Minimizing heat build-up when milling?

HMEM,

I'm milling quite a few 1/4" wide grooves in carbon steel to a depth of .315". I'm using a nice carbide end mill and taking passes of .020" at a time. I've been running the spindle at 1200 rpm but the part is getting pretty hot by the end of milling one groove. I don't have a coolant system and probably won't for a while as I work pretty slow anyway.

I know the tool can take much higher RPM's so my question is: Would cranking the mill up to 5200rpm (it's maximum) help to cut down the heat?

The passes would take less time as I could feed faster but there will be more friction at a higher RPM too...? Which way would win out?

Things I should probably already know...but don't.

Thanks,
-J.Andrew

Consult a good speed feed calculator. There are several on line. the heat should be carried away in the chip not be retained in the part or tool.
Tin

You don't say how fast you are feeding or wat metal you are cutting but I would say you are not taking enough off and the tool is rubbing. Try 0.050" depth of cut and crank fast.

If you don't have a liquid coolant try rigging up a compressor to blow the chips away and cool things

An air nozzle directed at the cut helps to cool and evacuate chips. I have a mist system which has done OK by me. Not too much of a mess and keep the tool & work cooler then without.
The mist device I have was not too expensive, either.

As Tin mentioned you want to take a bigger cut, right up to the limits of the tool and the mill's rigidity. Insufficient chip loading will actually dull the cutter.

G-Wizard calculates (2 flutes, 1" stickout) that you can cut to .15" in low carbon steel without breaking the cutter. 4400 RPM and 10 ipm feed. Power for that cut is .28HP.

That cut is probably not useful for a hobby mill that lacks the rigidity. I'm with Jason and would recommend .05" DOC @ 5000 RPM and 13 ipm.

If you use aluminum jaws in your vise they can conduct away some of the heat. Note that carbide needs some heat to cut properly.

Hello,

I had some time early this morning to give it another try. I tried running 0.050" depth of cut and cranking at about 13 ipm. The bit survived the cut well enough but it sounded a more like a wood router than a mill. It did throw off a spark as it broke through the exiting end but I've read elsewhere this is ok with carbide tooling.

I should clarify that I'm approximating the feed rate as it's all cranking by hand and that I'm working from a collet block to index these grooves on a 2" round piece of steel. It's hanging off the side of the toolmakers vise a bit but is pretty rigidly clamped.

The work still did get hot but never hot enough to change color or show any signs of work hardening. I finished all the cuts needed but did settle on 0.030" DOC, 2500rpm and about 10ipm just to keep the vibration down.

I didn't get to try compressed air at all as I didn't want to make up the neighborhood with the compressor.

I have noticed a big difference in heat build-up when the part is clamping in the vise jaws vs hanging out the side of the vise as Kvom alluded to. The heavy milling vise does seem to dissipate a good majority of the heat.

Kvom, you also mentioned a 2 flute end mill whereas I've been using 4 flute. In the future would 2 flute end mills be better for steel? I had assumed 2 flute mills were for aluminum use..?

Thanks all for the suggestions and help. I'll post pictures of the project after I tap a few holes and deburr.
-J.Andrew

2 flute for slots where you are using the full cutter width, 4 flute when you are comming in from the side of the work and not using the full width of the cutter.

J

Jasonb said:

2 flute for slots where you are using the full cutter width, 4 flute when you are comming in from the side of the work and not using the full width of the cutter.

J

Click to expand...

That's why 2 flute milling cutters are called slot drills over here. You will find that slot drills are slightly undersize.

Paul.

Ah I see. That makes sense too with 2 flute end mills having more room for chip clearance.

Thanks JasonB and Swifty.

-J.Andrew

There is nothing stopping you from using a 4 flute to slot, but you have to know the drawbacks.

1. Increased feed rate for a given surface speed. Feed is per tooth, so more teeth means greater feedrate to keep it cutting rather than rubbing.
2. More power. It needs more power to make the cut because the material removal rate is higher than with fewer teeth.
3. Greater side load. This is where tool deflection and machine rigidity come into play. With twice as many cutting edges working the side load and tool deflection are that much greater. If the machine is not rigid enough you'll see the cutter pull to the side. Long cutters can bend enough to break. Even short cutters will break on a CNC if RPM (and feedrate to maintain chip load) is cranked up.
4. Less room for chips/coolant. Chip clearance is much smaller with four flutes. Maybe not so much of a problem on a manual machine, but much more so with CNC at high feed.

Cutting metal results in heat. If parts are getting hot enough to harden or blue, something is seriously wrong. I would never expect parts to get that hot unless the cutting parameters are very far off from the material being cut or the tools are very dull.