Impossible twisted Lofts?

[tormy.vancool]

Hi there

I was trying to design this object gear (Fig. 1) that I have already designed in Solid Edge, with Fusion 360 Personal Edition.

beside some small orientation error, I achieved this in Fig.2, but as yo ucan see the conical gear has 2 main issues:

1. some incorrect profile ONLY on one "tooth"

2. the conical shape is slightly turning (not able to turning more) and it's NOT helicoidal, as it should be from Fig.1

For the point 1 I think it's an old issue of Fusion (please confirm or correct me)

For the point 2.

I tried with "lofts" but they can't be twisted.

I tried with "sweeps" because they can be twisted, but they can't be lofted (I mean to terminate on different size shape than the original). "Tapered" doesn't do the job.

After several trials I just gave up and decided to ask to you suggestions.

The tutorial about the making of this part is here: https://www.youtube.com/watch?v=8ugL36boEX0

In attachment you find the file Solid Edge Part 32 v17.f3d .. why "Solid Edge"? Because i'm studying 2 CADS. Solid Edge and Fusion. And each object I have made in Solid Edge, I repeat it in Fusion. Till now I have made 31 objects without any problem. Just detecting the differences between the 2 CADs and managing them (learning a lot). But with the 32th I'm stuck.

Perhaps it's due limitations in the Personal Edition

Perhaps is due my lack of knowledge in Fusion 360

Perhaps is something else

Please help

Fig. 1 - OBJECT TO ACHIEVE

Fig. 2 - TWO MAIN ISSUES IN FUSION 360

[TrippyLighting]

I would suggest before moving to lofting, that you step up your sketch game.

Mirroring and patterning in a sketch is not a recommended practice for any parametric CAD software, including Solid Edge. You can get away with that in SolidEdge as it has a much more mature, stable and faster sketch engine (but 2D only!), but in Fusion 360 that's a recipe for failure. Fully unconstrained sketches a very dangerous and a performance nightmare.

[TrippyLighting · Accepted solution]

The loft fails because Fusion 360 gets confused in adding edges. This is a bug @Phil.E 

You should be able to work around this and create a computationally faster model by lofting a single tooth and circular patterning the loft feature in the timeline.  

[tormy.vancool]

Ok I wrote an answer meanwhile you posted another comment. I read it then I will be back

[tormy.vancool]

So far I understood, I have to redesign the gear keeping each tooth separated and the main internal circle of the gear, then lofting the circle and then tooth-by-tooth. Am I correct?

[tormy.vancool]

Ok perfect, and on top of what I asked with the "immediate reply",  my question is: how can I get the twisted shape?

[TrippyLighting]

You only have to loft a single tooth.

Then you create a circular pattern of the loft feature.

I believe the cone in your design is not a straight cone. It has some slight curvature to it. Is that desired ? 

[davebYYPCU · Accepted solution]

What Trippy said, from your geometry

Add Centre Circles, aligned / snapped to the tooth floor.

Loft the 3 circles - are thay constructed correctly?, the centre sketch is not providing a straight transition, it is slightly undersized for that, so the result is slightly concave (non cone).

Then you can Loft one tooth, the twist is not very pronounced, and I found the video way too slow, and not how Fusion works, anyway.

Might help...

[tormy.vancool]

Yes the whole gear is not exactly conic but a bit concave and the teeth are twisted. but they should be more twisted than what I was able to get in Fusion

Please in attachment the PDF I created in Solid Edge.

So your suggestion is to design the circular pattern and One tooth, loft them and then eventually round-pattern the tooth creating the other teeth? 

Yes the video is slow and confusing also. the other videos he have made are more clear, but this one created difficulties already on Solid Edge ... I just naively hoped do not find issues in Fusion, but I got them.

[tormy.vancool]

ok following your suggestions I finally got this result.

It's not yet identical to the project simply because didn't respect the sizes of the smaller sections. I just tried to check if I fully understood your indications.

I designed the main circle with 1 tooth.

Copied it (not projected. it's not editable. So only copied) on a dislocated planes.

I scaled down only the circumference (0.8 the first copy and 0.5 the second)

I rotated the 2 copies not linearly (10° the first and 30° the second)

Then lofted

I've made a circular pattern of the created body (the whole one, because to select the single tooth it was not possible, so I selected the whole body and patterned 12 times)

Yes I smashed my face against the bug od Fusion as wel, I corrected it by manually moving the points. I hope this bug will be solved soon. Meanwhile here below what I did. Thank you to both of you.

[davebYYPCU]

See if this works for you, 

pic of my sketches taken before I found the PDF, thanks it helps...

Conic Helix gear will twist as expected with correct dimensions. You had 5 and 15 degrees, but the PDF is 30.

I put the loft rail centre point at 15 (actually 75 in the sketch) but can be edited.

Shortest timeline I could get....

Sketch 6 is a 3d sketch , 

blue lines white points should keep you awake.

Happy to answer questions.

Might help...

[davebYYPCU]

Trick to the Circular Pattern, pattern Features - selected from the Timeline, (Sweep and Loft)

Both were created as Join, so only one body at the end.

What bug?  I didn't find it.

Might help...

[tormy.vancool]

The bug is highlighted by Trippy here: https://forums.autodesk.com/t5/fusion-360-support/impossible-twisted-lofts/m-p/12262317/highlight/tr...

I try now your suggestion for the pattern

[tormy.vancool]

Splendid!

yes my Fusion 360 file differs from the PDF because when I was using in Fusion the degrees of the PDF I got a disaster due the bug Trippy highlighted. I wanted to figure out what was the problem, so i diminished the rotation.
The PDF has the correct data

[davebYYPCU]

Ah, yeah, probably because you asked Fusion Loft to do too much with insufficient info.  3 sketches and 12 teeth in each, no rail, nightmare looking for someone to bite.

My loft is 2 profiles and 1 rail. sweet.

Might help...

[tormy.vancool]

The elegance of your design is jaw-dropping for me. I have a question: how did you draw the curved path for the loft in the conical twisted gear? The Sketch6. I mean there is a curved line.

[davebYYPCU]

Create Sketch.

Enable 3d drafting, Sketch Pallet bottom tick, but you have to also enable it in Preferences first (just once).

In this Sketch it's

Sketch > Project> Include 3d Geometry.  Select the mid point / end points, as required (3), 

Then coincident connect the 3 point spline to the purple points.  Done.

Might help....

[tormy.vancool]

Thank you really so much.

[jeff_strater]

This is a "loft default point mapping" issue.  Basically:  Loft has to try to map between points on each profile.  It is harder than it looks - there are a lot of points here, and the helical nature of this loft probably confuses the algorithm a bit.   You can fix it a number of ways.  You can drag the white dots in the preview to try to "untangle" the twisted edges, which is possible, but can be tricky.  Or, you can add rail curves.  Usually just a single rail curve is enough to avoid the confusion.  However, in this case, just lofting the other way seems to avoid the problem.  Not sure why, but it gets around the issue...

[tormy.vancool]

In act all the times I've made the loft, it was like the second one you shown. But getting the twisting issue.
Yesterday I applied the suggestions they gave me above and not only I learned something more about Fusion, but I was able to make it.

One question about what you wrote:
"Or, you can add rail curves. Usually just a single rail curve is enough to avoid the confusion."
Do you mean that it's sufficient to draw only one rail curve, and automatically all the gear teeth will be correctly made?