Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO


Page 1 of 2 12 LastLast
Results 1 to 20 of 22

Thread: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

  1. #1
    Member SteveS's Avatar
    Join Date
    Oct 2004
    Location
    USA
    Posts
    175
    Downloads
    0
    Uploads
    0

    Default Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    I need to cut some tool bench tops with a lot of 20mm holes in the top. Multi

    Cutting will be on a ShopBot Alpha with 4 hp spindle at 18,000 rpm. The shop frowns on over 100 ipm feeds, but...

    What I have read is that with MDF you should cut as fast as possible and 3/4" is practical in one pass.

    I plan to cut some in Baltic Birch and MDO also.

    I'm committed to a 1/2" bit so the 20 mm holes don't need any tabs to hold the centers.

    Whiteside is my usual brand of bits and I am seeing start with $20 2 flute straight (1069) then go to $60 for 2 flute upcut (RU5150) and then $70 for three flute upcut (RU5200T) with others in between. I want one that is going to give me some life time before sharpening.

    So, any advise on which bit and cutting speed? My normal cutting is solid wood and this is new to me.

    Steve.

    Similar Threads:


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

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    What I have read is that with MDF you should cut as fast as possible
    This pretty much applies to all sheet goods.

    A good 2 flute spiral is actually capable of cutting 3/4 in one pass at about 700ipm at about 16,000 rpm. But you'll be limited by spindle power and machine rigidity on how fast your machine is capable of cutting.

    At 100ipm, I'd recommend running the spindle at about 10,000 rpm. I'd actually try to cut in the 175-200ipm range at 10,000-12,000 rpm.
    You'll get the best tool life at the highest possible chip loads, which means high feedrates and low rpm's.

    3 flute tools are really only used at very high feedrates, as they should be cutting 50% faster than a similar 2 flute for a given rpm.

    High quality, long life tooling will run about $90 per bit, and are usually made of a harder grade of carbide. Vortex Tools XP series is one. I use a similar too from Active Tooling.

    A compression spiral is what I'd recommend, as an upcut will leave a rough top edge, which will worsen as the tool gets dull A compression spiral will give cleaner edges, even as it dulls.

    If you're not doing a lot of parts, 2 flute carbide tipped straight bits are probably your best bang for the buck option, especially if your limited on feedrate. They are much cheaper, and can be sharpened for about $5 each, compared to $15-$25 to sharpen a compression 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)


  3. #3
    Registered
    Join Date
    Jun 2014
    Posts
    777
    Downloads
    0
    Uploads
    0

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    Ply and Mdf is fairly forgiving speed wise, if it screams too fast, lower rpms or increase feed to a whistle. 120ipm @ 12000rpm is a good place to start.

    did you get any explanation as to why 3/4" doc was better than say 1/2" in Mdf. I don't find doc makes much difference to finish, I suppose the deeper you go the less time the bits in the Mdf so you would get more life out of the bit.

    Ply you will want a 2 flute compression spiral, use leads and plunge or Helix deeper than the upcut length of bit before lead in. And Mdf, I know there's bits that may be better but I use 2 flute downcut spirals and they work well, you can use compression to improve bottom edge finish but a bit of sanding is cheaper than gumming up a more expensive compression spiral imo.

    1/2" bits are great for pocketing or roughing out lots of material, but it would be pretty inefficient use of a sheet if you use for contouring, 1/4" works fine upto 25mm sheet. Obviously in multiple depths. 30mm sheet you might want to consider using an 8-10mm bit.



  4. #4
    Registered
    Join Date
    Jun 2014
    Posts
    777
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by ger21 View Post
    This pretty much applies to all sheet goods.

    A good 2 flute spiral is actually capable of cutting 3/4 in one pass at about 700ipm at about 16,000 rpm. But you'll be limited by spindle power and machine rigidity on how fast your machine is capable of cutting.

    At 100ipm, I'd recommend running the spindle at about 10,000 rpm. I'd actually try to cut in the 175-200ipm range at 10,000-12,000 rpm.
    You'll get the best tool life at the highest possible chip loads, which means high feedrates and low rpm's.

    3 flute tools are really only used at very high feedrates, as they should be cutting 50% faster than a similar 2 flute for a given rpm.

    High quality, long life tooling will run about $90 per bit, and are usually made of a harder grade of carbide. Vortex Tools XP series is one. I use a similar too from Active Tooling.

    A compression spiral is what I'd recommend, as an upcut will leave a rough top edge, which will worsen as the tool gets dull A compression spiral will give cleaner edges, even as it dulls.

    If you're not doing a lot of parts, 2 flute carbide tipped straight bits are probably your best bang for the buck option, especially if your limited on feedrate. They are much cheaper, and can be sharpened for about $5 each, compared to $15-$25 to sharpen a compression bit.
    Would you say a 2flute 1/4" is capable of 3/4" @ 120ipm Ger? Ive only ever pushed one to 1/2" pass. I know it would likely go more but It's deflection that bothers me.



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

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    Probably, but the risk of breaking them is very high. Also, the smaller the diameter, the shorter the tool life.

    I only use 1/4" bits when a larger one won't work, and typically use a 1/4" DOC at about 400ipm.

    I think that cutter deflection with carbide bits is actually a myth, especially with small diameter bits. What most people perceive to be cutter deflection is actually machine deflection. Carbide is extremely rigid, and a 1/4" bit will snap long before it bends.

    There's a recent thread here where someone was sure that there cutter was deflecting nearly .01". Until he put the same cutter in a mill and found out it was his router that was deflecting.

    At work we sometimes use 3/8" compression bits, cutting 3/4" plywood at 700ipm and about 17,000 rpm.

    Cutting in one pass not only extends tool life, but it also reduces your cycle times by more than half.

    1/2" bits are great for pocketing or roughing out lots of material, but it would be pretty inefficient use of a sheet if you use for contouring,
    Not when time is money, and you have a lot of sheets to cut. Especially at very high feedrates, where you need a large, stronger tool.

    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 SteveS's Avatar
    Join Date
    Oct 2004
    Location
    USA
    Posts
    175
    Downloads
    0
    Uploads
    0

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    My choice of of 1/2" diameter bit is to clear out the 20 mm holes. I didn't want to go back and clean up tabs if I used my normal 1/4" diameter end mills. A 3/8" would probably be capable, the remaining hole center would be sucked up in the dust collection.

    In trying to follow the logic, with 150 ipm and 18,000 rpm does it make sense to get a single flute compression bit like the Active Tooling compression AT10101 or AT10149?

    The Votec site shows single flute 800/900 Series Upcut Finishers for the 100 to 300 ipm cutting rate. #850 #950 (no real explanation on what is difference between 800/900) They are not compression.

    Vortec compression start at the 3100 series, 3135XP without upcut, and 3150XP(m) with upcut. Are those the ones you are talking about?

    Steve.



  7. #7
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    800's are upcut, 900's are downcut.

    I think a 3035 is probably your best choice. Actually, a 3030 should be a lot cheaper, and the 1mm core of your hole would not be an issue.
    Note that if you buy 2 or more you save about 30%.

    For Active, I'd say the AT10132. You want the shortest cutting length possible.

    All compression bits have an upcut bottom. The (m) models have a shorter upcut section.
    The 3130 or 3135 will probably give you the longest tool life, but you ideally want to run them hard. If you're under 200ipm, you need to keep the rpm down around 10,000.

    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)


  8. #8
    Member SteveS's Avatar
    Join Date
    Oct 2004
    Location
    USA
    Posts
    175
    Downloads
    0
    Uploads
    0

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    I am going to confirm the ShopBot ipm and spindle speed options I have on the machine later today.

    To use those bits, I need to get an ER20 3/8" collet. Brands I have locally available are RapidKut, Rego-Fix, ETM, Techniks and Parlec. Any to avoid?

    Steve.



  9. #9
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    I've only used Techniks. Not familiar with the others.

    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)


  10. #10
    Registered
    Join Date
    Aug 2009
    Location
    Canada
    Posts
    107
    Downloads
    0
    Uploads
    0

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    3/4 inch mdf single pass with a 1/4 inch compression @ 120 ipm
    1/2 inch mdf single pass with a 1/4 inch compression @ 160 ipm

    I use Centurion tools.

    Both of these give IMO the best feed rate to edge finish.

    Ger - Sounds like you are running some really pro level woodworking machines.



  11. #11
    Registered
    Join Date
    Jun 2014
    Posts
    777
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by ger21 View Post
    Probably, but the risk of breaking them is very high. Also, the smaller the diameter, the shorter the tool life.

    I only use 1/4" bits when a larger one won't work, and typically use a 1/4" DOC at about 400ipm.

    I think that cutter deflection with carbide bits is actually a myth, especially with small diameter bits. What most people perceive to be cutter deflection is actually machine deflection. Carbide is extremely rigid, and a 1/4" bit will snap long before it bends.

    There's a recent thread here where someone was sure that there cutter was deflecting nearly .01". Until he put the same cutter in a mill and found out it was his router that was deflecting.

    At work we sometimes use 3/8" compression bits, cutting 3/4" plywood at 700ipm and about 17,000 rpm.

    Cutting in one pass not only extends tool life, but it also reduces your cycle times by more than half.



    Not when time is money, and you have a lot of sheets to cut. Especially at very high feedrates, where you need a large, stronger tool.

    A lot of my clients would complain if I contour with 1/2" for wastage. Mostly the ones who supply nested cut sheets.

    I agree on bit deflection it would likely snap first. i think a lot of it is also down to swelling especially with sheet timber.

    Last edited by Jon.N.CNC; 04-07-2016 at 05:56 PM.


  12. #12
    Member SteveS's Avatar
    Join Date
    Oct 2004
    Location
    USA
    Posts
    175
    Downloads
    0
    Uploads
    0

    Default Re: Speed/Feed advise MDF/Ply - Check my math

    I talked with the shop and 18K spindle speed is available and 500 ipm. It can feed 600 ipm, but prefer 500 ipm max.

    Now I need someone to check my math and logic.

    The Vortex chipload chart shows Plywood for 3/8" tool diameter to be 0.017" - 0.020" per cutting edge. For double edge tool it is then 0.034" to 0.040" chipload
    RPM * Chip load = ipm
    12,000 * 0.034 = 408 ipm
    12,000 * 0.040 = 480 ipm

    The Vortex chipload chart shows MDF for 3/8" tool diameter to be 0.020" - 0.023" per cutting edge. For double edge tool it is then 0.040" to 0.046" chipload
    11,000 * 0.040 = 440 ipm
    11,000 * 0.046 = 506 ipm

    Do these calculation the pass the laugh test???

    If so, I am planning to get the Vortex 3130 two-flute compression spiral and using initial settings of 12,000 and 425 ipm for plywood, 11,000 and 450 ipm for MDF.

    Also, the shop suggested to "fine tune" the feed rate by sound, increase the rate until it sounds smooth, then increase in 10% increments until it starts to scream and back off one increment.

    Steve.

    Last edited by SteveS; 04-09-2016 at 12:22 PM. Reason: change title


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

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    Vortex chip loads tend to be maximums, and I think you'd want to go a bit lower with a shopbot.
    I'd start with similar feedrates and a bit higher rpm, like 13,000-14,000.
    Or, start at 12,000 rpm and 250ipm and increase feedrate from there.

    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

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    You can download a demo of G-Wizard. Its a good program for feeds and speeds. What type of bit are you using?
    Carbide or HHS, how many flutes, how thick is the MDF?
    This is what I get for a nice cut on a 1/2" carbide double flute endmill .
    1/2 " MDF ((one pass))
    Feed 56.446 inches per minute
    Spindle Speed 8561 rpm
    Plunge 28.2



  15. #15
    Member SteveS's Avatar
    Join Date
    Oct 2004
    Location
    USA
    Posts
    175
    Downloads
    0
    Uploads
    0

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    Quote Originally Posted by betonesto View Post
    You can download a demo of G-Wizard. I
    I bought G-Wizard, find it to be very metal oriented. Even in his blog he talks down about "soft" materials such as wood. I believe the G-Wizard formulas do not take into consideration the different angular geometry of the premium wood bits.

    Steve.



  16. #16
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    This is what I get for a nice cut on a 1/2" carbide double flute endmill .
    1/2 " MDF ((one pass))
    Feed 56.446 inches per minute
    Spindle Speed 8561 rpm
    At 15,000 rpm, I can cut 1/2" MDF at 1000ipm.
    10x what G-Wizard says.

    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)


  17. #17
    Member SteveS's Avatar
    Join Date
    Oct 2004
    Location
    USA
    Posts
    175
    Downloads
    0
    Uploads
    0

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    My first CNC class on a ShopBot was given by a guy with a great reputation as a metal CNC machinist. The class went into the 1/3rd rule, only cut at a depth 1/3rd the diameter of the tooling and then creep up. The procedure part of the class on the CNC was good, but set me back quite a ways in getting things cut quickly. I'm sure it was all relevant to metal.

    Steve.



  18. #18
    Registered
    Join Date
    Jun 2014
    Posts
    777
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by ger21 View Post
    At 15,000 rpm, I can cut 1/2" MDF at 1000ipm.
    10x what G-Wizard says.
    One hell of a vacuum bed for that required I can imagine.



  19. #19
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

    Two 10HP Becker's on a 5x12 table.
    10HP spindle.
    With a 3 flute tool, we cut in the 1200ipm range at 16,000 rpm.

    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)


  20. #20
    Registered
    Join Date
    Jun 2014
    Posts
    777
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by ger21 View Post
    Two 10HP Becker's on a 5x12 table.
    10HP spindle.
    With a 3 flute tool, we cut in the 1200ipm range at 16,000 rpm.
    Yeah you'd need to be doing those speeds just to pay the electric bill, how many amps?



Page 1 of 2 12 LastLast

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

Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO

Speed/Feed advise for 1/2" bit to cut MDF / BB Ply / MDO