Best tooling for 1/2" profiles on a micro mill?

[sansbury]

Hi all,

I have a project that will require cutting a bunch of 2D profiles in 0.500" aluminum on my Sieg X1 micro mill. I've done two pieces using an ordinary 4-flute, 1/4" endmill and baby-sitting it with a chip brush to keep the cutter as clear of chips as possible. I ran at about 1000 RPM (top end of the lo speed range IIRC) and 6-7ipm feeds.

The results were good enough but I was curious if there was room to improve. Specifically:

1. Would a 2-flute mill be better? Larger or smaller diameter?
2. Different suggested speeds and feeds?
3. Any benefit to something like a cobalt rougher with the serrated edges?
4. Would spray coolant help with chip clearing or is flood the only way? I have neither but an upgrade is possible.

Assume for the sake of this discussion that the X1 cannot be upgraded to something larger--I've got it CNC'd and the extended Y and for the size and cost it is a sweet little machine!

[Pres]

Since the spindle on the X1 is light duty I'd stick with 1/4"-3/8" end mills.
4 flute has less space for chip clearance and can load up quick.
2 flute can cause quite a bit of spindle "rattle" on the light duty X1.
3 flute is about the best compromise (imo).

To save the enormous mess/problem that flood coolant produces (besides NOT being able to see the actual cutting going on) a good solution is air/mist spray.
It helps cool the chips for easier ejection from the flutes. Also a good medium for including a light cutting lube and can help blow the chips over in the direction you'd like them piled up at.

You wrote: "for the size and cost it is a sweet little machine!"
I agree! Just keep it within its cutting capacity (i.e. light) and it will perform admirable for its price.

For some reason Taig/Sherline owners are able to do that ok but many X1 owners seem to want to hog stuff out and then complain that it's too weak. ?)

Whatever, just drag out the 'ol checkbook and you can do it faster with a bigger machine!

hth,
Pres

[MIKE JEFFERS]

a 2 flute hi-helix cutter ronning flat out ,2000rpm, would be better if you can justify the expense ,you could try smaller cuts/faster feed that would bring the cycle time down,
the more you run a program the more confidence you get in it
build a tray and flood coolant it is the ultimate answer ,but try rocol or similar tapping fluid with a bit of parafin (kerosene in the us i think) to thin it and dispense it with an oil
can
x1 a great little mill within its limits

[digits]

I am not a great fan of my X1, but I have had some pretty decent results since I threatened to cut it in half!

I am cutting through 1/2" 6082-T6 aluminium with a 6mm (0.236") 4 flute hss end mill, 0.4mm (0.0157") per pass full width at 450mm/min (17.7IPM) and 2000 rpm. I am however running full flood coolant - which is messy, but great at removing the dust-like chips.

I got the cutting speeds and RPM from the excellent ME Consultant Pro BTW.

One major word of warning, the X-1's gearbox is very frail - I have exploded the gear selector fork at least 4 or 5 times! It usually happens during the first pass of any cut, as if I'm aiming for 0.4mm deep but the surface irregularities are also of that order, the X-1 can suddenly find itself cutting 2x as deep as I had intended. Sometimes it just chatters like mad, and I intervene, but other times, the gearselector just shatters in an instant! If you program to cut some air for the first mm or so, you will probably be fine, but IMHO it's crazy that some fairly gentle surfacing cuts can break the thing!

[MIKE JEFFERS]

run mine with a belt drive tho i had no problem with the gears
i usually run with a ramping cut ,this gives everything an easier time ,i use the excellent dolphin partmaster cam and ramping is just a tick away

[sansbury]

Thanks everyone. It's obvious that I was cutting WAY too slow. I was probably running the cutter at 750RPM or less, when I should have been running it wide open (~2200 allegedly).

I tried a few quick test passes at full spindle speed and it cut some very nice slots .065" at up to 10ipm, which was deeper than I planned but still working out some Z-axis quirks. I'm only using 125oz motors direct-drive so I'm guessing I top out at 15-18ipm, so I will try some experiments cutting faster and shallower, but it's clear this is the way to go.

For giggles I ordered a 3-flute 1/4" cobalt rougher, so I will see how that works out. The cobalt is probably overkill but it was only a few bucks more so I figured why not.

I've been starting to plot out a flood system. At some point I'd like to be able to run semi-unattended (i.e. working on something else three feet away) and it seems like flood cooling is the ultimate, if messy, answer for that.

[aviator411]

Sansbury,

Can you tell us what you spent to CNC the X1?

[sansbury]

I'm using parts from my other machines so no out-of-pocket to speak of. Bought new it would probably be around $250.

The mill itself is 100% stock leadscrews and nuts. I have the extended Y and will be adding the long X eventually which are optional. The motors are 125oz unipolar driven by a Hobby CNC Pro board. I made motor mounts using some 1/2" aluminum plate and skate bearings which will fit the leadscrews with just a tiny little bit of filing. These coincidentally are great even with the handwheels on.

I am still figuring out the Z. Right now I am driving the quill using a 125oz motor in direct-drive. The quill on these is famed for being a sloppy mess. It rides on a mushy spring and has more backlash than a loose bicycle chain. So far I've found that with s/w comp and endmills of 1/4" and smaller, it seems to work well enough for 2.5D milling. I'm using a 125oz motor on the quill because that's what I have but it's probably too small as it stalls after plunging about .02". However that's with a poorly-aligned motor mount and no flex coupling (didn't have one handy). I am getting another jaw coupler and will see after that.

Most guys CNC the column and lock the quill. This has pluses and minuses. You get a lot more Z travel (~8" vs ~1") and there are now worries about problems with downforce pulling the tool into the work. Backlash can be reduced to very little and some people have done very nice 3D surfaces with these. However, the mill is more rigid with the head locked to the column. When moving lifting the head up off a surface, sometimes one edge of the cutter will cut a little divot as the head tilts due to the loose gibs. Brass gibs and big motors allow for more tightening but this is a non-issue with the quill method. There is a lot less weight to move which is always beneficial. Also this required nothing more than a motor mount plate and a few holes tapped in the mill head.

So far I am getting parts accurate to .01" or better. That won't impress too many here but I got it without spending more on the CNC than on the mill. Right now that seems good enough for my projects thus far so I am happy. If I wanted I could remake the sloppy hand-made motor mounts with CNC'd ones and then make delrin anti-backlash nuts and that might improve it. Others have gotten these to better than .005".

Bottom line is that you can CNC one of these pretty inexpensively and get decent results.

[aviator411]

Sans,

Many thanks for your reply. I'm considering it. Will look forward to your progress with the Z axis.