Page 1 of 2 12 LastLast
  1. #1
    Howdy,

    My belt drive cnc was built for milling foamboard but recently thought it would be nice to cut plywood and acrylic. Basic spec: nema 24, t5 belt, Gecko, Mach 3, 900w spindle (12-26,000rpm)

    I was reading this very helpful F&S thread below, which gives a good indication of what i should be aiming for. However as my machine uses, belts and v-groove bearings and is a light weight design for speed I am wondering if there are setting I can use which will at least give me a chance of cutting something denser with multiple passed with reasonable success.

    http://www.mycncuk.com/threads/4330-...-and-feed-rate

    I can see from cutting through 9mm ply using 2mm passes that the tip of the single flute cutter is blacking pretty quickly. The timber is not blackening but 20mm/s is not very fast is it ha ha and probably part of the problem.

    It could be that the whole machine needs rebuilt to cut more resistant materials but any indication of
    where I can look first to at least try to get the machine i've got cutting ply would be useful.

    Thanks.

    Click image for larger version. 

Name:	cnc machine.png 
Views:	58 
Size:	1.65 MB 
ID:	22457
    Last edited by marbles; 03-08-2017 at 12:16 PM.

  2. #2
    Ger21's Avatar
    Lives in Detroit, United States. Last Activity: 9 Hours Ago Has been a member for 5-6 years. Has a total post count of 500. Received thanks 66 times, giving thanks to others 0 times. Referred 1 members to the community.
    Quote Originally Posted by marbles View Post
    I can see from cutting through 9mm ply using 2mm passes that the tip of the single flute cutter is blacking pretty quickly. The timber is not blackening but 20mm/s is not very fast is it ha ha and probably part of the problem.
    What size tool, and how many flutes?
    What feed and speed did you use?

    Try 4-5m/min at 15,000 rpm.
    Gerry
    ______________________________________________
    UCCNC 2017 Screenset

    Mach3 2010 Screenset

    JointCAM - CAM for Woodworking Joints

  3. #3
    Quote Originally Posted by Ger21 View Post
    What size tool, and how many flutes?
    What feed and speed did you use?

    Try 4-5m/min at 15,000 rpm.
    Hi Gerry,

    Thanks for reply. I was using a single flute spiral bit. 4mm dia and 12mm cut length. Spindle set at 'No 6', which i would take to be about 26,000rpm

    I'll need to get back to you about the exact feeds and speeds tomorrow. I set the feed rate in Aspire to 80mm/s in 2mm passes but of course this doesnt necessarily relate to the actual rate, which i'll work out tomorrow in Mach3.

    I did notice that it was rounding corners again so that'll need a tweak in motor tuning for wood. Currently settings are for foamboard carving.

    Thanks

    Click image for larger version. 

Name:	feeds.jpg 
Views:	23 
Size:	373.7 KB 
ID:	22458
    Last edited by marbles; 03-08-2017 at 09:29 PM.

  4. #4
    Quote Originally Posted by Ger21 View Post
    What size tool, and how many flutes?
    What feed and speed did you use?

    Try 4-5m/min at 15,000 rpm.
    Hi,

    I set Aspire to profile cut a 400mm square at 100mm/s and timed how long it took to mock cut out the full 1600mm. This took 51.40 seconds. So at 30.9mm/s actual speed, clearly not the 100mm/s set in Aspire. The spindle speed is not set in Aspire but on the actual spindle.

    I tried the test again using a faster speed but it gave exactly the same time to travel 1600mm. So it must be that motor tune setting are incorrect or inhibiting speed.

    My config settings are 26 stesp- 2000 velocity - 1000 acceleration

    (As as side note I recalibrated X and Y axis so they are scaled correctly).

    lets say as a rule of thumb I wish to cut out 12mm plyood in forms less that A4 scale with a mixture of straight corner and curved shapes, 10mm slots and 8mm holes etc. So reasonable detail.

    I'm a little bit stumped why I couldnt change its speed in Aspire and why 100mm/s does not translate to its actual speed. I'm missing something basic am I not ha!

    Any ideas welcome

    This is the gcode file.

    ( Profile 1600mm test )
    ( File created: Friday, August 04, 2017 - 09:52 PM)
    ( for Mach2/3 from Vectric )
    ( Material Size)
    ( X= 410.000, Y= 410.000, Z= 4.000)
    ()
    (Toolpaths used in this file:)
    (Profile 1)
    (Tools used in this file: )
    (1 = End Mill {3 mm})
    N100G00G21G17G90G40G49G80
    N110G71G91.1
    N120T1M06
    N130 (End Mill {3 mm})
    N140G00G43Z20.000H1
    N150S20000M03
    N160(Toolpath:- Profile 1)
    N170()
    N180G94
    N190X0.000Y0.000F6000.0
    N200G00X4.620Y4.260Z6.000
    N210G1Z-0.500F600.0
    N220G2X3.120Y5.760I0.000J1.500F6000.0
    N230G1Y405.760
    N240G2X4.620Y407.260I1.500J0.000
    N250G1X404.620
    N260G2X406.120Y405.760I0.000J-1.500
    N270G1Y5.760
    N280G2X404.620Y4.260I-1.500J0.000
    N290G1X4.620
    N300G00Z6.000
    N310G00Z20.000
    N320G00X0.000Y0.000
    N330M09
    N340M30
    %

  5. #5
    Well is sounds like you have a max vel. setting somewhere that will limit your commanded speed. What software are you using?
    ..Clive
    The more you know, The better you know, How little you know

  6. The Following User Says Thank You to Clive S For This Useful Post:


  7. #6
    Quote Originally Posted by Clive S View Post
    Well is sounds like you have a max vel. setting somewhere that will limit your commanded speed. What software are you using?
    Hmm..i hadnt thought of that i'll have a look in Mach3 tomorrow. Thanks

  8. #7
    Ger21's Avatar
    Lives in Detroit, United States. Last Activity: 9 Hours Ago Has been a member for 5-6 years. Has a total post count of 500. Received thanks 66 times, giving thanks to others 0 times. Referred 1 members to the community.
    Your velocity is set to 2000mm/min, which is about 33mm/sec. The Velocity setting is the Maximum Mach3 will move at.
    Gerry
    ______________________________________________
    UCCNC 2017 Screenset

    Mach3 2010 Screenset

    JointCAM - CAM for Woodworking Joints

  9. The Following User Says Thank You to Ger21 For This Useful Post:


  10. #8
    Quote Originally Posted by Ger21 View Post
    Your velocity is set to 2000mm/min, which is about 33mm/sec. The Velocity setting is the Maximum Mach3 will move at.
    Ah its the max! Of course..better increase it a bit. Thanks!
    Last edited by marbles; 05-08-2017 at 09:43 AM.

  11. #9
    Quote Originally Posted by marbles View Post
    I did notice that it was rounding corners again so that'll need a tweak in motor tuning for wood. Currently settings are for foamboard carving.
    Check on the general config page if you have set the "Stop CV on angles > xx Degrees" You can try a value of 50 deg. and reduce it if needed.


    To set the velocity and acceleration in motor tunning, increase the values and test by manual jogging and applying some force by hand against the moving axis until the motors will stall to easy. Then decrease a bit the values. You have to restart mach3 for the modified motor tuning settings to take effect.

  12. The Following User Says Thank You to paulus.v For This Useful Post:


  13. #10
    Quote Originally Posted by paulus.v View Post
    Check on the general config page if you have set the "Stop CV on angles > xx Degrees" You can try a value of 50 deg. and reduce it if needed.


    To set the velocity and acceleration in motor tuning, increase the values and test by manual jogging and applying some force by hand against the moving axis until the motors will stall to easy. Then decrease a bit the values. You have to restart mach3 for the modified motor tuning settings to take effect.
    Thanks. All very helpful advice. As I have re-tensioned the v-groove wheels i've noticed it stalling a few times. so will modify and restart.

Page 1 of 2 12 LastLast

Similar Threads

  1. Help with speeds/feeds please?
    By examorph in forum Tool & Tooling Technology
    Replies: 5
    Last Post: 29-01-2017, 01:54 PM
  2. Speeds and feeds
    By eurikain in forum Workshop & Equipment
    Replies: 3
    Last Post: 26-03-2016, 06:00 PM
  3. Feeds and speeds software?
    By Leadhead in forum Computer Software
    Replies: 9
    Last Post: 31-10-2015, 09:34 PM
  4. Feeds and speeds
    By dudz in forum Tool & Tooling Technology
    Replies: 0
    Last Post: 26-08-2013, 11:42 AM
  5. Speeds and Feeds
    By Web Goblin in forum Tool & Tooling Technology
    Replies: 0
    Last Post: 20-09-2012, 01:38 PM

Bookmarks

Posting Permissions

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