Strange revolve tool behavior


Dear fellow-shaprs,

I hope to get some clarity from the staff about a strange behavior of the revolve tool (and hopefully a fix anytime soon).

In my task of creating true-to-standard ISO-metric threads I always got stuck with the revolve-tool not allowing for a full revolution (aka 360deg) with a height of the sidelength of the revolved equilateral triangle (which guarantees the standardized 60deg flange angle).

As in the pictures below revolution settings of 360deg/10mm are not accepted.

Anything above and close to 10mm is okay:

But if you enter 10,0001 as the height Shapr3D rounds it to 10mm and accepts it:

I just managed to create a 0.75mm revolution for my 0.75mm triangle by entering 0.7505 as the height for my thread, but this is a really annoying behavior of the app…

Please make creating threads more easy - I can’t believe that your targeted professionals
are content without the possibility to reliably create standardized threads when it comes to real-life design and not just visualization.

Regards from Germany



Nice depiction!




Thanks for all the profound collaboration taking place here…

My example with a 10mm triangle was just to be a bit more generic and to get away from my .75mm extra fine thread, because the maths are independent if we use a 5mm or .75mm pitch, or even a 5 inch pitch if we make the leap to real big assemblies.

In each of those examples the pitch width means that the distance between two corresponding points on adjacent thread-lines (I think you know what I mean here) is exactly this pitch.
The construction method we use here is to substract a revolved, equilateral triangle from a shaft of given width to get the characteristic cutout with a flange angle of 60deg.

To get the theoretical precise dimensions we use a triangle with a sidelength corresponding to the sought pitch and revolve it one complete revolution (360deg) over the length of one pitch.

This method should yield the thread with the characteristics corresponding to the ISO definition.

So, that’s the theoretical description of the process…
Criticism is very welcome!

Cheers Chris



All screenshots of my examples correspond to a 10mm pitch.

The last sentence should have been a little more clear in stating that I also (besides the depicted example) managed to achieve the same result with a .75 pitch.

Sorry for this slight imprecision.

Cheers Chris


I also made a test with the sweep tool the circle radius was 5mm, and 4,999 mm.
With the 5mm was same result. After with the 4,999 mm radius I made a section from the tubes. The distance was 0,002.
i think in the program not possible the thouching surface when using the sweep comand.
BUT after i made an offset from the cilinder edge and the result is no rounded :>> spline


Let‘s hope that someone of the staff will jump in and clarify things.

Perhaps there’s a person out there with a background in thread-modeling and can shed some light on our findings…

Are the other desktop-programs behaving in the same way?

Let‘s wait for further insight.

Cheers Chris


The reason why the revolve fails in that case, is because it generates a non manifold body (the two vertices would meet). When you set it to 10,0001mm, it will actually change the height of the spiral (we just don’t display the all the digits), thus make it a regular manifold body, because the 2 vertices will not be coincident then.

It doesn’t fail in Fusion because it allows creating non-manifold geometry. Most CAD systems do not allow the creation of non-manifold geometry, Fusion is an exception.


Absolutely correct … 2 regions/doodles conflicting for a similar space … Some allow conflicts others prefer not … most prefer not… :crazy_face:


I think we should make a thread tool :slight_smile:


Yeah!!! I strongly (!) second this…!!!

Thanks Chris