.
I've been pretty good at "guessing" speeds and feeds for endmills which come out very close to the formulas you suggested but what about calculating cutting info for drills? General rules?
Peck = (1/2 drill diameter?)
Feed = ?
Speed = ?
dstryr-
The guidelines I showed work well for drilling also, although typically you can be more aggressive on the chip load/feed than the guidelines show.
For example, lets calculate the feed and speed for a 1/2" HSS drill bit in mild steel.
RPM = 4 x SFM/Diameter = 4 x 100/0.5 = 800 RPM
Chip Load = Diameter/200 = 0.5/200 = 0.0025"
Feed Rate= RPM x Num of Teeth x Chip Load = 800 x 2 flutes x 0.0025" = 4ipm
But with drilling, this feedrate will be on the conservative side, look to bump it up if the machine can handle it.
Regarding pecking, I follow the rule to go 2 x Diameter on the first peck, and the 1 x Diameter for each peck after that. Note that like a lot of the info in these guidelines, I believe I "borrowed" this suggestion from one of Stan Dornfeld's posts.
Keep in mind that these guidelines "get you in the ballpark". If you are making a lot of parts, I'd go to the manufacturers websites for the cutting tools you are using and look at their recommendations. Keep in mind that these recommendations typically assume a perfectly rigid machine and workpiece, but they can still be useful to look at.
Fpworks also had a good point regarding maximizing your metal removal rate (MRR). If the speed suggested by the guidelines puts you too far out of the range where your machine supplies maximum HP to the spindle, you could end up with a lower MRR than if you back the RPM down to the HP max for your machine.
This is something you have to play with on your machine. On my machine I run out of rigidity on roughing cuts before I get HP limited, so I typically run at the guidline RPM settings and then adjust the feed until the machine complains too much.
Paul T.