Bottle Neck- SP400 Modified Buttress Thread (M-Style)

Bottle Neck- SP400 Modified Buttress Thread (M-Style)

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Description
Structural packaging design is one area I'm exploring. I enjoy bottle design in particular as it offers a lot of opportunity to explore form. But a respectable bottle will need respectable threads! Herein lays the challenge. When I attempted to make threads using current Fusion360 tools, I discovered the following: a) The Thread-Tool only makes standard machine thread profiles and pitches b) The Coil_Tool does not allow for sketching custom cross-sections c) The Sweep_Tool did not allow for constraining the orientation of the section as it moved along the helical rail I constructed. Thus I came up with a workflow that combines several tools and techniques to yield accurate, beautiful threads! Have a look at some of the process images.
Comments

Hi Patrick,
Here are two URL's that should put you on the path to finding the information you need.
Nice article on thread design and uses - https://cnocoutdoors.com/blogs/blog/lets-talk-about-threads
Thread Drawing Downloads - https://www.isbt.com/threadspecs-downloads.asp
Blessings,
Vince
aka SkillCoach

26 days ago

Hi Vince
where can i find models of SP410 plastic bottle caps
& plastic bottle necks or their dimensions so that
i can model them up.

26 days ago

Hi Dennis, I'll be happy to help step you through the remaining steps to model the threads. At present, I'm not certain which "not full cylinder" you are referring to. I'm guessing the cylinders that have been trimmed using the large and small helical coil features. Their diameters correspond to the height of the inner and outer vertical faces of the thread section. The loft tool was used to cap the top and bottom faces of the thread section. I've sent you a direct message so we can follow up and get your questions resolved. - Cheers, Vince

over 1 year ago

Hi Vince, I am also trying to make a 2L soda bottle thing. I follow what you are doing and thing it is an very cool way of going about it. The thing that has me, not being a Fusion 360 professional, is how do you create those two empty cylinders? Are they planes of sorts. I cannot for the life of me figure out how to create a cylinder that is not full and becomes a bar!

over 1 year ago

Hi Tim,
To date, I have not made a video of this workflow. I'm in the midst of developing new modeling tutorials for a CAD course I will be teaching at Virginia Tech. Perhaps I can incorporate an in-depth video of making threads. Fusion has a lot more functionality and there may be a more streamlined approach to modeling the thread profile. In the meantime, if you want to give a shot at modeling the threads or some other model, I'd be happy to review what you come up with and guide you through the build process. Feel to direct message me and we'll see what we can do!
Blessings,
Vince

almost 3 years ago

Hi Vince,
I have limited ability with fusion 360, self taught and only use to print hobbyist projects. I'm enquiring as to whether or not you have produced a video explaining the work flow as this would help me grasp the concepts that you have highlighted above ?

Kind Regards,

Tim

almost 3 years ago

Is there a way to download this file?

about 4 years ago

Jin,

Perhaps it's a settings issue within the loft command. When performing the loft there is a drop down menu that let's choose PROFILE or RAIL. You have to manually set each 3D curves to the desired type.

almost 7 years ago

It's coming along. Still trying to figure out all the vagaries of Fusion. For instance, it appears I cannot loft the spiral 3D sketch curves properly in model mode, they must be lofted as T-splines.

almost 7 years ago

Ok, Perhaps I remembered wrong regarding the need to caps the coils. To make the coils properly you need:
1) Create a PLANE - offset a distance down from the bottle neck and use it for the coil profile plane.
2) Select a TYPE - choose one that includes the pitch since the thread reference image tell the required pitch. (Revolution+Pitch) or (height+pitch)
3) Set DIAMETER - The coil diameters must correspond with the OD and ID cylinder diameters.
It is not necessary to work in the T-Spline environment if you have Design history turned on. With history you will be in the Model Workspace when creating the coils. With history off you would work in the Patch Workspace. I'd appreciate having the opportunity to see your finished work so hopefully you will be posting to the gallery. If not, let figure a way to connect offline.

Vince

almost 7 years ago

Okay, that was very helpful. How did you create your coils? I used the coil command, which does not require any end capping. Also, creating the 3D sketch curve (which I wasn't even aware was a thing) was key for the lofting, as you mentioned. Also, it is apparently necessary to be working in the T-spline form environment, which may not be totally obvious to someone new to Fusion 360.

almost 7 years ago

Jin,
Yep, you're getting it! Note though that it is not necessary to trim the coils. But, you do have to cap the ends of the coils and stitch before Fusion will allow you to use the coil features to split the ID and OD cylinders. Once split, hide the coils and then delete the unwanted portions of the cylinders. Also before being able to loft between the resulting helical surfaces you may need to create a 3D sketch curve from the edges, as the loft command asks for sketched geometry to use for profiles and rails. I've added some more images to reference.

Vince

almost 7 years ago

That gives me some idea of how to proceed. Just to be more explicit:
You have two cylinders with coils embedded in their surface. You intersect each coil with its cylinder to get you two half coils with flat outer facing surfaces, which you can then loft between to get your thread. Does that sound about right?
It's all very ingenious, thanks.

almost 7 years ago

Jin,
I had to figure a way to manually construct every face of the swept thread section. After which I stitched them together to become a solid body.
1) I use the circular helical sweeps to intersect two cylindrical surfaces, one corresponds to the ID or base of the thread section, and the other is an offset cylinder that corresponds to the OD of the thread section. The diameter of the circles was chosen to correspond to the need vertical heights of the thread section. I then use the circular helical sweeps to trim the ID and OD cylindrical surfaces, thus forming two faces for the tread.

2) Next I created the top and bottom faces of the thread section by lofting two surfaces; one using the top edges of the ID and OD faces, and the other surface using the bottom edges.

3) I then construct geometry to cap the ends of the helical sweep.

4) Finally, I stitch all the surfaces together to for a solid body that gets combined with the bottle neck.

Creating the run-off's at the ends of the thread required some special construction to make sure they were tangential to the sweep. But I'll let you play with that for now. If you end up needing assistance let me know. I hope this clears up a few questions.

Vince

almost 7 years ago

I'm trying to model a plastic bottle thread and discovered exactly the same issues you ran into. I must admit though that I don't quite understand your process. You model the thread profile, sweep two circular helixes, and then...?

Thanks for that M style thread profile photo, too, can't find that information anywhere.

almost 7 years ago

I really enjoy your eye for simplicity.

about 7 years ago

A beautiful illustration of your work flow! I think you are on the right track in your bottle design. I really like your "respectable threads for respectable bottle" concept. These kinds of bottles can be made by the "Extrusion Moulding (Molding)" method.

about 7 years ago
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Vince Haley | SkillCoach
Virginia, United States of America

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