threadmill test results

[KTP]

The cheap bastard attempt to cut freewheel threads (1.375" x 24TPI) into an aluminum timing pulley hub by using a cnc mill and a modified 3/8 x 24TPI tap looks like it is a go go go!

I just ran a test on a piece of alumninum bar stock and came out with some amazingly nice threads. I took about 5 passes to cut the threads because I was not exactly sure how deep I wanted to go or how much load I wanted on the modified tap, but the freewheel screws on perfectly!

Here are a couple of pics:

 

[dumbass]

The cheap bastard attempt to cut freewheel threads (1.375" x 24TPI) into an aluminum timing pulley hub by using a cnc mill and a modified 3/8 x 24TPI tap looks like it is a go go go!

I just ran a test on a piece of alumninum bar stock and came out with some amazingly nice threads. I took about 5 passes to cut the threads because I was not exactly sure how deep I wanted to go or how much load I wanted on the modified tap, but the freewheel screws on perfectly!

Here are a couple of pics:

/quote]

Very nice and well done but how much did that hunk of test alm cost? I mean the real market value. Wish my mill was a CNC.......

Bob

 

[KTP]

Very nice and well done but how much did that hunk of test alm cost? I mean the real market value. Wish my mill was a CNC.......

Bob

I have no idea...it was a leftover from about 200 pounds I bought at Boeing Surplus 10 years ago (before they closed up shop). I seem to remember getting it during a sale where the 6061 T6 alluminum was going for under $1 a pound. At any rate, I only used 0.6 inches of the 2 inch bar for the test, so probably only a couple of bucks even if bought new.

You should cnc your mill, it is not really that hard or expensive nowadays.

 

[TylerDurden]

Sweet.

More info on the process?

 

[Thud]

Looks fantastic.
congrats.

 

[KTP]

Sweet.

More info on the process?

Thanks. It actually was a lot easier than I thought it would be.

First I ground off 3 of the four sides of a 3/8" x 24TPI tap, and ground the end down so it was like a bottom tap (no taper)

Next I machined the aluminum bar stock end to 1.375" diameter at a length (depth) of 0.6"

I then put the tap in the drill chuck (I don't like doing this but I didn't have a collet or endmill holder that would fit the tap shank, and I figured there were very small forces for this cut).

With the bottom at the tap at the level (z=0) of the top of the machined down aluminum bar (bar mounted vertically), I ran the following G-code:

//typical starting strings go here
G01 Z1 F30
G01 X-1 Y0
G01 Z-0.5
G01 X-0.8585 F4
G03 X-0.8585 Y0 Z-0.4583 I0.8585 J0 F4
G01 X-1 F30
G01 Z-0.5
//insert several passes and test fits here until the following last cut:
G01 X-0.845 F4
G03 X-0.845 Y0 Z-0.4583 I0.845 J0 F4
G01 X-1 F30
G01 Z1
//ending strings go here

This performed a counterclockwise helical path cutting the full thread length starting at the bottom and going up exactly one pitch (1/24"). Because the tap had over 1 inch of thread cutting edge left even after grinding off the bottom, I was able to cut the full length of 0.5 inches of threads in just one ccw helical revolution (G03).

 

[recumpence]

Very cool! We did this at the shop with a wierd diamons shaped cutter endmill. Glad to know it works with a tap as well.

So, I would have thought climb cutting would work best? I guess not. That thing looks beautiful!

Matt

 

[KTP]

Very cool! We did this at the shop with a wierd diamons shaped cutter endmill. Glad to know it works with a tap as well.

So, I would have thought climb cutting would work best? I guess not. That thing looks beautiful!

Matt

Thanks Matt. I wanted to try conventional milling first by going from bottom to top ccw, but yeah, I could have gone top to bottom cw and done climb cutting. I wonder if the tap would have had the tendency to grab into the work? I was taking such light cuts with the conventional milling that I don't think it pushed the tap away from the part, but for lots of threading, climb milling might make the tap last longer...I dunno, my background is electronics, machining is just a hobby I picked up a few years back.

Hey, so while I have you caught in my thread What do you think is the smallest size jackshaft I could get away with using this freewheel mounted to a timing pulley arrangement? I sort of want the jackshaft to be fixed and have bearings pressed into milled pockets in the front and back of the timing pulley, but at least one of the bearings would have to have a smaller OD than the ID of the freewheel (plus a bit for wall thickness). I know a 3/8" ID bearing will fit easily, but I am unsure if a 3/8" jackshaft would be strong enough. Possibly I can find a 1/2" bearing with a small enough OD though...

 

[Thud]

KTP,
I have these working in my 2 speed. They are kinda fragile on install & require a nice pocket to fit into.....I am confident you will have no problems

http://www.vxb.com/page/bearings/PROD/1-2inch/kit834