Dimensional accuracy of endmills?

[Cushing H.]

So ... i was puttering yesterday an making a centerline scribing tool (after one of natleks designs), and this included creating some 1/8" holes in a piece of aluminum. Since i had my endmill holder in place on my mill, and was feeling too lazy to swap out for my drill chuck, i thought i would take a stab at creating those holes with a 1/8" endmill.

No problem with creating the holes, *but* what i expected no be a tight (near press) fit between the inserted 1/8" brass rod and the holes revealed a really loose fit. Measurement revealed the hole diameters to be something like 0.131" versus the expected 0.125". I also checked the slot i recently milled into a piece of brass (for a bolster/guard) and sure enough, its width was like 0.131 versus the 1/8" (0.125") mill i had used.

Redrilling the holes with a 1/8" drill bit produced a hole with diameter more like 0.125", and a nice tight fit between brass rod and hole.

Now i know dimensions are not exact, but i would have expected better dimensional accuracy out of an endmill. What is going on? Is it typical for an endmill to produce a hole or slot that is so much different from the labeled dimension of the endmill, or am i maybe just looking at a not-so-good endmill?

 

[CallumRD1]

An end mill is fairly rigid so any runout in your mill/collet/toolholder will be transmitted to your hole dimension. And any lack of rigidity will allow the work to push the tool around making your hole oversized. It’s common practice to rough slots with smaller end mills and then take a finish pass to get the desired dimension. Precise holes are better drilled and reamed or cut with a smaller end mill and bored to final size with a boring head, rotary table, or CNC circular interpolation.

 

[Cushing H.]

So a drill is more accurate because of the higher flexibility of the drill versus the endmill? Interesting. For my purposes i am usually *not* that interested in high accuracy ... i was just surprised to see something like a 5 mil variation. This is just a mini mill after all though. Ill have to remember this if i need to do something with higher accuracy...

 

[AVigil]

If you want a precise hole you use a smaller diameter drill or end mil then you ream to the proper size.

When milling a hole or drilling a hole do not expect a perfect size hole.

 

[CallumRD1]

Stick an indicator just above the tip of your end mill and rotate the spindle in reverse by hand. Look at the maximum runout. I'd bet it's not anywhere near zero.

 

[Cushing H.]

If you want a precise hole you use a smaller diameter drill or end mil then you ream to the proper size.

When milling a hole or drilling a hole do not expect a perfect size hole.

Hey adam. Yeah, i know that. I was just surprised at the degree of variation. Like i said, lesson learned...

 

[HSC ///]

So a drill is more accurate because of the higher flexibility of the drill versus the endmill? Interesting. For my purposes i am usually *not* that interested in high accuracy ... i was just surprised to see something like a 5 mil variation. This is just a mini mill after all though. Ill have to remember this if i need to do something with higher accuracy...

hang on a second... you have potentially too many variables going on here

in general a drill makes a triangular hole, try drilling a hole in sheet metal, you will see a triangle hole.
as mentioned a precision hole is reamed out, a reamer is stiffer and makes a round hole.

on endmills, what you described is usually called plunge milling, drilling a hole with an endmill that is bottom cutting (center cutting) not all end mills are bottom cutting. was the endmill stub length or long?
endmills can machine to higher tolerances (i.e. .0005) and this is commonly done is machine shops.

However, the diameter tolerance from the manufacturer can vary, for example, if you look at an 1/8" end mill specifications, the diameter tolerance can be - Diameter Tolerance: +0.000 / -0.002 or it can be +.0005 / -.0005 depending on the manufacturer and model

but there's too many variables in your setup, quality of mill, setup rigidity, runout of holder, is the endmill HSS or carbide (stiffer), accuracy of measurement device used. etc etc

If you want to nail this down for precision, you have to check all of the above,
a good place to start is the slot you milled out that measures .131, did you just take one full pass with the 1/8" end mill?
that won't work if you want a precisely milled slot

 

[Cushing H.]

hang on a second... you have potentially too many variables going on here

in general a drill makes a triangular hole, try drilling a hole in sheet metal, you will see a triangle hole.
as mentioned a precision hole is reamed out, a reamer is stiffer and makes a round hole.

on endmills, what you described is usually called plunge milling, drilling a hole with an endmill that is bottom cutting (center cutting) not all end mills are bottom cutting. was the endmill stub length or long?
endmills can machine to higher tolerances (i.e. .0005) and this is commonly done is machine shops.

However, the diameter tolerance from the manufacturer can vary, for example, if you look at an 1/8" end mill specifications, the diameter tolerance can be - Diameter Tolerance: +0.000 / -0.002 or it can be +.0005 / -.0005 depending on the manufacturer and model

but there's too many variables in your setup, quality of mill, setup rigidity, runout of holder, is the endmill HSS or carbide (stiffer), accuracy of measurement device used. etc etc

If you want to nail this down for precision, you have to check all of the above,
a good place to start is the slot you milled out that measures .131, did you just take one full pass with the 1/2" end mill?
that won't work if you want a precisely milled slot

Yes my endmill (stub length) is bottom cutting - would not have even tried if otherwise. On the slot - i did not have a choice given the thickness of the stock the guard is to slid onto. I would have preferred a smaller mill and making multiple passes to widen the slot - but i could not find a mill with enough length to cut the full depth of the slot. Worked out ok .. but as i said at the time, i got lucky.

Everything you say to consider is absolutely true - but i dont really want to take the time to over analyze, because as i said i am not usually after any real level of accuracy. Just wanted to know if that level of variation (0.006") for a straight plunge is typical (or at least expected). Sounds lime it is?

 

[Pinoy Knife]

yes a 5 thou oversize in not at all uncommon.
most people do not check their run out... i have a well known knifemaker friend that finally checked his run out after 15 years
and found out why he has never been able to make good/accurate holes.. he borrowed my indicator and instructions on how to use it
his son works with him and will be here in a hour or so to make "Custom Pivot pins" and Bushings for several knives he is working on ..
ive told them both to seriously look into buying better tighter tolerance gear to avoid these problems .. they have not done so yet..
if you want accurate holes you drill undersize and ream to size
if you want a accurate slot you go undersize as well and adjust to perfect size... Never trust the size marked is what YOUR machine will make..

 

[Hubert S.]

Since i had my endmill holder in place on my mill, and was feeling too lazy to swap out for my drill chuck, i thought i would take a stab at creating those holes with a 1/8" endmill.

You can be lazy and use a drill bit in a collet if the tang is not chewed up from a chuck, and you happen to have the right size collet for the drill size already in there. You'll probably get less run-out from the collet compared to the drill chuck, one of the few occasions where laziness might lead to a better outcome.

 

[Nathan the Machinist]

You can get away with this technique if you pre-drill the hole undersize and use an endmill as a reamer most of the time. The endmill is usually around .001 undersize (more if it's cheap or dull) and your runout in the tool holder might be .0005 so you can often get a good snug hole with accurate hole location. I do this all the time because I make pinned fixtures for my work in process regularly with about a thou tolerance total stack up and it somehow usually works fine. I'm often holding tenths without even trying, so the technique is apparently pretty valid.

After doing this for years I ran into trouble yesterday because my drilled holes were too shallow, and the material built up on the tip of the endmill and caused it to wallow around a bit at the end of the cut and ruined my press fit. That's on a pretty stout mill and it still wiggled around enough to spoil the fit. So, you can use an endmill as a reamer (I like to because it gets the location dead on), but it won't work well if you're just plunging without clearing out the hole first.

 

[CallumRD1]

You can get away with this technique if you pre-drill the hole undersize and use an endmill as a reamer most of the time. The endmill is usually around .001 undersize (more if it's cheap or dull) and your runout in the tool holder might be .0005 so you can often get a good snug hole with accurate hole location. I do this all the time because I make pinned fixtures for my work in process regularly with about a thou tolerance total stack up and it somehow usually works fine. I'm often holding tenths without even trying, so the technique is apparently pretty valid.

After doing this for years I ran into trouble yesterday because my drilled holes were too shallow, and the material built up on the tip of the endmill and caused it to wallow around a bit at the end of the cut and ruined my press fit. That's on a pretty stout mill and it still wiggled around enough to spoil the fit. So, you can use an endmill as a reamer (I like to because it gets the location dead on), but it won't work well if you're just plunging without clearing out the hole first.

I do something similar for quick and dirty one-off fixturing when I don’t want to bother with pins. I’ll plunge a 1/4” end mill to create a hole on a fixture plate or part for a 1/4-20 fixturing screw. The location will be correct and will leave a couple thou clearance around my screw. The majority of my quick and dirty single ops can withstand a few thou error so it has been a fantastic time saver.

 

[Crag the Brewer]

Machine shop 101

Something that also hasn't been mentioned (I think?) is measuring....?

you can not put a .125" pin into a .125" hole.
Size on size is Not a slip fit.
If you are getting a slip fit on a 1/8" hole its probably .126" or bigger.
Gauge pins are best for measuring.

Nathan sorta mentioned the effects of chatter from bottoming out..... Increasing the bore, or slot.
Tool pressure is why milling the slot, the tool flexes/walks during the cut. Is the feed too strong, is the tool dull, etc?

Go smaller first.... center drilling, then drill a pilot, then with the endmill, followed by a larger one. It will look cleaner/true too, not key-holed looking.
For true holes, a reamer is your friend.

Material makes a difference too.
Drilling plastics will often drill a smaller hole.
metals will drill a larger hole.
stainless likes a strong feed & low rpm, and likes to work harden. aluminum likes to weld itself to tooling, and brass sucks.

we've got bellmouthing, and tapering to talk about. all kinds of things.

Making chips IS Fun!!!



* My BEEF is watching Youtube videos, and Everyone is using 1,2,3 blocks for everything..... ugh, it Kills me.

 

[Hubert S.]

You can get away with this technique if you pre-drill the hole undersize and use an endmill as a reamer most of the time. The endmill is usually around .001 undersize (more if it's cheap or dull) and your runout in the tool holder might be .0005 so you can often get a good snug hole with accurate hole location. I do this all the time because I make pinned fixtures for my work in process regularly with about a thou tolerance total stack up and it somehow usually works fine. I'm often holding tenths without even trying, so the technique is apparently pretty valid.

After doing this for years I ran into trouble yesterday because my drilled holes were too shallow, and the material built up on the tip of the endmill and caused it to wallow around a bit at the end of the cut and ruined my press fit. That's on a pretty stout mill and it still wiggled around enough to spoil the fit. So, you can use an endmill as a reamer (I like to because it gets the location dead on), but it won't work well if you're just plunging without clearing out the hole first.

I tried this out using a 3/8" end mill to ream a hole that was pre-drilled to 23/64" and got an oversize hole. The material is 1/2" thick aluminum. I think the drill size may be a bit on the small side, but if I use a reamer in the same size hole, I get a press fit with a bushing that fell right through the hole made with the end mill. I have to make a hole for a press fit in a pretty tall component where I don't have enough travel on my mini-mill to use a reamer, so I was really hoping this would work for me. Is there a chance I might get a better result by pre-drilling closer to the final size?

 

[CallumRD1]

I tried this out using a 3/8" end mill to ream a hole that was pre-drilled to 23/64" and got an oversize hole. The material is 1/2" thick aluminum. I think the drill size may be a bit on the small side, but if I use a reamer in the same size hole, I get a press fit with a bushing that fell right through the hole made with the end mill. I have to make a hole for a press fit in a pretty tall component where I don't have enough travel on my mini-mill to use a reamer, so I was really hoping this would work for me. Is there a chance I might get a better result by pre-drilling closer to the final size?

First you need to measure the runout at the tip of your cutter. If you have 4 thou runout on a 0.375 end mill the best you can expect to get is a 0.379 hole. Alternatively, cutting down the shank of a reamer can provide more reach, but you want to leave as much as possible because you'll get a more accurate hole when the reamer shaft can still flex a couple thou to center on the hole and eliminate the runout in your system.

 

[Hubert S.]

First you need to measure the runout at the tip of your cutter. If you have 4 thou runout on a 0.375 end mill the best you can expect to get is a 0.379 hole. Alternatively, cutting down the shank of a reamer can provide more reach, but you want to leave as much as possible because you'll get a more accurate hole when the reamer shaft can still flex a couple thou to center on the hole and eliminate the runout in your system.

I have measured the runout on an end mill, and it appears to be less than half a thou. Maybe I should buy a set of gauge pins to figure out how big the hole actually is. The bushing (just over 0.376") feels pretty loose, I think the hole in the test piece ended up at least 0.377", probably bigger.

I figured there is a reason why reamers come with a long shaft, your explanation makes a lot of sense. I might cut one down, but I just remembered that I have a couple different end mills I could try to see if they give me a better result. I'm also wondering if I should run the end mill slower when using it to ream a hole. I'll do some more testing.

 

[CallumRD1]

I have measured the runout on an end mill, and it appears to be less than half a thou. Maybe I should buy a set of gauge pins to figure out how big the hole actually is. The bushing (just over 0.376") feels pretty loose, I think the hole in the test piece ended up at least 0.377", probably bigger.

I figured there is a reason why reamers come with a long shaft, your explanation makes a lot of sense. I might cut one down, but I just remembered that I have a couple different end mills I could try to see if they give me a better result. I'm also wondering if I should run the end mill slower when using it to ream a hole. I'll do some more testing.

Another issue with plunging an end mill could just be rigidity of your mill. There is no cutting geometry to center the end mill in the cut so it will try to push your head around. A reamer or drill has tapered cutting edges that stabilize and center the cut. This becomes exceedingly obvious if you’ve ever tried to do something foolish like chuck up an end mill in a hand drill to drill a flat bottomed hole.

 

[Nathan the Machinist]

I tried this out using a 3/8" end mill to ream a hole that was pre-drilled to 23/64" and got an oversize hole. The material is 1/2" thick aluminum. I think the drill size may be a bit on the small side, but if I use a reamer in the same size hole, I get a press fit with a bushing that fell right through the hole made with the end mill. I have to make a hole for a press fit in a pretty tall component where I don't have enough travel on my mini-mill to use a reamer, so I was really hoping this would work for me. Is there a chance I might get a better result by pre-drilling closer to the final size?

You either have runout, a lot of wobble when plunging or a flute loaded up and pushed your cutter off to one side. Plunging a .375 endmill with a 23/64 pre-drilled hole should have given you a .373-.375 hole.

Your spindle speed for this should be around 500-1000 RPM and your feed should probably be between 20-60 IPM. Try pecking if you're getting a flute build up pushing your cut off. Flood coolant helps, especially in aluminum which can stick to the side of the cutter and spoil your hole.

Obviously a reamer will give you better size control. But it will also tend to follow the location of the drilled hole which will not be accurate. An endmill will give you accurate hole position but less hole size stability. It's a tradeoff.

I recently ran into a problem with this technique where my drilled hole wasn't deep enough and the endmill touched the bottom of the hole and wobbled. It was oversized because of wobble and this was on a pretty stout and accurate mill. The technique isn't foolproof.

 

[Hubert S.]

You either have runout, a lot of wobble when plunging or a flute loaded up and pushed your cutter off to one side. Plunging a .375 endmill with a 23/64 pre-drilled hole should have given you a .373-.375 hole.

Your spindle speed for this should be around 500-1000 RPM and your feed should probably be between 20-60 IPM. Try pecking if you're getting a flute build up pushing your cut off. Flood coolant helps, especially in aluminum which can stick to the side of the cutter and spoil your hole.

Obviously a reamer will give you better size control. But it will also tend to follow the location of the drilled hole which will not be accurate. An endmill will give you accurate hole position but less hole size stability. It's a tradeoff.

I recently ran into a problem with this technique where my drilled hole wasn't deep enough and the endmill touched the bottom of the hole and wobbled. It was oversized because of wobble and this was on a pretty stout and accurate mill. The technique isn't foolproof.

Thank you for the detailed response. I don't remember the exact speed I was using, but it was likely faster than the range you gave, and there may have been build-up on the endmill. I will try again and pay more attention to the details.

 

[Nathan the Machinist]

Thank you for the detailed response. I don't remember the exact speed I was using, but it was likely faster than the range you gave, and there may have been build-up on the endmill. I will try again and pay more attention to the details.

When using an end mill as a reamer, your RPM is much lower than using it as an endmill. But your feed rate is quite high. Chip load per tooth is substantially more than normal machining operations