Tool Diameter

This is probably a simple question but ashamedly this is something I have never actually known for sure.

Should the diameter of the tool (either shank or cutting flutes) be the specified diameter of the bit or undersized? For example if I have a 10mm end mill, should it be exactly 10mm in diameter anywhere in the cutter, or slightly undersized?

I have been measuring a bit of my tooling and some tools are the exact correct diameter specified while others are not. Some of my more expensive tools are undersized whereas some of my few dollar Chinese tools are the exact dimension stated, which really has me wondering.

I'm being fairly general, whether it be end mills, drills, taps, reamers, etc.

Many end mills are somewhat under, drill bits tend to be closer to nominal dia. It can be cumbersome to measure a three- or five-flute tool with a caliper. With CNC machining to be on safe ground I store the nominal value or something bigger. Then from the measures on the work I crawl up to desired dia. Tool flexing, work bending, more factors weigh in.

PartScrapper9000 said:

This is probably a simple question but ashamedly this is something I have never actually known for sure.

Should the diameter of the tool (either shank or cutting flutes) be the specified diameter of the bit or undersized? For example if I have a 10mm end mill, should it be exactly 10mm in diameter anywhere in the cutter, or slightly undersized?

I have been measuring a bit of my tooling and some tools are the exact correct diameter specified while others are not. Some of my more expensive tools are undersized whereas some of my few dollar Chinese tools are the exact dimension stated, which really has me wondering.

I'm being fairly general, whether it be end mills, drills, taps, reamers, etc.

Click to expand...

.
obviously depends on how sharpened. if in a tool holder with runout sharpened on size and you put in a tool holder with different runout it will cut different cause tool holder runout different. say 10.000 mm end mill but micrometer measure it it measures 9.990 and it cuts likes its 10.010 and it cuts tapered sometimes end cuts bigger and sometimes cuts smaller. sometimes end mill sharpened slightly bigger on end to counter tool deflection. other times they dont do anything special.
.
actually worse if it measures 9.900 mm on end but near shank its 10.000 so its easy to over cut cause test cut done with end says cut more than you need too.
.
just saying sharpening job can be all over the place. tool can have runout cause it was sharpened with the runout

The only time I wouldn't define a 10MM end mill as ON size if it had been resharpened.
99.9% of the time when you get an end mill from the manufacturer it's a tiny bit undersized. Usually .0002"-.0004" or so on most of the major brands.

Along with other comments, I'll add that carbide end mills tend to measure a little smaller than nominal and HSS tend to be closer to nominal.

Four flute slightly undersize as manufactured. Two flute exactly to size.

Interesting. So what about tools like reamers and form taps? Would they be the exact diameter as they are intended to bring a part down to final dimension?

Reamers will be the size they are marked. Form taps are oversize by the H value of the tap.

Well, reamers are bit tricky, as they should have a slight amount of backtaper. Depends on maker and style of reamer, but this amounts to maybe 0.00025-0.003" per inch of length. (There's more than an order of magnitude there: 2-1/2 tenths vs 30 thousandths.) So if you put a micrometer on the end of a reamer and get one measurement, fully expect to get a slightly smaller measurement an inch or two up the flutes.

When new, a typical machine reamer should be exactly on-size at the cutting end. Only in very special cases would a new reamer be created undersize in order to create a larger hole due to cutting conditions. When resharpened, either flutes or end or both, a machine reamer will become slightly smaller.

Catalog cutters should be made to size and up to 2 tenths or .005mm under IMHO. I have made many new cutters and they are most often made to a print spec.
Cutters are hard to measure with micrometers because the flutes need to be exactly spaced. Agree now CNC made cutters should be evenly spaced. We used to order reamers with a nub left between the flutes so to get an accurate micrometer measure.. Yes we had to grind away the nub to use them.

Reamers can be bought oversize/ undersize and any place between.. Reamers are needed to be press fit , slip fit , running fit ,dowel fit so very often a shop will hold a resharpened reamer for as sfriedberg mentioned they get smaller diameter as the have stock sharpened off the end in the way of back-taper. drill also have back-taper and also get smaller at diameter.
catalog reamers are often +-.0002 or size - .0002 depending on the brand..

Usually drill blanks are -.0002
And reamer blanks are +.0002

taps are made to GH tolerance and metric to D tolerance often oversize taps used for heat treated parts so after heat treated screw still goes in tapped hole
.
reamers are marked either size ground to OR the size hole it suppose to make which can often be different that reamer size. reamers are effected by tool holder runout and how stiff the tool holder is.
.
you can easily have a .7460" reamer make a .7500 shallow hole if tool holder has runout and the machine and tool holder is very rigid and stiff.
.
can also ream a lobed hole or not perfect round and ream a curved hole where short ground pin goes in but a long ground pin will get tight and stuck in the curved hole. why hole lobed and or curved various reasons. worse is when you do 100 holes and get a random 10% have problem like cannot get long plug gage in in hole by hand. you reream hole with new reamer 10 times same hole and STILL cannot get long pin to go in hole all the way by hand. thats why they make +.0005 reamers
.
you can easily have reamer stick out of tool holder 4.0" and get one hole size and then have reamer stick out of tool holder 6" and get smaller hole cause it will flex and follow hole rather that cut all the oversize tool runout amount. hard to describe but have seen many times

i have seen 2" dia end mills 10" long flute with no center hole on end. tool resharpener could not align to center hole cause none there. put in tool holder on tool grinder often long end mill is resharpened with runout. that is flutes might measure 1.990 but it cuts 1.995
.
cant just measure end mill with micrometer and assume it will cut that size. usually got to comp +.005 (sometimes more) and do a test cut

Flutes should not run out after resharpening. Best to find a sharpener source with an air spindle so run out will be reduced. Often a poor grind will make it hard to indicate in..so with this one can leave a tad of shank stick out of holder and indicate on that. yes in a tube or collet. One can turn a cutter shank held in a V block to get a circle land si re-establishing the true round to the shank..then flute grind just to take away that land.

DMF_TomB said:

you can easily have reamer stick out of tool holder 4.0" and get one hole size and then have reamer stick out of tool holder 6" and get smaller hole cause it will flex and follow hole rather that cut all the oversize tool runout amount. hard to describe but have seen many times

Click to expand...

yes, it's the concept behind a floating holder.
at least for lathes.

michiganbuck said:

Flutes should not run out after resharpening. Best to find a sharpener source with an air spindle so run out will be reduced. Often a poor grind will make it hard to indicate in..so with this one can leave a tad of shank stick out of holder and indicate on that. yes in a tube or collet. One can turn a cutter shank held in a V block to get a circle land si re-establishing the true round to the shank..then flute grind just to take away that land.

Click to expand...

.
i have seen many many resharpened end mills with runout. many 2" dia end mills with 10" flute after made the center hole on end is lost by the sharpening so it makes resharpening difficult. roughing corncob end mills usually the worst for runout as they sharpen by making flutes wider not by sharpening land OD to smaller dia.
.
i literally have seen 10,000's of end mills with over .005" runout on a optical tool setter. thats why most set tool comp +.005 and do a test cut. micrometer measured tool dia is usually not what it cuts cause of runout.
.
also obviously each cnc tool spindle has its own runout. you can take SAME tool and on one cnc need +.001 tool comp adjust and on another cnc need +.005 tool comp adjust cause each cnc has its own spindle runout
.
also with set screw holders runout changes depending on how tight its tightened. and collet holders get runout when they get rusty or dried coolant on collet and collet holding taper. obviously runout changes depending on how clean everything is
.
always with boring bars each cnc machine or spindle has a different runout and boring bar usually needs to be adjusted for that particular machine. obviously depends on tolerances needed
.
i have never known any cnc to maintain same runout as spindle taper picks up dirt, rust, oil, coolant, etc. runout can easily change day to day especially if small stuff like plastic chips or dust sticking to tool holder tapers in the tool magazine. sometimes air blast at tool change doesnt blow it off cause its stuck on either by static electricity or by dried coolant. i always clean tool holder tapers when setting on optic tool setter. usually cleaning off rust, dried coolant, oil, dust and chips, etc the longer tool in machine usually the worse it gets. many tools in machine for weeks if not months