I took a look at your file, there are a few things to discuss, first focusing on your first setup (with the carbide 3D #102 1/8" endmill):
- Let’s ignore the first operation of boring 6 holes, I suppose you intended to clear the descent path for the upcoming toolpath, but you should use ramping instead (as you figured out in later toolpaths)
- then your first 2D adaptive toolpath begins, but the way you defined your selections, it does straight a down plunge, then starts “adaptive clearing” at a depth of 0.47".
The problem is, at this stage you have not removed any material yet, so what this ends up doing during the first moments of the cut, is a 0.5" deep slot, as shown on the beginning of the simulation:
0.5" is 4 times the endmill width, so your are slotting at 400% DOC, while a conservative value is around 50%. The feeds and speeds also make things harder for the spindle:
9200 RPM, 50ipm for this 2-flute endmill is a chipload of ~0.003". That’s three times what I would usually start with for a 1/8" endmill in hardwood. So long story short, no wonder you spindle stalls
You second set of toolpaths is much closer to what needs to be done : helical ramping down to full depth, and nice large adaptive arcs:
Your feeds and speeds in this one is also much more reasonable (0.001" chipload), so that should work much better, but doing the full 0.62" depth of cut in one go may still be hard on the endmill/machine.
Side note: those yellow lines indicate that the tool will fully retract between each arc. To avoid this, you can set the “retraction policy” to “minimum retraction”, and you end up with this:
I have no time to check the project in further details tonight (it’s getting late this side of the pond), but hopefully this can give you a few pointers, and I’m sure others will chime in.