Results 1 to 12 of 12
Thread: Chip Load Questions
05-12-2011, 10:10 AM #1
Chip Load Questions
I am still sort of new to this area of life, and have a question for the more experienced. I am cutting acrylic, and have been running test coupons to determine feeds / speeds for best appearance straight off the machine / having minimal clean up. I came up with 7200 rpm at 500mm per minute, using a 0.02" two flute endmill. My chipload (if my fomula is correct) is CL=RPM/(Feed*Flutes) = 0.0013
RPM = 7200
Flutes = 2
Feed = 19.685" per minute
Here is where my questions comes in. 1. What if I go from the .02" endmill to a different diameter tool?, and 2. Can I theoretically just triple my speeds and feeds with the same finished look?
05-12-2011, 10:52 AM #2
I use standard three flute end mills. Rule! "No more than 2 flutes in the cut at the same time." This is good for any "toothed" cutter.
Chip load is directly proportional to the cutter diameter, including drills.
General chip load for a drill is 1.6% of its diameter per flute on 2 flute drills.
Divide the end mill diameter by 120 for an end mill chip load when using a full diameter "slot" cut. Then the finish cut can be made by another pass on the same numbers.
Divide the end mill by 80 for a roughing cut using near 66% of the end mill diameter. This yields a 50% increase in feed rate.
Depth of cut for end mills: steel 35-40% diameter. 6061 aluminum 50% 7075 t-6 40%
Stainless 30% These are general recommended values. The chip load is good. Start shallow and increase to optimum.
Climb cut unless you have damn good reason to do otherwise.
I find that three flute end mills cover anything you want to cut. When the end becomes dull re-point only for sharpening, then you always have a full diameter end mill size. Sometimes of course you will need to go outside these suggestions, but for the most part this is pretty universal.
05-12-2011, 10:28 PM #3
I'll bump this to the top. Somebody will chime in and suggest using a calculator to set your speeds and feeds, because you can't throw a chip with out one telling you how.
05-12-2011, 11:23 PM #4
My dinky little CNC doesn't have a tach...One's in the mail, but I have to go by sound.
Yet another cool thing to learn.
05-13-2011, 05:29 AM #5
I've had no problems using more teeth in the cut. As long as the machine has the power to drive it, the part has the rigidity to take it, and the chips are flowing out of the cut....bury it.
BTW, do that "Rule!" with a 4/6 tooth saw blade in 1/4" wide stainless steel and you'll be missing a few blade teeth. Well, not missing really. You'll know where they are, it's just that they won't be on the saw blade any longer.
Last edited by PixMan; 05-13-2011 at 07:43 AM.
05-13-2011, 05:47 AM #6
05-13-2011, 08:30 PM #7
Well I did ask for comments.
And you all did, finally wake up. >>
Those are just general rules I use. I can cheat when I use a woodruff cutter if I alternate chamfer the corners of the teeth so the chips aren't wedging the slot sides.
I never did have much use for four flute end mills in aluminum. I just get chatter. Not many of my machines have been bigger then a Bridgeport, so perhaps that slows me down.
Maybe the difference is, I like to run at a good cruising speed so I can run unattended. That could make me a more conservative than some of you. No matter, we all get 'ur done.
I have run parts on the Red Line before; but when the bubble came down the coolant pipe I had to rebuild the set up.
Thank you for stopping in.
05-20-2011, 04:31 PM #8
If your RPM is 7200 and your chipload is 0.0013" per tooth on a 2 flute end mill. Your feedrate would be 18.72" IPM. Chipload is determined by the machinability of the material you are cutting and the diameter of the cutter. The number of teeth/flutes you select also should depend on the material and what type of cut you are performing (i.e. slotting, profiling, etc.) You don't want to have to many teeth when slotting because the cutter can load up, filling the flutes with chips, and break. For example in the plastic you are machining, you would want to use a single flute, two flute, maybe three flute tool but nothing more if you are cutting a slot. If you are profiling around the part, you can use more teeth because the chips can get out of the cut very easily.
05-20-2011, 09:42 PM #9
Chip load calculations
Formulas are good for getting in the ball park, but your ears and eyes and results are what counts. I don't run a lot of small diameter endmills, but my experience is that the formulas don't work down there. Go ahead an run that .02 dia tool at 18ipm and see how long it lasts. I would be running it about1-3 ipm at that rpm. Generally, any endmills over .125 diameter I use M.A.Ford 3 flute endmills and love them. Bassets for 2 flute endmills.
And in case you don't know, IF-- you have a way to contain the fumes, heated methylene chloride, or super glue will polish your acrylic parts.
Bad stuff but it works great.
05-21-2011, 06:31 AM #10
Your CL DOES NOT depend on the milling cuter diameter! The formula for the chip load (correct term is the uncut(undeformed) chip thickness is valid only for straight flute milling tool. If you use helical mill or reamer/drill, this formula does not work.
There are two major limitations on chip load is milling: the strength of the tool as the cutting force that potentially can break the tool, is in direct proportion to CL; the chip spacing, i.e. the size of the flute available to remove the chip. It the latter is insufficient, the toll would re-cut the chip, at best, or it breaks due to chip clogging (common for machining aluminum with high feed rates).
05-24-2011, 12:12 PM #11
500mm/min is very slow according to me. I cut acrylic with a 3/32" endmill 2 flute(sgs serie 52) .105" D.O.C at 8000rpm and 1500 mm/min full width and it works great. I tried a single flute endmill for plastic but didn't had good result. You need a very sharp edge to cut acrylic so coated endmill are not recomanded. Sorry i read .2" endmill instead of .02" big difference!! Is 7200rpm your maximum speed? If not, at this diameter run at the top!
05-24-2011, 09:54 PM #12
"I'll bump this to the top. Somebody will chime in and suggest using a calculator to set your speeds and feeds, because you can't throw a chip with out one telling you how."
From the guy who sees nothing wrong with running a 6" cutter in steel at 600rpm.... so, lets see you figure a chipload. Oh yeah, your imaginary mill you run totally by feel doesn't depend on accurate setup, it operates by "feel". You have failed to provide any useful information once again. Good job! Gotta wonder why you post here?