I was going through my Machinery Handbook, and trying to figure out the optimum drilling RPM. I ended up having to look at one table to get recommended FPM for the material, and then another table to convert FPM to RPM. The RPMs seem high to me, so I wanted to run them by you guys as a sanity check.
For HSS drills in low carbon steel, I read 100 FPM, and maybe half that for harder steel.
Converting that to RPM, I will list a range of RPMs for a given drill diameter.
1/4 inch - 1500 to 750 RPM
1/2 inch - 750 to 400 RPM
1 inch - 400 to 200 RPM
Is this anywhere near right? If so, I need to change the pulleys on my drill press, as I drill a lot of holes in the range of 1/4 inch to 1/2 inch, maybe set it to 750 RPM or so. It is a pain to change, so I want to pick a compromise value.
The other question relates to pilot drills. I did not find anything in my Machinery handbook on pilot drills. Does it make any sense to use a pilot drill for finished hole sizes of 1/4 inch or less? If so, what is the rule of thumb for pilot drill sizes? Do I need to change RPM between the pilot hole and the final drill size?
Assume that most of my drilling is in low carbon steel of 1/4 inch to
You're in the right ballpark. Running HSS a bit slower won't hurt much. Remember MH is written for guys for whom time is money, and big $$ at that. Use some cutting oil and take it easy on feed.
For HSS on mild steel, remember "300 divided by your drill bit size."
For example, 300 / ¼ = 1200 rpm, or 300 / ½ = 600 rpm.
And if you ever see blue chips coming off a HSS drill bit, STOP and slow it down. Running really small drill bits often leads to breakage. If your drill press table is really rigid (unlikely) then drill 1/8" right through and then drill your final hole in one go. Else take it in a few steps. - GWE
Yeah, looks like what I use. I mostly do 1/8 to 1/4" HRS/CRS, plus whatever aluminum castings I'm working on which are most often thicker. As long as the chips aren't blue (use lube) and you slow down at the end (especially in thin material with the sort of drills I have, which make a flat-bottomed hole aside from the split point pilot), then it's good... more often for me with our crappy drill press I have to slow it down to keep it from chattering. I can still do 1/4" holes at 1500RPM or so, so that's not bad I guess. I did 3/8" at 1200RPM the other day, making some nice spirals. :)
Sounds like you need a new drill press. :D I just loosen the motor, chunk the belt down a step, retension and go. Sounds like you need cone pulleys?
If you want to. I don't bother for the most part. Cutting the web out of something >3/16" is going to make it go a lot faster, for sure.
- Cut the web width. For 1/4" that might be what, 1/8"?
If you want the pilot to go at proper speed, yes.
Tim
-- "I've got more trophies than Wayne Gretsky and the Pope combined!" - Homer Simpson Website @
Those numbers look about right. The only things I would add are:
Use cutting fluid. Even motor oil helps quite a bit if you don't have access to the "real stuff". Just avoid the fumes if possible as it smokes.
If you start to get chips iin any color other than silver, slow down either the feed rate or RPM. The chips will discolor before the tool is ruined because the chips are actually colling the tool end as they go by... Hard to imagine, but they are... But eventually, that tool tip will overheat and stop working.
If you ever need RPM guidelines, you can cound on the MHandbook. Although I suually suggest RPMs that are around 10% less than what they do for customers as people tend to mess a perfect environment up every time.
Pretty close. If you want to convert SFM to RPM precisely, what you do is:
1) Multiply diameter in inches by Pi (3.14149.....) to get circumference in inches.
2) Divide circumference in inches by 12 to get circumference in feet.
3) Divide that figure into the desired SFM to get the needed RPM.
Note that it is common to simplify that a bit by converting 12/Pi (3.8197) into 4 as an approximation, so you divide the diameter by 4 to get an approximate circumference, and divide that into the SFM to get an approximate RPM (close enough).
As I keep a good pocket calculator handy -- one which includes Pi built in, I do the more precise way, as it is almost as quick.
Note that these SFM values (and the resulting RPM ones) are considered maximum speeds for a good tradeoff between tool life and number of parts machined per hour. You *can* run much slower, and the hole will just take that much longer to drill.
Not normally -- and even less if you have a set of split-point drill bits. The primary purpose of the pilot drill is to eliminate having to force the chisel tip of the drill bit (the blunt line at the center) into the workpiece. When running a 1" drill bit into a workpiece on a lathe or drill press, that chisel tip takes a lot of force (and thus is more likely to bow the drill sideways and enlarge the hole). If you make a pilot hole with a much smaller bit (just a little smaller than the length of the chisel tip) the force needed goes way down, and the job gets easier.
Of course, the same could be said for any size drill bit, but it gets rather insane to pilot drill for a 0.100" diameter drill bit. :-)
As above -- just a little smaller than the length of the chisel tip.
It would make the drilling faster -- but might take you longer to change the speed than to drill at the slower speed. Mine is pretty quick to change, so I tend to change when it feels right. (I probably drill too slow most of the time, anyway. :-) Some of these days, I will pull the single-phase motor from that drill press, and pop in a three-phase with a VFD to allow me to change speeds more easily (just a twist of a knob, unless I need a really big change, as when going from drilling a 1/16" hole to a 1" hole), so it will be done more often. Obviously, with the really big changes, I will still need to change belt settings.
With other materials, of course, the SFM changes (and the resulting RPM), but nothing else does.
Not insane at all. Pilot drills are usually fat and stubby so the point won't wander. I've used a carbide pilot drill with a 1/8 shank and 1/32 tip to set up a close tolerance pattern of 3/32 holes. If we drilled the holes directly with a 3/32 bit (even a split point), there would be differences of several thousandths when compared to the same pattern that was pilot drilled first.
We seem to have a confusion of terminology here. What you appear to be talking about is the combined drill and countersink intended to be used for making center holes for lathe turning between centers. (And it is normally double-ended as well.)
Hmm ... I would consider that application a "spotting" drill, not a pilot drill. And there are spotting drills purpose made, which have a center-cutting single-flute design with nothing much beyond the single flute -- sort of like a single-flute countersink.
A pilot drill -- as I was using the term --and as I think the original poster was using the term -- is a smaller drill bit used to drill full depth clearance for the web to reduce the forces needed for pushing the chisel point of the larger drill through the workpiece.
Yes, in fact, quite accurate. You'll get good performance within those speeds for mild steel. Do keep an eye on the sharpness of your drills, however. Dull ones will cut quite hot, whereas sharp ones will cut cool.
One tip-----the color of chips coming off your drill are a great indicator of a desirable speed. If you chips come off steel colored, you're likely running too slow. Look for chips to come off ever so slightly yellow when you drill dry. Anything more than that, you're going too fast. By the time chips are coming off blue, you've likely already damaged the cutting edge from speed and heat.. When your chips come off pale yellow when drilled dry, the drill should do quite well when you lubricate it with cutting oil.
Pilot drilling:
If you expect a ¼" drill to cut size, it's good shop practice to open the hole using a smaller drill first. Generally one chooses the next size down when using fractional drills, so use the same rule of thumb for number or letter drills, meaning you'd choose a drill approximately .015" smaller. Not only will the finish drill cut size that way, but the hole will generally be a much nicer one with fewer irregularities. Needless to say, lubricate the drill when you're drilling. Even an acid brush dipped and wiped will be quite beneficial as opposed to nothing. Flood cooling works even better, but it's messy and not many home shops have a drill press so equipped.
Not to be confused with the concept of double drilling holes to insure hole size. It's poor practice to drill holes in one step when the diameter is critical. Even when not stated, holes have a standard tolerance which is easy to miss with a twist drill. By double drilling, starting roughly .015" undersized, you have a much better chance of ending up with a hole of the desired size. It usually take three steps to drill a proper hole. Center drill (or spot drill), drill undersized, drill desired size. .
Not at all DoN - I do this all the time when making small printed circuit shield enclosures. I want the connectors to wind up in the right spot, within a few thousanths - so I lay out with dial calipers used as a scratch gage, under a microscope, and then centerpunch with a scribe.
For the larger holes I centerdrill with a carbide 3/64 drill to keep the larger (0.10 inch or so) holes from wandering. This sort of layout technique will get everthing in within about five thou and is a lot faster for prototyping than trying to drag everthing down to a milling machine and sticking it down with double-stick tape.
Again -- we have a difference in terminology. You are discussing "spotting" -- to locate a hole.
I was discussing pilot drilling -- drilling a smaller hole (about the thickness of the web of the larger drill) full depth, to reduce the force needed to push the chisel point of the larger drill through the workpiece. For *that* function, there is little point to a pilot drill for a drill as small as 0.100.
There is still adequate reason for spotting for accuracy of hole location.
That's what I meant, sort of round about. My experience in the missile industry taught me that one was not free to stab a hole in any part and call it good. While holes often had a specific tolerance, there were times when they did not. In that case, QC reverted to specific standards, in my case to MIL specs. My point in posting what I did was that it's a good idea to double drill holes *because* one is likely not free to end up with holes, size be damned. You just told me the same thing, only supplying the references to which you must work. Do you wonder how many have ever considered that holes must be held to a specification?
It is rare that I see a drawing without a general tolerance guide in the title block.
Well, application is important. I drill a lot of clearance holes for screws in the dies at work. Sometimes the holes are greater than 400mm deep, perhaps Ø16mm+. In this instance, the diameter is pretty loose and the holes are too long and numerous to double drill.
Of course, the panels produced using our dies require very specifically sized holes.
That doesn't even register. There is always a specification/tolerance.
From you reply, I get the idea that you seem to think you do.
Sorry, Charlie. That does not apply to drilled hole diameters.
Your training in the tool and die industry will likely make a good toolmaker of you, but a poor production machinist. The rules are not the same.
Starting to get a clue?
Perhaps in your limited view of the world, and in your limited exposure to the machining world. As I suggested, there are many that have no idea that a hole has a tolerance. It appears you may a part of them. Block tolerances typically can *not* be applied to holes, if that's what you're suggesting. Based on your theory, a ¼" hole specified as a decimal (.25), with a block tolerance of ± -.010 for two place decimals, you're alluding to the idea that one could drill that hole to .240" and it would be per print. *It would not*.
The tolerance of which I speak limits holes to a very small amount of undersize, and a somewhat greater amount oversize. For example, and it is likely not correct, you might have a + .004"/-.001" on a .250" hole. The tolerance increases with hole size. I can not cite specifics because I don't have that information available to me, but I can attest to rejects on many occasions based on the concept when I was involved in production work, early in the apprenticeship of my career. It's one of the reasons you learn to double drill holes, aside from taking great pride in getting it right.
Needless to say, the home shop type is not affected by the elusive tolerance of which I speak. They are free to stab that hole I speak of with no concern for repercussions. Toolmakers often are not, either. In all my years as a toolmaker I never had a hole specified, not even to location, if it pertained to the assembly of the tool. No one had to tell me where to put a hole, or to counterbore a hole for a socket head cap screw, nor did I have a tool rejected on that basis. I knew where and how to do it. Only functional, or critical holes, were individually toleranced and specified. It was assumed that the builder of the tool knew what was expected. Most toolmakers aren't the dullest knives in the drawer of metal workers. The dull ones never make the grade.
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.