I've been somewhat successful on cutting out aluminum parts out of 1/8" aluminum, but I'm still breaking bits more than I'd like. I'm now working on getting my settings the way they should be. I'm currently using 1/8 microstep and I was wondering if I should go to 1/16 or lower it. I was also hoping that someone could check out the settings I'm using to make sure that they seem in the correct ballpark. I'm currently using the Arduino CNC Shield. Thanks!
is 15000 your real spindle speed? step size will not make any difference, IMHO, unless your current steps are larger than your intended 'cut depth per tooth' in which case you simply cannot do it. given what I recall , 200 step/rev motors on 8x8 threaded rods at 8x microsteps gives you 200 steps per mm, which is a very tiny bit of mm per step. reducing that will not improve anything and will halve your maximum feed rate. but I see your problem, plunge rate is 200"/min which will definitely break bits unless you use ramping (you are) and take care to never actually plunge. and remember, the plunge feed rate is used for ramping moves so 200"/min is a little fast for that on the C-beam (though ok on big commercial machines But remember that feed rate depends a lot on RPM. reduce stepover to 33% which limits the engagement angle to less than 70 degrees, saw somewhere that aluminum likes that. of course this does not apply to full width slots, so one may need to reduce feedrate for those. so, given 15000rpm as your real spindle speed, we can calculate the feed rate but first let us calculate the rpm from the sfm for aluminum. rpm = cutting speed * 4 / diam (the 4 can be Pi for the dedicated) carbide cutting ali likes 1000 to 2000 surface feet per minute ergo rpm = 1000 * 4 / 0.125 = 32000 is the low end of the range so, your spindle a a little slow (-: however, having a known spindle speed we can calculate feed rate 15000rpm 2 thou per tooth 2 teeth gives us 60"/min feed rate (I have forgotten the actual formula and got this from a program I wrote many years ago) there are many online programs for these calculations, and the best one to use is the one from the makers of your cutter. so maybe your 20"/min is a little slow? however, do plunge at a lower rate, also reduce feed for full width slots. feeding too slow means that the chips are very thin, thin enough that the tool can be rubbing on some passes, instead of cutting, then the next tooth comes and cuts twice or more times the depth. this breaks cutters! 20"/min is less than 1 thou per tooth, so unless it is very sharp it is going to rub some of the time. gets hot, then overloads. hot means the ali starts to stick to the tool. then it really gets hot. having calculated the feed rate the thing to adjust is cut depth. set this to whatever the machine can handle, feed rate is the important thing to maintain. A C-beam should be able to do 0.5mm/20 thou per pass quite happily. like this next thing, cutting coolant. kerosene is very good. rubbing the part and tool with wax (bee or candle) between passes also works. WD40 works but is not so good, it is after all a 'Water Displacer'. commercial cutting fluids made for aluminum are astoundingly good. NOT 'oil'. number of teeth: do not use a cutter with more than 2 flutes in sizes under 1/4". in fact, under 1/8" rather use single flute cutters. this provides space for the chips to get out.
No Currently I'm cutting at 16000 on a Dewalt 611. I've ordered a Super PID and when it gets here I'm thinking that I'll be cutting at 14000 This supports what I noticed. It seemed to cut best at 8x, but I thought it was my imagination. I've noticed that my through hole plunges didn't work at all. I had to set it at 5% depth and then hand drill them. Now I see what I was doing wrong. Does this mean that I need to have one program for drill holes and then one to cut out the part using the ramping, Would it be better to set the plunge rate to something like 150"/min Will do I need to read over this a couple more times. I can see this answers my question, but I need time to process it. This exactly describes how my bits break. Things are going fantastic, but then I notice a change in sound and the bit seems to bod down. Within a couple inches of cutting the bit breaks. I've been using WD40 or oil and it seemed to glue the chips in place. I'm planning on building a fogless coolant machine that seems to get good reviews. I just emptied an old propane tank so we'll see how that goes. I've been cutting with 2 flute upcutting bits. I ordered some single flute bits from DrillBitsUnlimited, but I misread the description and got ones that are only 1/16th inch. With my current skill level I'd break them by looking at them. Thank you very much for the detailed response. It was extremely helpful. Using a cnc seems so easy, but there's so many small details that keeps tripping me up.
