Troubles with splines

[DaveGadgeteer]

I'm trying to replace a decorative plate, to hide a hole.

I put a photo of the plate, scaled to the right size, on the sketch XZ plane, and proceded to trace the irregular curvy complicated outline.

Because I can't figure out how to make sharp corners between splines, I ended up using close spacing of spline points to work my way around the sharper corners, so there's an unreasonable number of points defining the spline outline.

However, I can select the interior and extrude it to form an acceptable starting base for the part, even excluding two holes for the screws.

Then I want to fillet the edge. Can't be done. The holes (defined by circles) fillet just fine, but no matter the fillet radius or other settings I always get an error message that the fillet can't be generated.

I'm surprised that the outline can be selected and the surface inside it pulled up, with no problem (OK, at first I had a stray piece of line doubled that had to be found and removed, but after that it worked), yet there's no fillet possible. I tried making a simple closed curve with splines, and that extruded and also filleted without problem.

So the trouble has to be the complexity of my traced spline.

There ought to be instructions somewhere for how to draw with splines, including how to create corner points and what the checkmarks mean, but I can't seem to find it for Fusion 360.

I'd upload my file, but I guess it's in the Cloud--not a file on my computer. Is there a way to upload it to show my problem? Export shows an Archive format, would that be the one to use?

A Noob

[carl_bass]

Please upload the photo so people can take a look and give suggestions

[DaveGadgeteer]

The screen shot also puzzles me--it only shows dots on the upper part of the outline, yet if I click anywhere on the periphery the whole line shows up as selected.

And sometimes I see all the control handles too, haven't figured out what triggers that view.

[DaveGadgeteer]

I exported as archive.f3d and tried to upload as attachment here.

It's complaining the contents don't match the file type. How can that be?? Fusion360 exported it!

[cekuhnen]

Silly form system - just zip the archive, then you can upload it!

[DaveGadgeteer]

OK, here it's been zipped.

[dunderhead]

I took a look because I haven't figured out how to join splines either (cekuhnen has written much on this subject) but I know a quick workaround: you can pseudo-join any line segment or another spline segment by just snapping it to then end of an existing one!! That won't usually give you tangent continuity but that's exactly what you want in your case! So you can use a lot of small line segments and open splines as long as they all form a loop. You can also save yourself half the work by using symmetry in sketch! 

The vertices become strangely occluded as you orbit your sketch around. I think that's a bug actually, but you can get around it by adjusting the opacity of the canvases (right click on the bar 'canvases' and choose 'opacity control'). I chose 50%.

I see you have some trouble with the timeline: you've defined the same object up to three times! And you reimport the canvas for no reason.  Save yourself a lot of trouble and look up a tutorial on how all this works!

Did you confuse fillet and chamfer? You chamfered around the edge loop on one side, and I could do it on the other side as well, no problem!

-dh

[DaveGadgeteer]

Thank you!

Yeah, the design was a mess because I've tried so many things in so many ways, and don't know how to back everything out cleanly.

So I started over (attached version).

This time I used far fewer spline points and didn't try to edit them, so the spline perimeter should be free of unknown glitches.

I didn't use symmetry because I wasn't sure the original was quite symmetric, and because I figured that would open new issues like correcting open loops--one of the big time consumers in Inventor used to be trying to fix a loop so it would extrude (be closed) even though it looked simple and closed to me. That seems to have gotten much better in Inventor 2015. I suspect those problems had to do with projected geometry getting mixed in with new geometry somehow.

The reason I had a bevel on one face and a fillet on the other was I was trying to figure out what was causing the problem, and both failed similarly (had unreasonably tiny sizes at their largest possible working radius).

This simpler version has a tiny fillet around the top edge at 3mm thickness. I then selected the inner plane (up to the edge of the fillet) and extruded that another 1 mm, which was extremely slow but did eventually work. Then I hoped perhaps I could bevel that one, at 45 degrees, and stack such layers up to simulate the beveled edge I want around the periphery.

But no, it's impossible to bevel the upper edge of this new layer (well, perhaps one could get a few microns, but you can't get a visible bevel or fillet on it).

I presume the problem is the small radius of some of the spline curves, but the limit seems unreasonable to me. Surely it ought to be able to fillet or bevel further than it does--the current result does not appear to be nearly ready to kink or otherwise break.

Surely there must be some way to make a shape with outer periphery like mine but sloping in along the edge. 

I also tried draft, which I demonstrated by using it to make the holes for bevel head screws--it does work there, which I realize is not what draft is intended for, but it won't work on the periphery, even with very small draft angles.

So how can I make progress?

Perhaps I can turn this into a mesh solid, generate an STL for 3D printing, say, and somehow import that again and work on it as a mesh object? I haven't spotted a tool that changes my geometric solid into a manipulable solid--is there one?

Or I can just fab the solid as is and fix it with a hand grinder and a file, but that's hardly educational. I'm doing this project just to get over the hump so I can try Fusion for real projects.

Yes, I clearly need to work through more training materials. I've done some tutorials and downloaded more lessons, but had thought trying to solve my own "very simple" problem would be a reasonable exercise for learning too.

[cekuhnen]

I looked into the file and am not fully sure what form you want to generate, howevere here are some observations:

The fillet command creates here and there triangular shaped edges edge patches. This is not really ideal for edge rounding as an outcome.

Changing the corner option for the fillet feature  freezes Fusion on my side - I assume Fussion just needs longer to calculate than I want it to so I force quote it.

I noticed that when moving a point in this sketch the screen refresh rate or better the speed with which the point can be moved tanks and turns into stop motion which

makes me belive that this sketch maybe is too much to work with - it has no constraints and thus should be fast if I would compare it with Alias.

Reflecting on the speed issue and the corner type issue here is one suggestion: Simplify your sketch by eleminating those tiny corners in your sketch.

The lower left corner I turned into a G0 point while kept the original lower right as is.

The reason for this is you can later extrude the sketch with less points and the resulting vertical sharp edges you fillet at the same time.

As you can see in my screenshots I get perfect smooth edges ready

if you want to you can also in the same fillet command round the vertical edges first and then with a new radius round the rest to build a custom ball corner edge where you can specify the radius for each direction

[cekuhnen]

so here is a rebuild of your file.

The design is fast now again and not as sluggish as the previous version.

I am not sure if that is because I removed all mini rounded corners in the sketch and replaced them with G0 edges.

Below are two screenshots. I am not sure if I read your design right.

But to mee it seems to extruded a top surface at one point and then wanted to add a draft to the top skrew opening.

So I combined it in case that is what you want. Instead of using draft I simply rotated the extrusion cut.

You can see all edges round perfect and smooth producing clean surfaces and edges.

The archive is attached

[DaveGadgeteer]

Thank you Thank you Thank you!
A Google search for Fusion G0 yielded something on Fusion Patches, which explains about G0 G1 G2 meanings (new terminology to me).

And now the deep, foundational, question at the root of this problem: How did you turn the corner point into a G0??

I had tried all the modifiers I could think of while drawing the sketch outline, but couldn't find a way to draw corner points (using Mac). I found I could get the overall shape pretty well by using two spline points near one another to simulate a corner. (My previous experience with this sort of thing is mostly Adobe Illustrator, which understands corner points and point conversions, but Fusion doesn't seem to work similarly.)
I've searched for Help on editing Fusion Splines, but somehow haven't found it.

BTW, my goal was to build a base plate about 3mm thick with the given outline and beveled edges, then start adding decoration on top, and perhaps some text, then 3D print it. Its purpose is to remove the old doorbell button, which is no longer connected and causes confusion, which has been replaced by a video SkyBell on the nearby door frame. I need a removable cover plate, hence the same screw positions, because the SkyBell connections have to be made inside the wall, and the SkyBell gets replaced occasionally due to beta testing etc. Of course, I could just use a rectangular shape, but I want to learn how to make fancier shapes that I can then print in plastic or mill from aluminum. So this is a training exercise--I never expected it to be difficult!

[dunderhead]

cekuhnen, thx for posting solution. yeah, so the simple stuff works!  My computer started huffing and puffing as well when manipulating Dave's original spline (delays lasting minutes!!!) I hope that's just a bug, not a sign of a deeper problem.

I tried the following alternatives to allow more flexibility in choosing the shape of the edges, all failing:

• For an edge routed with a more complex profile, using sweep. It's a built-in limitation of the Autodesk CAD engine (and others I think), the path has bends that are too sharp. 
• So what's needed is a nice 2D offset curve from Dave's spline. That could be used for a lofting rail. But the current sketch offset function surely fails here, as in many simpler cases.
• So use control vertex splines? It takes 200 edges to extrude Dave's spline in sculpt mode. The next step, the scaling of the edge loop almost works, except that normals are flipped along a small part of the curve.  Closer inspection will probably reveal that the scaled curve is not really the intended offset at all! But I don't know of any other way too offset in T-splines. Moreover, the algorithm for filling the two 200-edge loops fails: ' fill hole' produces self-intersections. Things become rather slow, too. And I ran into a bug where updating the scaling factor manually stopped working. The new multi-port view is great though for doing this kind of manipulation (screen shots below) including the failure to convert.

-dh

[cekuhnen]

T-splines and tries are like water and fire.

I would rather either:
A: cap the top and bottom face with an NGON
or
B: only extrude the sides and in patch mode simply close the caps stitch and fillet if needed.

thats the nice power of TS and timeline drive BREPs via TS poly models.

[dunderhead]

Thanks for suggestions to close surface:

A) How do you make a 200-gon without clicking about 200 times? If not obvious please vote for my modest idea along the lines of making an n-gon in one fell swoop. 

B) Do it in patch mode --- absolutely, a thrill to build complex shapes this way !

[cekuhnen]

Hi Dave

G0 to G2 are easy explained
G0 two curves just meet with their ends
G1 one curve has one extra CV that moves the same direction for the other curve to make a smooth blend
G2 one curve has two extra CVs to make that smooth transition

 

G1 vs G2 you can see how the G2 green line longer follows the blue direction and then only bends meaning you have a smoother but longer transition.

G2 to G3 is prefered for quality produduct design but also harder to make. G1 looks rather click and done.

So here is a curvature comb telling me how mathemarically even the green curve blends into the blue curve

you see the comb is nice and even - good highlights you will never in the product see where those seams were.

the position of the CVs are important to nicely stretch the curve to make the flow smooth

G2 is not an automatic winner bad spacing makes bad combs.

and here is G1 you see the comb even has no fluid transition - for your eye the two curves might flow nicely but in reality it is bad

here another example:

Blue arc is G1 very clean but terrible in making a transition. Green blend curves are G2 they are not circular but make good blends.

when turning on the zebra you can see that in the right example the patterns break. in real live here on a plastic surface you will see a seam in the hightlight which is not desirable.

that is why all Apple products do not use G1 at all as for us it is considered rather undesirable and mechnical - also it requires no skill.

Car bodies use G3 and more which why they are so hard to make getting the flow right means you need space to relaxe the surface curve

I used Alias here because it has some of the best tools to explain this.

In Fusion G0 is done by drawing a spline and then drawing another spline starting from one end point or dragging two end points onto each other.

G1 and G2 in Fusion are Tangent and smooth constraints.

Surface Fillet has G2 option or is by default G1.

Loft comman has G1 G2 as tangent and smooth.

And here everything again as video

https://drive.google.com/file/d/0Byzv_NlyKp_2Q0gzbnRvbkI4NjA/view?usp=sharing

here is a screeny from Fusion

showing you G0 G1 and G2

pay attention to the highlight

left terrible sharp edge center ok but G1 style right better smoother wider transition

I hope this helps!

[DaveGadgeteer]

The video was very helpful! At first I was convinced I need to get and learn Alias, but when you moved over to Fusion I was startled to see how much it could do.

My problems are at the most elementary level--I understand the differences between G0 G1 etc., now that I know what is meant by them, but I couldn't figure out how to create them.

Apparently the trick in Fusion is to end a spline where you want a corner and join it to another at the corner point. And it was useful to see you using the checkmark to end a spline.

There were still a few mysteries left, like pieces of spline disappearing suddenly with no apparent cause, but since you recreated them similarly at once, I presume those were just glitches in the Fusion interface.

I had expected a way to decouple the two direction handles so they could go in different directions from the point, and even if in the same direction, the possibility of having different lengths, for different stiffnesses. But I guess that's not how these splines work.

And I haven't yet figured out how you access the CV controls, or why you were able to click on points and move them or the handles while I seem to have to right click and select move, then select point, then click again to move the point. It's very awkward compared to what you were doing in the video.

I tried to make small edits in the periphery curve, but often find the whole curve moving instead of just the desired point, so the process isn't converging well and I use many undos.

I've discovered that the reason my points come and go has something to do with the orientation of the sketch plane--if I rotate the view slightly, it will change from one half the plane to the other for whieh points are visible. It's like the sketch points are only visible in front of the screen (or perhaps behind it), and the sketch plane crosses the screen plane as I move it. But in addition, sometimes all the visible points show their control handles too, and other times they don't, and I don't know what I'm doing differently that causes the different behaviors. It acts like sometimes they're all selected and other times not.

Anyway, I guess I'll start with an empty design and play with simpler splines to imitate what you did in the video. It helps enormously to know what's possible and how it should look. The actual tool selections and modifier keys go by so fast it's hard to figure out what was actually done, of course, but trial and error should get me there now. And perhaps I can find a viewer that gives good frame at a time control.

I have made a simple flat beveled version now, and managed to get it into an STL file that I can print. I'm ready to see something physical!

Thank you very much for the large amount of time you've spent on my problem! Presumably others will benefit from the video too.

Dave

[cekuhnen]

Fusion is not like Rhino Alias using CV curves where I edit different CVs to weight the G1 G2 effect.

A G2 curve in Alias has both the tangent CV and the Curvature/Smooth CV to work with.

Fusion currently does not offer CV curves - big bummer because I am not a big fan of spline curves for every task. To me they are like EP curves from Alias and hardly anybody uses them because they are hard to work with.

EP curves in Alias act like splines in Fusion if you edit a point a lot of the curve left and right will change which can be sometimes good - in my opinion often is rather extremely hard to use because I end up tweaking curves more than as a designer I should.

To get this under control try to break long curves up into smaller segments and also if you need to make a simple curve use 2 max 3 points and work with the handles to bend the curve. You can also mix lines and splines well.

Regarding handles the tangent handle can never have the left and right handle point in different directions or have different lengths. This is not Illustrator.

But we can have different handle length if we break a curve into 2 segments and then adjust the tangent handle for each end point.

Watch the video I hope it helps. My mic is broken if this makes no sense I will record at the University tomorrow something again with a voice over.
https://drive.google.com/file/d/0Byzv_NlyKp_2MFlhSG5YaEN3SU0/view?usp=sharing

[DaveGadgeteer]

I printed the simple part in ABS plastic, and discovered that the photo I used was taken off-axis by enough to make things too distorted, so I started fresh, with a scanned image of a traced cardboard, which ought to preserve shapes well. I then examined the scan in Illustrator, and used Illustrator to trace over the shape, which I then exported as TIFF. I placed the TIFF in my file on a canvas, and then made a sketch over it. Pity one has to do the tracing all over again instead of just importing the vector art, but I couldn't see a way to do that.

So I tried to trace the shape in Fusion once more. After a few frustrations I tried just using a lot (200+) of short straight lines to approximate the curves. That version resulted in an extrudable loop, but it was completely impossible to put a bevel on it.

So I started tracing once more, using my newfound understanding of spline curves. The main difference was I drew the spline in small sections, editing each piece to optimize the placement of its points and controls. I got a decent approximation to my shape, though it was not painless--whenever I accidentally made a control line vertical, it locked there with a constraint. I don't know what makes it think it's supposed to insert constraints automatically--I looked for a while but couldn't see how to turn that off--but eventually I discovered that if I hold the Cmd key down, the constraints don't get generated and another big advantage: the points stop snapping to the grid, which they've been doing even though I've turned off snap to grid. Sheesh.

OK, so I finally got it looking good, but it turns out it's not recognized as a closed loop, so I can't pull/extrude anything.

I can't find tools for closing loops. I tried applying coincidence constraints, but they don't behave sensibly--maybe that means they are already present. I can't tell where the problem is, because it lets me select each piece of curve separately even though I know I joined the ends as I went.

The file is attached. I'll be glad for advice/diagnosis/hints!

[cekuhnen]

In Illustrator you can save a design in SVG format and insert that into a sketch in Fusion.

However you cannot in Fusion really edit the curves - you can only move parts around. Lines are fine to be edited. Fusion and AI splines are not the same.

All photos done have a perspective lens distortion.

Either scan it in - or step far away and perpendicular to the object with a tele lens zoom in to cut down the foreshortening effect.

After scanning in clean up but don't waste time tracing it in AI - do that right in Fusion.