To date I’ve managed to not do any threading on the parts I’ve made on my Pocket NC v2-50. However, I’m about to do a number that require both M3 and M2.5 threads, so I figured it was time to figure out how to do it.
Online tutorials are kinda all over the place in both how you handle things in the model, and how you program the CAM. Some assume you model threads as a hole of the major diameter, some as a hole of the minor diameter, although none that I could find used the new Fusion 360 “threaded” hole type, which is what I wanted to use. That said, using the “threaded” hole type appears to be treated basically as a minor diameter hole with a minor caveat. You would expect that since Fusion knows the minor and major diameter, the “pitch diameter offset” would be relative to a zero tolerance thread, but in fact it appears to be relative to the minor diameter as if you had modeled a minor diameter hole. Oh well, I just experimented with increasing pitch diameters until I had threads that fit relatively tight for the two that I cared about, which fortunately can be both made using identical tools, although the M2.5 hole is only on the edge.
|Tool||Datron 2mm single 5mm flute 0068620G||“”|
|Ramp Angle||2 deg||“”|
|Stock to leave||-0.02mm||0.0mm|
|Tool||Shars 1/8″ 90 chamfer 416-3509||“”|
|Chamfer tip offset||0.25mm||“”|
|Tool||Lakeshore Carbide 3-SPTRMLB||“”|
|Pitch diameter offset||0.538mm||0.430mm|
Interestingly, Fusion’s simulation reports that the M2.5 holes have a collision when inserting the threadmill, not on the first couple of insertions, but on the 4th and subsequent ones. This does appear to occur in real life too, as you can hear slight interference when the tool is inserted. I don’t fully understand this, as I would expect Fusion’s CAM to just stick the tool down the middle the same way each time.
Here’s a video machining a few M3 and a few M2.5 threads in the same operation, then testing them out.