Curving between corners

I'm having an issue where corners are being rounded when there is no compensation or curves set in the GCode file, in fact the file specifically contains a G40 and G49 at the beginning to cancel any compensatory moves.
I've used the same GCode files before on my old install so I'm assuming it's either a wrongly configured setting or something new in LinuxCNC since my old install (2.6.4). This is the first time I've used these files since my upgrade (I changed my controller to a GeckoDrive from a cheap Chinese one at the same time as upgrading) and the only thing that I think is different is the max speed and velocity (The only one had to be quite low to avoid skipping steps).
I did notice the same issue occurring on vertical moves in other files where it would start lifting just before it got to the end but I had assumed that was to do with the higher speeds it was running at which is evidently not the case now I have encountered this file.

This sounds like it is due to the new trajectory planner. If your machine has relatively low acceleration and high speed then the changes will become more obvious.

linuxcnc.org/docs/2.7/html/user/user-con...#_trajectory_control

Should explain the changes you can make. You can have the old behaviour back, or configure somewhere in between to get some of the speed improvement that the new TP provides.

Ahh that's definitely what's going on. I turned up the feed speed on the file and it cut the corner off even more. My max speed is 4x what it used to be now I don't get skipped steps but I had to keep the accel down to avoid wobble in the gantry in hard stops/starts. I didn't realise it had any effect on paths so I was happy with the accel that I had left it at until now...
I think I might set it back to the old method as I'd rather expected results over slightly faster cuts.
Thanks for the help, I didn't even realise it was a thing!

How do I disable that so it instead follows the path exactly?
I've tried setting ARC_BLEND_ENABLE = 0 and COORDINATES = {blank} in the INI file under [TRAJ] but it is still doing some kind of trajectory plan.

The best solution is to set G64 P0.001 (or what ever P tolerance is appropriate for your machine and application) in the preamble of each g-code file. Or you can set the machine to G61 (exact path) mode, but then the machine will halt a every corner in the g-code.

The default G64/G61 setting in Linuxcnc is G64 with no P tolerance, which equals constant velocity (or as near as possible) with maximum blending.

This has always been the case, but with the new trajectory planner, higher feed rates are possible with some g-code due to the farther read ahead (more than 1 line) when planning accelerations. The result is greater corner rounding than with the old system when no blending tolerance is specified.

Thanks for clarifying that. I think it's a combination effect of both the new planner and the higher speeds I am now running at that caused it to be so off. Those files all specified G64 with no tolerance specified hence the significant deviation. I guess that's something I'm going to have to be mindful about in the future and revisiting the machine's acceleration settings is going to be worthwhile too.