[cnczoner]

Hi all,

Using 1/8" Enco 2-flute, 3/8" LOC, 3/8" shank, uncoated HSS endmills on 6061-T6. Slotting at 1500rpm, 0.05" doc, 5ipm, the endmills are breaking. I'm also lubing with ATF. So I slowed down the feedrate to 1.5 ipm and that worked, but a simple part took 1.5 hrs!

I hear of people machining much faster than this, so is this related to my 1500rpm spindle? Should I use less DOC and faster feed? Is there perhaps a different type of endmill I should be using? Most other endmills talk about harder cutting edges, but I'm not sure if Carbide or other materials are actually stronger so that I can cut faster...???

Cheers,
-Neil.

[Belding]

For effecient machining with a 1/8" end mill in aluminum you want to be above 5000 rpm. Ideally in the 10,000 rpm range. Thats what my speed an feed calculator tells me.

zac

[cnczoner]

So a higher spindle speed will allow me to use a higher feedrate without breaking the bit? I could easily make a mount for a dremel rotary tool on my spindle head, but I may run out of hp... I need to lookup how my hp a dremel tool has.

Does your calculator give you hp required? If so, how much hp is required to run 1 1/8" endmill at say 10,000 rpm and 20ipm, with a 0.05" doc? Or perhaps I should ask how fast can I feed with a dremel at 10,000 rpm and 0.05" doc?

Thanks,
-Neil.

[Belding]

What kind of machine do you have? You may want to consider a spindle speed increaser. I don't think dremels have a very stable spindle..... You could also try to find a high speed spindle. Like this one http://www.homeshopcnc.com/page7.html

zac

[cnczoner]

This is my mill. The motor does 1800rpm (1.5hp), but after gearing it will do 1500rpm max. Last year I was planning to swap the motor to a 3600 rpm version, but the motor is some not-so-common frame size, and getting a higher-rpm version would only be from a few sources with a high price tag (IIRC ~$400-$600). I could make an adapter plate and adapter bushing to use a more common motor (like Nema 56), but I also want to keep it 110V (as I'm running this in a detached garage), and I wanted to get a motor which would let me use a VFD, but that would probably mean getting a 110V-in, 220V-out VFD, then using a 220V motor. A simple motor swap became a bit involved, so I put it on hold for now.

If I found the correct-sized motor right now, which allowed me to use it on 110V and 220V, I'd jump on it, but for now I've got to work with what I have. BTW, I'm not doing anything production, but I still think 1.5ipm is ridiculously slow.

Cheers,
-Neil.

[mrainey]

Maybe you could try an end mill with a shorter length of cut (stub end mill).

Also consider a four-flute. With only .050 depth of cut, you might get away with the chips not packing in the flutes - air blast or coolant will help.

[cnczoner]

Currently using a 3/8" LOC, which is quite short already, and I'm cutting to a total depth of just over 0.25". Also, squirting on ATF and vacuuming periodically. Interesting thought on the 4-flute -- I have a set of 4-flutes here, but need to check if it goes down to 1/8".

But still wondering if different types of endmills might allow me to get higher feedrates?

Cheers,
-Neil.

[mrainey]

But still wondering if different types of endmills might allow me to get higher feedrates?

That's the benefit of a stub end mill. I didn't realize that you were going .250 total depth. The stubbie would work with one or two .050 passes, but not five.

[mrainey]

Maybe you could get all but the last pass with the stronger stub end mill - LOC on these is 3/16


http://www.richardsmicrotool.com/page29.htm

[mactec54]

Hi cnczoner
Is this cnc or are you turning the handles, by the link it is a manual machine ATF is not that good for cutting fluid WD 40 would be much better in your case & cheaper how are
you holding the endmill if you are using a drill chuck that is not very good as it does not hold the end mill rigid enough you need a soild or collet holder to hold the cutter.

[cnczoner]

The mill is CNC'ed. I recently switched from WD-40 to ATF after some recommendations. So far I think I get a cleaner cut with ATF, but I haven't run comparisons to see which way is making the endmills hotter. I really need to get a cooling system, but I'm still evaluating compressor-less systems (since I'm doing this in a garage in an apartment complex and need to be as quiet as possible), plus I need to figure out some type of enclosure.

The endmill is held in R8 collets now.

Cheers,
-Neil.

[cnczoner]

I found this interesting writeup, and it seems that I should get more feed-rate from solid-carbide, smaller LOC, and a few more flutes. I have an Enco order going out shortly, so I'll add in some endmills that fit these parameters.

Cheers,
-Neil.

[JDenyer232]

I found this interesting writeup, and it seems that I should get more feed-rate from solid-carbide, smaller LOC, and a few more flutes. I have an Enco order going out shortly, so I'll add in some endmills that fit these parameters.

Cheers,
-Neil.

buy a good quality 3 flute carbide endmill, Spend the extra $$ to get a name brand one like niagra etc.

[wwendorf]

I have been able to cut with a 1/8" endmill about about 5IPM at .045 DOC spinning at 3400 RPM's and running my fogbuster coolant at a VERY light coolant stream. I'm planning on trying to get that up to about 6 IPM or better, but I'm guessing i'm probably going to go thru and endmill or 2 at those speeds.

Wade

[Mcgyver]

Neil,

forgetting for a sec changing endmill length - that may be a good solution, but the following theory applies to any length (at some feed you'll bust a shorter end mill as well.) Those little end mills can only handle so much of a chip load or they break. I'm surprised you got to 5 ipm, when i hand fee them going at say 3500 rpm, I can see them start to bend long before 5 ipm, then again that’s in steel not AL. If you're breaking them, decrease the chip load - that means increasing speed and/or slowing feed....you could reduce DOC but that accomplishing nothing so far as removal rates concerned; it'll just wear out the bottom bit of the cutter faster taking more passes. based on the hardware you have, that's the only solution; reduce feed.

A new spindle is a possibility, but dremels imo are a bit of joke - they don't have much power, burn out and may have so much run out that you start busting endmills for that reason. A router might be a solution??

carbide won't solve this problem, they'll bust even sooner. the problem is your feed is restricted by chip is restricted by spindle speed and carbide doesn't alter that. take the spindle speed up to 15,000 and you see an advantage in tool wear and removal rates with carbide.

[cnczoner]

Hmmm... I'm curious why runout would be so bad, since these tools (dremel or rotozip) cut through acrylic and fiberglass at a very good rate, and this would just be a CNC-controlled version of that.

Either way, this all makes sense to me now (about chip load), and I know my spindle speed is way too low for *any* aluminum machining, which is 95% of what I do. I usually use 1/2" 2-flute endmills btw. So I should really consider the motor-swap now. My current best plan of action is to drop in an equivalent-dimension 3600 rpm motor, but I'm evaluating other options such as changing to a pulley/belt system, etc.

I do have some 2-flute and 4-flute carbides on order, and I'll actually be able to compare performance of those in the meanwhile.

Cheers,
-Neil.

[Belding]

You probably can't just "swap" the motor for a higher rpm one. Your spindle is designed to run at a certain max rpm. If you exceed this speed you may be looking at bearing heating issues, out of balance issues, and any number of other problems. You would be better off finding a spindle that can take the speed.

zac

[wwendorf]

Sorry, the DOC was .035.

Wade

I have been able to cut with a 1/8" endmill about about 5IPM at .045 DOC spinning at 3400 RPM's and running my fogbuster coolant at a VERY light coolant stream. I'm planning on trying to get that up to about 6 IPM or better, but I'm guessing i'm probably going to go thru and endmill or 2 at those speeds.

Wade

[cnczoner]

You probably can't just "swap" the motor for a higher rpm one. Your spindle is designed to run at a certain max rpm. If you exceed this speed you may be looking at bearing heating issues, out of balance issues, and any number of other problems. You would be better off finding a spindle that can take the speed.

zac

I had discussed this with some of the motor suppliers, who all felt that going to 3000 spindle rpm on these machines is not a problem. (But I got some warnings about 6000+ rpm). Some felt that the gears would be a problem though, which is why I'm also considering a pulley/belt system instead of swapping motors.

[Mcgyver]

I had discussed this with some of the motor suppliers, who all felt that going to 3000 spindle rpm on these machines is not a problem.

what feeling are they going to have if the spindle is buggered? Probably not much of one - you on the other hand will be feeling some pain. I'd looking for some engineering information, like what the bearings are etc, and satisfy yourself, maybe they have some reasoning behind the feeling?

yeah, maybe its fine, I just wouldn't want to see you do damage on the advise of someone who may or may not know what they are talking about and aren't much of a stakeholder in what happens

my comment on the run out was that you the smaller the cutter, the more it matters, and the cheaper the spindle bearings the more likely it is - so you might get a lot of runout with a dremel that'll contribute to it busting. the affect it has is to make it the end mill essential cut on one tooth so the chip load is much higher than theoretical.