Now here's a real End Mill Flute design I've never seen before -
outside of some off-the-wall router bits.
It's for cutting composites. A lot of times when cutting composites
they tend to delaminate, what we did is sandwich them between a couple
of layers of sacrificial material. Time consuming since the clamping
would have to be moved from one side to the other. For drilling we
made sure they were sitting on a scrap subplate for bottom support.
Anyway here's a different solution from an article in Modern Machine
Shop Online. Excerpts from the article follow:
Cutters Compress To Effectively Machine Composites:
This cutter has both up-cut and down-cut spiral flutes that compress
the layers of composite materials during milling operations, preventing
delamination at the outermost layers and also between inner layers.
Machinists, on the other hand, sometimes struggle to effectively
mill and drill composites because the materials possess atypical
properties that require special machining practices.
Onsrud Cutter, a member of the LMT Group, offers six-flute composites
cutting tools with specific geometries and coatings to overcome these
machining challenges. The company?s ?compression cutters? have
intersecting up-cut and down-cut spiral flutes that push individual
composite layers together during machining to prevent the layers from
separating from each other. This action prevents delamination from
occurring at the outermost material layers. It also averts delamination
of inner layers, which can be a less noticeable workpiece imperfection.
The company currently offers these tools as customs, but a standard
product line will be available in 2010.
Interesting. Does it really "compress", or does it just alternate
between lifting and pushing down? I wonder how it compares to a fine-
It actually compresses , that is cuts simultaneously up and down . At least
the solid carbide two-flute type we use in the CNC router at the cabinet
shop do . I suspect the six flute is a bit more difficult to make . I use
the cast-offs (they can only grind 'em so small , then the geometry of the
edge doesn't cut wood so well) from work in my mill-drill . They do a pretty
decent job in aluminum and mild steel . Prolly better if I used coolant ...
40,000 RPM routers aren't exactly the same thing as a 7,500 RPM Haas.
Didn't I suggest you call some tooling manufacturers to see if they
recommended using router bits in VMC's or HMC's the last time you
suggested this? Have you since done so?
I've found that 3 flute end mills give a better finish than 2 flute
end mills at the same feed rate in aluminum. Now to go from 3 flutes
to 1 flute seems to be going in the wrong direction to me. But if
you've got some data that supports this idea, I'd be willing to listen
We already went over the increased scallop height issue & chip load
comparison of running a one flute end mill vs. a three flute end mill
at the same feed rate.
It's not the aluminum that's the concern (alum. seems to have a very
high SFPM limit - I'm not even sure we even know what that limit is).
What's of concern is the most efficient end mill for the machine tool
No. Why would *I* call Onsrud? You're the one making the
suggestion/claim. Do you have any support for this suggestion backed
up by end mill manufacturer's suggestions?
Plus, a router bit would only be useful in soft material like aluminum
or magnesium, whereas three flute end mills could be used in a variety
of materials. Why tie up a shop's resources for tooling by buying end
mills for just one material, and just roughing at that, if they aren't
likely to improve material removal rates?
And another factor is that most heavy material removal is done
now-a-days by inserted end mills.
For the same material removal rate at the same RPM and Feedrate a one
flute cutter would have to have three times the chip load. Have you
seen how flimsy router bits look compared to 3 flute end mills?
Gee, how fast can you remove X cubic inches of chips? Per HP?
What are the limiting factors?
You seem uncertain.
Perhaps they make & sell exactly such tools.
Perhaps to save costs by making parts faster thus increasing any
OTOH you could use a file.
Do they last longer for the dollar than HSS or Carbide in Aluminum?
IIRC HSS has greater strength than Aluminum ....
Consider chip formation & flow.
Let's stay focused here. You're suggesting/claiming that router bits
would be better for VMC's or HMC's. I haven't seen any evidence of that.
I'm NOT certain. Router bits *might* remover material faster. I've
yet to see any evidence of this. But anything is possible.
Here is some info on Onsrud's 2 & 3 flute cutters with a coolant
through feature, that THEY recommend for aluminum. Roughing AND
They're not exactly pushing router bits in their ad.
That's unsupported speculation. Evidence, evidence, my kingdom for
HSS? You're kidding, right? Inserts are cheaper than End Mills.
Push them too hard and you'll see what aluminum can do to HSS or Carbide.
Let me just summarize some of the reasons why I didn't think following
up on your suggestion was such a hot idea.
1. Poor finish - One tool cannot be used for rough & finish passes.
2. Greater tool wear - One flute doing all the work would likely have
greater wear on it than if the work was spread between 3 flutes.
3. Limited to soft materials like plastics, Alum. & Mag. Ties up shop
4. Inserted End Mills have coolant through holes that are able to blast
the chips away with coolant in pockets.
5. Inserts are cheaper to change than whole End Mills.
6. Hard to measure the diameter of router bits, especially if they've
7. The chance of a router bit deflecting and gouging is probably
greater than a 3 flute End Mill or inserted End Mill since they don't
seem to have the body strength that regular End Mills do, or especially
that inserted End Mills do.
8. They look funny. Just kidding, I wouldn't care what they looked
like if they worked and lasted. But that's the crucial question - DO
they work? You can see from Onsrud's own ad for cutters for aluminum I
listed above, that they were pushing 2 & 3 flute End Mills NOT router bits.
But hey, if you can dig up some data to support your router bit
theory, or if someone posts about using router bits in their VMC at
higher removal rates than 3 flute End Mills - I'll be more than willing
to listen. Until then, it's just so much unsupported speculation and
not worth spending much more time on.
Just a little addendum here while I have a few spare minutes.
Horsepower rating is determined by the MMR X Unit Horsepower
MMR = DOC X WOC X Feedrate (number of flutes or RPM doesn't matter)
HP = MMR X Unit HP (.25 for aluminum)
So calculating the horsepower difference between a one flute router
bit as opposed to a 3 flute end mill is inconsequential.
The limiting factor for feedrate is the amount of back clearance on
your flutes. If you feed faster than the amount of clearance you have
you'll hit the backside of your cutter and just rub and possibly
deflect it and maybe even snap it off.
Now a rule of thumb is that you can safely feed your End Mill with a
chip load of 1.5 to 3% of the diameter per flute. So lets take the
lower limit to give the router bits their best shot. On a 1/2" three
flute end mill that would be 1.5% of .500 or .0075" chip load per flute
for a total of .0225" forward movement per revolution.
Now from the Osrud site on speeds and feeds:
We'll pick the largest recommended chip load for a one flute router
bit in aluminum, in the 1/2" column. We'll pick the column for cutter
63-000 which is a one flute router bit with a recommended chip load of
.011 - the other ones with .015 chip load are for 2 flute end mills.
That chip load of .011 is per revolution since it's ONE flute.
That is 1/2 the amount of feed of the 3 flute End Mill we just
calculated for, that moves .0225 per revolution.
So the conclusion I draw from these calculations is that a router bit
can only be feed at 1/2 the feed rate of a 3 flute end mill.
Now, that's just theoretical calculations, if someone can produce some
verifiable evidence that router bits are more productive than 3 flute
end mills - I'll be more than interested in seeing it.
"When pocketing or contour machining we generally recommend
using a single flute end mill for optimum feed rates and material
removal. Because of the high rate of material removal, the surface
finish sometimes is compromised. Therefore sometimes a finish cut is
required with the single flute. If surface finish is critical and not speed,
we recommend using a double fluted end mill at a lower RPM and
"High Speed Roughing 6061 T6 Aliminum"
Do you want to remove stock or not?
Do you have jb's confusion about VMCs & HMCs?
It's partly in the gullet I think. And such tools are claimed to be a
Not for 2 & 3 flute cutters.
Do the calculations.
Do a total cost calculation.
So getting the chip out might be important.
So what, even in cases where true?
Ever heard of a "toolchanger"?
Or of not over-finishing?
For the total production cost dollar?
I did say Aluminum IIRC.
Or tumble them back in?
Shut own machine & change inserts or just call for a toolchange?
Easy to test on the machine if you have some stock to touch. IF it
matters all that much (roughing).
Might be stiffer/stronger too.
So use 4 fluters in routers too, right?
IOW Not to see & try ......
Not if you can change cutting parameters such a DOC & IPR.
There are other limitations.
Remember that the task is material removal.
.050 IPR, 20,000 RPM, 10 mm diameter cutter.
DOC probably .5 to 1 diameter.
That chart seems unclear.
For single-pass & roughing.
Someplace they list tools by material. For Aluminum roughing only
single-fluters were suggested IIRC.
> So the conclusion I draw from these calculations is that a router bit
>can only be feed at 1/2 the feed rate of a 3 flute end mill.
> Now, that's just theoretical calculations, if someone can produce some
>verifiable evidence that router bits are more productive than 3 flute
>end mills - I'll be more than interested in seeing it.
Well I'll have to admit that .050" sure sounds like a healthy chip
load alright. I wonder if they are actually achieving that in their #1
video. If their machine had a 1G acceleration I figure it would take
like... (32 feet per sec. = 384 inches per sec., 1000"/384" = 2.6 sec.
to get to full speed) and the tool has to decelerate at the same rate
since they are stopping at the top to stepover in Y. But it's big chip
load in any case.
I've never heard of this Rocky Mountain Tool Co. Perusing their
web-site, they seem to be a distributor for some more recognizable
brand name tools, and they appear to do resharpening.
I find it odd that Onsrud (Which IS a well known and respected tool
manufacturer) doesn't recommend anywhere near a .050" chip load for ANY
of their router bits. In fact the most they recommend is .020 and
that's for a 3/4 dia. cutter. On a 3/8" dia. router bit (closest to
10mm) they only recommend an .008-.010 chip load.
Also in the #1 Rocky Mountain Video it looks like the tool is going no
deeper than about half the tool diameter, or about .2 deep.
Here's some info about a 2 flute end mill from Helical Solutions.
Crafted of certified premium sub-micron grain carbide, the H35AL-2R is
ideal for roughing and slotting applications and is available in stub
and regular lengths. In testing with tool path optimizing software
cutting 6061-T6 aluminum, this end mill achieved 1,000 ipm, compared to
the 300 ipm for aluminum cutting tool designs previously available in
The test conditions were 1 in depth of cut, ½ in width of cut, 12,000
rpm and .0277 in chip load per tooth. This 100 cu ipm metal removal
rate was achieved with a mere 10 percent load on a 20 hp (14.9 kW)
vertical machining center. Over time, putting less stress on the
machine results in longer machine life and longer tool life.
So if the claims for this "Helical Solutions" 2 flute end mill are
valid, it seems to be cutting approx 5 times the depth of the Rocky
Mountain router bit, and with the .0277 chip load times 2 it would be a
.0554 chip load per revolution or 10% more than the single flute router
I don't see any speed or feed data at the above site you listed.
I don't see any specific feedrate data at this site either.
Ahh, now this one has some data. 15,000 RPM and 500 IPM gives a .033"
chip load per revolution for one flute. Pretty speedy, but still not
up to the "Helical Solutions" 2 flute end mill with .0554 per revolution.
So far it looks like the 2 flute end mill is in the lead.
Actually, my first choice would probably be a 3 flute end mill with a
.010 chip load per flute and at least twice the depth of cut as the
router bit. It seems even that would end up with a higher material
Opps sorry, wrong bait to catch a BB-halibut.
IMO, attempted insults & appeals to emotion aren't constructive in
an objective evaluation of cutting tool properties.
From the pictures at the Rocky Mountain site (side view and the one at
the upper left of the site), with the deep gullet the cutter "looks"
pretty wimpy. Maybe that's why they were only taking about half the
diameter for a DOC in their 1000 IPM video. Plus it has to have a back
relief of AT LEAST .050" so the back of the cutter doesn't drag. But a
cross-section end view of the different cutters would sure be helpful
to estimate relative core strengths, between the 1, 2, and 3 flute tools.
But they make router bits as well, and they didn't suggest using them
in their ad.
Like I said, it seems like the end mills are in the lead in this horse
I don't know, the router bits "look" weak from the pictures, and that
.050 chip load slamming into the part like a hammer just seems like it
would be deflection city.
Well, if someone sent me a couple I'd sure go to the shop and give
them a test run. I LOVE testing stuff to destruction. LOL
I thought that sounded a little odd at the time. I figured the they
must have made a misprint on the HP percentage. But let's do a little
rough horsepower calculation:
MRR = DOC X WOC X Feedrate (number of flutes or RPM doesn't matter)
HP = MRR X Unit HP (.25 for aluminum)
Using their above "Test Conditions" from the article:
1" DOC X .5" WOC X 1,000 IPM = A MRR of 500 cu. in. per minute.
500 MRR X .25 = 125 HP Yikes! THAT's unlikely.
The article itself says it was a MRR of 100 cu. in. /minute - so
there is a discrepancy right there.
So much for truth in advertising, eh. LOL
There needs to be some independent verification of all these
Yeah, you're slackin' dude. You'll never get above 250 political
troll posts in this weeks statistics at this rate.
My original point being, the HP difference should be inconsequential
if the DOC, WOC, or Feedrate remain similar between a 1 flute end mill
or a 3 flute end mill.
Sure, what particular limitations are you thinking of?
The above is a video of a regular end mill milling away on a part.
I'm not sure what relevance that has toward your contention that 1
flute router bits make better roughing CNC roughing tools than end mills.
Yeah, the DOC "appears" to be about 1/2 of the diameter. But I'm
still not positive they actually reach their full programmed 1000 IPM
feedrate. Perhaps they should have done a spiral out instead of
stopping X movement at the top of the circle to stepover in Y on every
I don't know. Seems pretty straightforward to me. It's a chart of
their recommended chip load per flute in cutting aluminum for their
their single flute cutters. Only single flute cutters were listed
because that's what the chart was about.