Face "pocketing" on a lathe?

[BT Fabrication]

I've never used a round button insert before... But isn't this something they'd be good at?

on end facing, no not as much as the heel on the bottom of the tool likes to drag too much. A DCMT insert is a good spot to come in and machine it to the center.

 

[gregormarwick]

This is the kind of answer I was hoping for. I have this kind of tool, but when I try this approach. it still rubs on the inside wall. It's already a 0.25" IC (VCGT221) insert so going smaller is possible. Solid carbide was supposed to be the answer, but turning from OD to ID to completely clear the floor didn't work well. I suspect it was because the solid carbide wasn't designed to cut on the outside and inside of the tip. It cut fine while moving down the wall in Z, but crummy while moving across the surface to center.

I haven't tried any tool like that with a V insert.

All of mine are 55deg D inserts, or the same geometry in solid carbide. Certainly the one I linked would have no trouble cleanly cutting that geometry as I do it frequently enough, but as EG kindly pointed out it is too big.

 

[Mike RzMachine]

It seems like an insert drill that also functions as a boring bar would work well here. Facing may not be ideal.

 

[DethloffMfg]

Why is an end mill not a good solution for this? Are you having roundness or finish issues? Frankly for changing hole sizes frequently, in a shallow hole on a Y axis love tool lathe, I can’t think of a better solution than an end mill.

 

[Radar987]

Historically, I've just turned blanks on the lathe and milled the pockets. More recently, I bought a new lathe with live tooling and Y-axis which allows me to mill the pockets, but it seems like there must be a way to turn them.

Just mill them. You have something against using an endmill? Trying to reinvent the wheel?

Add a finish boring operation for cosmetics, if you want to.

A machinist is his own worst enemy. Wasting effort and brainpower to avoid doing something that already works.

 

[Radar987]

Why is an end mill not a good solution for this? Are you having roundness or finish issues? Frankly for changing hole sizes frequently, in a shallow hole on a Y axis love tool lathe, I can’t think of a better solution than an end mill.

Goddammit you beat me by 1 minute.

 

[Donkey Hotey]

Is the nub / finish at the center the bit you're having issues with? This still seems like an ID boring tool, carefully set to center height would do the job but, that artifact at the center would depend on careful setup.

 

[rjwalker1973]

Well I must say that I'm impressed with all the responses. Based on what I'm hearing, it looks like I'm probably not going to get away without a roughing plunge of some kind. That opens up the options for the finish tool. If nothing else, I think this puts to rest the thought that there was some "perfect" tool for this that I just hadn't found.

Why not? Like I said earlier plunge in on center with a center cutting end mill leaving a little on the walls and floor. Finish with carbide bar even if you have to get two different ones to finish the walls and floor.

 

[guythatbrews]

A ccmt or tcmt will finish both the wall and floor. Somethings wrong if you can't make this happen. Either of these tools will be more robust than a v or d style.

I'd either mill or flat drill the center leaving a few thousandths for finish. A center cutting endmill isn't flat, and they don't cut near as well as a flat drill. You can get closer to finished size by offsetting and milling the bottom, but it might take longer.

A face grooving tool will work for the whole part and will cut to center, but in this small size they are kinda fragile and $$$. I'd only use them as a last option.

Run some numbers and see which method makes the most sense for your particular situation. Take tooling cost into account.

 

[Houdini]

Looks like a job for a little PhHorn grooving tool IMHO.

 

[Kalsek machine]

Allied Machine and Engineering has a tool called the ECOcut drill. (Its actually a Ceratizit product originally) I love them for drilling and pocketing features like what you posted. Pricing isn't bad either and they leave a great finish.

 

[rwskinner]

I've looked for a long time and never found a good answer. I'm hoping that I'm just not describing the problem in the right terms. Most of the small parts I make have a circular pocket in the top or bottom (or both). pockets range in diameter from 25mm to 32mm and depths from 0.5 to 2mm. The floors need to be smooth and flat. A radius in the wall/floor edge is not a problem at all.

Historically, I've just turned blanks on the lathe and milled the pockets. More recently, I bought a new lathe with live tooling and Y-axis which allows me to mill the pockets, but it seems like there must be a way to turn them.

I've tried using a boring bar for V inserts with the tip pointed forward "SVMBR" (drags on the walls), standard boring bars (rubs on the surface), small solid carbide bars (poor finish on the floor), etc. I've seen face-grooving tools used to make wide grooves, but never tried one and the demos never show them machining to the center. I've seen some single-insert drills that look like they might work, but I don't know how flat of a floor they would make.

Parts are Aluminum, 17-4PH in the H1000 condition, and plastic. Pics attached are an example and drawing.

Heck, I would just plunge straight in with a center cutting end mill then use a small boring bar to finish it up to size. It would only take seconds.

 

[Dan from Oakland]

I just use a Kenametal Top Notch Full Radius Groove insert and increase the OD side clearance angle so that the insert does not rub.
They work great for grooves up to the depth of the insert. These were kinda deep so I used the single end longer top notch insert.

 

[Marc 1982]

Historically, I've just turned blanks on the lathe and milled the pockets. More recently, I bought a new lathe with live tooling and Y-axis which allows me to mill the pockets, but it seems like there must be a way to turn them.

If you are a good lathe guy you can do it without milling it. If not, then just mill the pockets. It's up to you to make that call as there comes a time when its more practical to mill something.
As far as lathe, all you need is a flat bottom drill or endmill, and a ccmt 80* boring bar to do this. maybe add a semi-finish pass and a final finish pass on the wall.