn't make any sense to me.

Richard

[Anonymous]

Even when I select a fillet and select "edit Attributes" and try to reduce the fillet I get errors. There definitely seems to be something wrong with this application in this area.

Richard

[Anonymous]

Sorry to keep posting stuff but I'm getting more and more confused. On a wim I decided to open the file in the fusion web browser and hello hello there is a fillet all the way round, all even with no missing bits. I don't think I even got that far so how is there a fillet when I open it on the web?

Richard

[TrippyLighting]

Please open your own thread and share your model, screenshots and a detailed explanation of where you're stuck.

[Anonymous]

Thanks for responding. While I am figuring out how to start a new thread...... here is a link to the file that is giving me grief!

https://a360.co/2OgXEdI

thanks

Richard

[TrippyLighting]

Non need to. Old story answered about 1-2 times a week on this forum. You extruded the first shape from an crappy imported DXF or SVG file.

Crappy because the individual curve segments its broken into are neither tangent or curvature continuous.

Just nearly tangent, which is the problem.

I should not take longer than 15-20 minutes to trance the imported shape with Fusion 360 native sketch geometry.

[Anonymous]

Peter,

Thanks for your time reviewing my situation. That was one of my first thoughts (svg causing problems) and I then tried to trace using the spline tool but had pretty much the same issues occur around my attempted use of the fillet.  I used the same technique (svg file import) on another project I was experimenting with, and had no issues with the use of fillet. I will knock up another one (of this particular project) based on a trace and if that still causes problems, then I'll again post the file for examination.

regards

Richard

[Anonymous]

Hi there,

I traced the shape using the Spline tool and as I suggested there are still issues with the fillet function. I will confirm that there are less issues than the extruded SVG. While being able to fillet the whole edge I am only able to add a small amount more fillet before the errors again re appear. 

Regards

Richard

[TrippyLighting]

Would you have that traced file ?

[Anonymous]

Dear TrippyLighting,

Thanks for you continued interest, see below the shared link. I am still experimenting with what is possible and the repeated recreations is making me better at manipulating Fusion (or I seems to think it is). My intention is to produce an electric guitar that can be reliably reproduced on a CNC machine and if there is a small amount of work (tidying up a fillet) then that's fine with me. I have all the other components satisfactorily created (well I think I do). 

https://a360.co/2Mw5nUI

regards

Richard

[TrippyLighting]

ou projected some the geometry from the old design into the new one and then deleted the old body, or sketch.

1. That's why your new spline sketch has a lot of yellow lines in it as it is missing the references  you projected from.

2. You also used too many spline control points and probably can approximate the shape with 2/3 or even half of them . It takes a little practice and patience to master this. 

I deleted these obsolete references and I believe that some of those threw a wrench in your wheels when you extruded the body.

Everything seems to fillet fine. Model is attached.