Lying about bit size to affect part size

[John David]

You should set the bit to the actual size and re run the test. It looks to me like you will be with in machine tolerance.
JD

[daski]

There are many things that will affect the final size of a part, even the sharpness of the bit will have an effect, new bit cuts, dull bits poiund. We found that we would do an accurate drawing, then do a test part using two pass system, first being almost all the way through, the second cutting the oinioskin. The 1/4" bit will deflect when cutting, plus the slop in the gantry, z axis, bearings in the router, resistance from the panel density, they all add up to a number that will remain fairly constant given the same situation in the future. We found that a 1/4" bit needed to be enetered as .243, climb the conventional cutting.

You are better figuring out what the cumulative number is and allow for it in the bit as opposed to a percentage,

[bobmoore]

You havn't said what material you are cutting or whose bit you are running. O flute bits should not be miced. You are much better off to lower them into the material you are running, raise it up and mic the hole diameter. Some plastics can compress when being run and then relax after the bit passes. There are reasons for tolerances in manufacturing and sometimes the customer needs to be reminded of them. Maybe have a company with a big gun CNC run some samples for you and see what there quality level is with the same material, no sanding, ect.
Bob

[sbd1]

Bob: I like your idea of drilling a hole with the bit & then measuring that, rather than trying to measure the bit. I did mention I am using a 2-flute bit in 3/4" MDF. Interesting info about plastics, but I'm not there yet. The drill hole size measured .247.

John: I reset the bit size to .247 & recalculated the toolpath & then recut the test block (see image of 2" test square). X is out by only .001 and Y is out by .008, which probably tells me that I need to address some play in my Y travel/hold system, but at this point in time I'm pretty happy with these.

Dave: I'm using a new 1/4" upcut spiral bit with two-climb cut passes. The results seem acceptable to me, but once I get more comfortable with everything I'll give the opposite direction cuts that you mentioned a try.

Thanks everyone for your advice & information. From this I've learned that I need to be more accurate with my bit size & that I can make changes to a parts' final size in 3 different ways:
1) By changing the proportions of the part file in the fill-in sheet.
2) By recalculating the toolpath with an offset or allowance.
3) Changing my bit size & recalculating the toolpath.