Tag Archives: threadmill

Update on Pocket NC v2-50 Threadmilling

After machining a fair number of parts with threads, I’ve tweaked my thread milling feeds and speeds to both go a little bit faster, give a more reasonable fit, and remove the last bit of niggling interference with the M2.5 recipe.

I’ll list the changes here, and have updated the original recipe

Old New
Chamfer Width 0.10mm 0.05mm
M3 Pitch Diameter Offset 0.538mm 0.568mm
M3 Stepovers 10 6
M3 Repeat Passes NO YES
M3 Lead To Center NO YES
M2.5 Pitch Diameter Offset 0.430mm 0.480mm
M2.5 Stock to Leave 0.0mm -0.02mm
M2.5 Stepovers 7 4
M2.5 Repeat Passes NO YES
M2.5 Lead To Center NO YES

Notably, the “Lead To Center” option found on the linking tab is what prevents the M2.5 threads from rubbing when inserting in later passes.  Thanks to Quincy Jones from Implemented Robotics for that tip over in the mjbots discord!

 

Thread milling on the Pocket NC v2-50

UPDATE 2019-11-27: The feeds and speeds have been tweaked based on further experimentation.

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.

 

M3 M2.5
Hole
Tool Datron 2mm single 5mm flute 0068620G “”
Stickout 14mm “”
Feedrate 400 mm/min “”
RPM 42000 “”
Ramp Angle 2 deg “”
Stock to leave -0.02mm “”
Top height +1.0mm “”
Bottom height -0.5mm “”
Chamfer
Tool Shars 1/8″ 90 chamfer 416-3509 “”
Stickout 18mm “”
RPM 8500 “”
Chamfer width 0.05mm “”
Chamfer tip offset 0.5mm “”
Thread
Tool Lakeshore Carbide 3-SPTRMLB “”
Stickout 16mm “”
Feedrate 300 mm/min “”
RPM 10000 “”
Pitch 0.5mm 0.45mm
Pitch diameter offset 0.568mm 0.480mm
Stepovers 6 4
Stepover 0.05mm “”
Repeat Passes YES “”
Lead To Center YES “”
Top height +1.0mm “”

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.

Results

Here’s a video machining a few M3 and a few M2.5 threads in the same operation, then testing them out.