Fusion 360 parts oversized

[Zombie (Rob M)]

I’ve been trying to learn fusion for awhile and every time I think I’ve got it, something goes wrong. Lately I’ve been having trouble with the finished part size. The outer profiles are too large and the pockets are too small. But the places I spot dill are within a few thou.

All parts had a roughing and a finishing pass. Part B actually had two finishing passes.
B&E were over sized by 0.015-0.017"

D2 was over sized by 0.028-0.0305" and the pockets were under sized by 0.020". The shelf was 0.003" too deep (not worried about that)

The Bit used is a 0.25" 3F endmill.
Running at 18000rmp
108IPM with air.
Max roughing stepdown was 0.110"
Full depth finishing pass 0.020"

Machine is an S3 with linear rails, ballscrews, an HDZ and a 2.2kw spindle.

Part B

Fusion

Part D2

Fusion

Part E

Fusion

Finish wall pass

EDIT: ADDED VIDEOS that work
https://www.dropbox.com/t/aDuh5tefmEQquqTH

Things I’ve checked.

I put a 123 block (Measured 3.0000") in a vise and found the -x edge with an edge finder, moved over half the diameter, zeroed, found the other side, subtracted half of the diameter. Rotated 90deg and repeated for y.
X was 2.9995" and Y was 2.9990". The machine is accurate enough for me.

Measure diagonally across the oversized finished parts and they were 0.001" off from each other. So it’s cutting square.

I thought maybe my bit was undersized, but when I measured it was 0.2500".

Bit was 1/4" with 3/4" flute length. Stick out was around 1.25"+/-0.0625" , so I would assume there is not much bit deflection.

I put the gcode into NC viewer and the found the finishing pass, found the +x, added the -x and subtracted the bit diameter and the numbers was spot on. I did the same for y and perfect.

Now I’m at a loss and need help. Any thoughts or ideas would be greatly appreciated.

[mhotchin (Michael Hotchin)]

OK, I’m just throwing out an idea to see if it sticks - could the tool definition in F 360 be incorrect?

What you are seeing is consistent with a tool definition slightly larger than the actual tool. Since the tool is correct, could the tool definition be oversized?

[Zombie (Rob M)]

Here is a screen shot of the tool I used.

I had another part I made last week with a 0.25" 0 flute and it also was 0.015" too large in both X and Y.

[wilmatos1989 (Wilson Matos)]

Did you measure the bit with calipers? This sounds like the cause. Your bit could be 6mm not .25in

[Zombie (Rob M)]

I did use calipers. Put light pressure on the jaws and spun the bit in my hand.

Bad pic. I didn’t have the bit that far into the calipers. Only measured the flutes.

[Tod1d (Tod (with 1 'd'))]

Your machine is dialed in & calibrated. The toolpath is correct. The tool is the right size.
I think that only leaves deflection / slop.
With the machine on, and the spindle stopped, can you move the tool side to side, front to back?
Are you climb cutting? If so, can you try to re-run the same finish path with conventional cut?
Climb cutting pushes the tool away from the material, whereas conventional will pull the tool into the material.
0.020" seems like a healthy amount of finish stock for wood. With aluminum I typically leave no more the 0.005". If I’m dialing in a high tolerance dimension I’ll leave maybe 0.002" and take additional passes shaving 0.0005" at a time until I measure within tolerance.

[Zombie (Rob M)]

I am climb cutting. I’ll try a smaller stock to leave and add a convention finish next time I head out to the shop. Thanks.

[Zombie (Rob M)]

Tod with one d, that was it. Snuck back out to the shop and cut a piece with a 0.005”conventional finish pass. Couldn’t be happier with it. Thank you