Results 1 to 8 of 8

Thread: Cutter Choices

  1. #1
    Join Date
    Mar 2010
    Location
    Somewhere in the Land of Lincoln
    Posts
    1,056

    Cutter Choices

    What are your thoughts on what you prefer to use for roughing and finishing cutters or the same for both? I know two flute end mills have more chip clearance but will 4 flute give better first pass cut quality? I was cutting some white pine(because I have some) and the cut was pretty "woolly" on the roughing phase. It was't the finish pass so I didn't worry about it but if it were it would have been quite ragged. The wood may have been more of the issue but I was just wondering what you experts prefer.

  2. #2
    Join Date
    Dec 2008
    Location
    WV
    Posts
    3,591
    Quote Originally Posted by Ronald Blue View Post
    What are your thoughts on what you prefer to use for roughing and finishing cutters or the same for both? I know two flute end mills have more chip clearance but will 4 flute give better first pass cut quality? I was cutting some white pine(because I have some) and the cut was pretty "woolly" on the roughing phase. It was't the finish pass so I didn't worry about it but if it were it would have been quite ragged. The wood may have been more of the issue but I was just wondering what you experts prefer.
    Are you asking with regards to 3D toolpaths? I honestly dont know of many wood-type cnc routers with high speed spindles that would be able to benefit from a four flute cutter. You just wont be able to push them hard enough.

    Roughing and finish passes for me usually speak more to diameter, and tip radius, than they do flutes.
    Sometimes I just want to look at pretty pictures,... Thats when I go to the Turners Forum

  3. #3
    Join Date
    Apr 2017
    Location
    Tucson, Arizona
    Posts
    519
    Quote Originally Posted by Ronald Blue View Post
    What are your thoughts on what you prefer to use for roughing and finishing cutters or the same for both? I know two flute end mills have more chip clearance but will 4 flute give better first pass cut quality? I was cutting some white pine(because I have some) and the cut was pretty "woolly" on the roughing phase. It was't the finish pass so I didn't worry about it but if it were it would have been quite ragged. The wood may have been more of the issue but I was just wondering what you experts prefer.
    Hi Ronald,
    For a given chip load, you would need to either increase the feed rate, decrease the RPM, or some combination of both when switching from a 2-flute to a 4-flute cutter in order to keep the chip load constant. The finish quality may also be influenced by the cutter geometry, sharpness, and the material being cut. I would expect that soft material would be more prone to tearing than a harder material. Here is a feed rate calculator that you may find helpful.
    David


    https://cncrouterstore.ca/feed-rate-calculator/

    Feed Rate Callculator.jpg

  4. #4
    Join Date
    Jul 2015
    Location
    Broadview Heights, OH
    Posts
    638
    Ron,

    Chipload is something that is often overlooked. Onsrud makes a ton of CNC bits, and I don't think there are very many that are 4 flute. Sounds like a good idea but not many use them in practice. I use just a regular 1/4" two flute upcut for roughing, and then a 1/8" ballnose for finishing. For the 1/8" bit, I like to spin it at 12,000 rpm, and I use a .005" chipload. I use the calculator built into the operating system of my shopbot, but I'm sure the one above would yield the same result of 2 inches per second for movement speed. Spinning the bit faster, or increasing the number of flutes causes even faster movement speeds which brings it's own problems. Most machines have troubles maintaining constant velocity in a cut when changing cut direction.

    Additionally, if you cut in hardwood and softwood, it is different for each. The 52-240B ball nose I use for finish carving says chipload should be .003-.005" for hardwood, and .006-.008" for softwood. Keeping the spindle constant at 12,000 rpm, that yields 2 inches/second for hardwood and 3.2 inches/second for softwood which is a big difference. You should get in the habit of calculating your movement speed before generating toolpaths. It can make the difference in a great finish and one that is so-so. The values I used were .005 and .008 respectively for the example above. Note that the calculator linked above gives inches/minute. Divide by 60 to get IPS.

    Don't overthink it, just use a regular two flute cutter and a moderate speed and you will have great results. BTW, it's nor uncommon to have some fuzz on the roughing passes. Finishing is what matters, unless you tear out so much wood that the finisher can't clean it up.

    Hope this helps.

  5. #5
    Join Date
    Mar 2010
    Location
    Somewhere in the Land of Lincoln
    Posts
    1,056
    Thanks for the replies on this. I will use the chart and experiment. Find the feed rates that give the best results.

  6. #6
    Join Date
    Mar 2003
    Location
    SE PA - Central Bucks County
    Posts
    50,681
    95+% of my tooling is two-flute. I have one size of really small cutter (.022") for guitar fretboards that is three flute and a few one flute cutters for plastic/aluminum/brass. As has been noted, the key is chip load. Chips take away the heat which in turn helps the tooling stay sharper, last longer and cut more reliably. Calculating chip load so that your tooling RPM and feed speeds are reasonably close to optimum is a good thing. One thing I've learned over time is that many of us are more conservative than we need to be. That tiny cutter I mentioned? I originally was moving that puppy really slowing, fearing it would break too easily. After a conversation with Ron at Precise Bits where I bought it and his help with the math, I now push that itty bitty thing at 24 ipm rather than about 5 ipm and get to 2mm in only 5 passes at 18K RPM. 24 ipm isn't very fast compared to the 200-400 ipm I run .25" cutters at when I can, but still...the chip load is correct and I'm using that bit like it was designed to be used now.
    Last edited by Jim Becker; 12-07-2019 at 10:43 AM. Reason: Corrected IPS to IPM
    --

    The most expensive tool is the one you buy "cheaply" and often...

  7. #7
    Join Date
    Apr 2017
    Location
    Tucson, Arizona
    Posts
    519
    Quote Originally Posted by Jim Becker View Post
    95+% of my tooling is two-flute. I have one size of really small cutter (.022") for guitar fretboards that is three flute and a few one flute cutters for plastic/aluminum/brass. As has been noted, the key is chip load. Chips take away the heat which in turn helps the tooling stay sharper, last longer and cut more reliably. Calculating chip load so that your tooling RPM and feed speeds are reasonably close to optimum is a good thing. One thing I've learned over time is that many of us are more conservative than we need to be. That tiny cutter I mentioned? I originally was moving that puppy really slowing, fearing it would break too easily. After a conversation with Ron at Precise Bits where I bought it and his help with the math, I now push that itty bitty thing at 24 ips rather than about 5 ips and get to 2mm in only 5 passes at 18K RPM. 24 ips isn't very fast compared to the 200-400 ips I run .25" cutters at when I can, but still...the chip load is correct and I'm using that bit like it was designed to be used now.
    Hi Ronald,
    I think Jim meant to say ipm (inches per minute), not ips (inches per second) for his feed rates.
    David

  8. #8
    Join Date
    Mar 2003
    Location
    SE PA - Central Bucks County
    Posts
    50,681


    Edited...
    --

    The most expensive tool is the one you buy "cheaply" and often...

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •