End mill testing

I would like to get a cheap endmill, say from Shars, and an expensive
end mill of the same configuration (same number of flutes, same
coating or no coating, same diameter etc). Then, I want to try to
compare them.
The most obvious comparison is by how much they could cut before they
dull and break.
To that end, I could get a couple of identical cold rolled 1018 pieces
and just machine their faces in subsequent passes. I would see, then,
when the end mill breaks, but just seeing how much was milled.
I would think that 3/16" size, and a 5x10" sized piece of 1018, should
provide enough material to wear out, say, 3/16" end mills.
THis being a CNC application, I do not really care how long it takes.
Am I missing anything? What is a "meaningful test" here?
i
Reply to
Ignoramus6593
Loading thread data ...
Make sure your feedrate and surface speed are within handbook recommendations, which tend to be practical minimums.. Otherwise, it will be meaningless.
Reply to
Ed Huntress
There is a world of difference in endmills. My son brought home some Hanita 1/4" two flute endmills just for AL. Just amazing how fast they can cut.
Now if you want to be totally blown away, move up to inserts. Sandvik makes an R390 that cuts steel like butter. They are designed to put the heat into the chip and run best without coolant. My shop floor is coverred in blue to black chips. You can get these cheap on eBay. My son says everybody must be stealing from their work and selling on the side.
Karl
Reply to
Karl Townsend
I have an idea.
Instead of stupidly running many cuts with the same IPM, how about making a series of cuts with INCREASING IPM. That will make end mills break sooner, but still, the first to die, loses.
O sub # = #1 # = #2 G0 Z0.01 G4 P0 G0 Z-0.25
F# G1 X8 F#
G0 Z0.01 G4 P0 G0 X-0.5 O endsub
S100 M3 M8
# = 0 # = 1 O while [# LT 4] O call [#] [#]
# = [# + 0.25] # = [# + 1] O endwhile
M2
Reply to
Ignoramus6593
Ok - I'll throw in a wrench :-)
I cut HRS in 2D CNC - plasma. In the last couple of years, the steel from mills is more and more scrap. I think of car bodies....
I can cut a design out of a 48"x48" sheet and be over 1000 inches in cut along the way. From time to time I get hard spots - normally stretches or smears of ball bearings, races and such. Cuts nice and clean and then can't burn through at that speed - then back cutting nice.
Has the bulk 3D blanks gone the same way ?
Are sheets rolled out of lower grade steel than blocks and thick sheets ?
Maybe this is an endmill issue - running nice in 1018 and the endmill is deflected due to not 'biting' in and shatters.
Any experience in this ?
Martin
Reply to
Martin Eastburn
If you increase the feedrate, you're testing the elongation capability of the tool, not its life in normal service. The weakest one probably will break last. A high-cobalt HSS cutter, being somewhat brittle, may break first. But in normal service it may last two or three times longer than some Chinese "high speed steel."
The quality of a HSS cutter is based on its ability to resist wear and its ability to keep its edge at high temperatures. The two usually go hand-in-hand. Thus, an M42 ("cobalt") end mill will outlast one made from M2 (or M50 if it's Chinese) in normal use. But if you push the feedrate too much, it may break before the M2 cutter.
Reply to
Ed Huntress
It's not just cutting that breaks end mills. Direction changes and other changes in the loading of the cutter cause premature failure.
Reply to
Tom Gardner
Again, you are missing the point that too low a feed is as bad for end mill life as too high a feed. In order to make a meaningful comparison of the service life of different brands of end mills of the same type, you have to perform the test at optimum feeds and speeds for the material and end mill specs. Since you seem to consistently run *way* too low a feed / chip load, I'd suggest you work on getting the feeds up to snuff before you attempt any comparison.
At the moment you are milling AL, which is some of the easiest stuff where you can readily get very high feed rates with no issues.
Borrowing from Jon's reply to your previous post:
"2000 RPM on a 1/4" end mill is only 130 SFPM, quite slow even for HSS in aluminum. With a 4-flute end mill at 2000 RPM, this is .00075 inch per tooth, which is quite low."
There is no reason you shouldn't be able to get 100 IPM feeds at 2,000 RPM when pocket milling. That's only 0.0125" per tooth load on a four flute end mill, which is at the low end of the 0.009"-0.022" per tooth feed rate range listed in the Machining fundamentals book for an end mill in AL. Your feed rate was less than 1/10 of the lowest feed rate recommended.
SFM for AL is listed for HSS as 550-1000 SFM, carbide as 2200-4000 SFM. You are not even close to pushing the limits of the end mill material. The AL should be cutting like butter.
Please read over section 17.8 in Machining Fundamentals "Milling cutting speeds and feeds" and try to use milling parameters that are at least at the low end of the recommended range. Once you see how much better things perform at those minimum feed rates, then try moving up closer to the top end of the recommended range.
Honestly, in my manual milling over the years, I've broken something like two end mills over 1/8".
Reply to
Pete C.
Did Iggy say what kind of aluminum he's milling? Is it a wrought grade, or is he milling hypereutectic castings with HSS?
Reply to
Ed Huntress
I once had a shop coach who compared Al to modeling clay. :-)
Cheers! Rich
Reply to
Rich Grise
snip-
It's hard to justify the use of four flute end mills in aluminum due to the ability of the end mill to create chips larger than the available space for chip evacuation. Chip welding of aluminum is a common problem, often resulting in end mill breakage. You can avoid that problem by using two flute end mills, especially in small sizes, where a four flute end mill often has very limited chip space.
Beyond that reason, four flute end mills are typically ground with less clearance than two flute end mills intended for use in aluminum. Overall, performance can be well enhanced by matching the cutter to the material.
Harold
Reply to
Harold & Susan Vordos
...
You need a CNC, I've broke two in a day lots of times.
Karl
Reply to
Karl Townsend
Nope, but a reasonable assumption is that it is one of the common grades. At any rate, he is running less than 1/10th of the minimum recommended feed rate in the Machining Fundamentals book for aluminum.
Reply to
Pete C.
I noticed in some of his earlier postings that he was running at impossibly low feedrates, but I haven't followed the progress of his education.
The only reason I brought that up is that I was wondering if he was wearing out his cutters on high-silicon alloys, which can eat up a HSS cutter pretty quickly. Otherwise, with his low feedrates, I don't understand why he's breaking cutters.
As you and others have said, cutting ordinary wrought aluminum grades is like cutting cold butter. My cutters last forever in aluminum -- admittedly, with quite low useage. I can's imagine why his cutters are breaking, unless he's dulling them somehow, or unless his programs are jerking the cutter around in corners or whatever.
Reply to
Ed Huntress
I haven't broken any end mills on my CNC mini mill...
Reply to
Pete C.
Machining Fundamentals feed per tooth range: 0.009" - 0.022" Iggy's feed per tooth: 0.00075"
He needs to feed 12x faster (72 IPM) just to get to the minimum recommended feed. The end mill isn't cutting, it's just brushing a few AL atoms off each rev. 25x his feed (150 IPM) still won't get him to the top of the recommended range.
Reply to
Pete C.
Seems that it would be good (but probably not easy) to monitor current to the spindle and the x&y feed servos. That would give you an idea of how hard they're working to make the cut, which could translate into how well the mill is cutting.
Reply to
rangerssuck
Or, maybe that's not so difficult to do. Does your software, perhaps, have the capability of logging the servo feedback signals, or is that all completely internal to the servo amps?
Reply to
rangerssuck
Pete, the recommendations I saw, were 0.002" per tooth.
You are recommending 10x more, which is slightly surprising to me. I would be happy to run at 30 IPM. A lot of things that I am making, would take a lot less time.
i
Reply to
Ignoramus29973
Karl, tell me, if I machine AL with a 1/4" 2 flute carbide cutter, what feed per tooth should I use? I am very confused by various websites.
formatting link
says use .0005 - .0015 chip load.
formatting link
says use 0.003" chip load.
At 2k RPM, I get
2000*2*0.003 = 12 IPM.
i
Reply to
Ignoramus29973

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.