Share and compare your Mikini 1610L cutting data here

[Brian L]

OK, hard to second guess from pictures, but I suspect you are trying to bore too close or actually undersize of the minimum bore that the bar is allowed to do. From what I see there, the way the carbide is fractured all down the edge of the insert suggests it was rubbing below the cutting edge and flaked off. I don't remember where/what brand the bar is, but check and see if you are above the range of minimum bore.

One other possibility, try turning the bar slightly less positive, I know you think it's too negative already, but if you are approaching the smallest diameter, then even the slightest bit turned "up" is going to remove your clearance from the cutting edge. The bar probably has flats, so you will be limited as to how much you can turn, but try getting as much negative, rather than positive turn that you can and see what happens.

Those look like standard CCMT inserts, you have a slightly different chip breaker design in the two, but given you are boring tough steel, they would be more appropriate than the first insert.

[SWATH]

Thanks Brian, I think you're right. I emailed the place I bought the bar from and they said the minimum bore diameter is .58 and I was trying to bore .55. I opened up the bore to .6in with an endmill and did fine but the finish was still bad. I tried a different chipbreaker and it left a nasty finish, then I tried the chipbreaker in the picture again with a new insert and it cut great. It was quiet and and left a long thin piano wire chip but the finish was still no good. It looked like it was finely threaded with little ridges all the way down. I kind of figured it was because the IPR was too great for a fine finish. The minimum IPR for this insert is .004 IPM which is what I was doing so I'm think maybe try a different insert that is made for fine finishing. I also cut the boring bar from 6in. overhang down to 3in.

Any suggestions for a 21.5x or 32.5x insert (I have bars for both insert types) to get a fine finish in hardened alloy steel?

[Brian L]

I think the inserts you used are good, the bar is most likely the problem. You bought a carbide shank, correct? I know that given carbide is harder it should be stiffer, and that is the case in end mills, but in boring bars, unless they are short with little overhang, you are better off with a steel bar, they don't vibrate near as much. You would also want to keep the corner radii of the inserts as small as possible, maybe .005 or .007", whatever is available, therefor your feed rate is going to need to drop to more like .002-.003" per rev at the most.

If you have a method of sharpening, diamond wheel on a grinder, you would be worlds better off with a soldered carbide bar from Micro 100. You will find that with either a dead sharp corner or a small 45º ground on the leading edge will give you the best finish.

Another thought, if this is for a part that needs to be the same size, and you are going to make a few, you'd have much better luck with a reamer, it'll hold size and last a long time, and give you a better finish, most likely. Another option, if you can get a carbide endmill slightly oversize, have a tool grinding service grind it down to the size you need, they make great reamers, last a long time, and given the depth of your hole, might allow more chips/deeper pecks without loading up the flutes.

[SWATH]

4140HT
.375 TiALN rougher 1.15" stickout
2370 RPM
23 IPM
.1 DOC
full slot

This cuts but give major chatter at any feedrate. I also tried this cut with a regular .375 endmill instead of a rougher at 12ipm and it cuts too but still with the chatter issue. In fact it only stops chattering at around 5ipm.

I ordered a radiused variable flute endmill to try and see if that reduces the chatter when slotting.

[SWATH]

4140HT
.18 (#15) TiALN Cobalt parabolic drill
1370 RPM
5.6 IPM
1.25 deep
G83 full retract .15 increments

Cuts good, started at .18 peck but the faggy spindle started to bog down near the bottom of the hole and I could tell it was about to stall so backed off a little.


4140HT
.5 TiALN rougher 2.5" stickout
2600RPM
82 IPM
.238 DOC
.025 WOC

Cuts good but ended up chipping the $70 endmill because the @#*&$@* spindle halted a few minutes into the cut.

[Brian L]

So my numbers were pretty close. I suspect a lot of your broken tool problems and such are the spindle, you can't be feeding along with the stepper motor and have the rpm drop dramatically, even for a split second without putting way too much feedrate on the tool.

[SWATH]

So my numbers were pretty close. I suspect a lot of your broken tool problems and such are the spindle, you can't be feeding along with the stepper motor and have the rpm drop dramatically, even for a split second without putting way too much feedrate on the tool.

Yup you're numbers are always good but I was thinking about it yesterday. Almost every single tool I've chipped has been from a spindle halt. Not all of the them but most. Even the fatest toughest roughing endmill will chip the moment it stops spinning from a spindle halt. Something about the flutes slamming into the material without cutting it in addition to the increased chipload as the RPM slows down. So unbelievably frustrating. Even when drilling it becomes very easy to snap drills in holes because the spindle bogs down so bad, while at the same time the stepper motors seem to be quite powerful and happily continue on at the same feedrate increasing the chipload so much that the drill has no choice but to snap. In fact the steppers seem to be so potent that I completely broke a short 3/8 carbide rougher, I mean snapped it off at the collet when the part was pulled to the side in the vice causing too much of a DOC, that was my fault for not clamping down with the force of God. The axis motion didn't skip a beat, and it probably would have cut fine if the spindle didn't bog down.