What size chipload and depth of cut based on diameter of endmill?

[wwendorf]

Greetings all,

I've been doing a fair amount of playing with my new Syil X3, and let me tell you, it's been seriously exceeding my expectations. It's a great machine and i'm glad I made the purchase.

My problem however is coming in with me trying to do some milling with a 1/8" endmill. Frankly, i'm going a little nutz and have managed to destroy 4 - 1/8" endmills in 1 session.

There are 2 bits of information I am looking for.

1) How do I determine what size chipload I am going to desire for a particular diameter endmill?
2) How do I determine how deep of a cut I can make based on the diameter of a particular endmill?

I'd like to find information for all different sized endmills. I've been doing OK with anything bigger that 1/8", but a lot of them are guesses as well. I have been googling, but haven't found the right information or haven't found exactly what i'm looking for. Basically, I need a good rule of thumb to follow.

I have found a few things that give high and low ranges, but it doesn't make sense to me why or in what situation you would use the high or low range.

Any help would be most appreciated!

Thanks much,
Wade

[Chuck Reamer]

Try running about .001 to .002 IPT (inch per tooth) for a feed rate, should be good for the machine. As for depth a good rule for HSS endmills is half of cutter dia, so for a .125 cutter about .0625 should be about the most you should go for.

Spindle speeds for HSS in mild steel should be about 100 SFPM(surface feet per minute). So for a 1/8 cutter it should be like this

4 x 100(sfpm)
1/8 (dia)

If you are kinda new to machining the Machinery Handbook is a great buy, worth the $100 for sure.

What happened to the endmills that went bad on you?

Hope this helps a bit, anymore questions just fire away.

[wwendorf]

See, that's the problem. I understand this in Inches per Minute, the IPT completely confuses me. Also, i'm doing the machining in Aluminum.

On the cut I was doing I was doing, it was .05" for a depth of cut, my RPMs were 3500 and my IPM was 2.5". I used the feed/speed calculator in Mach3 for the calculation with a chipload of .0005" and it actually came back that I should be able to do a 3.0 IPM, but I figured i'd be safe and ramp it down to 2.5 IPM.

As far as the endmills, well, the cutting part of the end mill just twisted right off and stuck in the aluminum. There wasn't any heat and I was blowing a light stream of air on the part to keep the chips clear. After shutting down the machine and removing the broken part of the endmill, there was no evidence of melted aluminum, hence my confusion about what I am doing wrong.

Thanks,
Wade

[dertsap]

there would be enough friction for the aluminum to get a little sticky and break your tool , spray a little wd 40
also your speeds are painfully slow
at 3500 rpm you should be running around 10.5 ipm safely

[Geof]

Originally Posted by wwendorf .....There wasn't any heat and I was blowing a light stream of air on the part to keep the chips clear. After shutting down the machine and removing the broken part of the endmill, there was no evidence of melted aluminum, hence my confusion about what I am doing wrong. Thanks, Wade

When machining aluminum with a small cutter I think it is essential that some coolant or cutting fluid is used. A readily available substitute is automatic transmission fluid; just brush or spray it on along the cut line; nothing fancy is needed.

Aliminum has a tendency to adhere to the cutting edge and form a build up. This combined with the chips often becoming very thick as they come off the tool means the flutes on the cutter get jammed with aluminum; no melting has occurred the metal has just been deformed.

The figure you give for depth of cut is good being a bit less than 1/2 the diameter; your feed per tooth was a bit high, I would suggest 1% to 2% of the cutter dia. i.e. 0.001" to 0.002", with a four flute cutter a smaller chip load is better because there is less space in the flutes for chips.

I would expect using coolant and a feed of 0.002" per tooth with a two flute cutter should give you good results.

EDIT: misplaced my decimals in the feed per tooth calculation.

[Chuck Reamer]

RPM X #of teeth X feed per tooth

Higher feed and lighter depth should help with coolant or cutting fluid of some sort.

[masterblaster]

I would add that you allways use a coolant.lubricant(kerosene works great) and all ways climb mill. I have been amazed at how fast I can mill aluminum while climb milling. If you are using a longer end mill than a stub length, I would cut down on the first cut depth to 1/4 cutter dia. (.030) to cut down on torsial deflection.

[wwendorf]

If I had a coolant setup, i'd definately be using it. Unfortunately, I don't have the room to build a collection system around the mill, hence why I am trying to get the proper chipload on a 1/8" endmill. I also can't deal with the mess of coolant going all over the place right now. I use the shop for woodworking as well as metalworking.

If I can get the right chipload and speed down, then I'm hoping that I can remove material at the correct speed so that the heat is being removed as I cut.

Also, if I go faster than about 2IPM, then my endmill is basically history in the first few seconds. I don't see how I can go faster with a 1/8" endmill. Please note that with anything bigger, I have no problems going faster. 6IPM with a 1/4" is pretty good I think, especially running without coolant.

Wade

PS. I am considering the fog buster coolant system however.

[Oldmanandhistoy]

Originally Posted by masterblaster I would add that you allways use a coolant.lubricant(kerosene works great) and all ways climb mill.

If you have to much backlash in your system you will break the cutters even faster or spoil the part if you climb mill.

Also I didn’t notice you mention if the cutters are HSS or STC; they should be HSS.

John

[wwendorf]

I'm using HSS tin coated. Also, what do you mean by too much backlash? How much is too much?

Wade

[DareBee]

Your cutter extension (out of the collet) needs to be as short as possible.
IMO HSS is WAY too flexible, The cutter grabs, flexes sideways, overloads, and SNAP!
My rule of thumb is never use HSS under 1/4" cutter diameter. Small carbide cutters are almost the same cost.
Otherwise cut your DOC by 50% and increase your feed an extra 20 - 30% (over proper calculated).

[haslagl]

I been a toolmaker for 30 years and depth of cut is always a subject that no one, it seems, can give you a formula for. There are so many variables. I cut 1018 cold roll, thicknesses from 1/8 thick to 3/16 thick. I am using carbide cutters ranging anywhere from 1/16" to 1/8" diameter cutting slots. As the other gentlemen suggested using WD40 or kerosene is very important. Aluminum's nature is to stick to the cutter. Air will not stop this. You need to use some form of a lubricant. An air mister is good but it blows the lubricant into the air. I use a hand sprayer with WD 40 and shoot the lubricant at the cutter. Your choice is one of those two for starts if you don't or can't use flood. I am assuming your Syil is a small CNC. Make sure you are using a two flute cutter if you can with a high helix. They make cutters specifically for aluminum. Carbide is better as mentioned and the cost for 1/8" carbide is not that much different. Enco, basstool.com, are two good places to look for carbide at low prices. Their cutters are pretty good. I cut cold roll steel with those small carbide cutters at depths of about .030, feed rate from 8 to 10 for 1/8" and a spindle speed of around 5500 rpm. You should know the formula for finding cutting rpm and feed from what other individuals have given you. Aluminum has a SFPM up to 850 for HSS and 2020 with carbide for finding your cutting speeds, feed per tooth from .0015 to .0080". This is from the Machinery's Handbook. I would use values of about 1/4 of the maximums for feed. The depth of cut is then the big player here. I have always been told that 1/2 the diameter of you cutter is what you should figure, but if you are buzzing into your material at 40 inches you will snap it off. You will need to start on the low end of the feed and work your way up. You may want to start your cutting depth at .030 and go deeper as you find what’s working. Slow feeds and deep cuts or shallow cuts and high feed rates – make notes and see what you can get away with. You may want to start your cutting depth at .030 and go deeper as you find what’s working. Slow feeds and deep cuts or shallow cuts and high feed rates – make notes and see what you can get away with. If you are machining for a living you will have to find a happy medium with your cutting rate that is cutting good and making you a profit. Again the depth of cut is a big issuer so often. There is not a real formula for it such as you have with speeds and feeds. In many shops the tendency is shifting towards high speed machining using high feed rates, high rpm's, and light depth of cuts. But we are talking about 20,000 rpm spindes also and expensive machines. Sorry the long reply but I hope I could help. My phone number is 573-897-0700 - I own my own shop and I am a machine tool instructor.