Hello,
I need to make a two-inch deep cut for a project, and my bits are all too short. I know (think) I need a three inch bit (one inch in the collet and two into the wood), but I am not sure if I can make a cut deeper than the flute length. If anyone knows of 1/4, 1/8, and 1/16 endmills that would be able to cut two inches deep please let me know.
Thanks
Ali Ghafuri
Hi @Ali,
It’s not recommended since the shaft will rub on the wall, but sometimes…it’s not that big a deal and it just works
For 1/4" they exist (here’s an example of a 1/4" endmill with 2" length of cut, but that’s from my local supplier so you would need to find an equivalent somewhere else), for 1/8" you may be able to find them but you will need to be quite careful with the toolpaths to manage deflection (which can become a significant concern at 2" stickout on a 1/8" tool). I don’t think you will find a 1/16" endmill with such a long length of cut, it would break upon just looking at it the wrong way.
Is it a 2" deep pocket you want to do, or a cut through 2" of material ? (in which case you could consider doing it as a two-sided job, and carve 1" from each side)
I have a Melin bit that is 1.5 inch cut depth which was discontinued but here is some bits from their site that are 1.5 inch cut depth and 4 inch OAL. They are not cheap but there are bits available.
Name EDP DIA SHK LOC LBS OAL Fl Corner QtyOH QtyCA Expected List Code
| EMGN-.250 | H0129 | .250 | 1/4 | 1.500 | 2 | 4 | 3 | SQ | 10 | 3 | $40.74 | P1C2 | |
|---|---|---|---|---|---|---|---|---|---|---|---|---|---|
| EMGN-.250-ALTIN | H0353 | .250 | 1/4 | 1.500 | 2 | 4 | 3 | SQ | 1 | 0 | 3 Days | $45.72 | P1C2 |
The community has some notes on long endmill options at:
Amana has a pair of extra long 1/4 end mills with reduced shank, 3 flute flat and a ball mill. They go to 2.75 cut height I believe.
You are limited to how deep you can go with what tool you can procure. Find the best cutter for your material, research how deep you can go with what size is available. Options include two sided carves, or slicing your part into manageable sections and joining them together.
Extra Long 1/4 shank Amana Flat
Extra Long 1/4 shank Amana Ball Nose
I have this thing
Which allows me to cut quite deep into the workpiece, 62mm of flute and a good 70mm of stickout from the collet.
However, when you actually use it, terrifying is a good word. The amount of vibration, tool flex and noise when the end of this cutter is in the wood is quite something. You really can’t cut at anything like the rate you would with a shorter cutter and the finish takes more passes to clean up properly.
Larger diameter cutters significantly reduce the tool wobble, if you can go to 8mm then do so, I run 1/2" cutters longer than this and they’re fine but down at 1/4" not so much.
If you can flip the piece as suggested above and machine from both sides, do that, at least for the roughing out and then maybe a final finishing pass using a long cutter.
I’d also recommend only using the long cutter for the parts of your toolpath that really need it.
Agreed. It would be nice to have a list of 8mm tools which folks have found useful in the machines. Thus far I have a rounding endmill and a downcut.
Elaire Corp. sells an 8mm (5/16") collet which fits the Carbide Compact Router as well as the Makita at:
Agreed, 8mm is a substantial upgrade from 1/4" when it comes to cutter strength and vibration. It also brings the SFM up at the same RPM.
I have one of these in 8mm x 42mm flute
Which does an excellent job on plastics.
I also have these in 8mm
https://www.shop-apt.co.uk/3-flute-carbide-end-mills-for-aluminium-45-helix-uncoated/3-flute-carbide-end-mill-for-aluminium-8mm-diameter-45-helix.html
Which is a bit on the small side for 3 flutes in aluminium without air blast but I generally use it on the outside rather than opening a pocket where a single flute clears better.
They both do an excellent job of turning aluminium into chips, they also have a pretty decent finish on the bottom of pockets.
Worth noting though that at the 8mm and 10mm sizes running your router at full speed results in too high a surface speed for cutting aluminium without significant heating so you’re trading flutes and diameter for RPM on these cutters.
Not sure, I’d normally redirect that question to you 
I thought there was a surface speed issue where if you ran too high a surface speed you got heating of the workpiece (which I definitely do on aluminium if I run the spindle flat out on that 10mm cutter). If you have the machine rigidity and spindle power to keep cranking it up you can get to the other side of the hump where HSM happens and the temperatures come back down as per the graph here
I borrowed this book from a local university in an attempt to better understand HSM (and ultra HSM). I suspect that @spargeltarzan knows a lot more about this than I (or BW) do, but my takeaway was that increasing cutting speeds is generally a very good thing, especially for wimpy machines:
Some time back I used one of these:
With these (reasonable Shapeoko?) parameters:
And achieved these results:
In my router table with a Porter Cable Model 8902 120V 12Amp router:
ABDF0500J2AS.zip (1.5 MB)
Maybe @spargeltarzan will add Kennametal to his tool library!
Kennametal has an app that shows recommended and acceptable operating ranges for their products. IMO (albeit likely quite naïve), it seems important to use tools that were designed to optimize performance for the task at hand.
That screen grab from Millalyzer is a bit small to read the parameters on, do you have a larger one pls?
Is this a full-depth slot (cutting through the stock) or a pocket?
For a pocket, it is possible to avoid rubbing by shifting each depth pass away from the wall, that is, increase the stock-to-leave by a small amount (say 0.1 mm, 4 thou) for each step-down. Then, you would only need a very long flute for a cleanup pass that hardly cuts anything. In any case, I advise against using a 0.25" tool with that much stickout. It may not look like much of a difference, but
If on the other hand, it is not a pocket but a through-slot, I would use the Shapeoko to only mark the contour using a shallow slot with a 1/8" endmill and then cut it out with a saw, as you say it’s wood.
Cutting speed - well, that depends. The OP is cutting wood, and that can tolerate fairly high speeds if the feed is high enough. I run a 12 mm 4-flute at 25000 rpm (vc 940 m/min) for facing operations (less than 1 mm depth), at 3500 mm/min, in pine - so it need not be a problem. I wouldn’t try that in a deep slot where the dust/chips can’t get out!
With other materials, high cutting speed is a mixed blessing, because many metals are rate-hardening, that is, their shear strength increases with strain rate. In aluminium, cutting speed is often advantageous because the heating will soften the material without affecting tool life horribly. However, when looking at the speeds recommended by tool manufacturers, remember that most will simply assume that aluminium is cut with flood cooling or at least MQL, because that’s standard procedure.
Kennametal tools in the library - I would love to, but it doesn’t look like they publish edge geometry, so it would be all guessing. Should you have a contact inside who is prepared to share that kind of data, that would be great! (Rake angles and such are not really secrets, any large shop measures these anyway to determine when tools need re-grinding.)
This topic was automatically closed after 30 days. New replies are no longer allowed.
