Small diameter (.125") double compression router bits?


Results 1 to 18 of 18

Thread: Small diameter (.125") double compression router bits?

  1. #1
    Member
    Join Date
    Jan 2006
    Location
    USA
    Posts
    628
    Downloads
    0
    Uploads
    0

    Default Small diameter (.125") double compression router bits?

    Has anyone seen a small diameter "double compression" (upcut & downcut) spiral router bit? Sizes from 1/4" to 1"+ are easy to find, but I have not found anything smaller.

    Like this, just in a 1/8" diameter:

    http://www.toolstoday.com/p-5638-cnc...e-2-flute.aspx

    I'm cutting lots of small shapes in baltic birch plywood and it's very fuzzy using an upcut only bit. So, my strategy has been to run the toolpath one time with a downcut bit, and then complete the cuts with an upcut bit. This works nicely, but requires pausing the program, changing tools, resetting Z zero, etc.

    I'm also wondering if a bit this small can be used to take a full depth cut in a piece of 1/4" plywood? I generally cut in 3 passes of about .085", at speeds of 80-120 IPM. I would assume that I can make a deeper cut provided I slow down my feedrate accordingly. I'm not trying to improve my cut times, just avoid the tool change.

    Thanks!

    Steve

    Similar Threads:


  2. #2
    Registered Big-tex's Avatar
    Join Date
    Jul 2009
    Location
    USA
    Posts
    272
    Downloads
    0
    Uploads
    0

    Default

    I have never seen 1/8 compression. One way you can do is create tool path with say tool #1 (downspiral) profile starting at z 0 down to .25 depth and second tool path with tool #2 ( upspiral) starting .25 down to .5 .
    Another words 2 tool paths for 2 separate tools.



  3. #3
    Member
    Join Date
    Jan 2006
    Location
    USA
    Posts
    628
    Downloads
    0
    Uploads
    0

    Default

    Big-tex, that has been my technique, and it works quite well. Just requires a pause and a tool change - which I'd like to avoid.

    Depending on the geometry, I've been getting pretty good results with an 1/8" downcut bit. A little bit of fuzz on the bottom, but not too bad. My 1/8" upcuts have been miserable, so I probably need some better geometry for this application.

    I did finally find a .125" double compression bit. It's single flute, so lower feed rate but I'm going to give it a try. Expensive at $40, but the time savings on just a job or two may well be worth it. I'll report back after I run some parts.

    http://www.toolsxp.com/Onsrud-Cutter...s-60-100SE.asp

    Steve



  4. #4
    Registered Big-tex's Avatar
    Join Date
    Jul 2009
    Location
    USA
    Posts
    272
    Downloads
    0
    Uploads
    0

    Default

    Ok 1/4 baltic ply I would not cut 1 shot with 1/8 dia. tool. You can give it a try worst you break a bit. With 1 flute bit your feed rate would be lower comparing to 2 flute but what I worry about is stress put on small tooling. That is why I would recommend .125 passes. Just kind of curious what machine you got and whit kinda stuff is it cutting.



  5. #5
    Member
    Join Date
    Jan 2006
    Location
    USA
    Posts
    628
    Downloads
    0
    Uploads
    0

    Default

    Generally, I don't use a DOC more than the diameter of the tool. Most of the time, I'll use 1/2 to 1/4 of the tool diameter and take many light passes (so, 3 passes with a .125" cutter in .250 plywood). I've been doing this at 120 IPM with a pretty standard downcut spiral bit - with good results and no breakage.

    I expect that trying to cut full depth in one pass will require a significant slowdown in feed rate. Onsrud seems to recommend .010" chip load for that particular tool geometry. So, .125" tool, single flute, .010" chip load, 24K RPM = 240 IPM. That's for 1xDOC, so using their 25% reduction for 2xDOC, I could (should?) expect to run at 180 IPM.

    Maybe, maybe not. I figure I'll start slow and bring it up as I feel more confident. Worst case, I break a $40 tool. Not something I'm looking forward to, but it happens from time to time.

    BTW, I have an aluminum DIY machine. Linear rails, ballscrews and a 2.2kW spindle. I'm running 425 oz-in steppers (Gecko 203V @ 72VDC), but in the process of moving over to servos. My build thread:

    http://www.cnczone.com/forums/showthread.php?t=27527

    Steve



  6. #6
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default

    Quote Originally Posted by stevespo View Post
    I expect that trying to cut full depth in one pass will require a significant slowdown in feed rate. Onsrud seems to recommend .010" chip load for that particular tool geometry. So, .125" tool, single flute, .010" chip load, 24K RPM = 240 IPM. That's for 1xDOC, so using their 25% reduction for 2xDOC, I could (should?) expect to run at 180 IPM.

    Maybe, maybe not. I figure I'll start slow and bring it up as I feel more confident. Worst case, I break a $40 tool.
    Onsrud recommends .012-.018 for that tool. https://www.onsrud.com/xdoc/ChipHPlyWood

    The middle of that range gives you 360ipm - 90 = 270ipm @ 24K

    I've never used a 1/8" compression bit, but as a guess, I'd start at 18,000 rpm and 125ipm, which is close to the recommended feedrate with .012 chipload and 18,000 rpm.

    Unless your cutting at 300ipm, you don't need to spin an 1/8" bit that fast.

    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)


  7. #7
    Member
    Join Date
    Jan 2006
    Location
    USA
    Posts
    628
    Downloads
    0
    Uploads
    0

    Default

    Gerry, that's really helpful. I just realized I was looking at the MDF table when I saw the .010" chip load number. .012-.018 is recommended for hard plywood.

    I know these numbers are based on engineering, experience, real world testing, etc - but I always have a hard time (mentally) running the tools at the speeds they're designed for. Slow feedrates are no good for the tool, but some sort of safety margin is comforting to me.

    I'm expecting the tool in a few days, so I'll definitely report back my findings.

    Steve



  8. #8
    Registered Big-tex's Avatar
    Join Date
    Jul 2009
    Location
    USA
    Posts
    272
    Downloads
    0
    Uploads
    0

    Default

    Yeah Onsrud catalog and chip loads are always good to look up. I deal with them at work and have to adjust stuff based on new materials/tools used.



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

    Default

    Quote Originally Posted by stevespo View Post
    I know these numbers are based on engineering, experience, real world testing, etc - but I always have a hard time (mentally) running the tools at the speeds they're designed for. Slow feedrates are no good for the tool, but some sort of safety margin is comforting to me.
    At work, I recently realized I'd been running the RPM much too high for a long time. I used to program at 16K RPM and 300-400ipm with 1/2" tools. A few months ago I turned the spindle override all the way down, and it actually cuts better. I don't know the actual rpm, but I'm guessing around 10K-12K? You can hear that it's doing a lot more work, and getting some really big chips, especially in plywood. But I've found that the tooling lasts about 50% longer.

    From what I've seen, it's easier to break bits by going too slow and generating a lot of heat, then going too fast and exceeding the bits capabilities. I know that shops that do cabinet nesting cut 3/4" material at 1000ipm with 1/4" compression bits, so you shouldn't have any problems.

    Let us know how it goes.

    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 Big-tex's Avatar
    Join Date
    Jul 2009
    Location
    USA
    Posts
    272
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by ger21 View Post
    At work, I recently realized I'd been running the RPM much too high for a long time. I used to program at 16K RPM and 300-400ipm with 1/2" tools. A few months ago I turned the spindle override all the way down, and it actually cuts better. I don't know the actual rpm, but I'm guessing around 10K-12K? You can hear that it's doing a lot more work, and getting some really big chips, especially in plywood. But I've found that the tooling lasts about 50% longer.

    From what I've seen, it's easier to break bits by going too slow and generating a lot of heat, then going too fast and exceeding the bits capabilities. I know that shops that do cabinet nesting cut 3/4" material at 1000ipm with 1/4" compression bits, so you shouldn't have any problems.

    Let us know how it goes.
    My expeience is same w/ one exeption, I do not allow operator to mess with feeds or RPMs.
    When job calls for new type of bit I adjust it all myself by manufacturers specs first and further down by touching bit by hand and making sure there isn't heat any build up.
    Same goes for variation in density/hardness on materials cut. Routers are air cooled unileke mills with coolant. Heat= tool wear especialy on resharpened tooling.



  11. #11
    Member
    Join Date
    Jan 2006
    Location
    USA
    Posts
    628
    Downloads
    0
    Uploads
    0

    Default

    Do you have a rule of thumb for the Z feed rate? BobCAD/CAM doesn't support ramping for profile operations, so I'm doing a straight plunge at 1/3 the cutting feedrate. Is that reasonable?

    Steve



  12. #12
    Registered Big-tex's Avatar
    Join Date
    Jul 2009
    Location
    USA
    Posts
    272
    Downloads
    0
    Uploads
    0

    Default

    Based on tooling I do plunging at 50-60% feed rate.If I do have an option I ramp that will save on tooling wear.
    It worked for me so far............



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

    Default

    I used to plunge when we first got our machine. After a bunch of bit's with burned ends, I figured out how to ramp and never plunged again. It might be worth it to edit the code and add the ramps if you're making a single pass. Or, plunge outside the material.

    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
    Jan 2006
    Location
    USA
    Posts
    628
    Downloads
    0
    Uploads
    0

    Default

    My first impression of the Onsrud 60-102 (.125", single edge, double compression) is WOW. It's a great tool.

    No problems at all doing full depth cuts in .250" baltic birch plywood, 100 IPM and 18K RPM. The cuts were absolutely flawless on both sides and it created nice sized chips, not dust.

    My cutting time went from 50 minutes down to 15, and I'm sure that I can actually run it MUCH faster than 100 IPM. Potentially 270 IPM at 24K RPM, so that cut time could still get reduced significantly.

    The somewhat "high" price ($40) will be paid for with the first batch of parts.

    Steve



  15. #15
    Registered Big-tex's Avatar
    Join Date
    Jul 2009
    Location
    USA
    Posts
    272
    Downloads
    0
    Uploads
    0

    Default

    I am glad you like it.

    You will see this tool last longer as well. Onsrud has sister company that produces all carbide for them only. Investment in better tooling pays with better quality and less headache. I am glad you like it.

    Now what you need is find direct local distributor and get yourself wholesale pricing so do not have to pay retail. I never do........



  16. #16
    Registered
    Join Date
    Dec 2012
    Location
    United States
    Posts
    52
    Downloads
    0
    Uploads
    0

    Default Re: Small diameter (.125") double compression router bits?

    Quote Originally Posted by stevespo View Post
    My first impression of the Onsrud 60-102 (.125", single edge, double compression) is WOW. It's a great tool.

    No problems at all doing full depth cuts in .250" baltic birch plywood, 100 IPM and 18K RPM. The cuts were absolutely flawless on both sides and it created nice sized chips, not dust.

    My cutting time went from 50 minutes down to 15, and I'm sure that I can actually run it MUCH faster than 100 IPM. Potentially 270 IPM at 24K RPM, so that cut time could still get reduced significantly.

    The somewhat "high" price ($40) will be paid for with the first batch of parts.

    Steve

    Hey Steve/Anyone, any more luck on this bit? I've gone through a couple of them and just dont seem to last on 1/4" wood. Curious what other people are using for setting on 1/4". We have a small wood shop and would like to do more 1/4 sheets instead of 1/2 for cost and time.



  17. #17
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Small diameter (.125") double compression router bits?

    With small tools, hold down and machine rigidity are key to keep from breaking them.

    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)


  18. #18
    Registered
    Join Date
    Dec 2012
    Location
    United States
    Posts
    52
    Downloads
    0
    Uploads
    0

    Default Re: Small diameter (.125") double compression router bits?

    Thanks Gerry,

    We have a techno lc4896 thats pretty rigid, really happy with it. Cut 6-8 or so 1/2" 4x8 sheets of birch all day with two passes, 1/8" downcut, then 1/8" upcut. Do a 0.20" deep cut then 0.30" cut and works really well as we run 250ipm (max for machine) and only 2 passes like I said.

    We anchor the board with 10 or so screws every time as we do a lot of cut outs and don't want anything lifting up.

    Just curious if anyone has some real experience with this bit for some other settings.

    Steve mentioned 100 IPM and 18K RPM, just curious if he can reach out and give details where he found was optimal.



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

Small diameter (.125") double compression router bits?

Small diameter (.125") double compression router bits?