gene heskett wrote: > Hi Guys; > > I just broke my last brand new 1/16th carbide end mill in about 15 minutes > running time, a 4 flute with about 1/2" of working length, trying to get > started on another alu encoder wheel, getting about 80% of the way around > the outside, running at 2500 revs, and 1.5 ipm, cutting only .005" deep, > running in a puddle of cutting oil. > > Obviously the 4 flute is a no-no in soft alu as it was pushing alu ahead of > itself for 90% of what it did cut which tells me it was half plugged after > the first 1/2" of feed in that heavy duty (0.0037" thick) coors can alu . > Filled up the flutes nearly instantly even if it was swimming in cutting > oil. > > So, I need to find a more suitable mill for this, I assume only 1 or 2 > flute, and maybe only 1/8" of working bit. > > You ought to be able to do this. I use water-based coolant. The trick is to keep the WORK cold, and I do mean COLD where the cutting is going on. You should up the feed rate and/or make it in several passes, stepping down in Z each pass. 1.5 IPM is way too slow. At 2500 RPM with 4 flutes, that is 10,000 cutting edges per minute. So, each tooth is only cutting .00015", which is WAY too small. My McDonnell-Douglas slide rule suggests a .00062" feed per tooth, so that would be 6.2 IPM. You should only plunge 1/32" per pass with a 1/16" cutter (half the tool diameter).
I use a 4-flute cutter in aluminum ALL the time, rarely use a 2-flute. You should be climb milling, this causes much less rubbing and therefore heat generation. Climb milling causes the cutter to plunge directly into the un-cut material, conventional milling causes the cutter to slide across the already-cut surface until there is enough pressure to penetrate it. That rubbing causes heating of the workpiece, which makes the aluminum soft. > Since I don't have a 10,000 rpm spindle, 2500 is it, what mill should I > buy, and how fast can I feed it? Or am I doomed to go find some harder > sheet alu that cuts cleaner and won't plug up a mill? > Just keep it COLD, and it will cut fine, as long as it isn't 1000 aluminum or something meant only to feed into an extruder. That's the beauty of water-based coolants, the evaporation of the water really cools stuff off. Wait, you're only cutting .005" deep per pass??? WHY? I might tend to go a bit less than half the tool diameter, but that is too conservative even for HSS, and way too conservative for carbide. If you insist on such small Z plunge, you should be cutting this at 20 IPM or something! I don't have much experience with 1/16" carbide end mills, but use 1/8"carbide 4-flute mills as one of my most standard cutters for .060 - .125" aluminum panels. I frequently run a whole day on one cutter. And, I do it usually at about 2800 RPM. If the wad of aluminum around the cutter develops, you are already sunk, you have to avoid the softening of the material. Jon ------------------------------------------------------------------------------ Try before you buy = See our experts in action! The most comprehensive online learning library for Microsoft developers is just $99.99! Visual Studio, SharePoint, SQL - plus HTML5, CSS3, MVC3, Metro Style Apps, more. Free future releases when you subscribe now! http://p.sf.net/sfu/learndevnow-dev2 _______________________________________________ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
