Milling Thin Cylinder

Any suggestions how I can mill 1/4" 12L14 rod, vertically in the vice, to leave a cylinder 0.06 diameter and 0.22 tall?

I've tried: One pass, multiple passes to full depth sneaking up on the diameter and multiple passes at final diameter but working down. Whatever, I get a pyramid about 0.05 to 0.04 at the top!

Not really looking forward to using the lathe because what has to be milled below the cylinder requires precise centering and there are a couple of dozen to do.

would I be any better using 4140? Using 1/8 end mill but not sure this is an issue. 1"/min feed at 1900 rpm on a Taig mill

Thanks.

Define ''precise centering'' 0.001''? 0.0001''? I would build a soft jaw for my mill vice, or use my collet closer. Either way would allow you to locate on the center without further measuring once set up. Turning the cylinder portion in the lathe would be the easiest way.

What you need is a collet mount for the mill table. You can buy them, but I made my own.
Attachment 471628

Buy (ebay) an ER32 collet on a 20 mm PARALLEL shaft
Cut the shaft off just behind the head (slow but bandsaw OK)
Put 20 mm shaft into collet, then put shaft into lathe chuck.
Face the cut end of the shaft off to below the surface (ie rely on the rim)
Groove the side of the head
Make custom clamps to hold down onto T-slot

Then, put 10 mm shaft (a broken cutter shank maybe? Must have a few of those!) in collet, place on table., put other end of 10 mm shaft into spindle collet.
Bring down gently to just touching the table, and clamp firmly onto table
ZERO the CNC X & Y at that point.
Release 10 mm shaft and remove

Now you can mount any round shaft on the mill table 'exactly' aligned. I do lots of this.

Cheers
Roger

Brilliant. Thanks Roger also for the detailed explanation of centering.

John

Now there is one small possible gotcha here.

I was using this to mill hex flats on a special purpose nut (round rod stock), but the very first results were spectacularly bad. The nut was mounted on a threaded fixture in the collet. So far so good. But the normal clockwise spin of the cutter (M3) cause the nut to undo and spin off the fixture, with rather destructive results as the cutter chewed through it. You may have to sit down with a nut and bolt to visualise this.

The solution was to buy a left-handed cutter and do the milling with M4. Then use a spanner to get the nut off. So I have one left-handed cutter in the drawers, just for this.

Cheers
Roger

I hit the same problem.. In the interests of time printed hold-downs from filament with carbon fibre. Not good enough and undid the collet. Sort of fixed by changing the compensation - my mill won't go backwards. Will make proper metal hold-downs and I'm pretty sure it will work. Also need to take really fine passes as there was some vibration. I very much like the Taig mill but not if I were doing this for a living!

Thanks for the help

Quote:

---

Define ''precise centering'' 0.001''? 0.0001''?

---

is ok, i'll handle it :) understanding/talking tolerance and conditions requires time, so, if they are not there, you have to hunt them down, like a real detective :)

Quote:

---

to leave a cylinder 0.06 diameter and 0.22 tall?I've tried: One pass, multiple passes to full depth sneaking up on the diameter and multiple passes at final diameter but working down. Whatever, I get a pyramid about 0.05 to 0.04 at the top!

---

seems that 0.06 should not be 0.04, nor 0.05, thus ± 0.01 is too much :) let's cut it in half : ± 0.005 should be ok

now let's metric this : 0.06 ± 0.005diameter and 0.22 = (1.524±0.127)x5.588

now let's round it : (1.5±0.1)*5.6; 0.1 tolerance may be ok, considering that he doesn't want to use the lathe ?! :)

machining advice : rough it with a small tool, so to avoid stress inside the material, then finish with something even smaller, like dia 2-3 mm; the active length of the flutes should be <5.6mm, so to avoid recutting the top as you go down (this may induce a pyramid shape); one way to approach it, is to grind your endmill like a T shape mill, thus make it's active length shorter; for example, use 2.5mm active length

also, you may need a tool with sharp corner radius, otherwise lateral forces may induce stress into that tiny part

Quote:

---

because what has to be milled below the cylinder requires precise centering and there are a couple of dozen to do

---

that may mean that bottom milling occurs after top milling of that 0.06" cylinder ; in such a case, 1st operation alignment may not be precise, considering/hoping that there is enough stock left to align for 2nd operation ( is that thing, like when you have enough stock, so to avoid centering )

as for 1st operation chucking, another idea is to put the material in the spindle, then use a turning tool inside a vice ?! kindly :)

[QUOTE=deadlykitten;2478060]....even smaller, like dia 2-3 mm; the active length of the flutes should be <5.6mm, so to avoid recutting the top as you go down (this may induce a pyramid shape); one way to approach it, is to grind your endmill like a T shape mill,

That's good advice. Thanks. But if I grind a cutter to an inverted "T" why would it have to have a small diameter? Perhaps I'm misreading this. In any case would it be best to take cuts not quite as deep (Z) as the flute length and spiral in the the finished diameter, thus having best support without re-cutting higher bits.

is possible to achieve same mrr with different tools; the smaller the tool, the less cutting momentum will be created; this momentum is always there, in both tool and part :)

for example, a big tool may bend/rip a part, or even move it away from the vice, while a smaller tool will work really smooth

such things do not matter for common aplications, but your is at the edge :) from same perspective, tooling for gang lathes has smaller nose radius then tooling for normal lathes, simply because they are smaller, and have to be sharper

in other words, let's say that your part would be 10 times bigger in diameter, but same length : that pyramid effect that you just described, do you think that will appear as easy as before ? is all a matter of L/D ratio :) the thinner the part, the lower the cutting force has to be, so to avoid bending, etc :) i hope it makes sense :)

Yes perfect sense. A great weekend when I learn several new things. Thank you

okey :) as for clamping, if you intend to machine later the part below the cilinder, then you may avoid a collet chuck

mr rcaffin did a great job at explaining that approach, yet there may be a faster way for you; there are a few things missing from your request ( please, don't mind, i'm just saying ), so i will use an example to show what i mean : let's consider that below your 0.06cilinder is a shape that can be inscribed within a 0.1 circle, and that shape must have a concentricity of 0.01 with your upper cilinder; this means that the minimum stock that will allow you to craft your part is 0.11

whatever is bigger than 0.11, is simply room for errors :) so, calculate your stock, and whatever is there may simply allow you to avoid useless alignment for your 1st operation; a collet can deliver consistency, but maybe you can simply go with a v block inside your vice ( faster to clean, faster to mount/unmount )

is all about tolerances / kindly :)

Ah! Thank you. The shape below the cylinder is about 0.2" diameter and needs to be concentric to within 3 or 4 thou. So, I should turn my 1/4" stock to just above finished size for the whole length it will be in the vice. That way there will be no problem with a rough finish on the blank and it should be concentric with the small vertical V slot in my vice. That means about 2" of turning which I think my lathe can manage - an Atlas 612 - and I'll need to re-adjust the tail stock but that's something I do often! Again, thanks to both of you.

if i got it right, then your part is simply 2 diameters that have to be concentric; you simply avoided the lathe, because those diameters are relatively small

yet, you may actually machine it entirely on lathe, by using a false center for the tailstock, that you cut away once the part is finished :)

is it ok ?

Sorry, I confused you. Below the cylinder are bolt heads, some square and some hex. Sizes are not standard as a model of an 1840 factory engine. The thread is 0-80 about to scale and if I get this working I have some 00-90 to do.

I'm experimenting with both methods and think the collet may be better for me. In both case I need to turn the blank oversize so I have a smooth cylinder for the lathe chuck and either collet or vice. Difference is the collet will adjust for minor differences in the diameter of the blank With the vice I'll have to re-center. Someone with a better lathe is unlikely to have this issue. Will see next week.

Difference is the collet will adjust for minor differences in the diameter of the blank With the vice I'll have to re-center.
That is the key difference.

Cheers
Roger