Carbide bits keep breaking :(

[BrassBuilder]

I have a few (very few now) 1/8" carbide bits. I have a part that I am machining out of a 5/8" thick block of 6061 aluminum. The part is approximately 1" x 1-1/2". I also have an X2 converted over to CNC. In cutting some practice parts while learning the CNC functions, I cut my part out of 1/4" thick material using a 1/8" HSS end mill. Absolutely no problems and in fact, I have cut a few of the pieces with the same bit. I now needed a way to get a deeper cut (5/8" vs 1/4") and the only thing I could find was some "long reach" carbide bits with an 1/8" shank. I *had* four bits. I am now down to two. I didn't even make it down to 1/8" with my cuts before I lost two bits. Here is what I can tell you for sure:

Cut depth:
.020

Flutes:
4 (I now know 2 flutes would have been better)

Table speed:
approx 3" per min

Spindle speed:
unknown. I am running the LMS belt drive conversion. I have the belt set up on the "low speed" side and I am running the mill with the speed control turned up half way. I feel that I am running the bit about the same speed as when I used the HSS bit.

Coolant:
None. I do not have a coolant setup.

Searching around the site, I *think* I might be running the spindle too slow and the fact that I am not running coolant probably does not help either. I have seen WD-40 and automatic trans fluid mentioned as acceptable subs.

Any advice? I have three of these parts to cut and at $7.00 a bit, this is already getting to be a rather expensive cut.

Thanks
Mike

[jetski]

You need a mist type cooler and a tin coated carbide 2 flute will help. You can buy a cheep mister from enco like under 40.00 good investment. I am betting the cutters are loaded with alu. The cool tool or any water based coolant will work. If you cut a lot of alu. look for a coolant that brags on aluminum cutting. I use Marcool #983 for all cutting alu to air hard steel in a hurco. If you dont go to a cutting fluid the chips stick to the cutter when it gets hot almost like gauld and then your cutter is doomed. Hope this helps.

[BrassBuilder]

Originally Posted by jetski You need a mist type cooler and a tin coated carbide 2 flute will help. You can buy a cheep mister from enco like under 40.00 good investment. I am betting the cutters are loaded with alu. The cool tool or any water based coolant will work. If you cut a lot of alu. look for a coolant that brags on aluminum cutting. I use Marcool #983 for all cutting alu to air hard steel in a hurco. If you dont go to a cutting fluid the chips stick to the cutter when it gets hot almost like gauld and then your cutter is doomed. Hope this helps.

LOL, I am at the enco site and I was just going to look for coolant when you posted. I wanted to cut these parts today. Is there an accepetable substitute for the coolant for right now? I would suspect that anything that will keep the bit cool will help.
Thanks
Mike

[LeeWay]

Your probably not going to have a problem with the carbide heating up enough to do much damage to the cutter, but when the aluminum heats up, it likes to stick to it. That will cause trouble. WD40 spray works nicely to keep it from sticking. 6061 doesn't stick nearly as bad as some other aluminums. You need to crank the spindle speed all the way up. Faster than it can go would be preferable. I think in high gear, your mill may run about 4300 RPM. That will help.

Carbide is really brittle stuff. If you have any backlash or vibration at all, it can cause a small carbide EM to snap. No matter what DOC or feed and speed you are running. You need your steppers to run very smoothly and your drawing to have as few starts and stops as possible.
Cobalts are nice. They are only semi brittle. Again not the best choice for an X2. HSS is really going to be your best bet in aluminum. I use both two and 3 flute coated for aluminum or plain. I do run coolant in the mill.
When I was milling aluminum in my router, I did use 1/4" two flute carbide bits and used WD40. that worked pretty well mainly because of the speed being much higher. It is also a pretty rigid router made mostly out of steel and thick aluminum plates. The weak link with milling on the router is the open router motor and chips getting inside. Hasn't caused a problem yet (knock wood), but I won't be milling much more aluminum on it now that the mill is online.

[djr76]

You are running the endmill to slow. Whether it be hss or carbide, smaller endmills need to run much faster.

[LeeWay]

I forgot to mention to use lead ins as well. They really help take the stress off plunging in. Especially so with a small 4 flute cutter in aluminum.

[BrassBuilder]

Originally Posted by LeeWay Faster than it can go would be preferable. I think in high gear, your mill may run about 4300 RPM. That will help.

Originally Posted by LeeWay HSS is really going to be your best bet in aluminum. I use both two and 3 flute coated for aluminum or plain. I do run coolant in the mill.

Wow. That fast? I am definatly running too slow. I went out and bought some ATF for a coolant. I was going to pick up a can of WD40 but forgot it...sigh.

As for the HSS bits....I cannot find any with a length of cut over about 3/8". I need to go 5/8". The only thing I could find is the carbide bits. I just need to figure out the speed to run everything now.

My motors seem to be smooth and tight. I do not have any backlash (or very little...well under .001) in the axis. The first bit broke just before a turn and the second one broke on a straight shot. So...they are not breaking while the machine is changing directions at least.

I'll go down and try it again. I guess this will be a learning experience to say the least.

I'm also looking at a coolant setup now. I think I will scratch build it something like Hoss did. That is a pretty slick setup.
Thanks
Mike

[BrassBuilder]

Originally Posted by LeeWay I forgot to mention to use lead ins as well. They really help take the stress off plunging in. Especially so with a small 4 flute cutter in aluminum.

Hmmmm...lead ins....I suppose this is gradually putting the bit into the work versus straight down? I'll need to figure that one out.
Mike

[Geof]

You have bought the cutters so you cannot change that, however, do not get small diameter four flute again if you want to use them on aluminum.

Two flute, uncoated and if you can get it micrograin carbide; these cutters will have a shinier appearance than most uncoated carbide cutters.

Speed (rpm): With carbide you can easily go up to 3000 feet per minute and a simple calculation shows that to get this at the periphery of a 1/8" diameter cutter you would need to spin it at aroung 91,000 rpm. I think I am safe in making the assumption this is faster than you have available. Go as fast as you can; no matter what size cutter you are using go at top speed with your machine.

Feed (ipm): With two flute carbide cutters 1/4" and above it is probably possible to feed at 1% of the cutter diameter per tooth, i.e., 0.005" per rev or 20 ipm at 4000 rpm. But, you should only be taking a depth of cut of about 50% of the tool diameter with an engagement of up to 60%, i.e. 0.125" deep and 0.15" wide.

But you have 1/8" four flute and you are cutting full width so you have to be very conservative, stay down in the 2 - 4 ipm region for now until you have completed some successful cuts and then maybe start going faster.

Plunging? As Leeway suggests, NO, not a good idea. The flutes load up with chips very quickly; milling cutters are really meant to cut sideways not down. Ramping in is acceptable but make it a gentle wrap for a small cutter; maybe one cutter diameter down for each inch of forward travel.

Lubricant/coolant. Absolutely essential. You can probably get away with brushing it along the intended cut line or use a little spray can. I have never found WD40 to be very good on any material; the ATF works very well on aluminum but, of course, the best thing is a proper cutting fluid.

[BrassBuilder]

Wow. Thanks for that reply Geof! Very informative.

Here is an update from this morning:

I got two of the three parts cut. I went back to the store and got a couple cans of WD-40. Actually it was Advanced Auto's store brand, but it is close enough. I drenched the cutting area with lube as the bit went around. I didn't have a single problem other that it taking around 45 minutes to go through 5/8" of aluminum at .020 a pass.

I now have a bed full of lube and aluminum chips. I am not really certain how I will get that cleaned up.

My plans for next weekend? I'm going to dive in and build an enclosure and add a self contained coolant system based on Hoss's design. More time and money, neither of which I have plenty. But it should be fun. LOL

Mike

[Geof]

Now you have determined the outer limits of your problem; first, you discovered waht was too fast under wrong conditions so it did not work; now you know what does work but is slow. Somewhere between these limits is an optimum region which you can work towards; just be systematic and document things so you can refer back and know what worked when.