I am a new owner of a small metal lathe and milling machine. My first
milling project will be some half inch hinges for a Christmas present.
Materials will be brass for the hinge and drill rod for the pin. I am
reverse engineering a hinge that has a 5/64 inch diameter pin.
My third edition American Machinists Handbook states that for a press fit
the pin should be 0.0075 to 0.001 inch larger than the hole. For a running
fit the hole needs to be 0.0005 to 0.001 inch larger than the pin.
I plan on using an arbor press to install the pin in the hinge.
By going with wire gage drill rod and chucking reamers I have settled on the
The hinge pin would be #46 drill rod, 0.079 in. diameter.
The press fit hole will be either a 5/64 bit (0.0781) or a #47 ream
The loose fit hole will be a #46 ream (0.0810) sizing a hole left by a
(dimensions taken from travers catalog)
Here are my questions:
1. Which is easier to work with, Oil or Water Hardened drill rod?
2. Will I be able to use a cutoff tool on my lathe to cut the pins to
3. Are my choices for drill/ream/rod sane?
4. Is there something obvious I should know before starting on this?
Thanks for your help.
Well, first off, you want to do your work before you do the hardening.
That said, you won't find a lot of difference between the two.
For that diameter, you may find it simpler to saw them. Especially if
you're working with drill rod that has already been hardenend.
Try one and see if it works before you commit to doing more of them.
Both of them will be more difficult to machine than mild steel, but you're
likely to notice little difference between them until you have a little
experience machining. Because water hardening is only carbon steel, it
tends to be more economical than oil hardening, which is an alloy tool
That is more a function of your lathe than anything. Parting is very
difficult because parting is a rather demanding operation, especially if
you're using commercial parting tools,which can be rather broad. If you
have a very small machine, I would suggest to you that you hand grind a
narrow parting tool, something in the neighborhood of 3/64" wide, with
proper side, front, and back clearance, and with a chip breaker type of rake
on top. You want about 8° to 10° angle at the cutting tip, with the chip
breaker a fairly large radius that permits the chips to flow towards the
rear of the tool without interruption. That style of parting tool lends
itself extremely well to parting small, tough material. Use a slow feed (by
hand in this instance), reasonable speed, and lubricate well, using a sulfur
based cutting oil. They stink, but they work well. With a tool this
small, if you get in trouble, the tool will break instead of doing damage to
your lathe, a very negative experience I had when I was a boy and learning
the machinist trade. I ruined the ½"-20 spindle on my little Craftsman
Actually, yes. For a hinge pin you will start with material that is
relatively round, straight, has a nice finish, and is tough. You will have
no need to heat treat the material for a hinge pin, which I would recommend
you also do not do. Once you heat treat long, slender items, the chance of
them staying straight are not good.
Only that drills do not make very good holes. If you don't own any reamers
and think you'd rather not invest in them, a rather smart idea for bastard
sized reamers that may never be used again, you should practice drilling
holes in steps. Good practice in the shop dictates that you center drill
(or spot drill with a spotting drill), drill undersize, then drill to size.
That works very well in general, but in brass it can be a bad experience due
to the ability of brass to "hog in". That means that when you open up the
hole, the drill will grab and self feed. That can lead to ripped up hands
if you're holding things that way, broken drills, and damaged parts. If
you're familiar with how to reduce rake angle on drills, all you have to do
is reduce the rake angle to 0° and the drill won't grab, though. You can
also drill with your drill as ground, but you have to use a little drag on
the spindle of your mill, and must also be able to "feel" what is happening.
Again, without some experience, this may be a bit beyond your ability, but
it's not something that you can't learn by trying. There's really no better
way to understand things like this than to experience them.
One other thing to keep in mind. When you remove the bulk of material as
you're making the hinges, the parts are most likely to not stay flat.
Don't make the mistake of drilling your holes first, otherwise the parts are
unlikely to accept the pin. Rough the parts completely, then go back and
take finishing cuts. You could probably drill the holes after the roughing
operation and get by, but drilling them last might be your best choice. That
means that you will be drilling from boss to boss, so in this instance the
reamer may be a better choice because it has a better chance of achieving
holes that are in alignment. Play with some scrap stock at first if you
have that luxury. Try to make your mistakes on something that has little to
no value to you.
I always try to use standard off the shelve parts. A 3/16" x 1" dowel pin is
only is only $6.84/100 from Enco and a .001U/S reamer $4.75. I don't
think an extra 1/64 is going to make a difference in your design.
Either type of drill rod should be fine, and will be about as easy to work.
But, you are not going to be doing any appreciable work on the drill rod - just
cutting to length.
I wouldn't worry about cutting to length. You'll be pressing it into the hinge
barrels, and I would start with an over long piece, with a slight chamfer on
the end to be inserted. Press in until flush, then
cut/grind/file/mill/sand/hone off the protruding end.
Using a cutoff tool on such a small piece of rod isn't really necessary. In
any case, you'll end up with a small "tit" which you'll have to remove by hand
Whichever rod you use, it will be harder in its annealed state (as sold) than
the brass, and won't need hardening.
Your drill rod dimension doesn't make sense. #46 drill rod is .0810, same as
the #46 drill or reamer size.
You can get reamers in any of the fractional or number sizes, and in special
decimal sizes every .0005".
A running fit is for bearings - you don't have to worry about that. I'd
probably use the #46 reamer for both sets of holes, and, if the pin tended to
work loose, put some punch or chisel marks towards one end and then re-insert.
If you don't like that, use an .0005" undersize reamer for both sets and see
how it fits. If it doesn't move easily enough, open one leaf up to the #46.
I've thought about making hinges myself. Let us know how it turns out.
Yep, that's true. However, W1 is a carbon steel. W2 has vanadium added to
control grain structure (helping to keep it fine) after heat treating, so
otherwise it, too, is just a carbon steel. As you say, they are simple
I'd ream clear thru .001" over. A drop of Loctite 609 or 681 in the
last hole to engage the pin will secure the pin in place.
I wouldn't bother parting tool steel that small; just whack it off
with a thin abrasive cutoff wheel in a Dremel. It only takes a few
seconds and it doesn't matter how hard the material is.
Photos when they're done, please!
That's actually pretty good advice, but if one is trying to hold dimensions,
it isn't a solution. Using a parting tool with marked dials provides for
cutting parts to length repeatedly with precision. For a hinge, that may
not be a necessity, though.
If a heat treated pin was desired, making them from drill blanks would be
the solution, at which time the cutoff wheel would be a necessity.
Yep, I agree, a pic of the end product would be great!
I wouldn't think so. . I like "appropriate precision", which is
tenths sometimes but by no means always. I'd cut the pins a teense
short because there's no need at all for a hinge pin to be flush to
within .001" on both ends.