Milled size is wrong

hi i want to mill a rectangle 40x200mm.i use a 2mm bit. i told easel to cut outside shape path.
on the screen the size seems to be correct.
after milling my cut piece is 36x196mm . the hole is the board is 40x200mm.
so easel milled inside.

where is my error ?

i use a cnc3018 machine

thanks for reply


To achieve precise carves you’d need to precisely calibrate the axis steps/mm ($100 and 101)

1 Like

Also, …

Measure the actual width of your bit with a pair of calipers and input that value into Easel as the bit diameter. It is extremely unlikely that your 1/8" bit is actually 1/8" exactly. Normally there is a tolerance for dimensions with each manufacturer. Instead of the bit being 0.125" in width, it might be 0.93" in width. I know I have a 0.25" bit that is 0.245" width and a 0.125" Amana bit that is actually 0.096" in width.

Another option is to just test cut a square pattern with the bit you want to use and measure the kerf of the cut. This will help account for run out and deflection but obviously will not account for it all…


Brandon Parker

hi seth, brandon

i did the calibration. before 50mm was 49.79 now it is 50.07 for the x axis so i can life with that.
the 3 original values where 1600. now 1609.1 1610.63 1610.468 (x-y-z)
i checked the bit it was sold for 2mm but for me it is rather 2.3.
all these “small” diffrences don’t explain why my rectangle is 40x200 and not 40+4x200+4
(4=2x the thickness from the bit)

i will do a test rectangle one inside and one outside shape path
once done i will reply

anyway thanks for your answer

regards from a rainy belgium

1 Like


i tested again after calibration. i carved 4 rectangles (20x80mm) with a 1.9mm drill.
clear out shape gives 19.05x79.3 should be 20x80mm
outside shape gives 18.35x78.85mm should be 20x80
on shape gives 16.85x77.23 should be 20-diameter drill=18.1 x 80-1.9=78.1
inside shape gives 14.55x74.84 should be 20-2x 1.9=16.2 x 80-2x1.9=76.2

so the carving is still wrong.
is it the tolerance on my machine ?

can you do a check on your machine ? carve a rectangle 20x80 and mesure ?


I have a few machines and can repeat the carve for you, including a 3018.

What depth per pass, feed and plunge are you using… or you can simply share your project and I can see all of your settings:

When you are measuring those parts, what was measured? Obviously the pocket was Outer dimensions, and “inside the line” should be outside dimensions, “outside the line” should be inside dimensions, and “on the line” could be either way but shoyld be noted which one so that half of the bit diameter added or subtracted to determine whether the size is off or not.

Something else to keep in mind is the runout on the 3018 spindle, the antibacklash devices, and the TRAM. These 3 factors will effect the carve result even IF the $100 and $101 values are spot on.

here is the link

i checked the dimentions from a pcb that i milled. they are right.


1 Like

I’ll run it in a bit, but for the 3018 in pine, the feed is pretty spot on, the plunge is a little high, I typically use 100mm/min. And the DPP id use is 0.5mm.

In a couple hours I’ll run it to show my results… with both settings.

hi i did another test
rectangle on position 0mm. inside path
rectangle is 20x 80mm bit is 2mm
so when i start carving moter should go to position x=78
why 80- thickness bit

in the generated g code moter goes to position 79 so 1mm wrong
on the other side moter should go to x=y=2 but goes to 1/1
G1 X1.000 Y1.000 F762.0

g code :
M3 S12000
G1 Z3.810 F228.6
G0 X79.000 Y19.000
G1 Z-0.500 F228.6
G1 X1.000 Y19.000 F762.0
G1 X1.000 Y1.000 F762.0
G1 X79.000 Y1.000 F762.0
G1 X79.000 Y19.000 F762.0
G1 Z-1.000 F228.6

or am i thinking wrong ?


i checked again. rectangle 20x80mm on position 0
i followed the simumulation path.
inside seems to be ok. outside shape x is 1mm wrong
can there be something be wrong when i setup my machine in easel ?


inside outside
G21 G21
M3 S12000 M3 S12000
G90 G90
G1 Z3.810 F228.6 G1 Z3.810 F228.6
G0 X79.000 Y19.000 correct G0 X80.039 Y-0.999 x should be 81
G1 Z-0.400 F228.6 G1 Z-0.400 F228.6

btw does inventables follows this topics ?

I have not looked at the other claims but considering that the quoted statement is not correct, I think that it is most likely that you are not understanding how the GCode is supposed to be generated for each cut.

Also, the bit coming back to (1, 1) on return to near the Work Home position is located is also correct. The zero-point is the center of the bit, and since the bit has a radius of 1 mm (diameter of 2 mm) going back to (1, 1) will get the bit as close to the inside (0, 0) corner as it possibly can without going outside of the constrained “Cut inside shape path” that was specified.


No offense…

Also, since the GCode appears to generate correctly, I think the issue is most likely in the calibration of the machine as stated previously. Since the machine is not an Inventables’ machine and GCode looks OK, I would not expect Inventables to assist with 3rd party machine setup/troubleshooting.

I am sure that if you follow what @SethCNC is pointing you to, you will eventually get it working as expected.


Brandon Parker

hi brandon

thanks for info and nice drawings . calibration is done like @sethcnc suggested ( gain was 0.3mm on a 50mm movement)
i was not aware that (0,0) = center bit
easel inside g code = G0 X79.000 Y19.000 = go to right upper corner = correct to make a cutout 20x80
easel outside g code = G0 X80.039 Y-0.999 = go to right down corner = not correct to make a plate 20x80

if i follow your drawings y-0.999 is right because i need to go down 1/2 diameter bit
x=0 + 80mm +1/2 diameter bit correct for you ?

in the excell sheet you see the easel code for inside and outside shape
why is the x-axis moving in different steps for outside shape ?

i’ll try to carve the 3 codes this weekend and check the dimentions.

g code vergelijken.xlsx (10.8 KB)

after calibrating i milled again (mdf in the soft, plywood used)

inside shape gives a hole 79.4x19.4
outside shape gives a plate 79,1x19,1

i also used a gcode for pcb material (=feedrate reduced from 1016 to 254 mm/min)
gives 79,4x19,4

with these tolerances i can start milling my box that i wanted to make with “the boxmaker” app

what i have learned:
calibrate your machine
slower the feedrate and lower the dept per pass

thanks to everyone


1 Like

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.