What's new
What's new

Spot drill for chamfering, speed and feed?

cnczack

Aluminum
Joined
Sep 14, 2020
Looking for recommendations on speed and feeeds that you all run yours at. I program them for around 2500, 20 ipm but they keep breaking down quick. We also use them to chamfer holes for threading (VMC) on a variety of materials. mostly cast steel, carbon steel, and sometimes some foreign.
 
I usually use the same speed as drilling. 2500 sounds fast for those matl's unless you're spotting small holes. I usually use about .005 per rev. 20ipm sounds kinda heavy. Your chamfer sizes probably don't track very well from small spots to larger ones, do they?

For big spots or tougher matl, I like to use G82 with a short dwell to eliminate tool pressure and have consistency.
 
I usually use the same speed as drilling. 2500 sounds fast for those matl's unless you're spotting small holes. I usually use about .005 per rev. 20ipm sounds kinda heavy. Your chamfer sizes probably don't track very well from small spots to larger ones, do they?

For big spots or tougher matl, I like to use G82 with a short dwell to eliminate tool pressure and have consistency.

Well if im using it more like a spot drill ill slow it down like a drill. If im chamfering ill use a .5" to make a .06 chamfer at 2500 @ 20ipm
 
All depends on what spot drill you're using.
I've recently done away with spot drills and went back to a solid carbide center drill. So for spotting I only go about .03" deep. Just enough to get the drill started on location.
 
I run them at higher RPM... 6000 as a rule.

For chamfers, I run at 35 IPM. Any higher than that and I start seeing vertical lines in the chamfer.

I offset the Z down as far as I can without causing a secondary burr... avoid the tip and keep the top of the 45 degree portion above from the top of the part.

For plunge spotting, I back the RPM down to material specific SFM and back the feed way down (.001 IPT).

To a large extent, I have drifted away from using spot drills for the above operations. I find that I get better tool life and finishes using a 45 degree Drill-Mill... you know those stupid endmills that have a 45 degree tip. I always figured they were for people running Rong Fu conversions that wanted a 45 degree cutter but also wanted to do side cutting in case they forgot to change tools :) Turns out they run great in aggressive CNC applications.
 
I run them at higher RPM... 6000 as a rule.

For chamfers, I run at 35 IPM. Any higher than that and I start seeing vertical lines in the chamfer.

I offset the Z down as far as I can without causing a secondary burr... avoid the tip and keep the top of the 45 degree portion above from the top of the part.

For plunge spotting, I back the RPM down to material specific SFM and back the feed way down (.001 IPT).

To a large extent, I have drifted away from using spot drills for the above operations. I find that I get better tool life and finishes using a 45 degree Drill-Mill... you know those stupid endmills that have a 45 degree tip. I always figured they were for people running Rong Fu conversions that wanted a 45 degree cutter but also wanted to do side cutting in case they forgot to change tools :) Turns out they run great in aggressive CNC applications.

I have meant Drill-Mill this whole time not spot drill lol. DO you chamfer with them and if so, whats your speeds and feeds ?
 
I have meant Drill-Mill this whole time not spot drill lol. DO you chamfer with them and if so, whats your speeds and feeds ?

I chamfer with them all the time. 1/4” cutter is loaded all the time. I runs the rpms as high as they’ll go in aluminum. About 3500 in most steels. Feeds, I use 50 IPM at 10k rpm and proportionally adjusted for lower RPM. In theory I could run the feeds much higher, but chamfers look like hammered horse shit if you start getting lines. In production with large chamfers, I use multi flute chamfer mills. We recently got in some chamfer mills from Carbide Source that I’m excited to try.

Larger chamfers I also rough out with the corner of a roughing endmill using a 3 pass Flowline style toolpath. Unscientificly, it seems to break up the harmonics and makes my chamfer mills last 5x as long.


Sent from my iPhone using Tapatalk
 
Aren't Carbide Source and Carbide Depot different companies?

I've bought from the 'Depot many times, but never checked their calculators. Maybe they're as bad at math as I am...

I'm not even sure anymore. I get confused as to who is who. I just know I've had good luck with one of them and bad luck with another.

I've had good experiences with carbidetoolsource.com, they have good tooling at a reasonable price; however, it's just two guys and a bunch of automated grinding equipment. So you have to order on-line and no "helpful" tooling reps to give you drastically misleading technical assistance.
 
For spotting I run 6000 at 5ipm up to .25 deep depending on the hole. The only time I chamfer the hole with a spotting op is if I am running a thread forming operation afterward, otherwise I run them in a contour path to deburr. If im spotting a hard material I might bump the feed down to 4ipm.

For chamfering proper 10000 rpm at 60ipm in all materials works fine. Unless it is a beefy chamfer those are the parameters i use.

For reference I use an Everede NC indexable spot drill for spotting and a helical flute chamfer mill for chamfering. I could use the NC spot drill for chamfering but doesn't leave as good finish for me.
 
For spotting I run 6000 at 5ipm up to .25 deep depending on the hole. The only time I chamfer the hole with a spotting op is if I am running a thread forming operation afterward, otherwise I run them in a contour path to deburr. If im spotting a hard material I might bump the feed down to 4ipm.

For chamfering proper 10000 rpm at 60ipm in all materials works fine. Unless it is a beefy chamfer those are the parameters i use.

For reference I use an Everede NC indexable spot drill for spotting and a helical flute chamfer mill for chamfering. I could use the NC spot drill for chamfering but doesn't leave as good finish for me.

10,000 @ 60IPM for say a .01-.03 +/- ? we seem to use them a lot on chamfering for holes to be tapped usually .06" bigger than the nominal tap size

ex: 5/8-11 we would chamfer .685" in dia. with the drill hole size measuring .53125. So i guess about a .150 chamfer which is beefy to me lol

I may try multi passes on these like G00 Proto mentioned
 
All depends on what spot drill you're using.
I've recently done away with spot drills and went back to a solid carbide center drill. So for spotting I only go about .03" deep. Just enough to get the drill started on location.

I'm stupid, I didn't see that you were talking about chamfering until now.
:crazy:
 








 
Back
Top