Making my own timing belt pulleys - how?

[damae]

In my retrofitting of a Series I Bridgeport, I have discovered how expensive timing belt pulleys are! For instance, I need two 18 tooth and one 26 tooth pulley, both H-series (.5" pitch) and 1" wide. Here's what I ended up spending:

16H100 $38
26H100 $60

I cheated by using metric size pulleys (38.0mm bore) that aproximate the correct Inch size (1.500"). If I ordered the correct Inch size, the cost soar to about $175 for those two pulleys!

And I ordered them with a simple bore, no set screw, no keyway, just a stright hole. I reason that these aluminum pulleys represent about $2 of aluminum (at the most) and perhaps 10 minutes of machine time on a 4 axis machine. So it seems like a part ripe for DIY'ing! What do you folks think?

I already blew $100 on those two pulleys and discovered I have need for several more of them, of various sizes. What is the simplest and most cost-effective way to build these? Can it be done easily with a 3 axis machine?

Perhaps I could use an indexer and cut one tooth at a time, manually indexing to the next tooth? I don't mind if this takes an hour or two to make a gear. Would this indexer do the job?

http://www.use-enco.com/CGI/INSRIT?P...&PARTPG=INLMK3

I'm sorely in need of some machining advice on how to do this. My gut feeling is that the best way to do this would be to simply use a 4-axis machine. But I'm kind of up against a boot-strap problem; I need the new pulleys to make my 4th axis.

Actually, I will be hobbling together my 3rd axis pulley too. Hopefully that one will last long enough to help me machine its own replacement!

So please chime-in and offer any comment you can. I'll take it all - from hair-brained idea to tried-and-true techniques.

Thanks in advance!

[damae]

I should add that the minimum radius at the root of each tooth is about 1mm (.040"). That means a .080" (2mm) diameter tool if I try to cut it from the top view. Of course, a tool that small has a cutting length much, much smaller than 1" deep. That's why I tend to think it would require machining on an indexer or 4th axis.

Please help me with some innovative solution. I'd even take interest in broaching if it's something easy to setup. Any idea is welcome!

[Verfur]

I belive an indexer/ fourth axes would do the job. I belive you would need a formed tool on a horazontal machine, so as to cut the bottom radi and the ramps on the teeth at same time. I cant imagen the time it would take to use a small ball nose end mill even after a rougher.

Let me know if you wind up with a way and how much you would want to mill a few more as I too think the prices are high from the hobby stand point.

John

[damae]

Originally Posted by Verfur ... I belive you would need a formed tool on a horazontal machine, so as to cut the bottom radi and the ramps on the teeth at same time. I cant imagen the time it would take to use a small ball nose end mill even after a rougher. Let me know if you wind up with a way and how much you would want to mill a few more as I too think the prices are high from the hobby stand point. ....

I agree that ball end mills probably would be slow, because they would have to be of small diameter to get the small radius at the bottom of the groove. And the small diameter limits the depth of cut and feed speed.

That's why I was thinking I could use a rounded endmill like this one:

http://www.mcmaster.com/param/asp/PS...MainWidth=1068

This type of endmill could be the full width, as wide as the flat at the bottom of the groove. It's really just a flat end mill with a small radius at the outside edge. It should allow me to have a larger diameter tool (up to about 5mm or 0.2") and make deeper cuts.

So it seems like with some work, this setup might work. However, I am really hoping some machinist here has a hot tip for me about how to aproach this problem. For instance, I read this tip in another thread:

To chuck up a gear (or toothed pulley) in a lathe, first lay dowel pins between the teeth and then clamp onto the pins. This transfers force to the root of the tooth and prevents the tooth surface from getting marred up.

There are probably a dozen other gear/pulley making tricks out there! If you know of one, let me know! If you don't but have a crazy idea or comment, let me know that too! =)

Thanks!

[John S.]

Damae.

In alloy you can flycut each tooth with as simple cutter.
If you are worried about a flycutter lasting up then you could mill the bulk out first.

Here's a link to an excel spreadsheet that gives you all the info you need for cutting pullies.
The tip width and DOC is common for one size and the rest of the calculations are done when you enter the number of teeth.

http://homepage.ntlworld.com/stevens...%20pullies.xls

John S.

[damae]

Thanks for the spreadsheet John! For H-Series pulleys it recommends 0.165" cutter width by 0.120" depth of cut.

Can you elaborate for me what a flycutting setup would look like? Sorry for the ignorance. Until now, I thought flycutting was used only for surfacing flats, as in squaring up a piece of plate.

[John S.]

Crap drawing but dinner is ready and it's no contest

[mxtras]

Damea -

Have you looked into buying timing pulley stock and then cutting to width and boring it? I can't recall the cost - I may be off, but I thought the stock pricing was reasonable....?

Just a thought.

For the time it would take to make a pulley from scratch, I would shell out the cash, but my time is limited (except here at work :0).

A fly cutter is a good idea - you would have to feed slow for a smooth finish, so time would be a consideration.

Scott

[Verfur]

damae,

This is simaler to what I was saying only I would use a horizontal mill with a form cutter like mxtras is useing. the bottom of the vallys and the sides of the teeth are not flat, the bottom has a radi to match the OD. - depth of tooth and then the wall leads up on an angle. This makes the tooth look like a piramid on the top of a hill.

John

[ynneb]

Gear hobbing machine.
http://pacificsun.ca/~robert/travel2...h/Dscf3068.jpg

[damae]

Thanks to all for the excellent advice so far!

John, thanks for the sketch -- it's very clear and gives me a lot to think about. I'll need to buy a flycutting arbor, but that shouldn't be too expensive, I hope.

Verfur, I see you're right -- it's not a flat bottom, just a large radius, at the bottom of the groove. So I could only aproximate the bottom with a 5mm rounded endmill.Since trapeziodal belts are supposed to run with a small clearance at the bottom of the groove, perhaps I could get away with it?

Ynneb, thanks for the fascinating picture of the hobbing machine! A lot more machine than I want to be operating just to make pulleys. =) I'm still hoping for some kind of simple way to make these gears on my multi-purpose 3 axis machine.

Mxtras, the timing pulley stock could work for me if I have a source to buy it from. H-pitch pulley stock has proved hard to find. Do you know of anyone selling H-pitch stock? The upside? This is certainly justification for me getting a lathe! Hehe. (actually, it's unavoidable. I'll be stuffing a lathe into my garage eventually)

What about the spin/indexing fixture and method to make sure that I rotate the correct amount each time? I am hoping to cut the pulley blank on the mill, including the center bore, then fixture it from the ID. Any experience to offer here?

Thanks!
-D

[buscht]

damae, Here's another approach that might work.

This is just an example, you will have to adjust for your situation.

Assume you want a 1" thick pulley and you need 1/16" inside radii. This means you need a 1/8" dia cutter and the 1/2" cutting length on your cutter is inadequate.

Simply make 4 pulleys -1/4" thick. Use your CNC to put accurate dowel holes in each one, along with some bolt holes. After cutting all 4 parts, line them up with the dowels and bolt together.