Drilling feed rates

[Beardy MikeParticipant @beardymike]

My mill is a kx3, which has no quill – the only way to drill is to set a feed and let the motors do the work. While I’m very happy on a drill press adjusting feed by feel and the look of the chips, I’m having trouble putting a number to it (and am too slow to react on feed override when I can see it’s wrong).

I typically use the little machine shop calculator for milling feeds and speeds with good results, but when I take its numbers for drilling I just toast the drill and ruin things. Does anyone have a calculator that works better for hss drills in steel, aluminium, stainless etc.?

[JasonBModerator @jasonb]

As I use F360 for my CAM I tend to take their speeds ( subject to 5000rpm max) but use around 40% of the feed rate per rev. The feed rates per rev are fairly constant for all the materials they list and only change when you look at them as mm/min when the speed comes into play

So a 3mm drill will typically feed at 0.02mm/rev and a 6mm drill feed at 0.03 to 0.04. I don’t have flood cooling so that is one reason to reduce it and once more than about 1 x diameter deep will use “full retract” which is what they call peck drilling to reduce risk of swarf buildup in the hole and allow brush or fogbuster to get some cutting fluid on the drill.

Not cooked any drills yet. Tend to use Dormer A022 Stub length most of the time

Typical F360 chart and what I run

 

[Martin ConnellyParticipant @martinconnelly55370]

This is from a small handbook supplied by a well known drill manufacturer. Note you can reduce the rpm but should not change the feed per rev. The calculation for vertical feed is simply the rpm x feed per rev and will be in mm/min or inches/min depending on which units you use.

Martin C

[Julie AnnParticipant @julieann]

Out of idle curiosity I looked up some of my old CNC drilling cycles. My feeds per rev are roughly double those mentioned by Jason, more in the ranges given in the chart by Martin. So for a 3mm drill I’d be at 0.06mm/rev and for a 6mm drill I’d be at 0.15mm/rev. Like Jason my go to drills for small sizes (1mm to 10mm) are Dormer A002.

I tend to use G73 for peck drilling as it doesn’t completely extract the drill, just breaks the chip and is faster than G83.

As an aside I am a bit more aggressive than Martin’s chart when it comes to larger drills (>3/4″) on the lathe. The tailstock is wound as fast as I can go, often resulting in feeds of 0.5mm/rev or more. A drill is very efficient at removing metal at a high rate.

Julie

[JasonBModerator @jasonb]

The low end of Martin’s chart is actually very similar to the F360 suggested rates if you compare say 1/8″ to 3mm and 1/4 to 6mm . It is just that I choose to reduce them. Your flood coolant may help, I don’t want to weld aluminium swarf to a drill bit!

F360 also has a “chip breaker” option which is like G73

[John HaineParticipant @johnhaine32865]

I use Cambam to generate gcode which has a “spiral drilling” feature.  This works really well and usually I can drill all the holes on a job using the same cutter as for milling – usually a 3-flute end mill – which saves time changing and re-setting a drill.  I use the same feed rates as for milling.

[JasonBModerator @jasonb]

It would depend on the size of holes and the usual size of milling cutters you use.

I would say the majority of what I drill on the CNC is a mix of clearance and tapping holes for M2.5 and M3 for whch I use a drill as my usual milling cutter is 6mm dia or 4mm if it is a small part with internal corners.

Bigger holes >10mm I will often do with the milling cutter but again may drop the feed slightly particularly if they are deep to allow the chips a chance to get out. This also avoids the problem of the actual cutting edge of the tool feeding a lot faster than it’s feed rate as the rate is set to it’s ctr line.

This recent one all the small 3, 4 and 5mm holes were drilled and the big one done by milling.

Yesterdays items were drilled with drills and reamed 8 & 10mm on the manual mill then the holes used to hold the oversize in X and Y stock to profile the outside on the CNC. M3 holes in the metal in the vice were done with a drill bit, straight in as the split point stubbies start OK and I only use a spotting drill on more critical jobs.

[Martin ConnellyParticipant @martinconnelly55370]

The reason you should be wary of reducing feed rates is that it is responsible for the angle of attack of the tips of the cutting edge of the drill. If you reduce the feed rates then there is a high risk of rubbing not cutting. Increasing the feed rates is also likely to chip the tips of the cutting edge. You have to think of it like using a chisel on a flat surface. You need enough of an angle to cut but not so big an angle that it meets too much resistance. Where I worked I was constantly telling people (usually contractors) using a big Asquith radial drill that you need a higher feed rate for bigger drills, not a smaller one. You could tell when someone was not doing it right because of the squealing coming from the drill. Think of it like this. If you draw a line that is some multiple of the outside diameter of the drill and draw the feed per rev vertically from one end and at the same scale you will produce a triangle with a small angle at one end. You need to maintain this angle whatever size the drill is. So a smaller drill will need a smaller feed per rev. For many people, who have not been taught to use feeds and speeds properly, there seems to be a feeling that if you are using a larger drill you should reduce the feed rate along with the RPM.

I was drilling some 15mm stainless plates this weekend, 5x  Ø5.2 for M6 tapping, 2x Ø10.5 clearance for M10 and one Ø10 for location. Using either new or freshly sharpened drills I had nice shiny curls coming off the drills as should be expected and no issues with drills blunting, chipping or rubbing. Feed and speed tables make this easy if you can make good use of them. Manual drilling makes it a lot harder to hit this sweet spot. I have a useful little data book.

Martin C

[Beardy MikeParticipant @beardymike]

Thanks for the feedback folks – plenty to try out once my mill is back in action… (See other thread about spindle motors)

[Author]

Posts