How to accurately measure endmill diameter?

[PhoenixMetal]

Since I have recently gotten into making high precision parts, I have come to realize that most endmills are actually undersize. That is, a 1/2" (nominal) endmill might actually be 0.498" or so. Not adjusting for the actual undersize diameter of the cutting tools resulted in cavities that are too small, and bosses (protrusion type features) that are too big.

Now I always measure the diameter of each tool (at least ones used in finishing operations) prior to use and enter the actual diameter into my part programs. My part accuracy has improved, but I am not getting results as good as I need and I think it has to do with the poor accuracy of my tool measurements.

I have been measuring the endmill diameters using general-purpose digital calipers, however this is very clumsy and perhaps not accurate enough for my needs. I have seen special micrometers with a V base for measuring the diameters of 3 flute endmills (which cannot otherwise be measured directly across), but I have not found any measuring tools specific to measuring the diameters of regular 2 and 4 flute endmills.

Does anybody know of the best tool/method for making this measurement with high accuracy? I'm looking for accuracy and repeatability of around 0.0005"

Thanks in advance.

[holbieone]

the best way would be to use an optical comparator

a good end mill should only be minus .0005 from from the specified size

when i make a part I'll measure the part a few passes before the finish pass and make adjustments from there.

some times I'll make test cuts in a scrap piece of stock and use that to make offsets or change the tool dims in the cam , works well when adjusting for a ball end mill

sometimes i get spoiled and use our machine with the laser setter :lol:

[dertsap]

measure the shank with a mic , put the tool in a tool holder , put it in the machine check it for runout , then touch a tenth set indicator on the shank then check the difference at the tip of the tool ,
if you trying to get high precision then you should always be checking your tools for runout and depending upon the brand check the flutes for taper ,
its never a good idea to use a mic to measure the flutes , generally mics are carbide tipped and will chip the tool

[Switcher]

Like holbieone said, the best way is to use a optical comparator, with a v-block. This might not be an option for the home shop.

I did tool grinding for 9 years (that's a lot of carbide, lol), you can still get good results with digital calipers, just make sure you are measuring on the outer endmill land (actual cutting edge), & not the clearance, most endmills will have 2 clearance cuts on the OD, & a very small lip that is actually doing the cutting.

All tooling is not equal, when we made endmills, we would rough grind the same diam. as the shank, then do a finish pass with another diamond wheel, which created a small step at the end (shank side of the flute), to bring the endmills OD into spec.

[PhoenixMetal]

Thanks so much for your replies! It sounds like I need to get an optical comparitor for the best results.

The indicator difference-between-shank-and-tip method sounds smart too, and that's something I can do right now so I'll give that a try today.

Thanks guys!

[leptihor]

Precision of cuts also depend of material you cut. More elastic material make inside dimensions smaler and outside biger. Should be able to find Modul of elasticity of material from specications of any particular material.

[HuFlungDung]

I think trial cuts are probably the most accurate method, because that takes into consideration the real diameter, the runout and the cutter deflection.

Take your finest tool, cut a hole or a boss with it. Measure it. Rerun the program on the same part. IF the tool takes some more off, then it really was not of much benefit to know the actual tool diameter because cutter deflection (combined with high feedrates) was skewing the results anyway. So in actual running, you need to consider the dynamic results of the cut under actual cutting conditions.

In production, you need to know the dynamic result of cutting and adjust the tool accordingly. This means you will most likely spoil the part if you take a spring pass (zero deflection) by rerunning the tool on the same path twice. This is due to the fact that you need to program a small amount of overcut to hit size during actual running conditions. Obviously, it would waste too much time to be taking zero deflection cuts all the time, so this is why an intelligent overcut is required.

When you switch tools, again, knowing the exact diameter of the new versus the old tool is not likely the only factor to consider in resetting the offset. The deflection of the new tool will be different than where the offset adjustments had set the old tool during its useful life.