PDA

View Full Version : Clearing chips? Broken tooling...



jacampb2
01-03-2010, 10:55 AM
This is probably a really noobie question, but I have tried pretty much all I can think of and need suggestions.

While building my new high speed spindle attachment for my B'port, I CNC'ed a fair amount of "Mic 6" aluminum plate I bought on ebay. I believe the "Mic 6" is 7075 aluminum, but I could be mistaken. Anyhow, I broke nearly every 3/8" EM I have. All were brand new when I started, and all were high end Carbide that I got on trade a few years back.

Feeds and speed were 1650 RPMs and about 12IPM, the EM's were 4 flute, center cutting. Machining the outside of my parts and what not, no issues whatsoever. I also did a "profile" cut to cut two bores in the main fixture, one 4" diameter, one 2" diameter. Using a mist coolant setup and running heavier coolant:air ratio than I normally do. While cutting the bores through the 1" plate, I would get chips packing in behind the cutter. I had nice chips coming off, not little needles. DOC was .25" per pass. Down to .5" depth, and sometimes .75" we are fine, normally the last pass or two got to be to much and when the cutter came back around it would snap on the packed chips.

After the first time, I tried following it w/ a screw driver and digging them out. That helped, but I managed to get to close to the cutter w/ the screw driver and sucked it in and broke another EM. So, I tried following it w/ my big shop vac, but the chips get packed to tight, and bang, another EM. All the 3/8" EM's were at least 1" flute length, the first few I had the best luck with were 1.75" flute length. I ended up cutting the bores with a carbide .5" two flute EM and had better luck, but wasted more of my "pucks" from the bores which I had wanted to use for other stuff.

So, long story short, how do you get the chips to stay out of the cut path?

Thanks,
Jason

KiddZimaHater
01-03-2010, 11:37 AM
An air-blast system is the best thing for milling aluminum.
If you have a large compressor able to handle constant blowing, then rig-up your air nozzle to keep a steady blast of air on your endmill.
That will keep the chips out of the way.
Also, you should be using a 2-flute endmill on aluminum. It allows easier chip evacuation. 4 flutes tend to gall-up.
And don't be afraid to give aluminum a heavy feed, say .010 - .015 per flute.

RB211
01-03-2010, 11:37 AM
Use 2 flute instead of 4 flute, flood cooling.

Carld
01-03-2010, 11:41 AM
I think part of the problem was the four flute endmills. Two or three flute would be better. Perhaps no coolant and just a strong direct air blast on the cut area.

JoeFin
01-03-2010, 11:44 AM
Your problem is lack of Flood Coolant

I tried every thing I could think of to NOT use flood while cutting some slots in 6061. 2 flute, 3 flute, 4 flute, carbide, HSS, less feed / more feed. Finally I asked some friends and they all said the same thing,

"Run flood and push it right down the flutes"

Black_Moons
01-03-2010, 12:54 PM
Another thing you could try is buying high helix endmills that are *designed* for cutting aluminum.

you could also put your mill on its side or upside down... J/K, but it would work.. :P mmmm..

Steve Seebold
01-03-2010, 12:58 PM
Why 1650 RPM? I cut aluminum at 10,000 RPM because my machine won't go any faster.

BobWarfield
01-03-2010, 01:19 PM
2 or 3 flutes, not 4, strong air blast or flood, but also, your chipload is a tad high. Remember, SFM burns cutters and chipload breaks them. So, I would back off the feed to more like 9 or 10 IPM on your last 2 deep passes. If you can run 4600 rpm that'd be about right for this cut, then you could speed up the IPM more to maybe 25 IPM.

3/8" diameter going to 1" is really a deep diameter to depth ratio. It's really hard to evacuate the chips way down there, plus your circular slot means chips are always "around the corner" from your airblast.

In additon, with that diameter to length ratio you have to dial back both the SFM and the chipload to have a hope. G-Wizard automatically figures those compensations, or you can look through manufacturer's recommendations such as Niagara on their web site.

FWIW, your IPM at 0.25", 0.5", 0.75", and 1" would be 16 IPM, 13 IPM, and then 10 IPM for 0.75 and 1" depth.

Cheers,

BW

RKW
01-03-2010, 01:34 PM
I like the air stream solution myself since flood coolant would be messy. I have a pneumatic foot switch on my mill so that I can get a quick blast to clean things out or hold continuously for small pockets and slots. I stuck a small regulator on it so I don't get full pressure but just enough to do the job.

The foot switch was new and destined for the trash before I rescued it, so it was a great find. I have not ever seen one like it before or since.

mochinist
01-03-2010, 01:53 PM
Some coolant or wd-40 in a squirt bottle will do wonders, also a small 1" wide paint brush to clear out the chips before the finish cut, turn the spindle off so you dont break your cutter when the brush gets sucked in.

Black_Moons
01-03-2010, 02:02 PM
Foot valves sound expensive.. However, you can buy little 'roller' pnumatic valves at places like princess auto for $30, or 12v DC electrical ones and make up your own foot switch or button :)

jacampb2
01-03-2010, 02:32 PM
I did play around with the feed and didn't get any better results. 10IPM and they still would break, 8IPM and the cutter started to whine like it was rubbing.

1650 is about topping the primary spindle out. I can overdrive it w/ the VFD, but I prefer not to and that is the whole reason behind making an auxilary high speed spindle...

Funny thing, after I fished out each of these EMs, the cutting edge's didn't have any welded aluminum on them, I am pretty sure they just run into the packed in chips and snap.

I have the mist setup cranked and lots of air and coolant, the problem is what Bob describes, the chips are always around the corner. The chips in front of the EM clear great and snow all over the shop, it's the ones behind that get it on the next pass.

I managed to get the work done, but at the expense of a lot of tooling. I will look into getting some two flute bits for working in the aluminum.

Thanks,
Jason

whitis
01-03-2010, 08:58 PM
This is a non-expert opinion, but it appears that you have a number of parameters that are out of range.

- 4 flutes bad, use two
- Your feed rate is too slow. Try 65IPM (2 or 4 flute)
- reduce the depth of cut. baby the depth, not the feed.
- You should use a cutter with a high helix angle to better remove chips.
Positive rake, large clearance angle. Mirror finish inside the flutes helps.
There are coatings to reduce sticking. Small core diameter. In short, a
cutter intended for aluminum.
- Clear the chips after each pass, not while the cutter is in the cut and turning, before starting the next pass.
- spray the end mill down with WD40 before you start and shoot some down the flutes towards the cut while you cut, use flood cooling, or an air blast with mist. Lubricant helps prevent built up edge and helps chip evacuation.
Too much water and not enough coolant may not prevent sticking.

Put aside the problem of why the chips are packing for a minute. The fact that you are breaking the end mills on the last pass should tell you something. Think about it, you are cutting through 0.25" of aluminum and 0.75 " of packed chips. You might as well be cutting 1" deep on your first pass. Different physics but either way, you have 4 times as much chip to remove through flutes that are too tight and were demonstrated on the first pass to not be able to clear the smaller chip load properly.

With a feed rate about 5 times too low, you are making wimpy chips. These chips might take up more space than if you had removed the five times as much metal in one cut. And the wimpy chips may not be strong enough in compression to push themselves up the flutes of the end mill and clear the cut. They probably just crumple up or roll up in little rolls and pack. You also have a small chip to remove the heat. I am not sure about the chip clearance geometry here but there may be a middle regime where the chips are not fluid enough to clear one way and not stiff enough to clear another.

If you are going to use a 4 flute end mill, consider taking a cut that is only half as deep. That way there is less metal to remove from the cut and you may have less of a tendancy to to roll up like a roll of paper and wedge in the flutes. If your cut isn't too deep, you may get a helical chip that clears ok. But if the cut is deep, the turns of the helix overlap each other. Imagine a chip the width of your depth of cut. Now look at the end of your end mill and imaging pushing that chip across the cutting edge and watching it roll up. Does it helix up the clearance grove enough that it doesn't overlap itself? This, and some other factors, will vary with depth of cut and helix angle.

You can get away with a cloggy cutter for profiling but not slotting.

DigiSnapMark
01-03-2010, 10:36 PM
I've had my best results using a single flute cutter... Onsrud and the like. Even with 2 flute EMs, I get clogged up. I also use a micro-drop system, and make sure to keep the air flow enough to get rid of chips immediately.

Like everyone else, I'd say your RPM is way too low... but then, what's why I cut at 7 IPM as well!

Bruce Griffing
01-03-2010, 10:43 PM
A point that has not yet been made - Mic 6 is jig plate - cast aluminum. Not 7000 series at all. It is very soft and does not make chips as well as hard aluminum (eg. 6061-T6). You would be wise to follow the advise given above and be even more conservative because you are using Mic 6. On the question of overdriving the spindle with your VFD - I would for sure do that for these cuts. I would not be afraid at all to go to 100hz. If the spindle gets too hot to touch, then slow down. Otherwise, don't worry.

beanbag
01-05-2010, 04:37 AM
I have TWO air/coolant nozzles with small openings (1/16") and placed pretty close to the end mill. This really helps with chip clearance.

Also, don't use too much coolant, or the chips will get damp and clump up instead of flying away.

What's the rigidity of your machine? On a Tormach CNC with 3/8 EM cutting aluminum, about 3/16 doc, .3 length of cut, 4000 rpm, and 25 ipm is about the most it will want to do. Any more, and it starts to sound "unhappy".

Also, check that you have no backlash on your machine (by putting an indicator from the vise to the spindle and actually pushing on the table).

As everybody else says, use 2 flute end mills.

Carld
01-05-2010, 10:36 AM
beanbag, that's about what I found and do. mist coolant with very little coolant, small nozzle, high air pressure directed to behind the cutter as it undercuts and feed and speed that allows chips to escape. Most the time I use a dry air blast, no coolant.

lazlo
01-05-2010, 10:42 AM
A point that has not yet been made - Mic 6 is jig plate - cast aluminum. Not 7000 series at all. It is very soft and does not make chips as well as hard aluminum (eg. 6061-T6).

Like Bruce says, Mic 6 is aluminum cast into a die mold and then stress relieved, so it's very flat (as least for billet), and machines without warping. That's the reason it comes with adhesive stickers on the sides -- so you don't scrape the flat surface you've paid for.

Mic-6 is considerable weaker than heat treated aluminum, and it's really gummy -- not nearly as nice as 6061 or 7075 to machine.