Bore toolpath creates smaller hole

[sebastien_garvin]

Hi,

I am having issues with the Bore tool path. I am trying to machine a 20mm (0.787 in) hole in plywood but they keep coming out as 19.84 mm. I am not sure what to look at. The Circular tool path is doing the same thing. I don't know enough about G code to tell if the issue is that fusion 360 is post processing my file to 19.84 mm or if the exported file is fine and the issue is on the machine itself.  

I am using the CENTROID / centroid post processor.

Any feedback on what to look into would be very much appreciated.

Sebastien

[seth.madore]

That's because you're feeding at 280. inches per minute. In a circle, the linear feedrate is actually MUCH higher than that, due to a pesky thing called "math".

Your adjusted feedrate should be 80.35 inches per minute.

 

[seth.madore]

And honestly, even that might be pushing it. I'd be tempted to drop down to 40 or.

[seth.madore]

@sebastien_garvin have you had any success with lowering the feedrate and running the Bore cycle again?

[sebastien_garvin]

First off, thank you for your fast reply and sorry for the delay.

I had time to play with it again this week and feed rate does not affect the hole size.

I measured my router bit and it does seem to be a little smaller then 0.5". That surprised me as I heard good things from Whiteside bits (UD5202). But even with the exact diameter, my holes are still about 0.005 too small. I would be tempted to say 0.005 is good enough for my machine, but what annoys me is that they are consistently and precisely 0.005 too small every time. 

[seth.madore]

It's quite likely a combination of the tool and the machine.

What post processor are you using? It's not "too" difficult to look at the code, run some numbers and determine if the radii being cut is correct.

[sebastien_garvin]

CENTROID / centroid post processor from the library.

I will see if I can decode it.  Thanks

[HughesTooling]

NC Corrector is quite good for back plotting your code. 

[leo.castellon]

If your holes are consistently the same amount undersized, then you are in luck, this is much easier to fix. A couple of things to check.

Measure your cutter with a micrometer to see what the actual cutter diameter is. If it is undersized, adjust the cutter diameter in your program to match the actual measured diameter of the tool. Cut a test hole and measure.

If it is still undersized, perhaps there is some backlash in your machine. You can check this by getting a test indicator and interpolate the machined hole, the test indicator should measure consistently around the hole diameter as you spin it in the hole, if the needle jumps around one sector, then your hole isn't round and that is why it is undersized. if this happens, you will need to adjust your machine for backlash error. 

If these tests are all OK, then perhaps add a finishing pass using cutter comp, or adjust your parameters under the tab of "stock to leave". 

LeoC