[mkurtis]

I recently finished building a CRP 48x48 with a 2.2kW aircooled spindle and now I am doing some test cuts. I have tried with a 2 flute 1/8" endmill and a 4 flute 1/4" endmill. The cuts were done in 1/2" oak plywood, plunging down half the diameter of the tool and then routing in a straight line for 2". The 1/8" endmill I cut at 45 ipm and 18k rpm, based on a 0.01 chipload. The wood burned badly and there was a lot of splintering on the surface. Then I tried the 1/4" endmill, which I slowed to 13.5k and cut at 135 ipm based on 0.01 chipload. Again the wood burned badly, and the edges of the cut look folded up. I then tried various feed rates from 70 to 160 ipm, but didn't see much improvement with the edge finish or the burning. The 70 ipm definitely burned the most, as I would expect, but I would have thought that 160 ipm would have stopped the burning. Am I still cutting too slow?

[bhurts]

You need to get some bits designed for wood. Up spiral and down spiral. The down spirals work great to prevent chipping on the top. If you want the best of both worlds try a compression spiral. In the meantime change your calculations a bit. Feed in ipm is rpm x chipload x number of flutes. I can't really say if the .01 chipload is best but it's not a bad start for a 2 flute 1/4" tool. Try half that for 1/8 to start with the same 1/2 diameter step down. Using the formula you would get 540ipm for the 1/4 and 180 for the 1/8 at your same rpm. Doesn't really sound realistic for the 1/4. Try reducing your speed to 8000 and using a .007 chipload. That would be 224 ipm. Again the four flute will probably be problems no matter what you do but worth a try. Good luck.

Ben

[louieatienza]

As Ben said. you need wood bits not endmills. Wood bits have more rake and clearance needed. Check my thread on bits and endmills stickied to the top of this forum for examples.

[ger21]

Just a little to add to what the others have said....

As Ben said, your 45ipm was a .00125 chipload, not .01.
For a .01 chipload, you needed to be cutting at 360ipm.

You need to use a downcut bit when cutting plywood in multiple passes, or you will get splintering.

Once the bit has burned wood, it's probably become very dull, and will no longer cut cleanly.
Are you using HSS bits? You need to use carbide for wood, especially plywood and MDF.

And there are no cases where you'd ever want to use a 4 flute tool, unless you're cutting at over 1500 ipm.

[mkurtis]

Thanks for the replies. I misspoke on the bits, both were carbide downcut bits, but it looks like I was cutting way too slow. The formula I was using included the tool diameter, which is how I ended up with the low feed rate. I got it from here: Calibrating Feeds and Speeds with Carbide Microtools

Formula is: Feedrate = 0.01 x D x No. flutes x RPM, which is how I got 45 ipm for the 0.125" 2 flute downcut bit. Obviously that didn't work, and may have dulled the bit. I have a new 0.25" 2 flute downcut bit from CMT. How fast would you recommend cutting for that? If I use bhurts formula, I get 360 ipm at 18k ipm, but I would probably slow the spindle speed to 12k and then cut at 240 ipm. Does that seem reasonable? Obviously I'd like to avoid damaging the bits if possible.

[scedward]

Are you sure the spindle isn't turning backwords?

While the speed/feed is far from ideal, it seems to me that an .125" 2 flute downcut bit cutting .0625 deep, at 45ipm for 2 inches should go through that plywood like butter with a nice smooth clean top surface. Not burned and splintered?

-Scott

[xjdubber]

https://www.youtube.com/watch?v=CF9GiK_T4PA

[CYoung]

18K RPMs sounds really fast for wood. I run my Dewalt router at around 8-10K RPMs, 80-100ipm, and depth of about 0.1"- 0.2" and it goes through Hard Maple very well. I told me a long while to realize that fast RPM is not a good thing. You want your wood chips to be like curly Qs, not fine powder.

[CYoung]

I also use the 1/4" compression bits from Whiteside and they work very well and are about $30. Heres the amazon link;

Whiteside Router Bits UD2102 Up/Down Cut Spiral Bit with Solid Carbide Compression and 1/4-Inch Cutting Diameter - - Amazon.com

[mkurtis]

Thanks for the help everyone. I ended up increasing the feed rate and the 1/4 inch downcut cuts really nice.

[Dan911]

Are you sure the spindle isn't turning backwords?

While the speed/feed is far from ideal, it seems to me that an .125" 2 flute downcut bit cutting .0625 deep, at 45ipm for 2 inches should go through that plywood like butter with a nice smooth clean top surface. Not burned and splintered?

-Scott

I was really lucky coming across this thread! I was making some test cuts for the first time on my machine in some 3/4 mdf. Was very happy with results aside from the puff of smoke every time bit entered. I was searching and reading on speeds/feeds and read your post... My spindle was spinning CCW. Thanks!!!

Dan

[JoeBean_NEW]

As a general rule in life: heat is the enemy in any cutting operation, be it in wood or any other material. If you're getting burning/melting push it harder/faster or add cooling of some sort. A thread in the last year or so on PM showed dramatic tool life INCREASE when the tools were pushed to the limit. Not to mention the productivity increase.

If cut quality is then an issue you need different tooling or a different process.

[bzen]

I also use the 1/4" compression bits from Whiteside and they work very well and are about $30. Heres the amazon link;

Whiteside Router Bits UD2102 Up/Down Cut Spiral Bit with Solid Carbide Compression and 1/4-Inch Cutting Diameter - - Amazon.com

what settings are you using for this bit if you were cutting 4" coasters out of 6 mm plywood

[CYoung]

what settings are you using for this bit if you were cutting 4" coasters out of 6 mm plywood

I would run the speed at 120 in/min, 2 passes, with low RPMs, maybe 5-6K

[bzen]

you would do 2 passes with the compression bit?
i was previously running a double flute downcut at 15,000 rpm and 125 imp

[CYoung]

either one or two passes shouldn't make a big difference, I think your biggest issue is the router speed is too high. Exam your chips, are they small curly chips or are they dust? I took me awhile to realize that I was always running the router at too high of a speed. Cut the RPMs in 1/2 and you will get a better result.

[bzen]

currently im cutting with a double fluted down cut bit as the compression one is now unavailable until tomorrow,and the chips are a mix of dust and small curls

[CFANDZ]

I recently finished building a CRP 48x48 with a 2.2kW aircooled spindle and now I am doing some test cuts. I have tried with a 2 flute 1/8" endmill and a 4 flute 1/4" endmill. The cuts were done in 1/2" oak plywood, plunging down half the diameter of the tool and then routing in a straight line for 2". The 1/8" endmill I cut at 45 ipm and 18k rpm, based on a 0.01 chipload. The wood burned badly and there was a lot of splintering on the surface. Then I tried the 1/4" endmill, which I slowed to 13.5k and cut at 135 ipm based on 0.01 chipload. Again the wood burned badly, and the edges of the cut look folded up. I then tried various feed rates from 70 to 160 ipm, but didn't see much improvement with the edge finish or the burning. The 70 ipm definitely burned the most, as I would expect, but I would have thought that 160 ipm would have stopped the burning. Am I still cutting too slow?

18k is too high. I like to keep things in the 12-14k range and 180 IPM for bits under 1/2. I use vacuum hold down and think it's a good compromise on chip size and cutting force. I also ramp down to DOC. Much easier on the bit. For holes I always peck drill them down using uplutes. Ramp down is really important for downflutes.