Precise holes for bearing -> what endmill for aluminium?

Hello !

I've recently built a CNC machine which is somewhere between hobby and semi-pro level. It uses the ER25 chuck system so I can grab up to f16 mm(0.63'') tools.

I've tested the machine and it works very good, good positioning and made a hole for a bearing with the ISO tolerances for H7 for f47 hole. I needed to make three different holes by gradually increasing the offset with 0.01 mm(0.0003'') before my bearing fits properly into the hole with slight use of a hammer.

I wondered what the reason is and by using a micrometer, I measured the tool diameter. For my surprise, it was not f16 but rather 15.96 mm. I found out where my mistake was.

Now, to the question, what is the best endmill tool(material, coating, number of flutes etc.) to use for making precise holes for a series of parts(5/10 or 20 items) so that the tool doesn't wear quickly off if the speeds and feeds are not too aggressive? The above miller is low-cost, costs about $10 and is from China. After several hour use without going to aggressively, it wears off.

I am currently asking about aluminium which is the material I mostly use.

I don't mind spending much more money on a single tool if I am certain it will not wear off too quickly and I will be able to do my parts with a single or with 2-3 such tools.

That cheap endmill sounds like it's a little out of spec - big surprise. A solid carbide tool made by a reputable manufacturer will cost more but will work better.

You might have better luck if you use a reamer for the final hole size. Alternatively, try heating the part with the hole in it before putting in the bearing - you're not off by too much. And press the bearing in, don't hammer it...

Hello, thanks for your reply.

Of course heating the hole is a method to insert a bearing and slight hammering is practical as well, that's two methods which are known.

The question was more about the possible accuracy to achieve with end mills and what's the best approach. I've read tons of threads on several forums and people mention circular interpolation is known to not be the best for precise holes. However, it's the easiest way I can think of. In fact, it is only recently that I built the CNC machine. Before that we've worked on manual machines and making a precise hole was a big challenge with special heads for boring.

I believe it is a question of tests to see what's possible and what's not for my case.

I did spent more Than 500 € in Tools to Master Aluminium ...
On the end i found an swiss Made Single Flute miller which Looks like a Horror movie Tool but Works great high speed and accuracy but doesnt waer off but 27€ per 6 mm miller ...

There's a lot of methods you can use. If i'm using a cheap endmill, I mill the hole, then measure it and adjust. Otherwise, quality carbide are usually a lot more in spec than HSS ones are.

You could also use a boring head for a perfect fit everytime, but they are fiddly to setup. Most of the time, I just use an HSS endmill, and after the rough cut I do a fine finish cut with more than .010" of material left to be removed. This eliminates a lot of deflection and gives you a truer final diameter.

Wade

I don't really see a problem here mitis, three attempts and you nailed the hole size, that is what you do, it's just flat luck to load in some new gcode and have a perfect fit, it can happen just not the rule. Still, as has been mentioned here, do yourself a favor and lose the China cutter or save it for when your friends ask to use your mill :D buy a quality three flute carbide aluminum cutting coated end mill in the largest size you can tolerate and use with a finish pass for the final dimension.
Even once you get it you have to repeatedly check as the cutter, spindle and material temperature increases from friction and even coolant temp will change the cutting results.

Ken

mitis

since your machine in good case can step 0.01 mm, then the H7 tolerance only virtual to you..
you also have at least 0.01 mm backlash

most possible happen, the hole will be smaller or larger.. getting it size with a simple router likely a lottery..

even tool would be size it almost impossible to simply ""drill"" a H7 tolerance hole..

you would have better controlled method using a boring bar.. even just a homemade what you setting by setscrew..

endmill almost don't change nothing.. china using same carbide than any other country.. real difference coming when tool breaks
youll find a 60 dollar endmill breaks same easy than a 3 dollar endmill

from practical side for a 16 mm dia hole
leave in hole about 0.15 mm and finish with boring bar..

Guys, thank you for your answers. In fact, now that I see others also employ end mills for precise holes, it seems, as I said and you confirmed, it's a matter of experiments with the right cutting conditions for optimal quality.

@ Tkamsker, spending money on the right tools is something very important. In fact, having the right tool, even if it costs more might be the better option. I've once talked to a Swiss who told me it is more cost-effective for him to buy a tool from 70 Euro than to buy a tool from 10 Euro because seven from the latter survives less than one from the first.

@Wade, it seems I am doing the same like you with the difference that you seem to leave two times less than me for the final cut. For these 3 trial holes, I left 0.5 mm (0.02 ''). The results were good. It just turned out that the tool is not 16 mm but 15.96. Probably it was due to a wear or it was like this from the factory, I don't know. Now I use the micrometer to validate the tool size and will see what the next trials will lead to.

@Ken, I admit I am not the best in tool theory but why 3 flute is the most suggested for aluminium? I believe it is because at any moment you have one flute working but would like to get the practical reason behind this.

@victorofga, you are right. However, for a ф47 mm, the tolerance is 0.025 mm so in theory I am out but not by far. I have Bosch Rexroth ballscrews and linear guides but still as you say it is almost impossible. I liked the way bearings went into the holes after the rough + finish but of course it may be good luck which, by using the same GCode program, may not repeat with every part. Yes, braking a tool like this would cost you much but I if it is a more quality tool and doesn't wear off so quickly, and you get the right cutting conditions, isn't it better? With a low-cost chinese mill, 1 hour cutting with moderate conditions and it's not the same diameter.

i needed some 13mm holes for bearings....

my method was really dodgy, but not exactly quick...

roughed out to 12.7 with what i had.

waited 3 months (who knows what happened? the ship sunk?) for a 13mm endmill from fleabay. i waited 2 months, ordered another one, got a refund on the first one...and then they both arrived on the same day!!!!

plunged that straight in.

never measured them but heating to about 70 degrees C made for a perfect slide in fit...

it was quick once i had the tool :)

bigger sizes, id use a micro boring head myself, but hey...

We have had allot of luck using Straight 2 flute end mills to "bore" precision holes. Onsrud work well. Just make the end mill "run-out" to the size needed. (Holes are within 0.002" of a nominal size) Tolerance held 0.0002"

@Ken, I admit I am not the best in tool theory but why 3 flute is the most suggested for aluminium? I believe it is because at any moment you have one flute working but would like to get the practical reason behind this.

Mitis,,
Sorry about the late reply, never got notice of any .

It is always beneficial to use a cutter with as many flutes as possible, faster feeds, smoother finish and smoother cutting, with some of the softer aluminum and/or improper feeds more then three flutes have a tendency to load up the flutes and that is a big problem.

Ken

3 flute end mills are significantly stronger than 2 flute.

I have had very good sucess drilling both aluminum and steel with 2 flute circuit board drill bits. They are sharpened for drilling, so they self center properly and don't bounce around inside the hole, but the bottom of the hole has about a 10 degree point rather than flush. also, some end mills are sharpened at a slight negative angle such that the edge of the tool cuts first ( -1 degrees rather than the 135 degrees of a drill bit. my pcb drills might be 5 degrees.)

so if folks are recommending 3 flute endmills.. its simply they are drilling the hole very quickly and are running close to the limits of a 2 flute endmill.


also, most carbide endmills are undersized by a hair. that's what i heard for years. i would imagine you would have to buy a "new" tool made on new machines to get a full size endmill. the old tooling that produced undersized carbide is a funtion of tolerances on the grinding equipment, and supposing those machines got shipped to the east then guess where your cheap carbide comes from.. old machines.
do you expect the manufactuer to start with an oversized rod and then grind the shank down to size, while keeping the cutting edges on center, or just grind the cutting edges on center but .01 or .02mm taken down.

also.. did you check the distance from the center to the flute or just flute to flute.. the runnout on the cutting edges isn't always negligible.