Oval/Round Toolpath Chatter

[Absolute Steve]

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:

• Need Help!- Ford Oval DXF
• Need Help!- inner diameter oval
• How would you do an oval?
• Mori Seiki VMC, MV-50W 6M control. Tool magazine keeps going round and round.
• oval thread

[todd71]

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?

[cabnet636]

this can be a setting issue in wincnc.

do you have steppers or servo's

post your ini file

jim

[Absolute Steve]

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

[postalgbv]

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.

[cabnet636]

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

[Absolute Steve]

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

[setguy]

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.

[postalgbv]

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.

[cabnet636]

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

[Absolute Steve]

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.

[todd71]

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