Some gear cutting stuff

[Deanofid]

Hi all;

Some of you may have seen my little mashed up gear that let loose in the post about making a spindle
adapter for the little Atlas. It quit the job in the middle of that project, and the time has come to make
its replacement.

This post will deal with the method I use to cut gears in my shop. I'm not a real life machinist. Just an
impersonator. The way things are shown here are the way they work for me, and have done for quite
a few years. That doesn't mean they are the pro way of doing things, or maybe not even a preferred
method.

Cutting gears involves using single point gear cutters, in my shop, at least. Factory made involute gear
cutters just cost too much, for me. There have been scores of gears cut in my shop using this type of
cutter, and it works well on most free cutting metals. I don't think it will hold up against metals like
1018, or HRS. They are just a bit too tough on cutters that depend on an interrupted cut.

Here's that broken gear, and the 1/4" HSS tool bit that will be ground to cut the teeth of a new gear.
To grind it, just head on over to the bench grinder and start getting rid of what ever won't fit into the
space between two teeth on the old gear. It can take a while, and may take a few tries to get it to fit.
I use an Opti Visor so I can see close up when doing this.

When you have the shape pretty close, the last tiny bit that needs to be taken off involves barely
touching the tool bit to the grinding wheel. Check it after each little spark comes off the tool bit. It will
suddenly go from an obvious wrong shape, to a fairly good fit.

When I get it so close that I'm afraid to take another touch on the bench grinder for fear of ruining it, I
use a Dremel tool with a small diamond bit to finish it off. The Dremel tool is clamped to the work
bench, and the tool gently massaged to shape. Trying to do it with the tool bit in one hand, and the
Dremel in the other hand is like trying to hit a sewing needle with a sledge hammer. Putting the Dremel
in a stationary mount or vise makes things much easier.

After a bit of grinding, I have the tool bit to a pretty close match to the old gear teeth. I won't make
any claim about getting it perfect. Only as perfect as I can get it by eye. It needs to cut a close
approximation of the curve on the original gear.

If the gear you have is badly worn, i.e. teeth are thin, or leaning to one side, you will have to find one in
better shape to use as a model for grinding your tool. You also have to use a gear that is close to the
same tooth count. There is a reason for that. The shape of gear teeth change as the gear tooth count
goes up. The teeth on a gear with a tooth count of 20 look a little different than those of a gear with
64 teeth. So, match up your cutter to a similar gear as you want to cut.

I had cutters already ground for this gear pitch, but they were for different tooth counts, and didn't
quite fit the profile of the teeth in the gear that needs to be made here.

Okay, with the cutter done, I write down all the needed info to make a new gear blank. The main
things I need to know are the diameter of the blank, along with it's thickness and bore, and the depth
to cut the teeth.

I have a couple of books that tell all kinds of stuff about gears. Most of it is not really useful, or maybe
I just don't get it. The things really needed are on the sheet of paper in the picture, above.

Figuring the diameter or the pitch of a gear can be done provided you know at least one of those two
things. You can also figure pitch of one gear by using another gear of any size that it will mesh with.
For instance, if you have a gear that's been broken into pieces, and say you only have 1/3 of the gear
left. You can't measure the OD of that! Find a whole gear that it will mesh with, and determine the
pitch of the whole gear.

I think my scratchings in the picture tell what I did. One thing that may not be clear is for the depth of
cut for the teeth. That one number, 2.157, is a constant, and can be used for all regular pitches. This
works with American style involute pitches. I can't remember if it is the same for metric gears, and I've
never cut metric, outside of clock wheels.

With that stuff done, it's time to cut a blank for the gear.
The bore for this gear is .504", and I figured a drill bit would get it close. It came out right at that
number using a 1/2" bit. The piece is faced off to make a square surface and then parted off. Put that
piece in the chuck with a piece of tool steel backing it up to keep it square while the jaws are tightened,
the tool steel piece is removed, and the other side faced to a length of .375".

That's it for the blank for the moment.

Now an arbor is made up to hold the blank. Once this arbor is made, it is not removed from the chuck
until the gear is done.

A stub is turned on the end to match the bore of the gear blank, and a little short of the thickness of
the blank, so the cap screw in the end of the arbor can squeeze down on the blank and hold it fast.

Right behind the stub for the gear blank, a short distance is turned down to a diameter that is under the
depth of cut for the teeth. This will keep the cutting tool from dragging steel chips through the
aluminum gear blank when it is cut. If the gear were a larger OD, this wouldn't be necessary, as the
cutter wouldn't be going close to the arbor to take the cut.

Now, the blank is put on the stub, tightened down nice and tight, and turned to the diameter needed for
the gear. From this point on, the blank is not disturbed or removed from the arbor, and again, the
arbor is not removed from the chuck. Every thing should be happy in this relationship.

With the arbor and gear blank all made up in the same chuck setup, the chuck can be removed...

...and mounted on the dividing head.

The gear I want to cut here will have 20 teeth. Time to figure out how much cranking I want to do on
the handle between cuts. These numbers are particular to my dividing head, and any like it that use the
same worm gear tooth count, (which is probably not very many). Never the less, this is the way it is
done for any simple dividing head. Just plug in the number of the worm in your dividing head, and you
should be good.

This dividing head has a 100 tooth worm gear. I have a few division plates for it, and choose a plate
with 40 holes. Multiply the number of division holes by the tooth count of the worm gear, and you
have the total number of divisions possible with that setup. 40 x 100 = 4000. So there are 4000
possible divisions.

I want 20 teeth; 4000/20 = 200. That means I need to advance the crank on the dividing head 200
holes for each tooth to be cut on the gear. Instead of counting all those holes each time, the number
of holes in one rotation of the crank on the division plate can be divided into the total number of holes
needed to get full rotation turns of the crank, plus any remaining holes needed. In this case, 200, (the
number of holes to advance for each cut) divided by 40, (the number of holes in the division plate) tells
me the full turns; 200/40 = 5. Well, that's lucky. Exactly five turns of the crank for each cut on the gear.

It doesn't always work out that way, but I'll take it when I can get it.

After setting the dividing head square to the mill table, its crank handle is set to the "0" mark.
The cutter is set on center line of the gear blank. With the tip of the cutter against the OD of the blank,
the Y axis dial is set to zero. Move the cutter out of the way a bit, and crank the X axis back enough
so the cutter won't bash the gear blank on start up. Give the cutter a turn by hand to make sure it
doesn't hit the chuck jaws when the X axis is at its starting point. Dial in a few thou on the Y, run the X
to the right to make a cut, and return to zero. Keep dialing in Y a few thou and running the X back and
forth until the depth of cut is reached.

Stop the mill, crank in my five turn on the dividing head and return the Y dial to zero.

Repeat until there are no more places to put teeth on the blank.

Here's the last cut, just done.
Look it over well to see if they all appear to be the same, (hopefully!).

There's usually no going back once you take the gear off the arbor.
I checked the new gear against the old busted bit. Pretty close, though I have bumped them slightly
out of time trying to hold still for the picture.

I put the new one in it's place and turned the lathe spindle 'round and 'round, and 'round a bunch more,
waiting for a tight spot that never showed up. Okay, then.


This short vid shows the new gear in its place, doing its thing. It's the gear directly below the spindle
gear. All of the running gear is engaged in the vid, including the back gear, so you can hear a lot of gear
noise. That's the way it sounds, though the camera seems to amplify everything.


[ame]http://www.youtube.com/watch?v=Vmmuh9ZylZ4[/ame]


Thanks for having a look.

Dean

 

[1hand]

What Dean, no pretty spokes.......lol Great info here. Just had a look at your site and your clock build. Hence da smart azz.

Matt

 

[ariz]

very interesting post dean!
this approach seems easy enough that I too could try it ;D

thanks for sharing

 

[kendo]

Hi Dean
Nice little set up,and well thought out. Great job done.

Ken Thm:

 

[CMS]

Some very good info for cutting gears and also fortunate for you to have the backup lathe. Now I have a Big Dummy question about cutting direction, is there any reason that you cut away from the dividing head rather than toward it? My thoughts are the extra support you have to hold the part by pushing to the chuck and dividing head rather than pulling away from it.

 

[1hand]

In case someone would like to really like to get to be the gear master, here's a video that I got. Very well done.
4hrs long.

Just another bit of gear info if anyone is interrested. http://www.littlemachineshop.com/products/product_view.php?ProductID=2057&category=-511675330

Matt

 

[kustomkb]

Nice post.

Slick little dividing head too!

 

[mklotz]

Very nice tutorial, Dean. I suspect that, for the amateur, the skill most intimidating after single point threading is gear cutting. You've done a nice job of taking the mystique out of it and showing how useful results can be achieved in the home shop.

The folks who want to try this may be intimidated by the mathematics. I wrote my program, GEARSPUR, when I cut my first gears to condense all the math into one place in a form usable by someone who can't add two and two.

The code snippet below shows your case. After selecting the units in which I want to work, the program begins to ask me for information about the gear. I don't know the OD a priori so I enter zero to denote an unknown. Then I supply the known number of teeth and DP. The program now recognizes that it has two facts about the gear and proceeds to print out just about everything that can be calculated.

gearspur
[I]mperial or (M)etric units?

Enter whatever data you know. Enter zero (0) for unknowns.
You must enter two data items to obtain an answer.

OD of gear [2.35 in] ? 0
Number of teeth [45] ? 20
Diametral Pitch [20] ? 24

Diametral Pitch = 24.0000
Module = 1.0583
Number of teeth = 20
Outside Diameter = 0.9167 in = 23.2833 mm
Pitch Diameter = 0.8333 in = 21.1667 mm
Addendum = 0.0417 in = 1.0583 mm
Dedendum = 0.0500 in = 1.2700 mm
Whole Depth = 0.0917 in = 2.3283 mm
Circular Pitch = 0.1309 in = 3.3249 mm
Tooth Thickness = 0.0628 in = 1.5959 mm

B & S cutter number used to cut this gear = 6

 

[Stan]

I have another dumb question. Why do you not cut the teeth directly in the bar stock and then part it off instead of going the stub arbor route?

 

[Noitoen]

The toothed gear would be difficult to hold to machine the hole. 8)

 

[ksouers]

Dean,
Another great how-to write up Thm:
Thanks.

It was also very kind of the Atlas to allow you to finish the new Taig spindle for the dividing head before letting go on that gear. I suspect the job would have been a little more awkward without it.

 

[gbritnell]

Good work Dean. I've made plenty of them like you did, even as small as 64 pitch. I use and optivisor also, with the highest magnification available.
gbritnell

 

[BobWarfield]

Nice work, and I quite enjoyed seeing some of the nice tooling you've made.

Best,

BW

 

[Deanofid]

Marv, Ariz, Matt, George, Kevin, Bob, Noitoen, Stan, Kustomkb, Kendo, thanks much for all your comments!

Now I have a Big Dummy question about cutting direction, is there any reason that you cut away from the dividing head rather than toward it? My thoughts are the extra support you have to hold the part by pushing to the chuck and dividing head rather than pulling away from it.

Well, it's a perfectly good question, CMS. There are a couple of reasons in the case of this particular dividing head. I made it to be used on the lathe, so the crank is on the side where you see it. If the DH were turned around, you couldn't see the holes in the division plate. Secondly, since the crank on the DH has to hang over the edge of the mill table, the DH is located at the front edge of the table. This is a small milling machine, and there is not enough Y axis travel to put the DH on the back side of the spindle rotation. 3rd, the mill spindle on this machine only turns in one direction.
It would probably be better to have the cutter rotating toward the DH spindle, but it just doesn't work out. Thanks for asking!

I have another dumb question. Why do you not cut the teeth directly in the bar stock and then part it off instead of going the stub arbor route?

Another good question, Stan. There's no reason except for my own convenience. I already had an arbor with a lock screw threaded into the end. I also have to make a couple of other gears with the same bore, but different tooth counts, so I'll leave the arbor setup in that three jaw until the gear cutting job is done.

If you need to cut only one diameter of gear, then using the actual gear material as it's own arbor is a good way to do it, as long as you can do all the operations needed without removing it from the chuck. With this particular gear, you could; turn down the end for the OD, cut the teeth, bore the stock, part it off.

Once I have this arbor set, in this case, it's easier to do different sized gears using the same arbor set up.

Thanks again for so many comments, folks.

Dean

 

[Deanofid]

Oh, Marv, meant to say "thanks" for putting in the hint about your gearcutting program.

George, we had briefly mentioned using 12L for this gear in another post. I gave that some thought, then decided I would rather have this gear as a weaker link considering where it runs. If something got jammed up, I would rather have the smaller gear pop than do damage to the spindle gear. Those things are expensive.

Dean

 

[Stan]

Thanks for the response Dean. It makes sense if you have two lathes to prepare the blank for each size. I have problems when using an arbor with slippage and rigidity and only one lathe.

If the gears were reasonably close in size, I would start with bar stock big enough for the largest gear, make the bore long enough for all the gears and cut a relief behind the blank for the largest gear. After cutting the teeth on the first gear, part it off, and use the previous cut relief for the next smaller blank and repeat the process.

I am not much into gear cutting, but this method works for me to cut different sizes of ratchet wheels with an end mill. Now I have to try your method of grinding a gear cutter because my previous attempts have been less than stellar.

 

[Deanofid]

Hi Stan;
Just point of interest, I only used one lathe for this, and kept the arbor in the same chuck the whole process. After cutting the first gear, chuck goes back on the lathe, another blank put on the arbor and brought to diameter. Then more tooth cutting. The way you do it sounds every bit as workable, to me!

Dean

 

[Twmaster]

Dean,

That is yet another wonderful presentation of home shop how-to.

If not wandering too far off topic (or perhaps a pointer to another relevant thread) How to go about selecting a pre-made involute cutter? I've tried to read some of the explanations I've found on the web but simply end up tilting my head sidesways and saying 'huh?!?!?!!!'.

 

[black85vette]

How to go about selecting a pre-made involute cutter? I've tried to read some of the explanations I've found on the web but simply end up tilting my head sidesways and saying 'huh?!?!?!!!'.

Not sure if you want an explanation or have a particular cutter to pick. But check out Marv's program. Input the gear info and you get the cutter number you need to use.

BTW; I do the "huh???" thing a lot.

 

[mklotz]

For each DP (diametral pitch), there are a series of eight cutters which cover the tooth counts shown in the list below...

1 - >= 135
2 - 55 - 134
3 - 35 - 54
4 - 26 - 34
5 - 21 - 25
6 - 17 - 20
7 - 14 - 16
8 - 12 - 13

As an example, if you wanted to cut a 45 tooth gear of DP=24, you would look for a number 3 cutter marked DP24. If your gear required 18 teeth, you'd need a number 6 cutter.

In addition, there are separate cutters for each of the common pressure angles. Older equipment will often use a pressure angle of 14.5 deg while newer will tend to use 20 deg. (Don't trust that obvious generalization very far.)

So, a full set of cutters would be sixteen times the number of DPs you might envision using! As the following...

http://www1.mscdirect.com/CGI/NNSRIT?PMPXNO=1711027&PMT4NO=78808262

shows, that could get to be a *very* expensive operation very quickly. Buy only as needed or resort to other methods of gear cutting such as grinding your own single point cutter.