Removing a lot of material quickly

Hi All,

I have a SO3 XXL with the Makita Router. It is a stock configuration.

I’m in the process of creating a multi-part mold. During the process of creating the tool paths for the core I observed that the 1/4" flat end mill was removing a lot of MDF from the blank at what seems to be a very slow pace.

How can I speed up the roughing passes? (increase feeds and speeds to what values?)

Increase the cutter diameter and slow down the feeds/speeds? Does such an option exist? A 1/2" diameter end mill on a 1/4" shank that simply hogs out a lot of material per pass.
Thank you in advance!


Which feeds and speeds are you using? If the ones from Carbide Create, they’re quite conservative — try the ones at:

and then experiment to see if your machine / endmill / batch of MDF / finish requirements (esp. when roughing) allow faster: — alternately look into the CNC Cookbook software G-Wizard.

Thanks for the advice.

I have both a print out of the feeds and speeds you mentioned as well as G-Wizard.

I’m still getting my head around G-Wizard, and the fact that there is a huge “unknown” area of knowledge in regards to CNC routering MDF. I have done some scouring for related information, and I am not sure if it is just making me more confused or opening my eyes to the fact that there is a bit more art and science to this when it comes to MDF??

Is it unwise to use a plunge router bit with the SO3?

I found this source) for router bits that might be able to do what I am thinking about:

I have used that bit for large pockets and I am quite happy with it. The pocket walls are nice (in hardwood). The bottom could be better, but you can remedy that by following with another bit. Depending an the tool path and wood 60-80 ipm works fine for me. I have not done MDF with it. Give their tech support a call. They are generally helpful.

1 Like

Tem, the Makita is a router, so use large ROUTER bits (1/2", 5/8" 3/4, 1.0" etc) as a roughing tool and NOT a little 1/4" cutter.

Finish with small cutters (End Mills)

Makes sense?


Thanks Rich!

Maybe, I didn’t explain very well, actually fairly certainly a I didn’t.

After some sleep and a big cup of coffee, I realize that my question should have been about how to define the end mill in Fusion 360 and if the G-code from it will work well, or if there are any particular settings to consider or adjust.

I have found what seems to be some good advice about Milling MDF:

When cutting MDF to avoid rough surface end result.

15,000 to 18,000 at 100 to 120 ipm for hardwood, softwood, plywoods, MDF and melanine.

1/4-inch bits.

Using bits for cutting that are 2 to 5 flute downcut spiral bits. Downcut spiral bits cut the wood fibers down and shear the fibers off against the shape being cut out, hence the cleaner cut. Concerns about the channel left from cutting loading up with chips has never been a problem with good dust collection

For hogging out material for 3D cuts I use 2 to 5 flute downcut spiral bull nosed bit as they do not leave the sharp edge like an end mill will. This results in a cleaner surface for the final pass with ball nose bit, which in turn will leave a smooth finish.

For finishing on 3D cuts I use 3 flute downcut spiral bits. No special reason, just bought all downcut bits just in case.

Number of flutes I use depends on what I can find at the moment. Just like clamps, you can never have too may flutes.

Wood is fibrous, think of it like a lot of pieces of string bundled together vertically as the tree grows. When you cut these they are being pulled apart, so the smaller amount cut off from the whole, then the less likely that the entire piece of string will be inadvertently pulled from the whole [aka splintering].

Do not cut with slow speeds with high RPM. Heat will built up and the wood being cut will catch on fire … and you will feel really dumb and hope that no one is watching!!!

If you really want to know about wood, get this book: R. Bruce Hoadley. 1980. Understanding Wood. A Fine Woodworking Book. The Taunton Press, Newtown, CT. It is absolutely fascinating.

As MDF is like really really solid mash potatoes, if when cutting MDF the result is “rough and frayed” you need to feed a lot faster with a lot more speed [higher RPM] and a really sharp downcut spiral bit.

Also, a really good dust collections system with MDF as well, unless you have an overwhelming desire to vacuum your entire shop and everything in it.

Are you cutting on a mill? That’s very slow for wood, unless you’re feedrates are very slow too. I can profile or pocket cut solid ash at over 120ipm, with 3/8"doc and 13k-14krpm, with a 1/2" 1-flute mortise compression spiral.

Like the others have mentioned, you really need more spindle speed to cut wood. Really for MDF I prefer to use straight flute bits as opposed to spiral bits.

The other thing is machine ridgidity. If your setup is pretty ridgid, you should be able to climb cut all the way no problem. If not, climb cutting can lead to chatter, since the bit wants to push away. You might try slowing the feed and running conventional, to ‘pull’ the bit in the direction of slop.

Also like Gerry said, the geometries of wood bits are different; specifically the flutes are deeper and can evacuate chips faster. The cutting edge may also have more of a rake to shear wood.

If you can’t raise the spindle speed, the next thing would be to try more flutes which effectively does the same thing. But there’s a limit, because as you increase the number of flutes, the gullies get smaller, and therefore less chips get cleared. In other words, if you go too fast at 3000rpm, then your chipload gets too high.

Sometimes for problematic woods, you may not want the deep gullies of a CNC wood bit. A bit made for handheld use might be better because its design limits the size of chips that can be cut (an anti-kickback feature), though you will have to run them slower than a CNC wood bit.

You may also consider getting a downspiral roughing bit, leave a couple hundredths, and do a finishing pass with a 3-flute straight bit or such…

The recommended chiploads are given by the manufacturer. You just multiply the chipload by the PRM by the number of flutes to get the approximate feedrate. So if the chipload is say .003, and you’re going at 3000rpm with a 3 flute bit, you should be at 27ipm, more or less…

•	Use sharp carbide bits on mdf. I use alot of Onsrud cutters and had good results for the price of the cutter. To keep the "fuzz" down I sand cut areas with a 600 grit to close up the cut areas. They almost go glossy with the 600 grit. I lay down a "wash coat" of lacquer which is a precat lacquer thinned 50%. Sand with 400-600 and the fuzzies are not a problem. I do alot of mdf doors and this process has reduced my finish time and made for clean crisp corners and finish. Sealing the cut areas of the mdf is the key to keeping fuzzies away.

•	Southeast tool has an excellent bit!! sharp is the word. edge finish is all of them up, straight, down, compression when used with the material they are designed for and the right feeds are applied

Carving MDF:

vbits 1/4 1/2" wide 60 and 90 degree bits larger for big signs

endmills 1/8,3/16,1/4,1/2 for profiling pocketing and roughing (i like a serated hogger for material removal.

ballnose 1/16 1/8 1/4 3/8 1/6 i use 1/8 and 1/4 the most, some high detail requires 1/16th the larger ball nose make for great texture and rough outs

A rubber pad on the floor where you change bits, dropping them is expensive"


Way to much info (TMI).

So are you set or do you need info/help since I couldn’t find a question it the above text?

Really wish they’d make a chart for the other mill sizes, at least 1/8". I know the nomad has them for 1/8 but they’re very different machines.


I think this might be part of what is slowing you down so bad.
Hog with an end mill, and leave some for finishing.
It shouldn’t need to be nice before the finish.
The Bull nose has more surface area, which will call for slower feeds.


I’ve been lobbying for that for a while, and have been working off-and-on on creating one myself — hopefully now that Carbide Copper is launched, and the probe should be shipping soon (and with it, I guess a new Carbide Motion) we can do a bit more of that sort of thing — I should have more time as well, since I’ve finally gotten my daughter graduated from R.I.T., and won’t need to travel so much (until my son starts doing college visits).

1 Like

That would be awesome, I usually look at the nomad 1/8 and the shapeoko 1/4 and kind of average them and it’s always worked but a chart would help confidence level a lot. After that would love some improvements to CC but I bet the request list on that is huge :slight_smile:

1 Like

In comparison to what?

The optimal enclosure in terms of space efficiency and linear length for a given volume is a circle — shouldn’t a half circle present less area in this context (than a square/rectangular profile of a flat end-mill)? Or is there something about how the flutes are shaped which results in this?

FWIW, there is a bit of documentation on endmill shapes at: (and more on the wiki, but that needs to be reviewed and re-worked somewhat).

1 Like

Surface area was the wrong term, but you cant go as fast with a ball, or bull nose, removing the same amount of material as an endmill.

I can’t really remember why, maybe cause the flutes are shallower at the curve of the ball on the mill?

1 Like

Thanks. Curious as to what the mechanism is for this (and not remembering if it’s already on the endmills page or no).

Hey Rich,

I think I found more than just a starting point, taking all of this in, I have ordered a few Plunge router bits that should make quick work of the MDF. I will gather up what info I can from the seller and make the next step.
Also, I’ll see what I have to do within Fusion 360 CAM to define the bits, and add those to my expanding to library. I’ve done this with smaller end mills, but the shapes of these plunge bits are a little different.

Everyone, Thanks for chiming in!


1 Like

Actually, now that I think about it, it is the lesser linear area which causes the need to go slow, but it’s one of those counter-intuitive things — because there’s less surface area, the removed chips are smaller and are more centered in where they are taken from, which requires that one go more slowly so as to allow time for the endmill to get back around and remove some more to make room for it to cut.

1 Like

NYC CNC has some great tool library F360 tutorials.

Adding tools is a breeze, and fixing your library to only contain YOUR tools set to YOUR Speeds and Feeds is a great tip that John will show you how to do.