Oval/Round Toolpath Chatter


Results 1 to 12 of 12

Thread: Oval/Round Toolpath Chatter

  1. #1
    Registered
    Join Date
    Aug 2008
    Location
    usa
    Posts
    21
    Downloads
    0
    Uploads
    0

    Default Oval/Round Toolpath Chatter

    I am wondering if anyone else has had this problem before. When I am routing something oval or round my machines sounds funny and shakes alot when routing a radius. This also leaves some chatter marks on the cut. Straight cuts and diagonal cuts are fine. I am new to this and am looking for some advice on were to start. Thanks in advance.

    Similar Threads:


  2. #2
    Registered todd71's Avatar
    Join Date
    Nov 2006
    Location
    U.S.A.
    Posts
    303
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Absolute Steve View Post
    I am wondering if anyone else has had this problem before. When I am routing something oval or round my machines sounds funny and shakes alot when routing a radius. This also leaves some chatter marks on the cut. Straight cuts and diagonal cuts are fine. I am new to this and am looking for some advice on were to start. Thanks in advance.
    Are you climb milling or conventional? I would recommend NOT climb milling.
    Could be slide way screws to lose or too tight. Be sure to use a torque wrench to tighten ALL slide way screws. Could be servos out of sync. Which tech support should be able to help you with that. How long is your tool sticking out of the tool holder. Choke up tight as you can. Long tools deflect and scream when cutting. Don't know if this helps. But as you can tell there are alot of variables when it comes to tracking down problems. What material are you cutting? What are the speeds and feeds? Whats the tool diameter? Is it with all tools and all ovals? Have you checked your vectors? Do you have steppers or servos? Something may have nothing to do with the problem. Got any pictures? The machine shaking sounds real weird. Are all your screws tight?



  3. #3
    Gold Member cabnet636's Avatar
    Join Date
    Oct 2007
    Location
    usa
    Posts
    2459
    Downloads
    0
    Uploads
    0

    Default

    this can be a setting issue in wincnc.

    do you have steppers or servo's

    post your ini file

    jim

    James McGrew CAMaster 508 ATC
    www.mcgrewwoodwork.com http://dropc.am/p/EJaKyl


  4. #4
    Registered
    Join Date
    Aug 2008
    Location
    usa
    Posts
    21
    Downloads
    0
    Uploads
    0

    Default INI File

    Jim and other's

    I am using steppers. This happens when I am dry running also. I can reduce the the feed rate to about 30 and it is pretty good. Seems kind of slow to me. This machine is a Shop Sabre 7214 and it has almost no use since new 4years ago.
    Also another issue I have discovered is a problem I have been having with some programs I did with V CarvePro. WinCNC keeps choking on any G2 line in my program. The only way out of this is to delete the G2 at the beginning and then take out the I and J position at the end in the same line. If I just leave the X and Y position in this line it will run straight through without issue. Any info would be appreciated. I am fairly new to this so bare with me. Here's my INI File

    [Timer Card Settings]
    timertype=7200
    steppulse=p5d5
    g09=s10
    maxstepv=50000
    accel=s50

    [Axis Settings]
    axischar=XYZ

    [X Axis]
    axisspec=p0 s0 d0 r3999.5 a400 k1 o0
    axisvel=r300 f300 s20 m200 h300
    axislo=p3 b1 o0

    [Y Axis]
    axisspec=p0 s1 d1 r1884 a400 k2 o0
    axisvel=r300 f300 s20 m200 h300
    axislo=p3 b2 d100


    [Z Axis]
    axisspec=p0 s2 d2 r3999.5 a400 k3 o1
    axisvel=r200 f200 s5 m20 h150
    axishi=p3 b3

    [Auxins]
    auxin=c1 p2b5 o0 d40 [E-Stop]
    [auxin=c2 p2b4 o0 d40 [pin 27 - unused]
    [auxin=c3 p2b3 o0 d40 [pin 28 - unused]
    [auxin=c4 p2b2 o0 d40 [pin 29 - unused]

    [ENABLE SHUTDOWNS, MATCH ENAB=C? WITH AUXIN ABOVE]
    [enab=c1 m"E-STOP ACTIVE"

    [G28 Settings]
    g28move=x1 r.5 f200 m1
    g28move=y1 r.5 f200 m1
    g28move=z-.5 r.5 f200 m1


    [Arc Settings]
    arc_err=.02

    [Soft Limits]
    lolim=x-1 y-1
    hilim=x75 y130 z0
    lobound=z0
    softlim=t1m1

    [Aux]

    CMDAbort=m12c2

    [Table=x0y0h145w84

    [Abort Cushions]
    lim_cnt=20
    esc_step=3000
    lim_step=250



    [Data Directory and Search Wildcard]
    filetype=*.TAP;*.NC;*.H



  5. #5
    Registered
    Join Date
    May 2008
    Location
    USA
    Posts
    51
    Downloads
    0
    Uploads
    0

    Default

    you might try raising your G09 setting to S30 or S40 (I've tried up to S100 with success on my machine.. not Shopsabre, but uses wincnc). Also, you can add an F acceleration setting to the axisspec line. That way you can set a different acceleration for your feeds than your rapids. Right now you have a400 and since you have no f setting, it works on both the rapid and feed. I found on my machine, I liked to have my rapid with much faster acceleration, but my feeds more conservative, that way it slows down and speeds up smoothly. Your mileage may vary. Just make a .bak copy of your wincnc.ini and try a couple different settings. Do air cuts to see if you get rid of the chatter.

    by the way, I don't know much about your machine, but your velocities and speeds don't seem to high in general. Maybe add F175 to axisspec and change G09 to S35 and give it a shot, see if it helps at all.



  6. #6
    Gold Member cabnet636's Avatar
    Join Date
    Oct 2007
    Location
    usa
    Posts
    2459
    Downloads
    0
    Uploads
    0

    Default

    eric and i have done some work on this and for erics info there is not a lot of differnce in the setup. i am curious why is your resolution dramatically different on x and y, do you have a different drive or step setting. does you machine dimension corectly on the cut part ?

    jim

    James McGrew CAMaster 508 ATC
    www.mcgrewwoodwork.com http://dropc.am/p/EJaKyl


  7. #7
    Registered
    Join Date
    Aug 2008
    Location
    usa
    Posts
    21
    Downloads
    0
    Uploads
    0

    Default

    Guys,

    Last week I adjusted my G09 from the original 20 to 40 without seeing a change. Last night I cranked it up to 100 as suggested and it smoothed out almost completely at full speed. Only a very small amount of vibration on the "corners" of the oval. Worked great.

    Now my only other problem is the G2 issue I mentioned in an earlier post. Will WinCNC run a line with G2 at the beginning?

    Thanks for all the help for newbie.

    Steve



  8. #8
    Registered
    Join Date
    Jul 2008
    Location
    USA
    Posts
    20
    Downloads
    0
    Uploads
    0

    Default

    this maybe a silly reply, but this has happened to me. we do most of out layouts in AutoCAD and I have found if the curve I am trying to cut is a spline and not a polyline, I get the chattering and a jerky response from the router. A spline translates to a couple of thousand lines to make the curve.

    easiest way to check for this is to look at the G-Code if it is all X-Y coordinates and not I-J coordinates them more then likely it is a spline.

    Like I said it maybe a silly response but I tend to go back to the programming before messing with the WinCNC settings.



  9. #9
    Registered
    Join Date
    May 2008
    Location
    USA
    Posts
    51
    Downloads
    0
    Uploads
    0

    Default

    setguy, what are you using for your toolpath software?

    I use Rhino/Rhinocam and use splines for all curves (NURBS to be exact). When Rhinocam does toolpaths, it figure what can be done with I/J commands and what needs to be segmented, and the segmenting is controlled by what tolerance you set on the particular toolpath.



  10. #10
    Gold Member cabnet636's Avatar
    Join Date
    Oct 2007
    Location
    usa
    Posts
    2459
    Downloads
    0
    Uploads
    0

    Default

    yesterday i was doing a tool path (3d) with a lot of 2d arc's in offset pathing, i saw the chatter and stopped the file reset the g09 to s30 and the difference was amazing i have to fun this file several times so today i will check out other speeds and timing

    jim

    James McGrew CAMaster 508 ATC
    www.mcgrewwoodwork.com http://dropc.am/p/EJaKyl


  11. #11
    Registered
    Join Date
    Aug 2008
    Location
    usa
    Posts
    21
    Downloads
    0
    Uploads
    0

    Default

    Jim,
    I am assuming that you also are running WinCNC. On the G2 issue I explained in an earlier post, would you a be able to give me a sample of a G2 line that you have on a running program. I have not had alot of time to work on my router lately but hopefully this next week. This is a great forum and I really appreciate all the info I have received from you guys. I'm glad to see that your chattering was solved. I know that my is 1000% better. Thanks to all.



  12. #12
    Registered todd71's Avatar
    Join Date
    Nov 2006
    Location
    U.S.A.
    Posts
    303
    Downloads
    0
    Uploads
    0

    Default

    N10 G90
    N20 T5
    N30 G0Z0.5000
    N40 G0X0.0000Y0.0000
    N50 S11000
    N60 M3
    N70 G0X19.2525Y12.0016Z0.5000
    N80 G1Z-0.5000F75.0
    N90 G1X19.2525Y12.0016Z-0.5000F75.0
    N100 G2X19.2679Y12.4050I5.3201J-0.0012
    N110 G2X19.8274Y14.3904I5.2040J-0.3950
    N120 G2X21.4633Y16.2801I4.6879J-2.4055
    N130 G2X23.8335Y17.2055I3.0272J-4.2550
    N140 G2X24.9050Y17.2321I0.6667J-5.2720
    N150 G2X26.8904Y16.6726I-0.3950J-5.2040
    N160 G2X28.7801Y15.0367I-2.4055J-4.6879
    N170 G2X29.7055Y12.6665I-4.2550J-3.0272
    N180 G2X29.7321Y11.5950I-5.2720J-0.6667
    N190 G2X29.1726Y9.6096I-5.2040J0.3950
    N200 G2X27.5367Y7.7199I-4.6879J2.4055
    N210 G2X25.1665Y6.7945I-3.0272J4.2550
    N220 G2X24.0950Y6.7679I-0.6667J5.2720
    N230 G2X22.1096Y7.3274I0.3950J5.2040
    N240 G2X20.2199Y8.9633I2.4055J4.6879
    N250 G2X19.3588Y10.9442I4.2561J3.0278
    N260 G2X19.2525Y12.0016I5.1648J1.0532
    N270 G0Z0.5000
    N280 G0X0.0000Y0.0000
    N290 M5



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

Oval/Round Toolpath Chatter

Oval/Round Toolpath Chatter