? How to use really small end mills to mill really thin slots

[mmagliaro]

As I ponder future steps of this loco project (the 0-6-0), I am thinking about
milling slots into the frame for the bearings to sit in.

I don't mean the slots to allow the axles to pass through the frame.
I mean the ones "into" the frame that will allow the bearing tabs to be locked in place.

Something like this.  Imagine you are looking down from the top at the edge of the loco frame.
I want to be able to drop the bearings into so their edges are in small slots (the LIGHT red areas).

The thing is, these slots will only be 1.2mm wide (3/64" or about .047")
Yes, they certainly make end mills this small, and I could clamp this frame under my mill and mill
the slots perfectly.

The problem is, I will be doing this with all manual milling, and it seems to me that an end mill that thin
will just break right off when I try to cut this in a brass frame.   I have looked around for them,
and everybody seems to want to make these small cutters out of carbide.  My experience with carbide is that
although it is sharp and hard, it is brittle as heck and I never use carbide wire drills for that reason.

So... am I wrong here?  Would a 1.2mm carbide end mill hold up to cutting a slot like this?
Can I find HSS 1.2mm end mills somewhere?

[peteski]

I think you should rotate the frame 90 degrees and mill the bearing slots (fromthe side of the frame, not bottom) using either a narrow width keyseat or a T-Slot cutters. If you find a cutter which had a 1.2 mm cutting head then this would be easiest, If not, you just have to mill the slot multiple times until you get to 1.2mm width.

For cutter type identification see http://mindworks.shoutwiki.com/wiki/Cutter_Types_%28Mill%29

BTW, I use carbide cutters often and I haven't broken one yet. As long as you don't stress the cutter (too heavy feed or incorrect rpms), then the cutter should not break.

[mmagliaro]

EDIT
----------------------------------

Peteski,
I was looking around for keyseat cutters even before I posted this.
I didn't realize they made them that small!   

The bearing itself is 4mm across = 0.157  (a shade over 5/32"), and 1.2mm thick = 3/64 = .047"

I can buy a 5/32" diameter x 3/64" thick keyseat cutter with a 5/64"mm diameter shank (which is good because
that's less than the 1.5mm axle diameter, so this thing can fit in the slot!).

Whew.  They are pricey.  About $37 for one cutter from HarveyTool.com

EDIT:
This is a good idea.  Thank you.

The other big advantage is that with the frame lying on its side and cutting sideways into it,
the Z axis is locked, which eliminates the mini-mill's weak point.   It is much better milling side to side than it is
up and down.

[peteski]

EDIT:
This is a good idea.  Thank you.

The other big advantage is that with the frame lying on its side and cutting sideways into it,
the Z axis is locked, which eliminates the mini-mill's weak point.   It is much better milling side to side than it is
up and down.

Exactly.  You're welcome!   

[Andrew Hutchinson]

Max,

If the cutter is too spendy try turning one out of some tool steel. If you have a square block with hole for the shank and a set screw  to hold the cutter shank you can do it without any real dividing apparatus. If you want something similar but quicker, turn the basic dimensions you need and file a fly cutter out of the end. Heat treat, stone and test it out in some scrap. It is slow going but they work OK. For fly cutters/single use cutters I'll use anything (W1) but the more complex they get the more O1 and A2 I use. It is easier to screwup the heat treating small tools with W1 on account of bubbles on quenching that affect the toughness of the tool. Remember to run carbon steel cutters slow. Feed accordingly. Where you're going with this project is proper model making - more than half of that is tool making.

Andrew Hutchinson

[narrowminded]

Having difficulty using carbide cutters in small diameters, .062" and under (even 1/8"), while having some success with high speed tool steel is legitimate and is easily recognized when you digest what's happening with tool runout, chip load per tooth, and especially surface feet per minute, the key functioning parameters of any cutter at any diameter.  It is then further aggravated by rigidity.  This is also why there are very serious machines with very high speed, very true running spindles and collets, not cheap, specifically built for producing miniature machined parts in production and quite often, they use HS Steel cutters as their preferred tool material.  Do the SFPM calculation on a small cutter and it will quickly reveal itself.  Carbide wants pressure (helped by rigidity?) with SFPM up around 200-350 in brass, steel maybe 100 to 500, with aluminum between 600-1200 FPM.  Surface treatments can increase that.  High speed steel cutters don't function with the higher pressure of carbide and run speeds at about 1/2 of that.  About 100-200 FPM with brass, mild steel 80-100 FPM, and again, surface treatments can help that.   Then do the chip load per tooth (feed rate) which can be 1 to 1/2 thousandth and less per tooth the smaller you go and realize that without extremely true running tools you may THINK you have a multi flute cutter when in fact, with runouts down in the tenth of thousandths, it quickly heads in the direction a one flute cutter and you probably can't even measure it to be sure.  So you quickly have a cutter running WAY under speed with a feed rate almost assuredly WAY too high.  Here are a couple of examples starting with a 1/8" diameter cutter. 

For the lower end of the range for cutter speed in a brass part:

for a 1/8":  carbide cutter @ 200 FPM =  6,108 RPM
                          HSS cutter @100 FPM =  3,053 RPM
for a 1/16": carbide cutter@ 200 FPM = 12,213 RPM
                          HSS cutter@ 100 FPM =   6,106 RPM
for a .040": carbide cutter@ 200 FPM = 19,803 RPM
                          HSS cutter@ 100 FPM =   9,542 RPM
for a .010": carbide cutter@ 200 FPM = 76,335 RPM
                          HSS cutter@ 100 FPM = 38,168 RPM

NOW, let's consider that many mills and typical mini-mills have maximum spindle speeds around 2,500 to maybe 3,500 RPM for a nice Bridgeport and BAM... there it is.  It's WAY too slow for small cutters.  The ideal speed for a .0625" cutter in HSS is already 6,116 at the LOW end of recommended  and might well be able to go double that.  A mini mill with a 2500 RPM spindle can only achieve 40 FPM for a 1/16" cutter and a .040" cutter at full speed only gets 26 FPM.  Then try to feed it at .0002" per tooth (at those numbers assume one tooth).   It's tough duty.  If you sneeze you probably snapped it.  And your best chance is a sharp edged tool that can cut without pressure and might be able to stand a little more flex.  That means HSS.  

I have access to a small part CNC live tool production lathe and one of its features is spindle speeds of 6,000 RPM and will often perform milling operations in that machine with small diameter (under 1/8") HSS cutters as the preferred cutter of choice.  Even with 6,000 RPM spindles it's just not fast enough for carbide milling cutters in small diameters.  HSS and light passes for the reasons just outlined.  Sometimes I wish it had a 10k, 20k, or even 60k RPM spindle.   That machine is a key to being able to even entertain production of the super small chassis I've been developing.

NOW, that's not intended to be the whole story and it isn't BUT... it's a lot closer to the story than " be careful and don't feed it too hard".  It also shows why you probably had better luck in small diameters with HSS.  It's not just you. Hope that helps.

[robert3985]

So, what's the spindle speed for a 1/16th carbide endmill with a feed speed of 6" per minute?

I cut with really small diameter mills all the time, making shallow cuts and taking it slow....I haven't broken one yet...and I haven't calculated feedspeed either.

Cheerio!
Bob Gilmore

[narrowminded]

Bob, do you know the RPM or even a decent guesstimate?  And carbide or HSS?  Cutting what material?  How many flutes?  That's the starting data that you then use to figure out the recommended IPM travel.  There are online calculators that you can use with that data, too. 

Chances are you can't overspeed it by virtue of the machine's max RPM, especially at a light cut and with a stubby cutter (length to diameter ratio wasn't even mentioned yet), as that will allow the upper end of the recommended limits, not the lower ends I used in those examples. For that brass example above, if the setup is good and rigid and not cutting too deep or too wide, it should stand up to twice that shown and with different cutter coatings, even more.  And a change in one parameter effects all of the others.  And all while holding what accuracy, what surface finish quality?  That's why I closed that post with, "NOW, that's not intended to be the whole story and it isn't BUT... it's a lot closer to the story than " be careful and don't feed it too hard".  It also shows why you probably had better luck in small diameters with HSS.  It's not just you. Hope that helps."

Then your remark, "I cut with really small diameter mills all the time, making shallow cuts and taking it slow....I haven't broken one yet" suggests that maybe you should leave well enough alone if it's working.   Although, if you're ever looking to prove that you're in the range or run into trouble, there's a lot to be had in understanding those  parameters.  You've apparently fallen into acceptable parameters even if only by luck.  And sometimes luck is better than...

[peteski]

I have a Sherline mill with a high-speed pulley set. It gets me close to 10,000 rpms.

[robert3985]

I have a Sherline mill with a high-speed pulley set. It gets me close to 10,000 rpms.

Me too.

I cut brass, aluminum and Delrin with my small end mills since it's almost ALL for my own model train work nowadays.  However, I learned to run a Bridgeport Mill and Atlas lathe when I was 14 with a start-up company manufacturing eddy-current and ultrasonic probes for non-destructive testing of nuclear fuel rods, machining different plastics, aluminum, brass and lots of SS.  That was waaaaay before CNC, so much of what I learned was to "feel" the way the tool is reacting with the material with several starting point rules to get the required finish and save the tool. 

Cheerio!
Bob Gilmore

[mmagliaro]

Gents:
I appreciate all the calculations on feed speeds and rpms.  Believe me, I have already read enough online articles about this to know that my 2500 rpm mill doesn't turn nearly fast enough to do micro milling (which to me means bits at 1/16" or less).
The conventional wisdom is that if you want to start milling with 1/32" or smaller bits, you better have a 12,000 rpm spindle
and 20,000 would be a lot better.

And yes, I totally understand how the runout gets so critical at these small cutter diameters.

Forget about how it affects the flute and the real feed speed in surface feet/min.  Just imagine a little .020" bit
spinning in a mill head that has a run-out of .001"  If you are only cutting .001" into the metal, it's like
the bit is wobbling around and banging against the work by .001" every revolution.

Luckily, mine isn't that bad.  It's about .0002 (absurdly... using the 3-jaw chuck... if I use a collet in a
collet chuck, it's worse!)    In fact, maybe I'll invest in a few small collet holders to get the precision as high as I can.
Since the thing can turn a 3-jaw chuck with only .0002" runout, that means the spindle itself must be
pretty darn good, especially for a mini mill.

Yes, HSS, being more flexible than carbide, helps me "get away with it" better, given my limitations.  I won't be
buying another machine with a high spindle speed any time soon.

I have successfully milled brass with a 1/32 before on this machine, although I did eventually snap the bit, it lasted quite a while.

[mmagliaro]

Okay.... so I'm going to try some simple experiments.

First, just try to mill a slot in a piece of brass with a 3/64" carbide 2-flute cutter.
I will use side milling (not plunge).

My instinct, since the mill can only go 2500 rpm and I know that is definitely too slow, is to
just run it as fast as it can go, go easy with the depth (like, maybe .010" per pass) and
go easy on the handwheels to keep the feed rate low and try to feed it as steadily as I can.

How does that sound?  (It sounds like I'm going to snap the bit right off... I know... ha ha ha)

[narrowminded]

No!  That wasn't the point in that post.  It was to put some meaning to the whole mess.   You will never get production efficiency, tool life, or repeated, first time every time quality of finish or tight tolerance in a manual mill without the basic parameters met WAS the point.  It doesn't mean you can't coax a one or two time cut through with care (like for hobby use), especially with the ability to match parts, polish, light wipe with 1000 grit, and such, and even get lucky with a cut or two.  And the best chance for getting lucky is to start with a good understanding of what you're trying to accomplish (and then, is it really luck? ;.    Understanding the parameters and utilizing them the best you can gives you the best chance and helps to decide just what slow or fast cutter speed, light or heavy, fast or slow feed, means with the cut you're attempting.  Figure out the cut and feeds, get some sense of what slow is by doing the math and then having some idea what speed the handwheel should be turning.  There were times when manual milling that I had calculated feed guesstimates that when translated to something I had a chance to perform had me counting quarters of handwheel turns in seconds which was basically .0005" per flute, assuming only one flute on a two flute cutter.  Counting off slowly, one... two... three... four... five, and that was a quarter turn.  And on a manual machine but with power table feeds I often setup long, critical cuts, using that method with a stop watch to get the best feed setting. It gave me a reference that while crude, was better than, "just do it slow".  I used to get really lucky with tolerance and finish almost every time!   Then ,when the cutter is engaged, listen to it.  You'll hear if it's doing fine or not.  And fine might include that the cutter's running true enough that it's getting both flutes working which will then, with the exact same parameters being met, handle twice the feed.  That's the long way to attempt a description of what experience will eventually have you doing intuitively, including knowing when is it time to really think one through.  Hope that helps.

[mmagliaro]

I think we are misunderstanding the same idea.
Using brass, 2500 rpm, cutter diam .048, depth of cut .010, width of cut .048 (a full slot),
a calculator gives me a feed rate of 0.51 inches/min

I'm not completely guessing here.

My only guesswork came in about advancing the handwheels manually to approximate that feed speed.
I do like your ideas about using
a stopwatch and really trying to move the wheels at the correct rate.

0.51in/min = about .009" per second.   The handwheel is marked in thousandths, and is .050" per revolution,
so this is actually possible to estimate.  It would be about 5 seconds per revolution.

[narrowminded]

That's the idea.   Get you a good starting point based in facts of the matter.  I hope this doesn't come across as talking down to anybody as that is so thoroughly not the intention.  Based on the questions I was hearing a relatively sharp person but with minimal machine experience.  And that's just life and we've all been there, started somewhere.  It's why I am familiar and even sympathetic with some of your experiences and questions.

To add for clarity, the stopwatch remark was based on using a power table feed and finding a good starting (and often final) speed setting based on the data.  Using a stopwatch while hand cranking and trying to watch it while watching the cut, watching the dial numbers, etc. might be a bit too much while making the actual cut.  Too many things at once and something will suffer.  That's why I mentioned breaking a mental, rhythmic count, into quarter or maybe half handwheel turns was something I found to be manageable and useful when hand feeding something fussy.  Being new at it and trying to get the feel, you might make some practice runs cutting air and timing yourself against a stopwatch just to see how good your rhythm is.  You'll probably find a count that's pretty good and repeatable.  The body is sometimes more accurate than we give it credit for but we also have to give it something to work with.

Another tip that crossed my mind just now that may not apply on this cut but for another day.  When making cuts with multiple handwheel turns, instead of counting turns, dial it to the final position and with a sharpie, make a line that bridges the moving table to the fixed base.  Then, the only thing you have to remember is the final dial number.  You can pay full attention to the cut, speed, etc, right up until the lines get close then shift your focus to the final dial number.    When you're done, a little solvent and the mark wipes right off.  Really handy when making multiple parts that are setup against a vise stop.  Hope this is helpful.