How do I sweep a complex curving path while staying perpendicular to surface?

tim_martin786

I have managed to project a spiral path onto the inside of a bowl surface. So far so good. Now I'd like to sweep (I think) a line along that path and have it stay perpendicular to the bowl. The result should create a twisting spiral surface inside the bowl. Anyone have an idea how to accomplish this? Appreciate any feedback! Thanks!

Here is what I have so far: BowlSpiral

mahir

Check out Part Studio 3. I used a loft with multiple profiles and one guide curve. It's tedious to setup the first time, but it should rebult well if you tweak the bowl shape. The large number of profiles is so the inner portion of the loft remains spiral-shaped. Generating a second guide curve isn't possible as you know. This behavior should be supported in FeatureScript since there is a normal to surface option in the opSweep command, but it doesn't seem to work well.

@ilya_baran, any input on getting the normal to surface option to work in FeatureScript? I have a failed attempt at a custom feature in this same link.

https://cad.onshape.com/documents/a05aeff75e42296533f07199/w/3da90aff92f27b413a5f9fdd/e/1b69c22e4b6baa26f6c30545

Narayan_K

@ tim_martin786  , You can create a sweep.it will work for you?



https://cad.onshape.com/documents/57a0685fe4b00f18b475be73/w/51c670c4273a5bafa29edd8a/e/0b7fc6cd953c0376bb3f7eb1

tim_martin786

I can indeed create a spiraling sweep that runs along the bowl surface, however, how can I make the new surface stay perpendicular(normal?) to the inside bowl surface?

tim_martin786

As can be seen in the previous image, the spiraling surface starts at right angles to the top of the bowl, but as it traverses the path it loses this relationship. Is there another way to achieve the desired result? Would a loft be better suited? Anyone with ideas on how to proceed? Thanks!

mahir

The sweep isn't aware of the bowl surface - only the projected sweep path. The best you can do is maintaining normalcy to the sweep path. However, it's feasible to achieve something close to what you want with a loft using two guid curves. You could use the existing path as the first guide curve, but you'd have to project a spiral onto a smaller inner curve for the second guide curve. If the second curve matches the first one "just so", the effect will be to keep the surface more or less normal to the bowl surface. 

tim_martin786

@mahir, thank you for your comments! I attempted that route for a bit and found it challenging to create the second guide curve appropriately. The various curved shapes and projections became difficult for my brain to keep straight.  Then when I defined the loft I kept getting weird twists that were unexpected. (likely because I defined something incorrectly)
I was hoping there was someway to constrain the sweep line relationship normal to the bowl surface, but I guess not.
Since the bowl shape is likely to be modified often during our R&D development, it would be desirable to have the spiraling vane adjust "automagically" when changes are made to the basic shape... another reason I backed down from creating the second curve for a loft.

Maybe I could try creating additional planes/sketches along the spiraling curve defined similarly to the original sweep line and attempt a loft between the segments? Or maybe look into featurescript? (not sure I'm ready for that since I'm still learning the OS ropes)

mahir

Check out Part Studio 3. I used a loft with multiple profiles and one guide curve. It's tedious to setup the first time, but it should rebult well if you tweak the bowl shape. The large number of profiles is so the inner portion of the loft remains spiral-shaped. Generating a second guide curve isn't possible as you know. This behavior should be supported in FeatureScript since there is a normal to surface option in the opSweep command, but it doesn't seem to work well.

@ilya_baran, any input on getting the normal to surface option to work in FeatureScript? I have a failed attempt at a custom feature in this same link.

https://cad.onshape.com/documents/a05aeff75e42296533f07199/w/3da90aff92f27b413a5f9fdd/e/1b69c22e4b6baa26f6c30545

jon_sorrells

@mahir
The "f" in "lockFaces" needs to be capital

mahir

Thanks, @jon_sorrells. It's always the little things! @tim_martin786, if you use something like the Normal Sweep feature in my link above, that should exactly what you're looking for.

tim_martin786

@mahir, Wow! That is so sweet! Exactly what I needed!
Really appreciate the help! FeatureScript is definitely something I'll need to look into further as I become more proficient with things.
Thanks again! And thank you @jon_sorrells for the assist!

mahir

Yeah, I'm not sure why FeatureScript was even necessary. It seems like the "lock faces" option is already built into the sweep functionality. I suspect that at some point in the near future OS will probably update the sweep gui to include it. In the meantime, I'm glad I could help.

øyvind_kaurstad

@mahir: I'm trying to understand what you did, but I can't even seem to figure out the constraints applied in Sketch 3. What kind of constraint is this (highlighted in red):



It appears that the construction line is a two-point spline with pierce constraints to the top circumference of the bowl, and it also seems to be coincident with the bowl surface in the sketch plane, and I guess that is the shown constraint. However, for the life of me I can't figure out how that constraint is applied, and it is bugging me.  :-)

mahir

The construction spline was created as an intersection of the bowl surface and the sketch plane. That weird icon is the intersection constraint, available as a drop down icon along with convert edges. The profile line was then constrained to be normal to that spline - and therefore normal to the bowl surface. The reason the spline is shaped strangely is the sketch plane doesn't go through the origin. It was created as normal to the sweep path at its end point. 

øyvind_kaurstad

Aha! Then I learnt something new today! Great! Thank you!