Hi, there! I have broken two absolutely new end mills from different manufacturers. They both have similar geometry, specifically: up-cut spiral type, 1 flute, 3.175mm cutter and shank diameter, 17mm cutter length. They break when they have passed Ramp movement into plywood (to a depth of 3.3mm) and then proceed cutting movement on that depth of 3.3 mm. I have utilised the following speed/feed settings: Case N1: "Spindle Speed" = 7000RPM, "Cutting Feedrate" = 700mm/min, so with one flute of the end mills get "Feed per tooth" = 0.1mm; Case N2: "Spindle Speed" = 9000RPM, "Cutting Feedrate" = 900mm/min, so with one flute of the end mills get "Feed per tooth" = 0.1mm; I am relying on the "Feed per tooth" parameter when I set the speed/feed parameters, since I guess it's a good reference point to set "Spindle Speed" and "Cutting Feedrate" while keeping the same "Feed per tooth". I have taken 0.1mm value because (as approximate value from many successful examples of milling plywood, I have calculated it as Feed_per_tooth = Cutting_Feedrate/(Spindle_Speed * Flute's_number). So, 0.1mm Feed per tooth looks as a reliable value to cut not too aggressively nor to rub/burn the material. Nevertheless the end mill is broken. I can't understand what I do wrong, what is the cause of my failure? Maybe I use too low RPM, but at the same time the Cutting_Feedrate is slow as well and hence Feed_per_tooth value is adequate corresponding to many examples..., no idea, any help
looks like you are ramping at 350mm/min and then it accelerates to 700mm/min when the real cut starts, but that is fast enough to break the endmill. so, I would set the cut feedrate for 0.05mm per tooth. I would also halve the pass depth. A good starting point is half the bit diameter. I would rather cut faster than deeper. Plywood, esp pine based woods, have hard grain between the soft stuff (akin to a hardwood in the hard parts) and you have to set feedrate for the hardwood parts. also, if you have more RPM, use it. I like 12000 to 18000 for plywood
A two flute cutter will be stronger than a single flute most of the time, save the single flute for plastics and aluminum. Also, use the biggest cutter you can for a job so if the holes and inside radius doesn't require a 1/8" bit use something like a 3/16 or a 1/4". Until you get things dialed get cheap practice bits on ebay and experiment, the chip load value is not very useful for these machines, they just don't have the rigidity to take advantage. Cheers Gary
Looks like it is too small value. For 1/8" bit and plywood the Chip load should be in range 0.004-0.006" (0.1- 1.15)mm. See the reference table
tables are all very well, and I like them. but logic tells me 0.1 per tooth is breaking the endmill (whereas half that is NOT, the ramp feedrate is 350mm/min, half of 700mm/min), therefore I suggest using less engagement. and less depth, and more RPM. get it working, then later get it working faster (-:
For a very different machine (rigidity affect tool chatter which puts percussive loads on the endmill), and likely very different endmills. Depending on the source - not all endmills are sintered the same, and some are more brittle than others. Charts are never anything more than a guideline. Practise and experience will override charts
