The Home Machinist!

Thanks. Assuming leaded brass (or any free machining stock), and assuming that the width and depth of the cut will permit using a small end mill, I can see that it should work quite well, in particular if a roughing cut is taken first, then each side of the helix taken to width and depth independent of the other. Even with hand cranking, a respectable finish might be possible. Cranking through a gear reduction would be desirable, however. I'd suggest something like a 10:1 reduction, so there's more control over the feed rate.

I heartily endorse the idea of a loaded nut, regardless of other choices made. Without that, establishing a reliable lead will be questionable.

The use of less than free machining material would most likely be troublesome due to the extremely small end mill that would be required for the cut. A high spindle speed (in excess of 10,000 rpm) would be very desirable. Slow speed is pretty much a guarantee of broken end mills unless very light cuts are taken.

This project might require a little patience, but it's certainly possible.

Were I to make a recommendation of material types, without knowing more, I'd suggest leaded phosphor bronze. It has wonderful machining characteristics. It's horrible without lead, however.

Harold

Harold_V wrote: A high spindle speed (in excess of 10,000 rpm) would be very desirable. Slow speed is pretty much a guarantee of broken end mills unless very light cuts are taken.

Not going to get that kind of spindle speed out of any 3-in-1 that I am aware of. Mine tops out at ~5,000rpm. I did see a project somewhere on the web once where someone made an adapter to mount a dremel type tool to the quill of their mill.

That said, I have had no problems cutting 3/32" slots in steel (unhardened O1 tool steel) taking shallow cuts (0.025" or so, IIRC) but that's using the power feed on the table with a fairly slow feed rate rather than hand-feeding. I was using a new, good quality M42 two-flute end mill too -- not a cheap Chinese bit. I do find that makes a difference!

Torch wrote:That said, I have had no problems cutting 3/32" slots in steel (unhardened O1 tool steel) taking shallow cuts (0.025" or so, IIRC) but that's using the power feed on the table with a fairly slow feed rate rather than hand-feeding. I was using a new, good quality M42 two-flute end mill too -- not a cheap Chinese bit. I do find that makes a difference!

I got baptism by fire when I had to machine some 1/32" slots in 6061-T6 aluminum. Had only 2,700 rpm at the spindle. Not nearly enough. Your 5,000 speed would have been a gift from heaven.

Harold

As I said in the beginning I have a small that is SMALL 3 in 1 Its just a little bigger than the old NUMAT. I can't find a name on it so I guess finding part will be a nightmare. Any way I just checked on RPM and 2500 is tops on the lath and the mill does that mean I need to start looking to farm out the project or do you think it is possible on my machine keeping in mind I have two left hands when it comes making chips.

You can make the cuts at slow speeds, but the feed rate will be unbelievably slow. The slightest acceleration will most likely manifest itself as a broken cutter. The fixture you intend to use will advance the cut at a respectable rate, but because it's tied to rotation, you'll have to rotate at a dead slow pace. That's really the feed rate. I had suggested a 10:1 ratio. I'm now rethinking that. You may wish to drag it down to 25:1. You'll need the ability to just creep, assuming my thoughts are correct. I have no way of knowing because information isn't forthcoming.

Considering you're talking about a ten pitch, at best, you would hope to use a 3/64" end mill. They break like glass. Even a 1/16" would be a tough call. Rigidity is critical, for the slightest irregularity will break the cutter.

Again, it would really help if you could provide some more information. How deep the channel, and how wide you'd like it to be, for example. Right now all anyone can do is guess at what you're trying to accomplish. It may be obvious to you, but it isn't to those of us that don't understand your objective.

Harold

Harold
Sorry you are right it that old saying being to close to the forest ? The part has 5 groves .090 wide and .065 deep land between each grove as close as I can measure is.033 the diameter is 3/8 length is about .648. I'm inclosing a photo of a finished part That I hope will help clear up some details. Jim

Now we're getting somewhere!
You can use a short 5/64" end mill and enjoy success without any of the worries I mentioned*. That's not to say you wouldn't benefit by higher spindle speed, for you would, but you can do the job with what you have. You should be able to rough the part in two passes, staying on center, then take two finishing passes, one on each face, to depth. If you choose something like I suggested (leaded phosphor bronze), it should work quite well. Tougher material will most likely require a somewhat different approach, such as more roughing passes. Once roughed, there's no reason why you can't take a full depth pass on each face, for finish, even if you choose tougher material.

You likely understand that it's important that the end mill be on dead center, otherwise the helix will not be at a true right angle to the axis.

I hope you can see the value of providing total information. Had you made mention of the size of the groove originally, I could have responded immediately instead of playing the guessing game.

*You'll still have to have control over the feed rate. a 5/64" end mill is still pretty small.

Harold

Harold_V wrote:You can use a short 5/64" end mill and enjoy success without any of the worries I mentioned*. That's not to say you wouldn't benefit by higher spindle speed, for you would, but you can do the job with what you have. You should be able to rough the part in two passes, staying on center, then take two finishing passes, one on each face, to depth.

5/64" is roughly 0.078" so the finishing passes would be 0.006". Easy enough to accomplish by adjusting the table position left/right. Three questions:

1. Since this is essentially a slot-cutting operation, is it safe to assume that a 2- (or possibly 3-) flute endmill would be a better choice than a 4-flute?

2. Would you reverse the direction of rotation between finishing passes?

3. Is it better to use conventional milling for the finishing passes due to the manual feed, or attempt climb milling for the improved surface finish?

Torch wrote:1. is it safe to assume that a 2- (or possibly 3-) flute endmill would be a better choice than a 4-flute?

I'd be inclined to go with a 2 flute. If deflection is a serious concern, there's always carbide, although with a proper material selection, it may not be necessary.

2. Would you reverse the direction of rotation between finishing passes?

With a preloaded nut that would be desirable, but, again, material selection can play a huge role in finish. Even conventional machining, finish could prove to be satisfactory.

3. Is it better to use conventional milling for the finishing passes due to the manual feed, or attempt climb milling for the improved surface finish?

Climb milling is always the best option, assuming it's possible. I expect cutting forces on the finish cuts would be very low, so I expect climb milling would be the best choice. A great deal depends on the quality of the setup---how well the piece is supported and if there's any lash in the drive system. Instead of gears, belt reduction might be a good choice.

This should be a fun project to conquer.

Harold

Harold_V wrote: Instead of gears, belt reduction might be a good choice.

The same thought crossed my mind, especially at that ratio. I was visualizing a grooved wheel of sufficient diameter on the driven end and a double wrap around the handwheel shaft with a large diameter industrial o-ring as a belt -- somthing with a tiny bit of stretch to keep it taut yet stiff enough to minimize chatter and vibration.

This came to mind. Both pulley and drive wheel would move in and out together. just have to figure out pulley size to get 30 to 1 ratio

Ummm, if you want them to move in and out together, at a 30:1 ratio with a 10tpi driven shaft you would need a 300tpi pitch on the handwheel. That's getting pretty fine.

I think I'd just fix the handwheel shaft in place and let the "belt" roll along the shaft. That's one reason I was thinking of an o-ring -- the round profile will drive itself along.