1/8" Router Bit Feeds and Speeds

The critical factor with a slender bit is depth of cut: too deep, and it will snap. January 2, 2012

Question
I just set up an 1/8" 2 flute down shear bit and it tore off in about 3". I have the bit set at 5500 mmm (216 ipm) at 18000rpm. The overall length of the bit was just short of 5/8". I am not sure if I am running too fast for melamine but according to my calculations I am at .006 chip load which is right inside the .004-.007. I have a client who would like to use 1/8" backs on his cabinets and I wouldn't mind having the bit to do some engraving work on lumber and other materials for fun.

Forum Responses
(CNC Forum)
From contributor M:
Try starting out at 150IPM and increasing slowly until you snap one. Then drop feed by 10 to 15% and you should be fine. I have used 1/8" up and down shear at 18000 - 20000 and usually run 1/8 to 1/4" deep passes multiple times. 150 to 180 IPM works for me, depending on depth of cut and flute length, a long flute out of the chuck makes the bit more delicate, shorter is stronger. I think that the chipload tables really don't apply at these diameters very well. Keep in mind chipload is not a function of diameter, just of feed and speed. Too much at once or too fast will snap them right off, but they are plenty stable and reliable when you get in the right zone. I get the shortest flute length that will do the job, and if I can a 1/4" shank like, say, the Onsrud 61-240 so much the better.

I cut a lot of access panels in pre-laminated sheet stock with a 1/8 diameter, then edgeband the inner panel. This leaves a very small reveal and matched grain, for example under a desk for access to wiring chase imbedded in a diewall or an access panel in a cabinet side.

Another great application is to make MDF face frames, whether beaded or not and the MDF door that fits the openings all out of one piece of material. Very low on waste this way as the door is in place on the table and the 1/8" gap is the 1/8 " bit. Takes a while to run, but just set up the sheet, get a coffee and when you come back the frame and doors are all done. If you are really cagey the biscuit or spline to fix the frame to the cabinet can be done first as "reverse side nesting", but that is another story. These applications both require the use of a 3/4" flute length, which gets very touchy for breaking bits, but five or six passes at 150RPM works great. Two, three and four flute tools of this configuration are available from MSC and other places.



From contributor D:
I've been using 1/8" bits for years, primarily for bead removal in door profiles. Minor uses are sharpening corner radii and machining grilles. I've achieved the best life in hardwoods running two flutes 100ipm at 16k. Chiploads don't apply so much with such a delicate bit. I've noticed higher feed rates possible using 3-4 flute hoggers designed for aluminum, but only the HSS ones, so the life span is pretty short there. The carbide bits designed for aluminum have less of a hook angle, and trying to run these any faster is futile. You have to be vigilant running this slow with downshear bits - fire is a very real danger when cramming hot chips into a groove.


From contributor U:

Everyone is right, feeds and speeds in the scope of things really donít apply that much. Depth of cut does play into it and material. Also, check those collets and replace two-three times a year if they are being used every day.