Thread milling with Simturn boring tool

I need to create the M16 x 2.0 thread in the solid pillar for the Multifix toolpost. I don't actually have a tap for this thread size, so my plan is to mill it using a single point tool. Or more precisely, I'll use the Simturn boring bar with an internal threading insert. When I bought the boring bar from Cutwel, I bought profile, threading and boring inserts (2 of each). 

The threading toolpath is easy to set up once you have a suitable tool in the tool library. But therein lies the issue. The "threading tool" function in the tool library seems to have some sort of  "bug" ie the software engineer in charge fucked up and didn't test it properly. The result is that when I try to create a 3mm tool with a diameter less than around 12mm, the cutter profile created gets screwed up.

I posted about this on the Fusion manufacturing forum, so not much point recreating it all here. Sure enough, they seem to have fucked up.

Finally bit the bullet and created a form tool instead of persevere with the thread tool feature. The dimensions are all given in the datasheet for the DX tools.

This did the trick. CAD model visible:

CAD model hidden. You can see how the toolpath is expected to look.

Off we go. I mean, what could possibly go wrong etc

"Pitch diameter offset":

Went OK although I had to play with the "pitch diameter offset" setting in the thread operation CAM dialogue box. This wasn't well explained. 

You need to start off with a bore of the right diameter, ideally the root diameter of the thread. Then based on the form of the tool, root and crest, you need to specify the "pitch diameter offset". WTF is that? It's basically the amount of infeed you need to achieve the required thread depth.

John Saunders has a video on the matter, which helps to lay out some of the basics:

Metric thread dimensions - the theory:

It's not a black art but equally the dimensions of the std metric thread form are not necessarily obvious. There's a pretty reasonable, copyright-free summary on Wikipedia.

In short:

• The "major diameter" (in my case 16mm) is measured to the flats of the crest, not the "pointy" tip of the triangular form.
• The flats of the crest account for 1/4 of the pitch length.
• The flats in the troughs account for 1/8 of the pitch length.
• The 60 degree angle gives a height to pitch (H:P) ratio of cos 30 ie (sqrt 3) / 2
• The "effective pitch diameter" is positioned on the centre line ie midway between the "pointy" bits. This is not the same as the mid point between the crest and trough.
• The "pitch diameter offset" is calculated based on the radial difference between the flats of the crests and the troughs.

That all seems fairly reasonable. However, if you are dealing with Fusion 360 (or taking guidance from John Saunders), for an internal thread you need to set the tapping hole diameter to the correct dimension to begin with, as the other settings are derived from it. So rather than simply dimension the hole as a nominal 14mm perhaps, you might want to enter the correct dimensions in Fusion:

      Dmajor = 16mm

      D1 = Dmin = 2 x 5/8 x 0.866P = 1.0825P = 13.835mm

      Dp = Dmajor = 0.6495P = 14.70mm (for completeness - not required in Fusion)

And finally, if you have pointy tools with no flat (that generate no flat in the trough), the infeed needs to be increased by the depth of those flats. In my case for an M16 thread, this means a total infeed of 3/4H ie 1.299mm. This assumes the tapping bore is the correct 13.835mm diameter to start with and actually results in "pointy" troughs at a diameter of 16.432mm. 

Do it:

Here's how it worked out for me. This is the final pass - yes, I had to do a bit of trial and error in the end. 

Looks good to me and fits pretty nicely.

The final uncertainty is over the effective radius / diameter of the tool point. I could probably do a test cut and determine it by measurement. However, I think it's fair to conclude that the effective radius is NOT 5.5mm, as suggested by the datasheet for the insert. If I can be bothered, I may make a test cut and measure it. Time will tell.....