A really weird Sweep

[RogerInHawaii]

I'm trying to make a groove around the main body of a spacecraft model using the Sweep tool.

The Profile is a simple circle, defined in the Groove Tools sketch. The Path (Groove Path 2) is essentially an intersection between the main body and a plane that goes through that position in the model.

I select the Sweep tool and select the profile and path.

And when I select OK it initially seems to look pretty good.

But when I pull back from it, it APPEARS that only a portion of the path has been followed. There's a nice groove for part of the path, but it SEEMS to be blocked at one point.

Pulling back further I see that the path appears to have been followed only partway around the path.

 I then select to Save as Mesh and select to preview the mesh, which looks pretty good. It LOOKS as though the groove goes all the way around.

So I bring that mesh up in Slicer and take a close look and the groove does NOT appear to go all the way around, although the part that seemingly didn't become a groove comes up darker. ???

So I look very closely at it in Slicer and it seems that the darker, non-groove part, has fairly large triangles while the good-groove party has super small triangles. What's going on? It's almost as if the Sweep DID go all the way around but for part of the path it didn't sweep with the entire circular Profile. Very Weird.

I've attached the file and it should come up right at the point where I'm doing the Sweep. Hopefully someone will take a look and provide some insight as to what's going on. The pertinent Sweep SHOULD appear in the lower right corner when you bring up the design.

[andy.griffinP6ZT8]

You might want to look at the line across the flat section of the path.

It seems to be 2 lines which aren't connected. I replaced it with one line and it seems to work...

[Bunga777]

When selecting a Path in Sweep, it seems important to select from this Path.

I don't know why this is so, but if I select from the area near the Profile, for some reason it does not succeed.

[Bunga777]

The Distance of the Path also turned out to be important.

We found that even if you select from the No. 1 Path, if the Distance is as shown in the attached image, you will succeed.

[RogerInHawaii]

That extra line was just one of my attempts to get it working, figuring that maybe the lines segments weren't exactly meeting up at their endpoints. But none of my attempts at fixing the problem worked.

I'm quite surprised that by just deleting that extra line you got it to work.

Very weird.

[RogerInHawaii]

It's that "for some reason" tat's got me baffled. I tried a whole bunch of things and couldn't get it to do the sweep as intended.

I WAS able to get MOST of the grooves made, but for many of them I had to break it down into more than one Sweep operation in order to get the entire groove.

Plus, I'm still encountering odd problems and errors. Please take a look at my next comment in this thread.

[RogerInHawaii]

I was able to get most of the grooves made, although for some of them I had to break a single Sweep into two or more separate sweeps to get the entire groove.

But now I've encountered another problem.

It's on the same model rocket body, made the paths in the same way by creating a sketch that consists only of the intersection of a plane and the rocket body, which I'm pretty sure SHOULD create a nice contiguous path (no breaks between lines). The profile sketch is again just a simple circle. But when I tried to do the Sweep it generates and error.

I then simplified it. I selected to have it make a Body (instead of a Cut). I selected only the upper half of the circle. I selected the Path (didn't matter where along the path I selected, it always appeared to select the entire path). I also selected to have it follow only one direction of the path. Once I did all that it popped up an error, that

"The sweep would intersect itself".

which makes no sense to me. I have other Sweeps that go along similar curved paths and they worked just fine (well, most of them).

So, I grabbed the arrow at the end of the path and moved it back up the path so that the arrow (the endpoint of what it's going to try to make the Sept body) was up in the very top-most, initial straight line of the Path. And I got this . . .

And as you can see it's OK with creating a body from what I selected.

BUT, then I moved the arrow to be just past the point where the straight line connects with the first curved line, and I get this:

The body disappeared and instead I get an error. Again, that

The sweep would intersect with itself

But how can that be? Other Sweeps worked fine on similar paths. Plus, I only selected the upper half of the circle, so how could it possibly intersect with itself while following the path. I also tried both the Parallel orientation and the Perpendicular orientation to see if it made any difference. And it didn't. Same error each way.

Is this a BUG? Is it behaving correctly and I just can't figure out why and what I have to do to make it work?

[laughingcreek]

I was able to get it to work by putting the center of the circle profile on the path,

BUT

there is definitely some weirdness going on that seems buggy.

If I take your originally attached  file and do nothing but change the sweep from "cut" to "new body"-

the SOLID sweep creates a SURFACE body-

this is clearly not the expected result.  seems like a bug to me.

@jeff_strater ?  thoughts?

[RogerInHawaii]

Thank you for looking in to this.

There were also times while I was trying to get it working that it seemed to use just the circle itself as the cutting device, not the circle PROFILE, but just the edges of the circle. All very weird.

I'm attaching the design that I forgot to attach to the prior message, the one where I try Sweeping just the upper half of the circle. It should show exactly what I was doing when this particular weirdness happened.

[TrippyLighting]

Instead of all these sketches I would actually use the split faces tool to have edges to select  instead of sketches and then I'd use the pipe tool instead of a sweep. At least for circular profiles.

Generally I try to use as few sketches as possible and prefer to work with edges as that is much more stable.

[Bunga777]

@RogerInHawaii 
Oddly enough, I was attempting the same thing.

Distance seems to be very important in this case.

I presume it is a kind of bug, however, this model has a number of alerts on the history, and there are concerns that cannot be said to be a bug. I have tried to resolve those alerts, but it seems to be beyond my ability.

[TrippyLighting]

After inspecting the model a little closer I am not surprised some "oddities" happen.

The Inspection menu has all sorts of tools to inspect surface and edge quality. Curvature map, Zebra Stripes, Isocurve analysis, curvature comb. When using those, one very quickly discovers that the surfaces and edges are of rather questionable quality.

A more experienced user will be able to determine this with the bare eye!

The reason for this is almost always the same:

The loft inputs are inadequate:

1. Use of fit point splines when control point splines would have been more appropriate.
2. Too many spline control points.
3. To many loft profiles created with simple tangency (tangency might be OK, but ...
4. ...but then the Keep tangent edges check box was not checked.

@RogerInHawaii Your ever more intricate and complex models deserve better 😉

[RogerInHawaii]

So you're saying that it's the Bodies in my design that are not quite right, and it's that which causes the Path sketch to sometimes end up having lines that aren't properly connected.

If that is the case, then I find it odd that when I'm using the Sweep Tool and selecting the desired Path (which had been created by the Intersection of a Body and a Plane) it does indeed allow me to select the entire set of lines of the desired path, implying (to me) that those lines are indeed perfectly valid as a Path. But apparently they're not, apparently sometimes the endpoints of the various lines constituting the Path are in fact NOT properly joined, and they are (sometimes) that way because of the parameters I had used when doing the Loft operation that created the Body.

I would expect that, since the Sweep Tool apparently recognizes that the lines of the Path aren't properly connected WHEN it's actually trying to do the Path operation, it could also recognize that at the point where I'm initially selecting the path and it should ONLY allow me to select a properly contiguous path. Instead, it lets me select the entire path IN SPITE of the fact that the full set of selected lines are not properly contiguous and the Path operation will indeed fail to use the entire selected path.

Now, if, while trying to select a Path, it only left me select properly contiguous lines, it would be obvious RIGHT THEN that something was wrong with the desired path. I'd still have to ask for help, ask why it's not selecting the entire path that looks, to me, like a perfectly valid, contiguous path, but at least it would better isolate the problem.

It is absolutely true that I'm designing "ever more intricate and complex models". But then, Fusion 360 is incredibly intricate and complex. We learn as we go. I've watched dozens and dozens of videos, doing the best I can to understand all the intricacies of it. It would be incredibly helpful for all the people learning Fusion 360, if every dialog, every menu, had an information icon that could be clicked to bring up explanations of all the various options on the dialog, perhaps even with a link to a video that explains the options and the impact of those options. Even if an engineer is learning Fusion 360 as an employee of a huge company, it's likely that the person is expected to learn it mostly on his own. Having "training" built in to the product would be incredibly helpful.

[TrippyLighting]

I apologize for my overly critical tone. I guess that comes with the occupation  😉

I indeed suspect that some of the profiles are not properly connected when using sketch intersections. This has been a long standing problem with Fusion 360 sketches. Also, the sweep command is a bit temperamental in some situations. 

This happens more often with loft that are somewhat problematic, e.g. have curvature problems.

These are areas that we have no control over but I would hope the Fusion 360 can improve the tools.

The only control we have is to create very "clean" lofts". Even that doesn't work every time. What I suggested are simply techniques I have found to provide more reliable solutions. You are unlikely to find those in any videos from the usual Fusion 360 YouTubers. 

[RogerInHawaii]

Someone had suggested using the Pipe Tool since I was just trying to Sweep a circle. So I just gave that a try.

I selected the Path, and even though it didn't select the ENTIRE path I figured I try anyway. I left all the other parameters at their defaults, in particular the Section Size, which was set at 0.01 inches by default :

And it worked. I don't actually want it to be 0.01 inches so I changed the Section Size to the value I want, which is 0.025 inches. And it FAILED. It's OK with the default of 0.01 but doesn't like 0.025.

I tried several different size but it appears that anything other than the default causes a failure.

I tried selecting the OTHER portion of the Path and that FAILS even for the default Section Size.

I tried something else. I deleted some of the lines of the portion of the Path on the Left so that all was left was a single curved line on the left side, so that I'd only select that single curved line as the path for the pipe.

I then did indeed try to make a Pipe, selecting just that single curved line... 

And it reported an error that it would produce a SHARP CORNER. ???? What ???? There's no corners in the curved line. But then I zoomed in on the upper end of the curved line and it does indeed, kind of, look like it thinks there's a sharp turn. But that turn is OUT OF THE PLANE of the curve. How can that be a part of the sketch??

[jhackney1972]

Using your original posted model, the Pipe tool seems to work using the diameter you specified in your original sweep sketch.  Model is attached.

[RogerInHawaii]

Yes,  the pipe tool worked for SOME of the paths, but for others it failed when I tried a Size different from the default, including the size I've been using for the Profile circles.

I DID finally get all the grooves done, but I had to take a real round-about approach. I created the Path sketch in my normal way, doing an intersection between a plane and the body of the rocket. But then I dropped Points all along the Path, DELETED the lines and curves that had been made by the Body/Plane Intersection, and joined all the points with a Control Point Spline. That final spline (basically replacing the lines and curves from the Body/Plane Intersection) was accepted by the Pipe tool and created the desired pipe, as a Body. I then did a Cut Combine between the rocket body and the Pipe, discarding the Pipe body. And, ta daa! The desired groove.

I did that for every one of the desired grooves that was previously encountering problems.

So, I have a solution, but it still leaves the question of why both the Sweep and the Pipe tools sometimes don't like using the Path sketch created by a Body/Plane Intersection operation. I'm still thinking it's a bug in Fusion and not simply that my model is "too complex".

Here's what my model looks like, so far.

[TrippyLighting]

Here is what the bugs in your timeline look so far:

[TrippyLighting]

This is what the isocurve analysis shows on the surface that creates most of the problems:

That doesn't look too good.

I also noticed that the sketch intersect profiles start disconnection on that surface and a single pipe won't work.

So I removed some of the profiles (3, or 4) from the front section so the loft has fewer constraints.

After the timeline re-calculated all the sketch profile connected and I was able to create a single pipe tool cut.

In general I would approach this loft very differently. It's more loft work, but less sketch work and usually creates pretty clean geometry.

1. Only sketch/loft half of it

2. No fillets in these sketches, just sharp edges.

3. A start and end profile connected by 2 or 4 rails.

4. Loft, then fillet. A variable fillet could work, but I would likely use sketches and trim the main surfaces and then loft fillets.