I’m trying to figure out the largest and best bit to quickly hog out some pockets without destroying my router and machine. I’ve been using my 1 1/4 spoilboard bit in mdf lately but i feel like that’s probably not ideal. Anyone have any thoughts on what works best? This will mostly be for MDF and my wood projects usually don’t get quite as big. Any advice would be appreciated, thanks!
Hey Cameron,
this has been a topic here frequently.
The short answer is, the Makita is a hand trim router for short-duration, hand-held usage, as often stated in this forum, e.g. here and here. The bits that are sold by the manufacturer do not exceed 1/2″ but you will find that nonetheless many in this forum use bits of up to 1 1/2″ to surface the wasteboard, simply because they have no other milling motor and don’t want to wait this to be done with a 1/4″ or 1/2″ bit, and it works because surfacing is removal of only shallow depth, but using bits larger than 1/2″ is nothing that is good for such a hand trim router if you do it more frequently. The Makita hand trim router is a so-called carbon-brush, commutated series-wound motor, also called universal motor, whose speed, unlike the speed of a spindle on a VFD, is dependent on load (slows down under load), and the larger the bit diameter, the higher the load and the higher the current, and this at a lowering speed. It has been stated more that once here that when you burn up your makita, it’s usually while using a large diameter bit.
Milling pockets is usually not done with large diameter bits, as discussed here. Usually you do this with 1/4" or 6 mm – 8 mm end mills at high speed (24,000 rpm). I think this video (english version of video here) which tells which bits and which speed they used is able to give you an idea of what to use when milling pockets into wood.
If you’ve done surfacing with a 1 1/4″ bit, what do you expect from another bit?
Welcome to the forum!
EDIT: Updated to provide the link to the video in english
1 Like
My issue isn’t surfacing, it’s cutting a really large pocket with a 1/4 bit takes an eternity. (3ftx3ft). I actually haven’t had many issues using a surfacing bit for pockets other than the router getting hot, but I’m trying to find a better sweet spot between speed and longevity of the router and I wasn’t finding much about it.
Hey Cameron,
yes, talking about pockets. The power of the Makita is rather limited, both by the type of motor that it is and by the weak power rating too, that’s why it is not advisable to use bits larger than 1/2". Did you try to increase the speed and change your feed rate and your depth of cut?
What do you think of the values used in the video?
I guess what I’m trying to ask is can I reliably push a 3/4 or 1/2 bit through a sheet of mdf as a more long term replacement for the 1 1/4 bit I’ve been using. I’m not as worried about eventually burning up a router as they are cheap enough that the amount of time I save would more than pay for a new one.
Ive been running it at 80ipm at 4 on the Makita router at .09 depth, nothing too greedy and it actually works really well, just trying to improve my workflow because I have a lot of stuff to cut. I wouldn’t try that in real wood, but in mdf it’s been just fine.
Hey Cameron,
on the web, there are a lot of tables for cutting parameters, e.g. this one here that includes wood as material and also refers to pockets (PDF).
Usually you can have more succes with higher speed rather than taking a larger bit diameter.
The only serious answer to this can only be that if you want you pockets reliably and quickly, don’t use a hand trim router. But I assume, this is not the answer you are looking for 
Ok when sticking with a 1/4" that you own, did you try to increase the speed and change your feed rate and your depth of cut?
What do you think of the values used in the video?
What you are looking for is material removal rate, you can achieve the same rate with smaller bits and larger depth of cut/stepover/feed rate in many cases while requiring less torque from the router. Ideally you want to run a bit that has a helical/spiral cutting edge vs a straight one as it keeps more consistent force on the cutting edge and router. The challenge is those cutters are usually the same or smaller than the 1/4" shank diameter the Makita router can accept. You can use a 1/2" straight cutter with a 1/4" shank with larger stepover/DOC/Feed rate but I wouldn’t go larger than that with the Makita router, it doesn’t have the horsepower required for larger bits.
2 Likes
Hey Cameron,
also if you want to remove large amounts of material as the first step, you usually use a roughing cutter. It is made for an increased MRR and better chip evacuation.
Thanks, appreciate it. Just trying to push the limits, time is money and I’m low on both 
.
Hey Cameron,
this I understand very well . But a good roughing cutter could be what would be worth it for you. Unfortunately I only know sources in my region but I’m sure there are similar in your region
1 Like
Hey Cameron,
here you can see a video of the 8 mm Sorotec Roughing bit in action while milling black locust (an extremely hard wood) (and here the project behind the video)
Hey Cameron,
just in case you don’t buy some new bit, just a little improvement, assuming you use a 2-flute endmill, according to the formula linked above, I get 124 ipm (3.2 m/min.) with your 1/4" (6.35 mm) bit and 22.500 rpm for MDF material.
22.000 rpm would be “4” on the Makita (but as explained above motors like this do not reliably hold that speed).
However with a roughing bit you could increase feed rate.
1 Like
I usually run my 1/4in bits at 160 because that’s what the manufacturer said to use and have never had any issues. I run my 1.25 at 80 because the router gets hot at higher speeds. At 80 it stays half way cool and seems to work ok. I’ll look for a roughing bit and see if it’s right for my application, looks good though.
1 Like
Understood, I run the 80mm spindle and 0.5" upcut bits with climb milling for most roughing operations in wood.
Material removal rate examples assuming a 50% stepover, I generally would not use a stepover less than 50%.
MRR = stepover * depth of cut * feed rate
MRR using 1.25" surfacing bit = 0.625" * 0.090" * 80ipm = 4.5 cubic inches per minute
MRR using a 0.5" upcut bit = 0.25" * 0.25" * 80ipm = 5cu in/min (you could increase this feed rate)
MRR using a 0.25" upcut bit = 0.125" * 0.25" * 160ipm = 5cu in/min
This ignores acceleration but you can see that using smaller diameter tools can yield similar MRR. The 1.25" surfacing bit requires more torque of the router than the smaller bits at higher feed rates and DOC. This is how I landed on the 0.5" tool as the sweet spot for this setup as the 0.5" tool offers better rigidity than the 0.25" and the slower feed rate helps minimize the effects of acceleration, I will run the 0.5" with a feed rate of 120ipm.
2 Likes
The manufacture settings are only place holder settngs that are generic to all machines and are by no means the correct settings you should run for your machine. For every cut you should use a chipload chart to determine the speed you should cut depending on bit size,. flute count, rpm, and hardness of wood One setting does not work on every piece of wood or material each type has a different setting. https://informatyksiedlce.pl/_PROJECTS/feedrate_calc/index.php?lang=en&feedrate=ipm&chipload=in%2Fflute&settings=Save this is an online chart that I use to determine chipload. The makita router has a butter zone of 14000rpm or 2.5 on the dial. This is where the router will have the most power. This is the rpm you need to use to set up all your bits using a feed rate chart depending on how hard to the wood is. I also recommend watching Calculating Feeds and Speeds A Practical Guide | Wood CNC Router - YouTube and What The Chipload Formula Does Not Tell You! | Advanced CNC Router Lesson - YouTube to understand chipload better.
3 Likes
The makita router does not have enough hp to push any bit bigger than 1/4 for anything more than shallow cuts for very long. Not saying that it can’t do it, I am saying it will not last for long and the router will burn up. People who do not use chipload charts and do not set up their bits are fooling themselves in thinking that they are not wearing their bits out faster than they should and are also wearing the machi9ne out faster due to stresses that are not present when the bit is setup correctly. You will find that clearing out at 280ipm with 1/4 can go pretty fast.
i use those charts for most things, but cutting a 1/4 deep cut in mdf at 400ipm seems excessive. Are people having luck cutting cutting that fast and deep in mdf with a makita router?
No the the fastest the machine will go is 398Iipm. This is why you would want to drop the rpms down to 12000 or 2 on makita and run it at 312 which is the same chipload as 18000@468
@JDog agree wholeheartedly, staying in the correct chipload range is key to good cuts and bit life.
I check my bit temp to see how much it rises above the material surface temp whenever doing new speeds n feeds or material or bit. For almost everything* when i use the charts from the manufacturer or a reasonable approximation, I see 4-5°F rise on the bit. From my experience, if my bit is uncomfortable to touch after a cut, I need to adjust my feeds n speeds—and generally faster, not slower.
The good news is the onefinity is stiff enough to handle good chiploads on all the bits I’ve thrown at it. Picking the bits the makita can handle means I’ve not had any issues in tolerances, stalling, etc.
The exception is my Whiteside surfacing bit…that gets a 15+°F rise. The only times I get reasonable temps is when I take a big DOC on it, which runs counter to me wanting to surface a tiny amount to flatten waste board or inlay surfaces to make sure their are flat. I think it’s a combination of the 1” diameter, slow rpm and ipm, and small DOC so that even with a 80% stepover, not making enough chips to take the heat away.
*the real exception is my 30° amanan v bit when v carving inlays. High rpm, low ipm to finally get little/no tear out. Whenever I tried to hit chipload numbers for high rpm, I was breaking off small bits on the inlay/pocket. This one I run for inlays at 20k rpm and 35-40 ipm. Good news is I still see a very small rise in temp.
3 Likes