I’m new to CNC in the last year and have been chasing this question as well.
I am mostly working in wood, especially plywood as I am making larger things like cabinets and furniture pieces etc.
Before you even worry about bits, I’ve learned that making sure you have a decent quality material is key. I recently got a piece of poplar plywood that turned out to be quite a bit older (I should have checked the sticker on it) and if you looked at it sideways it chipped. It cut fine on the Shopbot 4x8 I was using, but once I took it off the table, the problems started. The bottom line is that I’m going to likely have to re-do a big part of that 4’x8’, 1.5h job because the material was dodgy.
Once your design is dialed in and you’re confident in the cut, definitely us a good quality material for serious projects or you’ll go down the time/cost rabbit hole.
I agree with Chris, when starting out use low cost bits even if they wear out quicker. I bought a very nice $80 compression bit from Canadian Woodworkers and it worked beautifully for the first sheet I cut, absolutely flawless, until about 85% of the way through the job I ran it in to a screw due to a zeroing error that cause me to end up in my “keep out” area at the edge. That sucked, but thankfully no one was hurt and nothing else got damaged.
The three main types of bits for basic wood cutting (versus sign making or carving) are:
[EDIT: I should mention all of the bits I’ve used so far have been 2-flute except the tiny one I used for cutting text]
UP SPIRAL (aka Up Cut) which pulls the material upwards. This will usually leave a rougher edge on the side you are milling and often will catch and tear any veneer or cause chipping on edges. It’s best suited (in wood) for when you are milling the bottom of something and the finished side is face down. As it goes through the bottom it will continue to pull upwards and give you a nice clear edge/finish on the bottom. For me, since I usually mill from the top down, up spirals are not really useful in wood where you want a nice finished surface. If you were rough cutting something it might be fine, and I can’t comment on how it performs in metals, plastics or foams.
DOWN SPIRAL (aka Down cut) - These compress the material downwards as they enter and cut, pulling the chips in to the cutline. This results in a nice top side finish but will generally cause a rougher bottom cut edge (although that is mitigated a bit by the spoilboard pushing back against it - the same idea of clamping scrap wood under something you drill through to prevent tear out). Down spiral bits are a good choice for milling the top of wood and getting a nice clean finish. However, because they pull the material down and pack it in to the cut line you need to be more careful as things will heat up and since the cutter has more material to push through, even if is loosely packed, feeds and speeds can vary.
COMPRESSION ENDMILLS (aka Compression bits). These are neat, they are a combination of up spiral and downspiral bits in one. The first portion of the bit, often 1/4" or 3/8" are in the up spiral cut pattern and pull up, and the remainder of the bit is in the down spiral profile. These bits are ideal for when you need a good quality finish on both sides of the material. When they go through the bottom they are pulling up, giving a good bottom finish. The challenge is making sure your tool path enters the wood correctly so you get a clean cut on the top. You must make sure the bit enters the material to a depth past the up spiral only portion, otherwise it will behave just like an up spiral bit and potentially damage the top side. You can either plunge the bit in (some people say this isn’t ideal for compression bits, but I am not sure this is correct - I never seem to get the same info twice when I ask CNC questions) or you can bring the bit in from the side (either from an edge). Since compression bits both pull up the material and push it down, it gets VERY TIGHTLY PACKED in to the cutline. Like you may need to take a flat head screwdriver and scoop it out/loosen it before you can really get much of it out. Knock the piece lightly will only shake a small bit loose. So there is a bit of work to do before you can get in and cut the tabs to finish the piece by hand once the CNC is done with it and you need to remove the tabs. Also, you need to watch feeds and speeds like a down spiral cut because it gets warm in that cut line too.
Some compression bits have a fairly short up spiral and are referred to as mortising compression bits. Essentially you can use the end to cut dados or mortises without engaging the downspiral portion. I’m not sure why you could’t also do that on one with a larger upspiral portion or if there is something else different about it.
I’ve read that compression bits are capable of doing full depth or near full depth cuts on large rigid commercial machines at incredible speeds. I’ve seen people talk about running at 300 inches per minute or more at 3/4" depth for single pass cutting. Obviously not something a Longmill is going to do.
What I did on that recent 4x8 full sheet project was I used Fusion 360 to tell it to plunge the bit in to the waste area between parts in my layout (I used a 32mm space between parts, still experimenting with what works there but 32mm was pretty good). Once it was plunged in a bit I had it ramp downwards to my desired depth and then it moved in to the actual outline profile cut at a depth that insured no tear-out in the part it was cutting. It didn’t take too much work to set up and I had virtually perfect finish on the parts during the cuts.
I can look at my fusion design and share my settings if you want. It was a 1/4" compression bit from Royce Ayr (what Canadian Woodworkers stocked and said was a good all-purpose, every day cutter): http://www.royceayr.com/en/products/standard-tooling/router-bits/solid-carbide/wood-wood-based-material/r60-120
It’s not optimized for Plywood but their site says it is good (middle ranking) for plywood and also good for various other materials.
Sizes are interesting. The makerspace where I use the shopbot recommends a 1/4" endmill but allow up to 1/2". I’ve used all the way down to 3/16" to do some very fine lettering. I notice a lot of the hobby machines lean towards 1/8" bits. Obviously you have twice as much waste material with a 1/4" bit but you can also increase your feeds and speeds as well - if your machine will support it. Also, depending on the detailing work and your design, you may need a 1/8" bit to get in certain spots.
FEEDS AND SPEEDS
This is the area I’d really like to learn more about the Longmill’s capabilities, both as a system and the details of the motors and the wheels etc. I saw a reference to the power supplies being able to support up to 4A on the motors but that they are set to 2.5A for the current design. It is unclear if you can or should send more power to the motors included or if it requires an upgrade and what that might enable for cutting speeds.
Here is an example of a more rigid machine but also using a trim router, cutting 3/8" depth through birch for a sign at 300 inches per minute (!): https://www.youtube.com/watch?v=SueCf171rdI
That video definitely made me wonder what the upper limits of the Longmill might be at the same depth in the same birch plywood material. For comparison I was cutting 3/4" poplar plywood with a 1/4" compression bit in 2 passes (so ~10mm/each) at 180 inches/minute on the Shopbot which is a ~US$23K machine. It will be interesting to see just how far we can go with the Longmill. given that it is <10% of the cost.