Hi all, I got into this by creating jigs to router insets and specific cuts by hand. Recently bought the Lead 1515 and I'm playing around with some calculations. I've done quite a bit of research, and accepting that I sound like a newb, I'm looking for some guidance and have a question: 1) I know there's no definitive answer for this, but is there a general rule of thumb for this machine when it comes to maximum feed rates (IPM)? I ask because when I've been running calculations, I'll plug some numbers in based on "general chip load guidelines" and my RPM number comes out extremely low if I use a number like 80 IPM. The other formula I'm using is spitting back higher feed rates. For example: Cutting Walnut : Recommended Chip Loads: .009 to .011. Let's say I use .01 to benchmark. I'm using this formula: RPM = feed rate / (number of flutes x chipload) RPM = 80 IPM / (2 x .01) RPM = 4,000 (which I can't do) Now, using RPM rates that I CAN use on my Makita router, here is what I'm finding using the following formula: Feed Rate = flutes x chip load x RPM Cutting Walnut : Recommended Chip Load: .009 to .011. Let's say I use .01 to benchmark and plug in 14,000 RPM (note: my router only goes down to 10,000 RPM) 1/4 inch 2 flute downcut bit at 14,000 RPM 2 flutes x .01 x 14,000 = Feed Rate of 280 ipm at 10,000 RPM 2 flutes x .01 x 10,000 = Feed rate of 200 ipm The brand SharkBits is what I'm using (1.4 inch, 2 flute) which recommends 80 ipm at a 25 plunge rate and a maximum cut depth of .0625. So it's throwing me off a bit. I've made cuts at various RPM's, cut depths, and speeds up to 100 ipm on the Lead 1515 and though I have not noticed many differences in the quality of the cut, I have noticed the collet and bit becoming very hot even after actively adjusting the RPM's. Last thing I want to do is prematurely jack up these bits, or cause harm to the machine. Any advice or guidance is met with open arms. Thanks.
you want to be producing chips instead of dust. so 180ipm at 10000RPM for 0.01" per tooth on a 2 flute or 100IPM at 10000RPM on a single flute for the same chipload of 0.01". adjust the depth of cut to suite your machine. many fast passes are just as quick as one slow deep pass. climb cut whenever possible. (in wood anyway, climb cut does not work in foams) in woods with hard and soft areas like pine, set feedrate for the harder wood. each wood will be different, make notes when you find good numbers, you cannot remember them all (-: collet becoming hot means you are cutting too slow (-: clear the chips! recutting chips creates heat and surface finish problems in a hurry.
Thanks for taking the time to respond David. I’ll give that some practice runs. Really appreciate it.
Hi Kyle, I am in the exact same boat, same setup, same bit. What did you determine? I am cutting plywood, so I am looking at a chip load of .011-.013. I am also trying to determine the be best way to cut Pockets, ie do I keep the stepover the diameter of my bit, or do I reduce it? I have done a ton of cutting, and I think I have dulled the bit ( I have two on standby ) and want to optimize before installing a new bit. I also keep a laser thermometer handy, and I periodically check the bit temp.
definitely reduce. down to <30% for hard woods, about 75% for softer woods. The gluelines in plywood will create especially dull nicks in the bit. bad enough to leave visible lines in a plain piece of wood, as though you hit a nail with a jointer. So try to vary your depths of cut from project to project. This means the whole (or more of it) bit goes blunt at the same time, this makes it easier to resharpen.
Hey - I am sure there are people here with much more experience than I have but I can share what I've learned so far. A lot of it obviously depends on the bit size. The plywood comments made make sense as I've gotten much cleaner cuts with other types of wood and less dulling etc. I typically have kept my machine running at 100ipm or less for all of these cuts that I'm doing. I've run into issues where my machine will do an errant cut through the workpiece if I go up to 110 IPM for example but maybe that's just my machine. The chip loads you see are pretty much guidelines. I've altered the chip loads a bit to test out and they've ended up working well for me. Here are some examples that I've had pretty good cuts with. 1/16 two flute downcut: 1) 72 IPM, 18000 RPM, Chip load .002, DOC .0625 1/8 two flute downcut 1) 96 IPM, 12000 RPM, Chip load .004, DOC .125 2) 96 IPM, 16000 RPM, Chip load .003, DOC .125 1/4 single o flute downcut (usually used for metal and plastic, but I've had success with it because my 2 flute 1/4 inch bits need a faster feed rate than I think I can achieve) 1) 98 IPM, 14000 RPM, Chip load .007, DOC .25 2) 98 IPM, 12000 RPMP, Chip Load .008, DOC .25 (a bit rougher but not by much) Still kind of messed up on V bits because I don't think I'm particularly using them right. 90 degree 2 flute - Have run them at 90 IPM, Chip load .003 (amana tool guidelines), DOC .25 for perimeter finish cuts just edging the outside of the cut I have made with a downcut), RPM 18,000. ANy advice on V bit would be very helpful. For stepover, I do a cut at one of these guidelines and then decrease the stepover with the same bit that's very small somewhere around 5% and the finish cut looks good, just takes longer. Rough cuts I'm at 40-50% stepover leaning toward 40.
Your calculations follow the formula perfectly Kyle although I'm guessing you have probably had to "massage" the chip load somewhat. Taking the second example... (1/8 two flute downcut) 96 IPM, 12000 RPM, Chip load .004, DOC .125 You are probably already aware that the chip load is doubled when using a single flute end mill i.e. 96/12000 = 0.008" which is probably nearer the optimum. That's why I like to use single flute cutters most of the time for these home workshop machines. My bits barely get warm normally so their life expectancy is pretty high. For me, the bits are the heart of the machine and a cooler running bit also means less stress on the router. Where V bits are concerned, mine are 2 flute which I use mainly for engraving. Your numbers are similar to mine for that tool although I run the router at 12-15k RPM. I can edge a piece at 40% stepover with good results (depth of cut set at 2mm)
I am cutting 2x12 pine using a 1/4-inch end mill down bit. What feed and plunge rate should I use on my Openbuilds 1515. Running 18400 rpm, I can adjust up or down.
I guess I will try 14,000 rpms, 40-inch feed rate, 15-inch plunge rate, .0.25-inch depth per pass, step over 0.100-inches
At 18000 rpms, you should be easily able to cut pine at 100ipm if you depth of cut is 1/8". I plunge at 40 ipm. I do not cut a lot of pine. This is what I cut oak and pretty much all woods at if pocketing or profile cutting. I go much faster if I am doing 3D cutting where my stepover is 40% or less.
