I have been running my LEAD CNC at 2600 mm/min (100in/min) and 10,000 rpm for bit sizes ranging from 1/8" to 1/4". This feed and speed has worked very well for me with all my projects. I now plan to experiment with miniature wood projects. I would like to use very small end mills ranging from .5mm to 2mm. Can anyone suggest feeds and speeds that would be more appropriate for these tiny end mills? While I have been using MDF and 3/4" ply for my previous projects, my miniature projects will be using oak. Thanks
max rpm on the router then calculate the feedrate from the rpm and the tooth count, single to 2 tooth cutters are what you want, 0.001 to 0.002" per tooth shallow depth of cut with many fast passes and make sure to suck up the chips so the bit never has to recut a chip answer from ChatGPT To calculate the feed rate (in inches per minute, or IPM) for a given spindle speed (RPM) and chip load (in inches per tooth), you can use the formula: Feedrate (IPM)=RPM×Chip Load×Number of Flutes\text{Feedrate (IPM)} = \text{RPM} \times \text{Chip Load} \times \text{Number of Flutes}Feedrate (IPM)=RPM×Chip Load×Number of Flutes Given: RPM = 30,000 Chip Load = 0.001 inches/tooth For a 1-flute cutter: Feedrate=30,000×0.001×1=30 IPM {Feedrate} = 30,000 * 0.001 * 1 = 30 {IPM} Feedrate=30,000×0.001×1=30IPM For a 2-flute cutter: Feedrate=30,000×0.001×2=60 IPM{Feedrate} = 30,000 * 0.001 * 2 = 60 {IPM} Feedrate=30,000×0.001×2=60IPM Final Results: 1-flute cutter: 30 IPM 2-flute cutter: 60 IPM
I used a 0.6mm diameter end mill to cut inlay pockets in ebony for a guitar fingerboard. Feed rate was 125mm/min (5" / min) @12000 RPM (the maximum speed for my spindle) with a 0.3mm step-down. The shell inlays were cut using the same end mill at 100mm/min and 0.2mm step down. I only broke one end mill in the whole process, and that was because I hit it with the workpiece when loading the machine The cutting speed formula above doesn't give any consideration to cutting forces - this is the limiting factor for these teeny-tiny mills. I arrived at the figures above after noticing the end mill flexing at ~50% higher feed rates. You may well be able to run faster - how lucky do you feel?
Thank you very much, Peter! I called it 'shell', but some people call it 'Mother of Pearl' - same thing. Just for posterity, it's worth pointing out that there is a theoretical risk when machining it due to the possibility of generating respirable silica particles. However: The amount of machining is tiny; the dust doesn't become airborne (especially if wetted); and milling tends not to generate respirable size particles, anyway; parts can be washed to remove residual dust (safer than vacuum cleaning or using an air line!). Best people be aware, though. Here's a link to the finished article. The fingerboard and inlays, fret slots, headstock inlay, bridge and rosette (decoration around the sound hole) were CNC'd. The rest was done by hand. Finished Photos - MisterG
How long is the stick-out/ cutting edge of the bits you have? The amount of 'thin' section will have a massive impact on how hard you can push the bits before they start to deflect too much. For example, I have an 1/8" shaft bit that has at its end a 3mm long section of 0.6mm diameter 2-flute cutter (carbide). I can run that slotting at 24krpm, 2000mm/min and 0.25mm depth per pass in oak. The deflection of the bit tip should be around 1% of the 0.6mm bit diameter. If the "stick-out" section went from 3mm to 4mm long, the deflection would increase to about 2.5%, and if the stick-out is 5mm, then the deflection is closer to 5% of the bit diameter (and probably not sounding great at all!). Evan
