On a Nomad 3, is there any rule of thumb to making holes.
For example:
If a hole is really big then that is obviously a pocket.
If a hole is really small then peck drilling could work.
Is there an area in between where the Nomad isn’t powerful enough to peck drill but it is also difficult to pocket and achive good chip evacuatation?
For example, in the 4mm to 6mm region I have been struggling with chip evacuation on aluminium even with a small single flute (it comes out aluminium coated) but I’m wary about putting in a large drill in a small machine.
I have a Nomad 883 Pro so my experiences are based on that version of the Nomad range.
For chip evacuation, I think you really need air blasting to continually blow the chips out of the cuts. This (for me) is crucial. Vacuum might work too, but I think it would be trickier when things are so small.
For a 3mm hole I would do a 2mm endmill with a inner profile, rather than a pocket. For 4mm, a 3mm or 1/8" inner profile… so, pocket is not always obvious.
Since adopting air-blast and preferring 2mm or 3.175mm single-flute endmills I’ve had no real issues with making holes up to 4mm deep in brass or aluminium at 10K RPM with 0.5mm or 1mm DOC.
Second the air blast - slotting or holes it really does help. I think the rule of thumb I have seen in a couple places is the hole should be at least 10% greater in diameter than the end mill diameter.
On a slightly related note, milling round holes near the same diameter as the end mill has an effect on speeds and feeds that is worth knowing about.
OK, all really useful replies. I do have the parts to add air to my Nomad, I just need to fab a bracket. I am using F360 bore operation. My current need is ~3mm hole with 2mm cutter. Does anyone have any advice on pitch/ramp angle to go along with the useful circular interpolation compensation advice?
@Julien is this why when cutting a square profile the router makes a higher pitch noise when hitting the corners of the job vs the straight lines of the squares?
Nope, the “corner” effect is just tool engagement increasing a lot when the tool enters a corner, because all of a sudden it cuts both from the side (as it was doing while running the straight line at a given stepover) and from the “front” (soon to become the new side, after it exits the corner, if that makes any sense). So the router temporarily struggles to cut much more material than during the straight lines (similarly to how it would struggle when slotting versus just cutting at the defined stepover)
To mitigate this corner effect, the usual trick is to go for adaptive clearing toolpaths, they eat up at corners in smaller bites,
rather than doing a brutal 90° turn
Or, if I remember well, there’s also a cool tool from @fenrus which will post-process a gcode file and slow down the tool temporarily in corners.
Not sure it helps, but looking back I have used the bore operation:
6061 aluminum
3.175mm (1/8”) Zrn coated end mill in a 5mm hole.
10,000 RPM (max for Nomad 883)
Lead in 762 mm/min
Ramp 333 mm/min
Pitch 0.05mm
Climb
This was a deep-ish hole so I used 3 bore operations stacked on top of each other with each operation using different offsets in the Heights tab. This in effect makes it ‘peck boring’ where the end mill backs out and allows the air blast to get in and blow things out more effectively.
