3dprintforums logo



Results 1 to 11 of 11

Thread: Trouble cutting circles with mach3

  1. #1
    Registered
    Join Date
    Oct 2011
    Location
    us
    Posts
    8
    Downloads
    0
    Uploads
    0

    Trouble cutting circles with mach3

    Hello

    I was hoping some one here could help , I am having trouble cutting circles in acrylic with Mach3 . what is happening is there is a small flat spot where the cutter enters and exits the cut . I remember someone telling me that there was a way to make the cutter cut past the spot where the cutter started the cut to make it completely round . kinda like extending the cut to clean it up . does any one have any ideas ?

    Thanks BIll

    Similar Threads:


  2. #2
    Registered Walky's Avatar
    Join Date
    Jul 2009
    Location
    Chile
    Posts
    690
    Downloads
    0
    Uploads
    0
    What you're looking for are probably "lead in - lead out" and "overcut" options (or something like that) in your CAM software. If you're using one of the Mach3 wizards, then I don't know really, since I haven't used those. Also, check that your Z axis is perfectly at 90 relative to both the X and Y axis.



  3. #3
    Registered
    Join Date
    Apr 2007
    Location
    USA
    Posts
    7908
    Downloads
    0
    Uploads
    0
    Try slowing down the Z axis plunge rate to see if it helps. If plunging too fast the cutter may be walking around in a larger circle than the diameter of the cutter as it enters the material. That would typically be caused by flexing in your Z axis if it is not as stiff as it needs to be, or some backlash in the X or Y axes.

    Mach3's Tools menu has a final step-over setting that may help clean up your problem.

    CarveOne

    CarveOne
    http://www.carveonecncwoodcraft.com


  4. #4
    Registered DonFrambach's Avatar
    Join Date
    Nov 2006
    Location
    USA
    Posts
    927
    Downloads
    0
    Uploads
    0
    Here's a snippet of g-code to cut a small circle. Since it plunges to the desired cut depth and then moves to the edge, you shouldn't get a flat spot.


    (cut circle) (radius = .125 )
    (depth =-.1 )

    G01 X0 Y0 (zero X & Y)
    G01 Z-.1 (bring cutter to cut level)
    G01 X .125 Y0 (move to start position)
    G02 X0 Y-.125 R .125 (quadrant 4)
    G02 X-.125 Y0 R .125 (quadrant 3)
    G02 X0 Y .125 R .125 (quadrant 2)
    G02 X .125 Y0 R .125 (quadrant 1)



  5. #5
    Registered
    Join Date
    Feb 2010
    Location
    USA
    Posts
    351
    Downloads
    0
    Uploads
    0
    I would simply make the first cut .005" (.010 on diameter), oversize, then do a second pass at diameter. I do this for any finish cut where I need a nice finish.



  6. #6
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Twp, MI....USA
    Posts
    24297
    Downloads
    0
    Uploads
    0
    I cut circles using helical cuts, so there is no plunging.

    Gerry

    Mach3 2010 Screenset
    http://home.comcast.net/~cncwoodworker/2010.html

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


  7. #7
    Registered
    Join Date
    Jan 2006
    Location
    USA
    Posts
    36
    Downloads
    0
    Uploads
    0
    An other option is to drill a hole that is 1/16" smaller than the cutter right where the cutter is going to plunge so that as it plunges into the material is cutting very little material.
    Gary :-)



  8. #8
    Like Gerry said, don't plunge your cutter straight in. Ramp it in to the cut at a low angle, like 5 to 10 degrees. Do this while you're going around the circle. Plunging straight in is hard on your spindle bearings.

    What cam software are you using?

    CNC mill build thread: http://www.cnczone.com/forums/vertical_mill_lathe_project_log/110305-gantry_mill.html


  9. #9
    I have a similar issue. I am using IJ code to plunge a 21/64 bit into 3/4" plywood. I am cutting a matrix of 1inch holes. Every single hole looks as if the path was followed perfectly through 3/4 of the circle then the last 1/4 of it takes on a different radius and leaves a flat spot in the circle.

    I checked all backlash and then ran a pocket cutting wizard from Mach3 which used the radius command and spiraled a perfect 1 inch hole. I tried all the usual suspects IE incr, CV, abs and nothing affected it. Tried feeds so slow i almost started a fire and still the exact same pattern.

    I tried the same file on a different machine(same style) with different bit (1/8") and faster computer. Holes were good. It got late so I havent tried fast computer on the first machine.

    1. Could the computer be choking on the interpolation and deceleration?
    2. Should I be pocketing all small holes?

    Any ideas?



  10. #10
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Twp, MI....USA
    Posts
    24297
    Downloads
    0
    Uploads
    0
    Is the problem visible in the toolpath display?

    Can you post the g-code?

    Gerry

    Mach3 2010 Screenset
    http://home.comcast.net/~cncwoodworker/2010.html

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


  11. #11
    Gerry,
    Funny you should mention toolpath. Les Newell also told me that everything in that path is exactly what gets thru the P port. I ruled out backlash but started looking into flex. My machine is very stiff, however with the z-axis it is difficult to keep it stiff and nimble at the same time. It turns out that I had a tool crash once and scorched my bit. I didnt think it was a big deal but it really dulled it. I was getting more flex from the dull bit. I put a fresh one in and also added a ramp to the approach and the circles came out perfect. Remember your father telling you never use a dull blade...nobody ever gets hurt with a sharp blade. I think he knew more than I thought ha ha.



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 from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed