Can't make arcs work on a lath

I am using 2.4.3 which I got off the CD image to run a small lathe. I am trying to cut spindles in wood that have arcs in their profile. When I program an arc using a radius format arc the tool will only go in a linear path from the start point of the arc to the end point of the arc. If I switch to center format arc the tool runs linear from the start point to the end point for about 2/3 of the travel. It then begins to curve and soon gives a joint following error. My Dolphin Cad system simulates the move correctly. A CNC lathe simulator I have shows the G Codes should run the tool correctly. Programming the moves manually produce the same error. Do I have something set up wrong?

Thanks,

John C

Can you share a little snippet of your arc code?

What plane do you have selected?

John

This is a finishing cut profile that I also can't get to work. Runs OK on a simulator. Cuts linear in AXIS


%
( Porgramme : O0000)
( PartNo : - )
( Sunday, May 15, 2011 : 15:36:29 )
( Source File - Spindle7cnc : Post - T_EMC_FrontTurret )
N5G20
N15G0G17G40G49G80G90
( Turning tool )
N35T4M06
N45G54
N55G90G00G43Z0.0H2
N65S500M03
N75G01X1.029Z-2.4894F20.0
N85S500
N95G00X0.6Z-1.75F2.0
N105G01Z-2.0
N115G03X0.5963Z-2.0149R0.0315
N125G01X0.3366Z-2.4995
N135G03X0.6Z-3.5R2.0315
N145X0.25Z-4.64R2.0315
N155G01Z-4.9546
N165G02X0.3775Z-5.1532R0.2185
N175G03X0.6Z-5.5R0.3815
N185X0.3775Z-5.8468R0.3815
N195G02X0.25Z-6.0454R0.2185
N205G01Z-6.36
N215G03X0.6Z-7.5R2.0315
N225X0.3366Z-8.5005R2.0315
N235G01X0.5963Z-8.9851
N245G03X0.6Z-9.0R0.0315
N255G01Z-9.25
N265X1.029Z-2.4894
N275M5
N285G00X1.9685
N295G00Z1.9685
N305M30
%


Thanks,

John C

Your in the XY plane and that is for mills so your arcs are being cut up and down. Lathes use the XZ plane.

www.linuxcnc.org/docview/html/gcode_main.html#sub:G17,-G18,-G19 :

www.linuxcnc.org/docview/html/gcode_main.html#sub:G2,-G3:-Arc

Also note that a lathe the Y+ is on the bottom and that determines the direction of your arc.

You don't need the line numbers they just clutter up your g code, also the % are not needed and M2 is the normal end of file.

www.linuxcnc.org/docview/html/gcode_main.html#sub:M0,-M1,-M2 ,

John

John,

G18 instead of G17 works fine now. Thanks for the help. I'll clean up the other stuff too. Don't know why my post processor set the plane wrong. I'll check that out. Wahoo! back to making sawdust!

John C