Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
Showing results for 
Show  only  | Search instead for 
Did you mean: 

round holes are coming out to small

Message 1 of 15
432 Views, 14 Replies

round holes are coming out to small

I have an odd problem. When I run my cnc to cut out a round hole they are coming out to small. For instance my part has a 5/8" round hole. But after machining the hole it is to small, slightly larger than 9/16". The holes always seem to be about 1/16" to small.


The weird thing is all other shaped pockets are the correct size. If I do a square pocket it is the correct size, as well as every other area and dimension being the correct size, any idea what is going on?


here is the code fusion generates for one of the holes it should be 5/8":

G0 X1.5544 Y1.064
G43 Z1.35 H1
G0 Z0.95

G1 Z0.8746 F50.
X1.5552 Y1.0653 Z0.8661
X1.5573 Y1.0691 Z0.8586
X1.5603 Y1.075 Z0.853
X1.5634 Y1.0825 Z0.85
G3 X1.3416 Y1.1675 Z0.7842 I-0.1109 J0.0425
X1.5634 Y1.0825 Z0.7184 I0.1109 J-0.0425
X1.3416 Y1.1675 Z0.6527 I-0.1109 J0.0425
X1.3338 Y1.125 Z0.645 I0.1109 J-0.0425
X1.5175 I0.0919 J0.
X1.4825 I-0.0175 J0.
X1.6675 I0.0925 J0.
X1.3325 I-0.1675 J0.
X1.6675 I0.1675 J0.
G1 X1.6672 Y1.1288 Z0.6456
X1.6663 Y1.1326 Z0.6462
X1.665 Y1.1358 Z0.648
X1.6633 Y1.1389 Z0.6498
X1.6616 Y1.1411 Z0.6525
X1.6598 Y1.1431 Z0.6553
X1.657 Y1.1454 Z0.6623
X1.656 Y1.146 Z0.67

Message 2 of 15
in reply to: tjtalma

50 inches a minute? What size is your tool, and what is the material?

Seth Madore
Customer Advocacy Manager - Manufacturing
Message 3 of 15
in reply to: tjtalma

You can't reliably move  a .110" arc at 50 ipm with a 1/2" endmill. Your machine can't keep up with it. 

Try the exact same code at F10. and measure that. 

Please click "Accept Solution" if what I wrote solved your issue!
Message 4 of 15

Exactly this.

@tjtalma give this a read to understand why. Essentially, circular milling with a feedrate of 50ipm is equivalent to machining a straight line at 125 ipm

Seth Madore
Customer Advocacy Manager - Manufacturing
Message 5 of 15
in reply to: seth.madore

Sorry should have included that. This is a wood working router, I'm using a 1/4" spiral bit, at 12,000rpm, cutting walnut depth of cut in this instance is 1/8"

Message 6 of 15
in reply to: programming2C78B

I will try cutting at 10 ipm tonight. 


But it's interesting, I am cutting the rest of the part at 150 ipm for a finishing cut, and roughing at 250ipm. There are arcs in the part that are 1" diameter and these are coming out fine. 


Is it the small size that is the problem?

Message 7 of 15
in reply to: seth.madore

Thanks that makes a lot of sense

Message 8 of 15
in reply to: tjtalma

Haas has a good video explaining about feed rates and circular milling:



Message 9 of 15
in reply to: programming2C78B

I had a chance to play with this today. I tried feedrates at 10, 5 and 1 ipm and all generate the exacte same size hole that is to small. I also tried is at 200, 150, and 100 ipm. The 200 hole was a little oval, but the 150 and 100 hole was the same size at when the feedrate was 10 or less.


I then used CamBam to generate the file, and it came out perfect (cutting at 50 ipm). Holding 2 parts together, one cut using the fusion 360's cam and one using CamBam (With all the same settings), the only difference is the size of the circular pocket. 


All I can figure is that this is a setting in Fusion that I have configured incorrectly. Any ideas on what I should be looking at?

Message 10 of 15
in reply to: tjtalma

Min cutting Radius on the Passes tab is pretty much all I can think of. Could you share your Fusion file here?

Seth Madore
Customer Advocacy Manager - Manufacturing
Message 11 of 15
in reply to: tjtalma

It would be nice to see the actual Fusion file for a better idea on figuring out what is going on.



Message 12 of 15
in reply to: tjtalma

Interested to see the answer for this.    I seem to also have this issue. But with 1/8 tool

Message 13 of 15
in reply to: tjtalma


I calculated your NC code with a 1/4 diameter cutter and it will produce a .585 diameter hole. Pretty much exactly what your experiencing. I'd check to make sure your not set to leave stock like a roughing operation would and I'd also check the model for it's actual size. Beyond that we would need to see the project if possible.

Bill Cain
Sr. Technical Consultant
Message 14 of 15
in reply to: tjtalma

I'm not seeing cutter compensation (g41/g42) Is your tool sharpened or undersized at all? 

Message 15 of 15
in reply to: tjtalma

I eventually discovered why my holes were 1.5 mm undersized. The comment about the "Stock to leave" was the problem. Ensure that this 'option' is NOT checked. If you leave it checked, it will make the holes 0.5 undersized (internal holes) or 0.5 mm oversized (outside).  There are probably other factors that wasted 5 hours of my time.... 


Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report