Why do my mill bits keep snapping?

[Gooserider]

I just started milling the small channels in my copper blocks over the last couple of days. They are coming out pretty well, except that I am snapping mill bits like they are going out of style. I would like to figure out what I'm doing wrong before I run out of bits... So far the cheapest new bits I've found are about $8.00 each for double enders, and it won't take going through many of those to eat up alot of cash.

I am attempting to mill a crosshatch pattern of channels in a copper block. The channels are 1/8" (~3mm) wide, with 1/8" copper between them. There are two sets of channels intersecting at 90*. I want to end up with a grid of channels, with 1/8" square pins separating them. (The idea being to get high flow with lots of turbulence - as soon as the coolant starts down one channel it will have a collision with the coolant going down the one at right angles to it.)

The bits I've broken have been a mixture of two and four flute 1/8" diameter bits, with 3/8" shanks. Most have broken in the middle of a cut, after having gone a good distance without apparent problem. There were no obvious reasons for the bit to have broken, it just snapped without visible provocation. When I checked after the bits snapped, the collet and remaining shank were fairly warm to the touch, but not hot.

I've been spinning them at 3,000 RPM (my milling text suggests 3,700 RPM, but 3K is as fast as my mill will run).

I am trying to take .080" per cut, working towards a total depth of about .5" (my books say one should be able to cut the same depth as the bit diameter per pass)

I am using the power feed to move the table, it is set up to drive at .320"/min (8mm/min) (as slow as I can go)

I am using a flood coolant of soluble oil and water, mixed to be heavy on the oil side.

I have the block mounted on a rotary table, and my approach has been to make all the parallel passes in one direction to .080", rotate the block 90* and make the passes in the other direction, so that all the channels are being cut down at a fairly even rate. (after the first pass I've been making two cuts per channel for a total of .160" which amounts to the same thing and saves a bit of setup time)

The bits I've been using and breaking are 'aerospace surplus' bought cheap off e-bay, so I'm not completely sure what kind they are, but I THINK they are either HSS or Cobalt. I am purchasing some new bits, which will be M-42 Cobalt, MSC's 'Premium Import' brand. (they are the least expensive, and if I'm going to snap bits, would rather snap less expensive bits than more expensive ones

At the industrial supply place this afternoon, another customer suggested I should try lowering the mill speed (he said 1500RPM). Also getting a .100" drill, and attempting to drill along the pattern of channels to remove most of the copper before milling. Another person suggested using solid carbide bits (which are stronger, but more brittle and prone to snapping. (and also far more expensive! )

I figure there may be more people experienced in machining small passages in copper here than in most areas. So I'm asking the experts, what am I doing wrong?

1. What kind of bits should I be using?

2. How fast should I be turning them?

3. How fast should I be moving the table?

4. What depth of cut should I use?

5. Any other suggestions?

Thanks,

Gooserider

[hara]

I think you should lower the depth of the endmill. The suggested is 1/2 of the diameter therefore 1/16"

Keep the RPM high

[bigben2k]

Yep, Hara is right: the cutting depth should be half the diameter.

HSS is cheap. Carbide or Cobalt is the way to go (Carbide is better ). Check out the endmills I linked in my waterblock thread.

By now, you should have been able to figure out which feed rate works out well for you.

[utabintarbo]

I'm sure jd or zymyrgy(sp?) are better equipped for answering this question, but just a few observations in general:

1. Use 2-flute EM's. 4-flute EM's tend to heat up the copper (due to friction) and make it even gummier.

2. It is generally better to take shallower passes at a higher feedrate.

3. HSS has a tendency to flex when it gets hot. Carbide can take more heat before it goes boom.

4. Feedrate should be determined by the size and condition of the resulting chips. This is more of an art than a science - experience is paramount here.

My $0.02.

Bob

[Fixittt]

Dude, your biting more then you can chew.

Your rpms are down, so it cannot take as much of a load. So you need to compensate. Seeing as you cannot move the table any slower, then lighten the cut depth.

Also. Stick your endmill up in the collet as far as it will go. Should help reduce flew in the flutes.


Good luck.

[jaydee]

Originally posted by Gooserider


I am trying to take .080" per cut,

Good god dude. Go .0625" at the most per pass but with that low of RPM I would suggest .030" for better results. 2 flute carbide works better than 4 flute as 4 flute cloggs up in copper. 3 flute is actually ideal as it keeps a better balance but they are hard to find. At utabintarbo pointed out solid carbide is the way to go. I just switched from HSS to carbide and will not go back.

[Gooserider]

I appreciate the many replies, it looks like the concensus responses are:

1. What kind of bits should I be using? Carbide, Cobalt, HSS in that order of preference, with a strong margin for Carbide. Also a couple recomendations for 2 or 3 flutes instead of 4.

2. How fast should I be turning them? Keep the RPMs @ 3K, since I can't get any faster.

3. How fast should I be moving the table? Probably about the same since I can't go slower.

4. What depth of cut should I use? Big concensus on this one for going shallower. General recomendation was for about .0625"

5. Any other suggestions? Suck the bit up in the collet.

Well, I just got some new 2-flute Cobalt bits, 3/16" shank, w an assortment of 1/8", 3/8" and 3/4" length of cuts. (MSC is neat, stuff I order shows up the next day) and I've got some bids in on carbide bits on E-bay.

I'll keep the RPM and table feeds the same for now, but reduce my depth of cut to .040" (I use .040" increments by choice since that is what the Smithy's downfeed dial is calibrated in)

I can't significantly suck the higher into the collet, though I understand the reason for wanting to do so. If I tried, I'd miss the setscrew flat on the bit. As the bits I'm using have larger shanks than the cut width, I'm not sure how much good it would do in any case as the taper is just about flush with the end of the collet already.

Thanks again for all the suggestions, I will keep folks posted as to how things work out.

Gooserider

[LiquidRulez]

Originally posted by Gooserider
I appreciate the many replies, it looks like the concensus responses are:

1. What kind of bits should I be using? Carbide, Cobalt, HSS in that order of preference, with a strong margin for Carbide. Also a couple recomendations for 2 or 3 flutes instead of 4.

2. How fast should I be turning them? Keep the RPMs @ 3K, since I can't get any faster.

3. How fast should I be moving the table? Probably about the same since I can't go slower.

4. What depth of cut should I use? Big concensus on this one for going shallower. General recomendation was for about .0625"

5. Any other suggestions? Suck the bit up in the collet.

Well, I just got some new 2-flute Cobalt bits, 3/16" shank, w an assortment of 1/8", 3/8" and 3/4" length of cuts. (MSC is neat, stuff I order shows up the next day) and I've got some bids in on carbide bits on E-bay.

I'll keep the RPM and table feeds the same for now, but reduce my depth of cut to .040" (I use .040" increments by choice since that is what the Smithy's downfeed dial is calibrated in)

I can't significantly suck the higher into the collet, though I understand the reason for wanting to do so. If I tried, I'd miss the setscrew flat on the bit. As the bits I'm using have larger shanks than the cut width, I'm not sure how much good it would do in any case as the taper is just about flush with the end of the collet already.

Thanks again for all the suggestions, I will keep folks posted as to how things work out.

Gooserider

your depth of cut should not exceed half the diam of cut.

the smaller diam of cut the higher the RPM

If you cant use a higher RPM then slow down the feedrate.

if you cant do that the DECREASE THE DEPTH OF CUT.

If this isnt working then increase the chip removal rate (ie, >30 degree helix angles) Which is really all you should be concerned about, because it will take care of all your problems.

Use 2 flutes for roughing cuts, 4 flute for finishing. 3 as a good in between, all around.


HSS for Cu is a bad idea. Cobalt is somewhat better but not by much in Cu.....Carbide can take a hell of a beating and last a long time if you keep withing the limitations of the bit and keep it cool.
They will snap quick, unlike HSS or Cobalt...they will bend increasingly until they snap off.

TICN coatings are the best if you plan on using standard (30 deg.) helix endmills with Cu, ........
DESPITE WHAT SOME PEOPLE THINK, THE TICN COATING WAS DESIGNED SPECIFICALLY WITH NON FERROUS IN MIND. Anything harder (TIAIN,ALTIN, etc.) is for hard to mill, ferrous , non magnetic steels, hardened steels, tool steels, and will perform rather poorly in Cu. TIN to me is just a pretty color and I see no real difference than plain mills using it.


A little extra advise....get the cheaper bits because with copper the extra cost doesnt justify the cost of the high dollar ones (Cu likes to eat those up even more for some reason)
Shop places like jtsmach.com or drilltechnology.com, wttool.com. etc. better buys and fast turnarounds. Mcmaster, MSC tend to charge alot more for import cutters than most places.....almost as much as the USA ones...best to leave them places for hard to find, precision tooling.
EBAY is getting to be a real pain to find something decent without getting ripped.

OH and....

And I cant say this enough CARBIDE, CARBIDE,CARBIDE!

The imports last just as long than USA made high dollar ones IME.

Later


Oh and I forgot something. ....invest in a decent collet chuck with a set of collets and junk those end mill holders as they are worthless if you want consistant accuracy. ER 32 is about the best bet(wider clamping range than most) and can even be used for drill bits too. ER32's TIR is always the same when changing out bits, etc. I love ER 32 collet set and would trade my wife for the set in a heartbeat.....SHHH here she comes...............

[JFettig]

Definately take less, If its still fast, like liquidrules said, decrease the amount your cutting.

What kind of mill are you using?


http://www.jtsmachine.com/jtswebshop...Tools/M496.asp

those end mills rule! thats what I use, they have lasted me a LONG time.

Get some cutting oil, or just some 5w 30 motor oil, Keep the end mill wet.

I like to take the first pass dry if Im not 100% sure on stuff. make it like .03" then I fill in the channels with oil, and keep adding more.

Definately keep your rpm as high as they can go. Ill soon be running my mill at 7500rpm

Jon

[Gooserider]

Thanks for the pointers to sources, with luck I won't need them (I may have enough bits to last) but will keep them in mind if needed.

As I mentioned in my earlier post, I've kept the RPMs and feed rate the same, but have gone to just .040" depth of cut per pass. Since I did that I've cut more than I had done when I started this thread, and only broken one bit.

That one was at least partly my fault - my current technque is to cut a pass with the power feed, disconnect it, and manually return to the start point. Then I drop down another .040", re-engage the feed and make another pass. I do the return fairly quickly, and as I was doing it I apparently snagged a burr on the end of the cut and popped the bit... Now I do the return more slowly, especially when re-entering the cut part of the channel.

I'd love to be able to cut in both directions, but I don't trust the position dials on this POS mill, and because of the flood cooling I'm using I can't really see the position of the bit easily. I'm afraid if I cut my way back, I would either snap a bit when I got to the end of the channel, or mill out through the side of the block... This is a little slower but safer, as my end point is the 1/2" wide cross channel already milled so I can stop anywhere in it.

LR - I have a few problems with my toolholding - given the increasing frustration I'm going through with this POS machine, I'm reluctant to spend very much money on tooling that I would probably sell with it if I put it on E-bay (increasingly likely!) The machine has an MT-3 taper which makes stuff hard to find and expensive compared to R-8. Currently I have 3/16", 1/4" and 3/8" bitholders, and an NR-40 collet chuck with collets for 1/2", 5/8", 3/4", 7/8" and 1" bits (the 3/8" came with the machine, the rest I picked up at a used equipment place) I also have an MT-2 collet chuck (Harbour Freight, unsure of taper) with collets for 3/8-5/8, and smaller sizes on backorder. I have a used tang style MT-2 / MT-3 adapter that I need to drill out so I can use a drawbolt on it, and mount the MT-2 chuck.

JF - I am currently using 2-flute Cobalt Import bits, 3/16" shank, 1/8" diameter, with different LOC's ranging from 1/8" to 3/4". (My target channel depth is about 1/2")

The machine I'm using is a Smithy brand, model Midas 1720CNC. (The CNC means that you can get a CNC kit to put on the machine, but I don't have it.) This is a combination Mill / Lathe, which I still think is a nice idea, but the implementation sucks big time. I've run into machine induced problems just about every time I've tried to use it - for more details on my tales of woe see this thread... Help, My copper bar is not flat

I am not using cutting oil as such, rather I'm using a pump fed stream of 'soluble oil' and water coolant, which is supposed to both lubricate and cool the workpeice. It also does a fairly decent job of getting rid of chips. I've found that if I aim the jet right at the mill bit, I tend to get alot of spray, so instead I just keep a slow but steady stream running into one end of the block, so that it runs down the channels at a pretty good rate. It seems to work as a coolant, I've never felt the bits or block get more than slightly warm. The only trouble is that the coolant solution is an opaque blue/white, and when it overflows I can't really see what I'm cutting.

Gooserider

[LiquidRulez]

Originally posted by Gooserider


LR - I have a few problems with my toolholding - given the increasing frustration I'm going through with this POS machine, I'm reluctant to spend very much money on tooling that I would probably sell with it if I put it on E-bay (increasingly likely!) The machine has an MT-3 taper which makes stuff hard to find and expensive compared to R-8. Currently I have 3/16", 1/4" and 3/8" bitholders, and an NR-40 collet chuck with collets for 1/2", 5/8", 3/4", 7/8" and 1" bits (the 3/8" came with the machine, the rest I picked up at a used equipment place) I also have an MT-2 collet chuck (Harbour Freight, unsure of taper) with collets for 3/8-5/8, and smaller sizes on backorder. I have a used tang style MT-2 / MT-3 adapter that I need to drill out so I can use a drawbolt on it, and mount the MT-2 chuck.

Gooserider

www.littlemachineshop.com has a nice MT3 quick change collet set that I have for when I bought my mini mill a while back, before I changed it to an R8 spindle and CNC'ed it...pretty decent set...8 collets ranging from 1/8th-5/8th " in 1/8th increments for around $129 and they also have a plain MT3 collet set 7 piece set for $59......www.micromark.com has the same quick change collet set for around the same price.Micromark also has collet blanks that you can make your own custom sized collets with for $10 a pop for the QC collet set mentioned above.

Ebay is a good source for cheaper priced ER collet sets , but MT3 is hard to come by though (R8 is too). A few weeks after I spent nearly $400 on mine, A set became available on Ebay for a fraction of the price....figures huh?

Take my advise and get an endmill or two designed for aluminum cutting, with higher helixed flutes and see what I mean about it taking care of your innability to cut the normal depth in Copper at faster feedrates. They cost a little more but they last as long or longer than an ordinary carbide endmill in ordinary stock (not Cu). Hell Ive even cut blocks without using coolant at all with these high helix endmills and surprisingly they didnt gum up like a standard helix endmill does WITH coolant(not advisable though.....)

[Gooserider]

I will certainly check them out if I end up needing more bits. However since I've reduced my depth of cut, I'm not going through bits anywheres near as fast. Between what I have now and the stuff I've got coming off E-bay, I should be able to get through these two blocks at least.

I'm getting close to done with the first block, I have all the channels about 3/8" deep at least, and have a quarter of them down as deep as I'm going to go. (I just hope I'm doing the math right so that I don't make a big hole when I cut the socket clearance step on the face of the block!) I'm leaving about 1/4" of copper on the base. According to the info Cathar and others have discussed here, should give good transmission to the pins and the rest of the block, without delaying the heat loss excessively.

It looks a bit ghetto, but I think it will work, and my next block should be a lot better...

Gooserider