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
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Make sure your feedrate and surface speed are within handbook recommendations, which tend to be practical minimums.. Otherwise, it will be meaningless.
--
Ed Huntress



Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
On Tue, 22 Mar 2011 20:37:20 -0500, Ignoramus6593

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
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

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<make_cut> sub #<y> = #1 #<frate> = #2 G0 Z0.01 G4 P0 G0 Z-0.25
F#<frate> G1 X8 F#<frate>
G0 Z0.01 G4 P0 G0 X-0.5 O<make_cut> endsub
S100 M3 M8
#<y> = 0 #<frate> = 1 O<while> while [#<y> LT 4] O<make_cut> call [#<y>] [#<frate>]
#<y> = [#<y> + 0.25] #<frate> = [#<frate> + 1] O<while> endwhile
M2
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

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.
--
Ed Huntress



Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Ignoramus6593 wrote:

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".
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

Did Iggy say what kind of aluminum he's milling? Is it a wrought grade, or is he milling hypereutectic castings with HSS?
--
Ed Huntress




>
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Ed Huntress wrote:

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.

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

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. <g>
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.
--
Ed Huntress


>
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Ed Huntress wrote:

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.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
snip--

I haven't followed this thread in detail, but I can't help but wonder if, maybe, Iggy is climb milling when roughing, and there's some slack somewhere? It happens so fast you can't really tell what's going on.
Harold
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

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
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Ignoramus29973 wrote:

Where did you see 0.002" per tooth? Machining Fundamentals, 2000 edition, page 309, figure 17-71 indicates a feed per tooth range for an end mill in aluminum of 0.009"-0.022". I don't know where you found 0.002", but even there, your feed was still less than half that.
I'm not recommending 10x more, the reference books are recommending that, and those rates are backed up by my AL milling experience. The Machining Fundamentals book is recommending up to 29x what you are running as a maximum, and 12x as a minimum. They say to start in the middle of the range which would be around 20x what you were running.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Pete C. wrote:

This has to be scaled by cutter diameter, however. My McDonnell-Douglas slide rule gives a figure for a 1" cutter, and then you multiply by cutter diameter to scale it for the actual cutter size you have. For an end mill in aluminum, it recommends .010" feed per tooth, but multiplied by diameter. So, for 1/4", that works out to .0025"
To cut at .025" chip load, you need a cutter ground with MUCH greater back relief so the back of the flute is not rubbing on the work. There definitely are special aluminum cutters made this way, but the typical noname stuff is not ground with that much relief.
Jon
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Jon Elson wrote:

The SFM calculation certainly takes the cutter diameter into account, but Machining Fundamentals does not indicate any adjustment to the feed per tooth based on end mill diameter. It also indicates the recommended feeds can be increased 100% or more depending on the machine rigidity and use of carbide cutters.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Pete C. wrote:

I once had a shop coach who compared Al to modeling clay. :-)
Cheers! Rich
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
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

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Harold & Susan Vordos wrote:

I use 4-flute end mills extensively in aluminum, with good results. Since I have limited spindle speeds, and often use small diameter cutters to get smaller corner radii, it helps to have more cutting edges per minute.
Supposedly, though, a 4-flute mill has a thicker web and is therefore stronger than a 2-flute one.
Chip welding is GREATLY alleviated by climb milling, I do almost everything in the climb direction.
Jon
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Certainly not implying they don't work---they do. They're just not the right tool for the job. You'd be better served going to a three flute in the circumstances you described. Finish cuts are always taken climb milling (at least by those of us that know the difference). Roughing? Not the smartest thing you can do.
Harold
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
...

You need a CNC, I've broke two in a day lots of times. <VBG>
Karl
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.