Helix generated via three techniques differ

[threeleggedcat.shop]

Hey folks,

Here are three examples of creating a helix with a circular profile. Any cross section bisecting the helix center point should display perfectly round circles. The ultimate goal is to have arbitrary shaped profiles.

The enclosed screen shot is a cross section of helices produced by three generation techniques:

1) The coil tool produces the leftmost helix. Cross section is round. Nice. Alas that one can't use profiles other then circles, triangles or squares! That would be problem solved.

2) The sweep tool produces the helix on the right with a straight path and a twist angle. It's pretty good. Bit tricky to get the angle right, but that's just me.

3) Middle body is a combo of coil tool, plane on path and sweep. Seems straight forward. Use the coil tool to produce a triangular helix body. Inner line is the path, outer vertical surface is the guide sfc. Plane on Path at start (zero) of path. I'd like to use the method but it does not produce circular cross sections. Somehow the plane on path is at the wrong angle (?). Is there anyway to make this technique work?

thanks,

mark

ps: the yellow circle in the screenshot is a round ball same diameter as the helix profiles.

[TheCADWhisperer]

@threeleggedcat.shop 

Helix in Fusion has never been right.

The Fusion developers should "walk across the hall" and ask their Autodesk Inventor Professional teammates how it is done.

[laughingcreek · Accepted solution]

instead of using math to figure out the angle for the profile construction plane, let fusion do it for you.  do a surface sweep using the same parameters as your eventual solid sweep, and put a plane along path on the edge. 

to get the cross section profile to be correct, put your profile on the ordinate plane, then project that in a sketch placed on the plane along path. use the projection for the sweep profile.

see attached.

[TheCADWhisperer]

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@laughingcreek wrote:

...then project that in a sketch placed on the plane along path. use the projection for the sweep profile.

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Not correct geometry.

[threeleggedcat.shop]

Yes!  I used the coil tool vs a formula and sfc sweep.  Silly me.  Thanks for pulling this together.  And the TheCADWhisperer has it right!

Another solution is to use the coil tool (any profile should work), put a plane on an end and profile there.   Think I'll stick to the formula.  In my designs, many different profiles follow the same helictical path so doing the complex stuff up front followed by many but simple to remember elements is the design goal.

For another time... what/why the difference between the planes on path generated by a coil vs a twisty sfc sweep?

mark

[laughingcreek]

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@TheCADWhisperer wrote:

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@laughingcreek wrote:

...then project that in a sketch placed on the plane along path. use the projection for the sweep profile.

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Not correct geometry.

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gah.  right, not correct geometry.  only reason I tried using a plane at an angle was to get over fusions limitation of not being able to sweep a profile that is parallel to the path (which should be possible once a twist angle is used).

maybe was over thinking it.  just using construction plane that is angled .000001 deg off path seems to work, and produced geometry well with in manufacturing tolerances.  no extra sweeps or math needed.

attached i used a square for the profile to make results easier to check.

[johnsonshiue]

Hi! These results are legitimate. The variations depend on how the actual profile is consumed by the Sweep (Coil also uses Sweep). To get the expected cross section, you will need to orient the section plane onto the profile plane.

Another technique you may consider is to use Solid Sweep. In this case, you may create a sphere in the same diameter and sweep the sphere along the helical path. You will get a more consistent cross sections.

Many thanks!

[threeleggedcat.shop]

Hi,  I tried that but it failed.  Created a plane on path on the horizontal line ending in center of the circle profile used for the sweep, used that plane to create a ball 25 mm diameter at the line's origin, attempted a solid sweep with the helix side as the path and Z as the axis.  It actually drew the solid, but on "OK", decided it had an error.  See enclosed project. 

But thanks for the solid sweep idea... I'll keep that in mind for the future.  I'll stick to the sketch profile for now.

mark

[johnsonshiue]

Hi! It does look like a bug to me. But it seems to be related to the new body isn't associated with any part. Delete the failed Sweep feature. Edit the "Solid Sweep" part and recreate the Solid Sweep. It should work.

Many thanks!