Ok I am about to become the “Feeds & Speeds” preacher. I see a lot questions that really depend on this topic so hopefully this helps… ( I know this became long, but would have been helpful when I started out)
To get a basic idea of what we are talking about, have a look at this video from Haas … yes I know these are metal machines but the principles are the same:
Rough idea of cutting depth is equal to cutting diameter. But… Cut depth 2x Tool Diameter reduce chipload by 20-25%, Cut depth 3x Tool Diameter reduce chipload by 40-50%**
Chip loads:
Tool Diameter
Hardwood
Softwood/Plywood
MDF/Particle Board
Soft Plastic
Hard Plastic
1/8″
.003″-.005″
.004″-.006″
.004″-.007"
.003″-.006"
.002″-.004"
1/4″
.009″-.011″
.011″-.013″
.013″-.016"
.007″-.010"
.006″-.009"
3/8″
.015"-.018"
.018"-.020"
.020"-.023"
.010"-.012"
.008"-.010"
1/2″ & up
.019″-.021″
.021″-.023″
.025″-.027″
.012″-.016"
.010″-.012″
From my limited experience none of these values are cast in stone, but +/- 10% should be a good starting point.
For example, to really ruin your part spin a 4 flute 1" in diameter bit at 30k RPM at a feed rate of 25 IPM, .2" depth of cut. That really fine finish you were looking for just started burning and your $100 bit snapped.
If you have to spin fast, fewer flutes are better. I am looking at Datron SINGLE flute endmills to do Al with a 3HP spindle.
One last comment, in wood when cutting WITH the grain and a “conventional cut” you can get strings of wood coming off. Your cutting action is somewhat like you were using a hand plane making shavings. Either go cross grain or “climb cut” to help the situation.
So please correct me if you disagree… I am ALWAYS learning.
For most hobby machines like the onefinity you cannot really push the entire diameter of the bit so its recommend using half the diameter to start. Their will be exceptions to this rule like compression and tapered ball nose bits but for most endmills you should stick with half the diameter of the bit. With the original onefinity I can tell you that most of your chiploads will be .002 less than what this chart gives but that can very depending on temperature and moisture content. The secret to best chip loads is looking for the coolest bit temperatures. If you pause the cut and router and feel how hot the bit is you will get an idea of if the bit is cutting good or not. You should be able to reach up and grab the bit and it only be warm to the touch. If its hot your chip loads are off. I also made a video about it too so hope this helps as well. Beginners Guide To Feeds Speeds & Chiploads - YouTube
I just watched you video … the info seems reasonable, well done.
All of this info is under the heading of “your milage may vary” but I hope reasonable starting points
As far as depth of cut is concerned, I believe a number of factors are going to be in play:
Machine rigidity … in this case smaller X-Y-Z is likely better, with the 50mm tubes.
Spindle HP.
In my case 3HP spindle (Z-20 mount with stiffy) on a Foreman … I am anticipating 1 dia depth of cut on a roughing pass. But ask me in a few weeks … sold the Journeyman, waiting on the Foreman.
By the way only an induction motor on a VFD (“spindle”) will hold the set speed nearly perfectly independently of mechanical load, up to its power limit, and if you exceed its power limit, the VFD will simply trip and with a correct emergency stop wiring, this will also stop the CNC program (to avoid breaking the bit). On a hand trim router (a carbon-brushed universal motor), you can set a speed according to the table in the manual, but (besides the fact that its rated wattage/hp does not correspond to the effective power on the shaft (with a spindle it should), and this motor type’s much poorer efficiency so is comparable only to a spindle with far less watts/hp than written on its package/homepage), as the mechanical load will slow it down and the more you reach its power limits, the hotter it will get and if you exceed its power limit, you have the danger of damaging it because of excessive heat (up to burning up).
So I think you’re right with assuming that with a spindle that produces 2.2 kW mechanical power at its shaft you can do a lot of depth of cut and width of cut more, thus more material removal rate, than with the router. I think with such a spindle, the bottleneck is then the machine rigidity and not the motor (unlike with the Makita hand trim router, which is the bottleneck then)
Yup agree completely… It is going to be fun finding limits.
It would be nice to see some standardized parts for comparison across machine manufacturer & models. Have you ever seen the computer benchmark tests… Something like that.
(10 mm 3-flute aluminium end mill through an 6061 aluminium block with 1000 mm/min feedrate, 10 mm depth of cut and 8 mm width of cut (for US customary users: 13/32" 3-flute end mill through an 6061 aluminium block with 40 IPM, 13/32" DOC, 5/16" WOC) – It exceeded 10 A (@ three 230 V phases) and with about 150% temporary overcurrent allowed, the VFD did just not yet trip)
