Routing MDF, feed rate, tool life

[balsaman]

Jen,

I heard you work with MDF alot. What thickness? What sort of feed rates, tools etc?

I was cutting 3/8" MDF in one pass at up to 40" per minute but tool life isn't great (1/8" carbide 2 flute endmill). I would say it starts getting dull in about 2 hours. Still cuts but you get more fuzz on the edges. The dull carbide still seems to cut oak and other materials fine.

Is there a trick to making the cutter last a little longer?

Eric

[HuFlungDung]

Hi Eric,

I think you're pushing it at that depth of cut for such a small cutter. Does it clear the chips really well? I'm surprised you haven't just broken it off.

[balsaman]

Well the MDF becomes super powdery and comes out no problem so far. Most of my cutting has been at 20" or so but lately with my faster machine I have cut at 40 with no problems. I broke a cutter at 25" in oak the same depth mind you... oak prefers around 15" at that depth.

Eric

[ger21]

At work I use 1/2" spiral cutters to cut 3/4" MDF @ aroud 400 ipm and 15,000 rpm. Our machine won't go much faster, but at that rpm I could probably cut almost twice as fast. Try slowing your router down to around 10,000 for the speeds your using, and use a larger bit whenever you can. ( I know a 1/2" bit won't work for those clock gears or probably your plane parts.) Also, endmills have a different geometry than wood spiral bits, which probably contributes to there short life. Bottom line, though ; go as fast as you can with the slowest spindle speed. To slow a feed and to many rpm's cause heat which dulls bits. I would think with your machine and a GOOD 1/4" spiral bit spinning about 10,000 to 12,000 rpm, you should be able to run it as fast as your machine can go. Personally, with anything smaller than a 3/8" cutter, I would cut the 3/8" in multiple passes, probably depth = diameter or something like that.

Gerry

[Rawb]

I run all sorts of thicknesses of mdf at work, typically I run a 2 flute 1/2in compression cutter at 17000 rpm and a 300ipm feed rate. I am limited by the holding power of the vaccum table (15hp machine isnt enough) and the feed rate of the machine. about 475ipm is max travel speed. I HATE that it doest rapid at something like 650.

about the .125 cutter, i use 2 flute downcut amana carbide tools and at 3/8 material, 275 ipm at 18000 is all the tool can handle. The tool remains sharp for many many sheets, but cant handle the sideways load of a full .375 cut past 275 ipm.

hope this helps