Rounding corners

I'm using a laser cutter and having an issue where it is rounding some of the corners, but not others. Has this happened to anyone else?

You have acceleration set to low or you need to add G64 P0.x Q0.x at the top of the gcode file, where x is the amount of tolerance that the path should be followed, i.e. G64 P0.1 Q0.1 would get you within 0.1mm of the exact path.

Thank you TommyLight. This did the trick. After researching your post, I ended up using G61, which made it go to the exact point programmed.

Just remember with G61 set the machine will be coming to a stop in all corners (no mater how small). You might be very surprised how much faster the machine might mill with G64P0.01 (or some other small number) and still give you acceptably precise corners. This can be especially true with cam generated g-code.

I think G61 should be the default in linuxcnc. It seems to come up so many times by users not familiar with the motion planner.
I almost crapped my pants with the default settings on my gang lathe. The rapids between tool changes had large radii that didn't jive with the clearance z retract. Blending right into a collision with the stock during the move to the next tool.
Same with milling, if you are used to a small z retract above the part say in spot drilling, if your settings are coarse, the z will clip the hole on the way up as the table is already moving.

Maybe, but it is also the norm for many commercial Fanuc controled machines.

People used to working with cnc machines know and understand the importance of having proper preamble codes at the beginning of your g-code files. it isn't safe to assume machine defaults are correct for your program.