Custom thread or at least a helix function

[product-ID]

I really need a custom thread function (I design all kinds of bottle closures) where you can create a custom thread by sweeping a sketched profile along a helix without rotating or twisting. Something like this is now available, but you have to use a third party add-in that creates a approximation of a helix. When you use this "helix" you get all kinds of problems because of the inaccuracy of the approximated helix. The custom thread feature of Inventor or the helix function found in Soildworks (create helix from circle) would be fine!

[HughesTooling]

You can use one edge of a coil then Sweep with guide rail. The path is the edge of the helix and the guide is the vertical line. Can't attach the file to the ideastation so if you want any help post in the design forum. Don't use a projected include 3d of the helix as it's not as accurate as the actual solid's edge.

[product-ID]

Hello Hughes Tooling mentor,

Thank you for the suggestion. I tried to do the same, but got an error message (see picture below). The guide rail is in the same sketch as the profile, but I also tried to sketch the guide rail in a separate sketch on the same plane as the section.

I also tried to get a result with the sweep function (Path + guide surface) after first inserting a triangular coil. It gives a reasonable result, but as you can see the swept surface becomes divided into many sub-surfaces:

 

[HughesTooling]

Like I said start a thread in the design forum or do a search as there are already several threads. Did you use plane along path for the profile sketch? Then you'll need another sketch for the vertical line, this line needs to be at least as long as the height of the helix and aligned with its axis. You'll notice my swept surface is not segmented at all.

Mark

[HughesTooling]

@product-ID Take a look at the temp.f3d file in this post. It uses a sweep with a twist to make a coil, if you modify the circle in the sketch to your thread profile it should make a good thread. Take a look at the parameters for how I've created the plane at the correct angle.

Mark

[product-ID]

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Hello Mark, thanks for the link.

That seems to work fine, but my knowledge of mathematics is 40 years behind me. If I had to create all these parameters for every screw thread I would have to create (and change afterwards), I would feel very sad. 

Therefore I would prefer a simple workflow as in Solidworks or Inventor. Create a helix (where you can define pitch (or height), number of revolutions, start angle, taper angle, clockwise or anti-clockwise), create a profile (aligned with helix or just planar) and create a sweep using the helix and the profile, thus creating a smooth thread without subdivisions so that applying a fillet or something like that won't be a problem.

Workarounds are of course welcome when functionality is not available yet in the software, but a simple to use feature would in the end be preferred.

And I think a lot of users of Fusion 360 would welcome the presence of a (simple) custom thread feature :-).

Richard

[HughesTooling]

Not saying it's not needed but a sketch helix has been promised for years so you might need to wait a while. You can use a coil to generate an edge you can use. Like i've said several times if you need more help getting it to work start a thread in the design forum. I'm just trying to help you get something done, you can wait for your idea to be implemented but you might be waiting another 3 or 4 years.

Mark

[araasch]

I like the new thread tool.  The fact that it offers all kinds of standard threads is great.  However, sometimes you want a thread that is not standard, but is just slightly different than a standard thread.

It would be great if one could select the standard thread which would set a variety of thread parameters, but that a customize option would be available to allow one or more of these thread parameters to be changed as needed.

This would offer the best of both worlds, simplicity and speed for common tasks, but flexibility for when one needs it without the pain of starting from scratch.

Thanks,

Arlen Raasch

[Anonymous]

If there was just an implementation of equation driven curves than a helix or other mathematically driven curves could easily be generated. This would also potentially allow trajectory parameters to be set so that the section could vary along the trajectory.

[richardpaulfox1968]

Hi

There are few different threads about this same thing in the forums each with votes, if they could all be incorporated into the same thread then perhaps more chance of getting it voted through.

[Anonymous]

Adding API rotary connection threads to the library would help greatly

[Anonymous]

Something like the thread wizard in solidworks would be super handy to have.

[product-ID]

Hello asira_91 Explorer,
The thread wizard in Solidworks is fine for "normal" thread with a symmetrical "section". That won't do it for the kind of threads that I need. Threads in closures etc. have an asymmetrical section with for instance a 60 degree slope at the top and a 30 degree angle at the bottom. Also sometimes these threads have no straight edge, but are fully rounded at the tip of the section.
So for my purpose a sweep of a custom (sketched) section along a helix (without twisting or other deformations ! ) is what I would like to have.

[jetpack5]

This is a good workaround, but this is also a useful feature. Pro/Engineer has a good helix implementation also.

[HughesTooling]

@product-ID  Here's a screencast demonstrating how to sweep without distortion. The key is to use a vertical centre line as the path and the helix from the edge of a coil as the guide rail. I made this screencast for someone else but is a good example for threads as well. The first sweep is just to show how using a guide surface doesn't create clean surfaces, the second sweep done at around the 2.0 minute point uses a path and rail.

Mark

[product-ID]

@HughesTooling Thanks Mark, I tried to replicate your way of producing a clean sweep/thread. At first I was able to get the segmented thread (with Path + Guide surface) but the Path + Guide Rail gave an error (see below). After some experimenting I found out that this method works fine as long the end point of the Guide Rail does not stop at the front side of the profile plane. So, if you make a coil (the first feature), make sure it is between 0 and 1/2 revolution ( or 1 and 1 1/2 revolution etc.) and not between 1/2 and 1 revolution etc. Otherwise you get the error message. So if you have to make a thread which has 3,75 revolutions, you will have to make a 4 revolutions coil and after the thread has been made, cut away the 1/4 revolution you don't need.

So, it is nice to have this workaround, but it has still a downside. Therefore I would still like to have a proper feature in Fusion 360 to make custom threads 🙂

[HughesTooling]

@product-ID  Hadn't noticed that before. Another tip is if you have problems with a solid sweep, it will quite often work as a patch workspace sweep. Not just for threads, sometimes you'll get segmentation in lofts and sweeps made in the model workspace but you get clean surfaces in the patch, just need to patch and stitch the open ends. And yes I agree Fusion need a proper way of doing this, a custom option in the coil command would make it work like other solid modeling programs I've used. Would also need the option for the profile to be perpendicular to the helix or the axis the coil wraps around.

Here's a coil 3.75 turns in the patch workspace, as you noted this fails in the model work space.

Mark

[product-ID]

@HughesTooling Hi Mark, thanks for the update. Indeed a good way to get around the 1/2 to 1 revolution problem. A bit more work, but at least another "impossible" feature is now feasible 🙂

[HughesTooling]

@product-ID  I found this would still fail occasionally using the coil command.

Here's another way that seems reliable. A couple of notes. For the patch sweep you need 2 sketches, the profile needs to be on a plane that's perpendicular to the path, in my example the path is on the ZX plane and profile on the XY. In the screencast I make it fail by turning off chain selection and only selecting the helix, with chain on it seems reliable. Lastly you could save this as a template with parameters then insert into designs, break the link and modify. One more tip, with this method the path is not restricted to a line, you can create a sweep around any path.

Mark

[richardpaulfox1968]

Thanks Mark I'll give that a try.

Regards

Richard

[product-ID]

@HughesTooling Thanks Mark, looks good. Will try this method but it looks foolproof :-).