Extending Router Bit Life

[aaron]

I have a project that requires me to use a 3/16" bit to cut some 1/2" birch plywood. I have been making .5" deep cuts at anywhere from 100 to 140 ipm & 15,000 to 18,000 rpm and can't seem to get more than 20 minutes of cut time out of my bit before it really gets dull. I posted a link to the bit I'm using below. Do you think I'm going too fast, too slow, need a different bit.... ? I have been using the trial & error method but it is getting expensive
Any input would be greatly appreciated.

Bit I'm using-
http://routerbitworld.com/Freud_03_128_3_16_Diameter_X_1_2_Single_Flute_S_p/freud%2003-128.htm

Thanks in advance,
Aaron

[knight_toolworks]

I show about 1.3 ips at 16000 rpm.
but thats at 3/16" deep cut per pass. it may be the bits too they are not that high of quality. why not try some 3/16" endmills.

[aaron]

Thanks for the suggestion. It could just be a poor quality bit. That was one of the only 3/16" bits at least .5" long that I could find though. I did try one of my endmills but it tore the top layer of the birch too bad (it has a very thin lamination layer on the top & bottom).

I bought a 3/16" down spiral bit that was.75" long today and decided that I would just try to keep going faster and see what happened. I finally stopped at around 200ipm & around 12,000rpm- full .5" cut. It cut great, sounded great, and I used it like that for about 30min & never broke. The bottom of the plywood looked a lot like the top when I used the end mill. I think a compression bit would be perfect but have not found one that small.

Is there not a router bit feed/speed chart or calculator somewhere like there is for end mills? I know wood has a lot of variables but it would at least give a place to start. I can't tell if I need to go faster or slower.

Thanks again,
Aaron

[aaron]

I found a speed/feed chart here-

https://www.onsrud.com/xdoc/FeedSpeeds

Aaron

[knight_toolworks]

I use theirs all of the time. it helps to have their catalog so you can find bits that are about the same. then under tools on the shopbot 3 software is a chip calculator.

[gene]

Aaron,
What brand bit are you using? If its a frued throw it out and buy a good bit, i use a 1/4 compression at .5 depth at 5.5 to 6 ips with a spindle speed of 13000
i get the cutters from fred at centurion tools for about 19.00 i tried frued and they just dont last.

[rcnewcomb]

I would have to agree that Freud bits do not work well in CNC applications.

We have been pleased with Onsrud bits. I haven't tried Centurion yet but I plan to based on the rave reviews.

[Gary Campbell]

Aaron..
If you need edge quality on full thickness cuts you should use a compression bit. I havn't seen many 3/16" bits tho. 1/4" will be more plentiful and probably cheaper. Hopefully your parts have the room to accept the bit dia. difference. Echo the comments on the Freud bits above. We dont get very long life out them in hand helds, let alone the Bot.
Gary

[paul_z]

Aaron

I did some work for Extreme Makeover : Home Edition which required about 1000 feet of cutting through 3/4" birch ply. The finish on both sides had to be very good. I bought three 1/4" compression bits :

http://www.bamcarbide.com/1shx1cutdix22.html

Both sides of the birch were cut cleanly and didn’t require any sanding.

I now have about 3000 feet of cutting on the first bit including 1500 feet of cutting MDF. All cutting was done at 0.25” per pass.

I burned the bit cutting some wood with a lot of pitch. It looked ruined but I soaked it in brake cleaner, scraped and wire brushed off the stuff that didn't dissolve. The bit was still sharp enough to shave with and I am still using it.

I don’t know why this bit lasted so long and other bits die after just 1000 feet of cutting. I did carefully follow the manufacturer’s recommendation of a minimum of 6” per sec at 21000 rpm. I have also used the bit at 4” per sec at 18000 rpm.

At $29 per bit, it has been extremely cost effective.

Paul Z

[richards]

Aaron,
Try a faster feed speed. For a chipload of 0.015" and 18,000 RPM, you should be moving 9-ips or 540-ipm. My rule of thumb when cutting plywood is to cut at a depth equal to the diameter of the cutter. Sometimes, when the wood sprites are working for me and not against me, I cut as deep as 1.5X the diameter of the cutter, which would be 0.28" with a 3/16" cutter.

I've just finished a job cutting MDF that took two days (24 sheets). The cutter was a Freud 1/4" upcut spiral. It did the entire job without complaint. The depth of cut was 0.3675" per pass, which left 0.030" skin on that batch of MDF (to keep the pieces from sliding around on the table). Speed was 14,000 RPM, feed speed was 7-ips. At the end of each sheet, as soon as the spindle stopped, I felt the cutter. It was only slightly warm to the touch.

[paul_z]

I think Mike is correct. The person at BAM Tools said the same thing - if you go too slow you will dull the bit rapidly. Go even slower and you will burn it. Go at the right speed and the bit remains quite cool (and will last a long time).

Paul Z

[aaron]

Wow! thanks for all of the great advice. It sounds like I need a better bit and move it faster. I did finally find a 3/6" compression bit here

http://www.toolsxp.com/on60-100SE.asp

that I think I will try. $43ea but if one lasts 2 hours it will be cheaper than several of the 20 minute Freud bits


One more question about the feed speed. I see the chip load calculations but how does that relate to cutting depth? Is Mike's depth = diameter (or 1.5xdiameter) formula pretty standard? I'd really like to be able to do a full 1/2" cut, especially if I have a nice compression bit. Is that just too much stress for the bit? At $43ea my trial and error with these bits will get exponentially more expensive.

I'd love to use a 1/4" bit but my internal radius in corners is the real problem. I can't tolerate anything more than 3/16. If I had an ATC I'd just do all of the corners with 3/16" and finish with 1/4" but I don't have one..... yet.

Thanks again for all of the wonderful help.
Aaron