advice on chipping and milling quality with 8mm bit on 10mm plywood


Results 1 to 20 of 20

Thread: advice on chipping and milling quality with 8mm bit on 10mm plywood

  1. #1
    Member
    Join Date
    Aug 2017
    Posts
    31
    Downloads
    0
    Uploads
    0

    Default advice on chipping and milling quality with 8mm bit on 10mm plywood

    Hi,
    I'm milling a profile cut full depth on a 10mm plywood piece.

    I'm using an 8mm, 3-flute endmill, downcut.
    My settings were:

    16000 RPM
    5mm/sec feedrate


    A few things in the attached images are clear to see:

    1 - some of the paths generate a "twirly" piece of chipping. Why is that?

    2 - The finished quality is not good. There are chipped off parts at the surface. It looks like what an upcut should do, but I have a downcut. What causes this effect?

    3 - The plywood get's darker as it burns, which is not something I want.


    During the milling, my RPM was too low and the axis "lagged" by about 5mm, so I had to restart the Z position because the bit was getting 'stuck' too much and being pulled the wrong way, so I realized i need to raise the RPM to make it go smoother into the wood. When I raised the RPM to 21000, the wood was getting a bit darker because of burn. Is there some balance here i'm missing?


    Attached are the images.

    Thank you!

    Similar Threads:
    Attached Thumbnails Attached Thumbnails advice on chipping and milling quality with 8mm bit on 10mm plywood-img_20190124_213012-jpg   advice on chipping and milling quality with 8mm bit on 10mm plywood-img_20190124_213039-jpg   advice on chipping and milling quality with 8mm bit on 10mm plywood-img_20190124_213102-jpg  


  2. #2
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    You should be cutting at 50-75mm/sec at 16,000 rpm, not 5mm/sec.
    Can you post a picture of the bit?
    What kind of machine is this?

    Gerry

    UCCNC 2017 Screenset
    [URL]http://www.thecncwoodworker.com/2017.html[/URL]

    Mach3 2010 Screenset
    [URL]http://www.thecncwoodworker.com/2010.html[/URL]

    JointCAM - CNC Dovetails & Box Joints
    [URL]http://www.g-forcecnc.com/jointcam.html[/URL]

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  3. #3
    Member
    Join Date
    Aug 2017
    Posts
    31
    Downloads
    0
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    I'm using a Stepcraft 840, with a MM-1000 spindle.

    The bit is attached in an image here.

    It doesn't make sense to me to run it at that feedrate... The machine max is 3000mm/min, so that's 50/sec, but it's not recommended (according to them) to run it at 100%.
    If I did it at 5mm/sec and 16000rpm, and it "lagged" because the wood was pushing on the bit too fast, making the axis go out of sync, that will probably have a much much worse effect if I try to up the feedrate to x10 of that... right?

    What do you think?


    Thanks

    Attached Thumbnails Attached Thumbnails advice on chipping and milling quality with 8mm bit on 10mm plywood-img_20190125_082657-jpg  


  4. #4
    Member
    Join Date
    Feb 2018
    Location
    Finland
    Posts
    0
    Downloads
    0
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    Toi don’t have enough power on a stepcraft to perform such deep cuts. Try doing several passes with eg 2-3mm doc


    Sent from my iPhone using Tapatalk



  5. #5
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    That's not a downcut bit.

    Gerry

    UCCNC 2017 Screenset
    [URL]http://www.thecncwoodworker.com/2017.html[/URL]

    Mach3 2010 Screenset
    [URL]http://www.thecncwoodworker.com/2010.html[/URL]

    JointCAM - CNC Dovetails & Box Joints
    [URL]http://www.g-forcecnc.com/jointcam.html[/URL]

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  6. #6
    Member
    Join Date
    Feb 2018
    Location
    Finland
    Posts
    0
    Downloads
    0
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    A stepcraft can’t cut that deep in one pass. Take from 1mm to 3mm passes with a higher speed.
    The stepcrafts tiny steppers can’t handle bigger loads and the frame isn’t rigid enough for cutting deep passes with a single cut.
    So go with light passes and keep the machine cleaned and lubed and it will work.


    Sent from my iPhone using Tapatalk



  7. #7
    Member
    Join Date
    Aug 2017
    Posts
    31
    Downloads
    0
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    Ah, my mistake indeed..
    Thank you for the clarification


    Do you have any suggestions about the other issues I mentioned..?



  8. #8
    Member awerby's Avatar
    Join Date
    Apr 2004
    Posts
    5727
    Downloads
    0
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    Try running faster but not so deep. If you only took 5 mm at a time and taking two passes to cut through, it would go smoother. Also, 4-flute bits like that are better suited to steel than wood. You only need one or two flutes for wood. With 4, it's equivalent to running at twice the RPM.

    [FONT=Verdana]Andrew Werby[/FONT]
    [URL="http://www.computersculpture.com/"]Website[/URL]


  9. #9
    Member
    Join Date
    Aug 2017
    Posts
    31
    Downloads
    0
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    Hi,
    Okay thanks. I think also compression bits would work better.

    You say 'try running faster... 5mm at a time', but this is an 8mm diameter bit, and my pass depth was 3mm... so 5mm would be deeper than what I did.



  10. #10
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    Try a smaller bit, either 1/4" or 6mm, like this:

    https://www.amanatool.com/46202-soli...-down-cut.html

    Lower the rpm to 10,000-12,000, and try 3mm depth @ 10-15mm/sec

    Gerry

    UCCNC 2017 Screenset
    [URL]http://www.thecncwoodworker.com/2017.html[/URL]

    Mach3 2010 Screenset
    [URL]http://www.thecncwoodworker.com/2010.html[/URL]

    JointCAM - CNC Dovetails & Box Joints
    [URL]http://www.g-forcecnc.com/jointcam.html[/URL]

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  11. #11
    Member
    Join Date
    Aug 2017
    Posts
    31
    Downloads
    0
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    @ger21,

    But lowering the RPM and raising the feedrate would make the bit cut less smoothly and go faster through the wood... isn't that the opposite of what I'm trying to achieve?



  12. #12
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by awerby View Post
    With 4, it's equivalent to running at twice the RPM.
    No.... this info is incorrect.
    the RPM is calculated to how fast the cutter is passing the material.... this is termed Cutting Speed (usually in SurfaceFeet/Minute or Metres/Minute). Once you calculate the RPM, you then multiply that by chip thickness, multiplied by the number of teeth on the cutter.
    RPM = CS / (Cutter Dia x Pi) x 1000.....metric CS m/min
    Feedrate = RPM x Feed per tooth x number of teeth

    so... a 2 flute is run 2x faster than 1 flute... but a 4 flute is programmed 2x faster than a 2 flute.

    your issue may be your feed is too slow to create a chip, it would make only dust..plus going slow also creates heat and allow burning of the wood.
    A 4 flute (steel cutting geom) doesn't have deep flutes for chip evacuation. So look for cutters made specifically for wood. You could utilize cutters designed for aluminium, as these have sharper edges, uncoated, and a greater helix angle for slicing instead of a scraping like action on the softer materials.
    Dust/chips should be removed from around the cutter to help minimise heat generation & to keep the cutter edges sharp. A vacuum system (1st choice) or a simple air blow (messier but would improve the part finish and extend tool life)



  13. #13
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    Quote Originally Posted by yafimski View Post
    @ger21,

    But lowering the RPM and raising the feedrate would make the bit cut less smoothly and go faster through the wood... isn't that the opposite of what I'm trying to achieve?
    If it does, decrease the depth of cut.
    Slower feedrates and higher rpm's generate heat, which dulls the tools, and makes things worse.

    Gerry

    UCCNC 2017 Screenset
    [URL]http://www.thecncwoodworker.com/2017.html[/URL]

    Mach3 2010 Screenset
    [URL]http://www.thecncwoodworker.com/2010.html[/URL]

    JointCAM - CNC Dovetails & Box Joints
    [URL]http://www.g-forcecnc.com/jointcam.html[/URL]

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  14. #14
    Member
    Join Date
    Aug 2017
    Posts
    31
    Downloads
    0
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    Hi,
    I'm a bit confused from all the answers.
    When I try to put my bit data into FSWizard for example, the result is to run the 8mm bit at 110 mm/sec, with 8700 RPM... MY machine can only go 50 mm/sec maximum, and i'm still confused - if I go at maximum feedrate but spin really slow, that will break my machine no?? It's like dragging a very slow spinning object really fast into something.. I can't image how 8000rpm + 50mm/sec is better than 16000rpm + 25mm/sec...



  15. #15
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    You need to adjust the depth of cut to compensate for the weak machine.

    Try what I said above, 10,000-12,000, and maybe 15-20mm/sec, but start at 1mm depth.

    Higher rpm and slower feedrates will generate a lot of heat and destroy your bits, as you've already seen.

    Gerry

    UCCNC 2017 Screenset
    [URL]http://www.thecncwoodworker.com/2017.html[/URL]

    Mach3 2010 Screenset
    [URL]http://www.thecncwoodworker.com/2010.html[/URL]

    JointCAM - CNC Dovetails & Box Joints
    [URL]http://www.g-forcecnc.com/jointcam.html[/URL]

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  16. #16
    Member
    Join Date
    Aug 2017
    Posts
    31
    Downloads
    0
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    Thanks ger21!
    I'll try that. Compensating by reducing depth seems like a viable solution.

    I'll report back with good/bad results.



  17. #17
    Member awerby's Avatar
    Join Date
    Apr 2004
    Posts
    5727
    Downloads
    0
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    Quote Originally Posted by Superman View Post
    No.... this info is incorrect.
    the RPM is calculated to how fast the cutter is passing the material.... this is termed Cutting Speed (usually in SurfaceFeet/Minute or Metres/Minute). Once you calculate the RPM, you then multiply that by chip thickness, multiplied by the number of teeth on the cutter.
    RPM = CS / (Cutter Dia x Pi) x 1000.....metric CS m/min
    Feedrate = RPM x Feed per tooth x number of teeth

    so... a 2 flute is run 2x faster than 1 flute... but a 4 flute is programmed 2x faster than a 2 flute.
    [I'm a bit confused by your reply, Superman. How is what I wrote incorrect? Since according to your formula, feedrate is determined by the RPM times the number of teeth (or flutes) on a tool , and doubling those doubles the feedrate, it's the same thing as doubling the RPM, no? If I'm missing something here, please point it out in terms mere mortals can understand...]

    [FONT=Verdana]Andrew Werby[/FONT]
    [URL="http://www.computersculpture.com/"]Website[/URL]


  18. #18
    Member awerby's Avatar
    Join Date
    Apr 2004
    Posts
    5727
    Downloads
    0
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    Quote Originally Posted by yafimski View Post
    Hi,
    Okay thanks. I think also compression bits would work better.

    You say 'try running faster... 5mm at a time', but this is an 8mm diameter bit, and my pass depth was 3mm... so 5mm would be deeper than what I did.
    [Originally you said you were running this profile cut at "full depth" which was 10mm, remember? 5mm would be half that.]

    [FONT=Verdana]Andrew Werby[/FONT]
    [URL="http://www.computersculpture.com/"]Website[/URL]


  19. #19
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by awerby View Post
    [I'm a bit confused by your reply, Superman. How is what I wrote incorrect? Since according to your formula, feedrate is determined by the RPM times the number of teeth (or flutes) on a tool , and doubling those doubles the feedrate, it's the same thing as doubling the RPM, no? If I'm missing something here, please point it out in terms mere mortals can understand...]
    RPM is calculated on the diameter of the cutter to suit the material being machined.
    so... changing a cutter from 4 flute to 2 flute means that the feedrate is only to be altered ...altering the RPM changes the cutting speed that has designed for that cutter geometry.

    you may not be locked in to what is specified by the tool manufacturers, but what works for your application/setup.
    say... a 10mm dia x 2 flute verses 10mm x 4 flute.... both run at the same RPM but the 4 flute would be programmed at 2x the feed as a 2 flute
    take material steel for example
    a HSS runs about 25 m/min. so the RPM using 10mm dia is set around S800, dia 5mm would be S1600. if you double RPM, your cutter runs the risk of not lasting too long.
    That's not to say you cannot do it, you need to weigh the pros and cons.

    The principle of thinking that doubling RPM is the same as halving feed is incorrect.... the time is quicker, but you have actually doubled the recommended cutting speed that the manufacturers have designed the tools to be optimally run best

    Last edited by Superman; 01-26-2019 at 07:28 PM.


  20. #20
    Member awerby's Avatar
    Join Date
    Apr 2004
    Posts
    5727
    Downloads
    0
    Uploads
    0

    Default Re: advice on chipping and milling quality with 8mm bit on 10mm plywood

    Quote Originally Posted by Superman View Post
    RPM is calculated on the diameter of the cutter to suit the material being machined.
    so... changing a cutter from 4 flute to 2 flute means that the feedrate is only to be altered ...altering the RPM changes the cutting speed that has designed for that cutter geometry.

    [Most cutters can run fine in a fairly wide range of RPMs, but 2-flute cutters are designed for different materials than 4-flute ones. In general, you should run smaller tools faster than larger ones; this is based on SFM (surface feet per minute) which should be adjusted to yield an optimum chip size.]

    you may not be locked in to what is specified by the tool manufacturers, but what works for your application/setup.
    say... a 10mm dia x 2 flute verses 10mm x 4 flute.... both run at the same RPM but the 4 flute would be programmed at 2x the feed as a 2 flute

    [I think you got that backwards. If the RPM is the same, then the 2-flute cutter would have to feed twice as fast to produce the same size chips.]

    take material steel for example
    a HSS runs about 25 m/min. so the RPM using 10mm dia is set around S800, dia 5mm would be S1600. if you double RPM, your cutter runs the risk of not lasting too long.

    [That would depend on factors like machine rigidity and the material being cut, but you can't expect to take as big a chip with a small-diameter cutter as with a big one; your formula has to take that into account.]

    That's not to say you cannot do it, you need to weigh the pros and cons.


    The principle of thinking that doubling RPM is the same as halving feed is incorrect.... the time is quicker, but you have actually doubled the recommended cutting speed that the manufacturers have designed the tools to be optimally run best
    [Not necessarily - you might have been going too slow before. As far as the formula's concerned, it's the same thing. Tool manufacturers typically specify a feedrate as a unit per tooth per revolution, as well as a SFM, which varies according to the material being cut. As long as you don't exceed these values, the tool should work fine. Here's a typical manufacturer's chart, which illustrates what I'm talking about: Niagara Cutter ]

    [FONT=Verdana]Andrew Werby[/FONT]
    [URL="http://www.computersculpture.com/"]Website[/URL]


Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

advice on chipping and milling quality with 8mm bit on 10mm plywood

advice on chipping and milling quality with 8mm bit on 10mm plywood