Machsupport Forum
Mach Discussion => Mach4 General Discussion => Topic started by: RecceDG on August 07, 2021, 04:15:31 PM
-
See attachment.
WTF?
-
I don't see any error on the history line, so Mach thought it was running an arc.
At first I thought you might have forgotten to set the XZ plane, but status line shows G18.
Did you try running this in air and watch the motion. Could it be a display artifact, but actually cut correctly?
-
It cut exactly as displayed.
-
This is the code for the toolpath:
%
O0000
(PROGRAM NAME - LATHE_LEAD_SCREW_V3.0_OP3)
(DATE=DD-MM-YY - 05-08-21 TIME=HH:MM - 22:01)
(MCAM FILE - M:\DOCUMENTS\DENNIS\SOLIDWORKS PROJECTS\LATHE_LEAD_SCREW_V3.0.SLDPRT)
(NC FILE - D:\DOCUMENTS\MY MASTERCAM 2022\MASTERCAM FOR SOLIDWORKS\LATHE\NC\LATHE_LEAD_SCREW_V3.0_OP3.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
G0 G54 G17 G40 G80
(TOOL - 3 OFFSET - 3)
(TOOL 3 INSERT - DCMT32.51)
G0 X1. Z-5.
T0303 M6
G97 S2500 M03
G0 X.4815 Z-5.0751
G99 G1 X.4621 Z-5.0926 F.006
X.3031 Z-5.236
Z-5.4472
G3 X.5081 Z-5.5497 R.1025
G1 X.5281 Z-5.5324
G0 X1. Z-5.
M05
M30
%
@Cbyrdtopper you are a lathe guy; can you pull this up and see if the last cut segment is an arc or not?
-
Actually I think I just caught it.... I have G17 in the safe start block, when it should be G18.....
It looks like I copied the safe start line from somewhere in the lathe manual that was either talking about lathes with a Y axis or was itself copied/pasted from the mill manual and not caught.
Whoops. I'll test this later and fix the Mastercam post tonight.
Isn't testing fun?
-
That fixed it - and revealed that my postprocessor needs to swap G3 and G2.