Corners are radiusing

I'm running 2.7.14, having a strange issue with this program.
(pocket)
G56
G0 G90 X-4.187 Y-0.173
M3 S200
M0
(SET Z DEPTH)
G1 F14.5 Y-1.547
X-2.313 Y-1.547
X-2.313 Y-0.173
X-4.187 Y-0.173
X-4.087 Y-0.273
X-2.413
Y-1.447
X-4.087
Y-0.273
X-3.987 Y-0.373
X-2.513
Y-1.347
X-3.987
Y-0.373
X-3.887 Y-0.473
X-2.613
Y-1.247
X-3.887
Y-0.473
X-3.787 Y-0.573
X-2.713 Y-0.573
X-2.713 Y-1.147
X-3.787 Y-1.147
X-3.787 Y-0.573
X-3.687 Y-0.673
X-2.813
Y-1.047
X-3.687
Y-0.637
X-3.587 Y-0.773
X-2.913
Y-0.947
X-3.587
Y-0.773
Y-0.868
X-2.91
M30

If I press T after the M0 the program will advance to each intersection, and stop waiting for the next T. If I press S, the program runs but puts radiuses in all of my corners.

I tried adding both coordinates on the lines to see if that made a difference, did not. When I run this in a virtual box on 2.6, it makes the sharp corners.

linuxcnc.org/docs/2.7/html/gcode/g-code.html#gcode:g64

I'll wager this is the base of the problem

Chris

Add this magic line of G-code somewhere near the start of your files.
By Default Linuxcnc is set to G64 with no blending tolerance. Which is constant surface velocity with blending, resulting in any corners in your code to be rounded so that the machine does not have to slow down. It will only slow if the machine can not at least touch part of each commanded line segment. Adding a Pn tolerace to the G64 command will restrict the blending so deviation from the programmed path does not exceed n.
linuxcnc.org/docs/2.6/html/gcode/gcode.html#sec:G64

Yes that worked. I don't use this machine much except to drill hole patterns, and those always have a hard stop. Don't remember anything like it in 2.6, assuming it's new in 2.7?

It has always been there, but before 2.7 added multi line look ahead it often was not as noticeable. In 2.6 and before the one line look ahead limited speeds to what the machine's acceleration would allow a controlled stop by the end of the next line. So unless line segments were relatively long the machine could not go fast enough to require large blends of the corners.

I'll play around with this later. I do some multi-part engraving using G52 temporary offset and call up sub programs. Speed is slow, 8 -10 inches per minute and the characters are only .125 high so there isn't much movement. I never noticed a radius, probably because it's so small but I think it's there none the less. I'll probably just add the G64 to both the main and subs but was wondering if it's necessary in the subs.

G64 and G61 are modal commands and will remain in effect until they are replaced by another G64 command with a different or no P value. G64 with no P is set when Linuxcnc is first started by default. You can change that behavior in your ini file.
linuxcnc.org/docs/2.6/html/config/ini_co...sub:RS274NGC-section

It is wise to have it in the preamble of all your g-code files, sub programs may or may not need it. It depends what they are, and how and when they may be used.