I'm lost regarding bits

Technical Details
1

Hey there,

I’ve backed the new Maslow 4.1 Kickstarter campaign and I’m really excited to get it next year !
I’ve started to 3D print community improvements but I’m stuck choosing the correct(s ?) bit(s) to run with the router.

For what I understand, the minimum router speed is 18,000RPM. If I am getting dust, it means the router is spinning too fast or the sled is moving too slow.

Some people on the forum are cutting using upcut bits, some using downcut bits and some using compression bits. Everyone seems to be happy with their bits and the cuts look clean.
If I’m not wrong, compression bit are not really recommanded because it can rise the sled above the material.

Is the official 2 flute upcut 1/4" bit still recommanded ?
What is the difference between a single flute and a double flute (except having twice the amount of flutes) ?

I plan to cut 3/4" (19mm) MDF and plywood.

Thanks for your help

2

ansering out of order

What is the difference between a single flute and a double flute (except having twice the amount of flutes) ?
For what I understand, the minimum router speed is 18,000RPM. If I am getting dust, it means the router is spinning too fast or the sled is moving too slow.

the bite that the bit takes on each pass of a cutting edge is based on how fast
it’s moving (the faster, the bigger the cut), how fast it’s spinning (the
faster, the smaller the cut), and how many cutting edges are on the bit (more
flutes means each one cuts less)

so fewer flutes make it less likely you will get dust.

There is a detailed science behind this that is used by professionals to figure
out how aggressivly they can cut while getting an acceptable life out of their
bits (if they can cut twice as fast, but the bit life is only reduced by 1/3,
that lets them cut more with the same bit. If cutting twice as fast reduces bit
life by 1/2 they still get the same distance from a bit, but get twice as much
cutting done in a workday)

for us hobbiests, this doesn’t really matter, especially in wood. So we can get
away with a very wide range of things.

upcut bits pull the waste out of the cut, but tend to splinter the top of the
cut (especially as they dull)

downcut bits produce the best top surface, but drive the chips down into the
hole/slot.

compression bits work if you are cutting the edge of a piece where you have an
upcut on the bottom to avoid splinters to the bottom, and a downcut on the top
to avoid splinters on the top. They are not a good choice when doing slots and
shallow passes as you end up only ever using the upcut portion whild paying for
the much more complicated bit.

stright bits splinter less than upcut bits but tend to be more noisy as the
cutting edge(s) lose contact with the work and then hit it (while the spiral
ones tend to have more continuous contact, but only if you are cutting deeply
enough with each pass for enough of the spiral to be in contact)

Is the official 2 flute upcut 1/4" bit still recommanded ?

it’s a cheap bit, and as long as you are doing shallow cuts, you don’t need a
longer cutting surface

I tend to get single flute bits, straight or upcut, whatever I can find cheap
:slight_smile:

I plan to cut 3/4" (19mm) MDF and plywood.

the additional glues in the MDF tend to be hard on bits, expect them to wear out
faster, watch for dust, the cutter to just not cut as cleanly, and any darkening
of the cut surface, and change the bit.

David Lang

1 Like
3

Awesome answer, thank you very much !

If I understand correctly, I should go with one of these single flutes:

Router speed should be set to 18,000 RPM (Speed 2) ;
Step down should be set to 1/4" (6.35mm) ;
Feed rate should be set around 40 in/min (1000 mm/min);
Plunge rate should be to 30 in/min (700 mm/min) ;

Am I correct ?
Should I get some 1/8" bits for smaller pockets and joints ?
With 1/8" bits, router should spin faster, right ?

If I want to cut hard wood, I’d better get a double flute bit (keeping previous settings but double feed rate), right ?

4

maslow just posted a video of cutting at 2000mm/m

it’s really going to depend on your wood, you need to experiment.

smaller bits do need to spin faster or move slower (they can’t take as big a
bite out of the wood

I went with a kobalt router from lowes that can spin as slow as 10k rpm and
always leave it at the slowest speed.

step down is something you will need to play with and see what works with your
wood and cutting speed.

the maslow is not as rigid as other CNC routers, so you have to cut
slower/shallower than they can get away with.

with the original maslow, I liked using a 1/2" single flute stright bit cutting
all the way through 3/4 plywood in a single pass :slight_smile:

David Lang

5

I also have a Makita router which can run at 10k RPM. I’ve printed the socket to install it on the M4.1.
Do you mind sharing the bits and the settings you use for plywood ?

Basic formula is: feedrate = chipload * rpm * no_flutes
So, if I’m not wrong, I should get the following rates with SpeTool O flute:

Data Value
Bit 1/4" single flute spiral upcut
Router speed 10,000 RPM
Chipload 0.01 for Plywood (Source)
Feedrate 100 in/min
Max depth (1/4)/2 = 0.125 in/pass
Data Value
Bit 1/8" single flute spiral upcut
Router speed 20,000 RPM
Chipload 0.006 for plywood
Feedrate 120 in/min
Max depth (1/8)/2 = 0.0625 in/pass

But it’s maybe completely stupid :confused:

EDIT: According to this google sheet, chip load is supposed to be way smaller.

Bit diameter Feed rate Speed # flutes Chip load
1/4" 78.74 18,200 RPM 2 0.002
1/4" 40 18,000 RPM 1 0.002
1/16" 150 18,000 RPM 2 0.002

So according to this chart, I should get something like that:

Data Value
Bit 1/4" single flute spiral upcut
Router speed 10,000 RPM
Chipload 0.002
Feedrate 20 in/min
Max depth (1/4)/2 = 0.125 in/pass

What do you think ?

6

Bonjour,
Un post relatant mon expérience sur les fraises et parmètres de coupe. J’ai beaucoup travaillé avec l’ancienne génération de Maslow, et ai commencé récemment à utiliser la Maslow4.
Les défonceuses ayant des vitesses de rotations minimales assez rapides, les régles usuelles imposent une avance et une profondeur de passe importantes, d’autant plus que le nombre de dents de la fraises est grand. C’est la théorie, mais il ne faut pas oublier que la Maslow n’est pas un centre d’usinage ultra-rigide. Je t’invite à ne pas tester directement des découpes avec des passes de 6.35mm à 2000mm/min, mais à y aller plus progressivement pour te faire une idée. A mon sens tu iras moins vite, avec une profondeur de passe moins importante. L’idée est donc d’utiliser des fraises avec peu de dents (1 ou 2). Même comme çà, ca va chauffer un peu, notamment à cause de la colle présente dans le contreplaqué. C’est pourquoi je te conseille, d’expérience, d’utiliser des fraises de bonne qualité: elles dureront bien plus longtemps, les efforts appliqués seront moindres et la précision sera meilleure, et surtout tes découpes seront propres et demanderont beaucoup moins de finitions a posteriori.
Pour résumer: fais tourner ta défonceuses le plus lentement possible, essaye d’arriver progressivement aux vitesse d’avance et profondeur de passe max en fonction de ta configuration (type de bois, rigidité de ton chassis, …) et surtout, n’utilise pas de fraises de mauvaise qualité.

Good morning,
A post recounting my experience with cutters and cutting parameters. I have worked a lot with the older generation of Maslow, and recently started using Maslow4.
As routers have fairly fast minimum rotation speeds, the usual rules impose significant feed and depth of cut, especially as the number of teeth of the cutter is large. This is the theory, but we must not forget that the Maslow is not an ultra-rigid machining center. I invite you not to directly test cuts with depths of 6.35mm at 2000mm/min, but to go more gradually to get an idea. In my opinion you will go slower, with a smaller depth of cut. The idea is therefore to use cutters with few teeth (1 or 2). Even so, it will heat up a little, especially because of the glue present in the plywood. This is why I advise you, from experience, to use good quality bits: they will last much longer, the efforts applied will be less and the precision will be better, and above all your cuts will be cleaner and will require much less finishing a posteriori.
To summarize: run your router as slowly as possible, try to gradually reach the maximum feed and depth of cut depending on your configuration (type of wood, rigidity of your chassis, etc.) and above all, don’t use poor quality bits.

7

The primary type of bit you’ll be using is an end mill, which is meant to clear out material. They are great for most cut types. Within end mills, there are upcut, downcut, and compression bits. Up sends the bits and forces upwards, down sends them downwards, and compression has some of each as a middle ground. Because plywood is in layers, the direction the forces are going can cause chip out and a rougher edge on the outermost edge in that directions. So a downcut bit puts pressure down on the top surface often making cleaner cut edges on the top, but, on the bottom-side, that pressure can cause a rougher edge and chipping since the forces are pulling the plywood layers away from each other on that side. An upcut bit does the same but with the side switched. That being said, I think the effect is significantly less with a downcut bit since your spoilboard is there to stop the layers from pulling away from each other as much, whereas, the top surface with an upcut bit doesn’t have anything really stopping chipping. For that reason, I have been doing a lot of my cuts where I want clean edges with a downcut bit. I mostly use an upcut bit when I don’t care as much about the edge (e.g., clearing out a bunch of material from a pocket). With an upcut bit, sending the chip up allows them to be removed much easier which cuts friction and heat (which will cause your bits to wear out and need replacing faster). Depending on what you’re making, you could most likely get away with just using end mills.

V-bits can really nice if you are interested in making some more detailed cuts. With v-bits, you want to consider the angle of the head (a smaller angle can get into areas tighter) and the width of the head.

Another consideration is the shank diameter. The Dewalt 611 router uses a 1/4" shank. You can get a 1/8" collet as well for the 611 allowing for 1/8" shank bits. The smaller shank can also help make tighter cuts. More often than not, I use the 1/8" collet and bits than 1/4".