Machine is rounding of square internal corners

Hi, im struggeling with a strange issue here.
My machine is rounding of internal corners that should be square with a tool diameter as corner radius only.

I initialy thought the machine was struggeling to get my velocity of 3000mm/min in the corners causing this issue but even when lowering the feed override to 50% 1500mm/min the corners are stil not square?

What is causing this issue? Please see attached pictures.

Sorry to take your time guys, this post fixed my issues.
Apparently it was a Fusion 360 problem and not a linux CNC

forums.autodesk.com/t5/fusion-360-manufa...-fillet/td-p/7689373

How do i determine my acceleration values?

I have now 100 velocity and 750 acceleration for x and y axis?
The acceleration is as it was when the machine was configured but i change my speed.

To figure it out experimentally, for a stepper machine increase the acceleration until the motor stalls, then reduce by a safety margin. I'd say at least 30% but depending on the machine 60% might be more appropriate. The test will need to be done at or near the max velocity, because that is where a stepper is weakest.

On a servo with feed back, it is simpler, set the f-error high for testing and the acceleration to something way too high. Do a test move watching the velocity feedback in halscope. The slope of that will be the max possible acceleration. Set the max acceleration to something less, perhaps 10%-20% less.

It might be wise to load up the moving joint with the max theoretical load for testing. (put something heavy on the table, load up your biggest tools...) and make sure the machine is bolted down good, this could be quite violent if the machine is powerful. (read this as it may not be safe.) Fortunately on a servo the speed doesn't need to be high or the move large to find the limit. so make the moves small and not particularly fast, just enough to see linear acceleration.

More importantly learn how to use G64 Pn in you g-code to get the path following tolerance you need.

A G61 would make linuxcnc follow the exact g code that fusion is spitting out but you will slow in the corners to change directions. You can play with a mixture of G61 and G64 P .xxx values to see what you prefer.

linuxcnc.org/docs/2.8/html/gcode/g-code.html#gcode:g61

what about using constant velocity g64 for roughing cuts and a finishing cut using G61 exact stop mode.

(as posted above)

careful of chip thinning / rubbing as it will blunt you tool / shorten it's cutting life.