[lerman]

I will be making some form tools for my new (to me) turret lathe in 3/8 inch thick O1 steel.

I'm planning to use a 3 flute HSS 10 degree tapered mill which is 3/32 on the thin end (and will be about .225 at the top of the material). What are appropriate speeds and feeds? The simplest way to cut this would be to just plow into the material cutting a slot outside the desired outline.

If necessary, I could take multiple passes gradually increasing in depth.

Does this make sense? My trusty calculator (ME Consultant) tells me that even with a constant diameter of .225 I would need to take multiple passes. (I'm assuming that O1 steel is a high carbon steel for the purposes of ME Consultant). ME Consultant wants to limit me to a depth of 1.5 times the tool diameter.

My guess is that I should pick an RPM that works for the large diameter. About 45 SFM for that material would give an RPM of about 750. Then set 750 RPM as the speed and use a tooth loading that is suitable for the .093 diameter (ME pro suggests .00006 per tooth) to calculate the feed rate of .140 IPM.

I suspect that I could go back to my High School calculus and consider the taper to be a stack of gradually increasing steps in diameter. Then for each step, I could do a depth of 1.5 times the diameter of the step. The limit of the sum as the step height goes to zero should give the depth that I could use per pass.

But I can't be the first one to want to do this. Can someone tell me the answer? Or is there a different way to approach the problem that I should be looking at?

Thanks,

Ken

[HuFlungDung]

I think your ideas on speeds and feeds are okay.

I'm not sure how much room you have for your tool to work, but I would probably rough the area with an ordinary straight endmill first, cutting to the profile outline at the bottom of the stock.

Then, I would make a series of offset paths for the tapered endmill at full depth. The effect would be that the heavier upper section of the tapered flutes would be cutting first. Using the calculator, I would determine how much offset of the profile would be required to cut about the first .125" depth, then for .25" depth and finally for full depth. The depth of cutter engagement would increase for each successive pass.

If chatter becomes a problem, I would go back and create intermediate profile offsets that would allow the tip of the tool to cut the final profile, but at only 50% depth into the material, followed by another pass (using a different offset profile) at full depth.

[lerman]

Thanks for your help.

Unfortunately, I don't have much room to work with.

But, I could take a 3/32 mill and cut to the full depth of .375 in three passes right on my calculated path. I could then take a 3/16 mill and (if I calculated the slope correctly), take a .114 cut at the top on my calculated path.

Then a final cut with my tapered cutter could clean things up without having to remove a lot of metal.

A nice thing about that approach is that a four flute 3/32 mill could spin at 1400 rpm at .34 IPM and in about 20 minutes chop off the bulk of the excess material. (A single pass will be around 2 inches long).

I suppose that if I wanted to, I could make the steps oversized. The taper is just to provide relief for the cutting edges. Once I'm away from the cutting edge, it would probably be ok to just step down.

Thanks again for helping to stimulate the thought process.

Ken

[Cruiser]

I get the impression your doing a tappered hole, so i'd set the pecks so the chips don't load the flutes much at all or they will ride the peck and go back into the hole and then and then and then !