Modeling Custom Threads - Yet another thread

[M&GToolWorks]

Just as a disclaimer, I have been through perhaps a dozen threads and 3 or 4 videos and have not found anything related to this yet. I most certainly may have missed something. 

In solid works, I could easily draw a thread form, and then coil that thread form around a part in a specified pitch. 

Fusion has the "coil" feature, however I find it lacking. What would be fantastic is if the developers put under "section" a selection where you could select the profile you wish to use. 

In my case the part requires a 0/30 buttress that is timed. That means I must be able to specify WHERE the thread starts. 

How do I accomplish this in Fusion? 

[M&GToolWorks]

This is an time consuming but viable option for creating the thread form, then creating the profile, then lofting. 

https://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/screencast/Main/Details/e4faa73...

Then it needs to be rotational and imported into the model, combined with the existing model in its timed position. 

I found a post sometime ago mentioning how "custom threads" were a sign of poor engineering. I would argue the complete opposite. There is a reason Buttress, ACME, and many other thread forms exist. 

[etfrench]

Here's one way to create a buttress thread:

Notes:

All of the settings are exposed in the Change Parameters dialog.

The coil should be in a separate component (or subcomponent) to allow rotating it to the timed position.  A joint would be the best way to position it.  This may require adding a joint origin at the center of the coil.

[M&GToolWorks]

Thank you for the suggestion, however this is an 0/30 buttress thread. I tried making a coil and drew the thread form on each end of the coil, then tried lofting, but could not get the loft to function. 

As you likely know, the buttress typically has flats at the root and crest, this along with the 30 degree is prohibiting me from using a square coil and modifying it. Perhaps one of the users who is more knowledgeable about loft can show how? 

 "A joint would be the best way to position it.  This may require adding a joint origin at the center of the coil."

How is this done?

[etfrench]

No lofts are needed to manipulate the coil's profile:

Screencast will be displayed here after you click Post.

2ab344c0-28d6-4dab-9e28-02434e7b7dac

Notes:

A little math will give you the settings needed to get the 30 degree angle (or just model it separately and use the dimensions when chamfering the coil). You can use the end face of the coil to verify the thread shape.

Chamfering one of the ends and creating the relief at the other end can be done with the method shown in this thread.

p.s. I don't think the forum software likes your name

[TheCADWhisperer]

Autodesk Inventor Professional is the Autodesk product equivalent of SolidWorks, not Fusion.

This is quite simple in Autodesk Inventor Professional.

[HughesTooling]

A big problem with coil is the profile is not perpendicular to the helix but perpendicular to the coil axis. This means a course pitch squashes the height of the profile.

To work around this you can use a coil as the base for a special thread and rotate the end faces to match the helix angle then sketch on the face.

For the sweep use a sketch with the profile and one with a line that's along the axis and the same length as the height of the thread, needs to be from the top of the profile to the top of the helix.

In the sweep select the vertical line as the path and the edge of the helix as the guide. Use the edge of the solid, don't use project include 3d geometry as it's not accurate. You can use @etfrench idea for simple flat sided threads but this method should work with odd profiles.

See attached file

Mark

Edit. Updated file as I found a problem if you were not using full turns for the helix.

[mroek]

@HughesTooling: That looks like a good method, but one question: Instead of calculating the angle and then rotating the end face of the solid before sketching on it, wouldn't it be just as easy to create a "Plane on path", using the edge of the solid as the path (positioning the plane at the end of the path), and then sketch the profile on this plane?

[HughesTooling]

@mroek Yes you're probably right. I've used a method similar to the one @etfrench demonstrated but rotated the end faces to make them perpendicular to the helix to make it easier to work with and I think that idea mislead me here.

Mark

[M&GToolWorks]

Hoping to have time tomorrow to work on this and between the suggestions get it accomplished. 

Really irritating that it is this difficult. 

[schngr]

Does Autodesk have any plans of adding a custom coil profile feature to Fusion? Making a buttress or acme thread shouldn't need to be this involved. Other CAD tools readily support a custom helix profile.