[ivandewolf]

I'm just learning, and I'm getting some conflicting information on CNC bits for wood.
The internet tells me 2-flute bits are "Suitable for roughing out material and aggressive cutting"
the internet tells me that 3-flute bits are "Can handle higher feed rates, increasing productivity"

which seems like they are both better for removing material quickly

... ? which is it?

[peteeng]

Hi Ivan - If you look at a tool supplier that has usage info for their bits that will be helpful. I use 1F (1 tooth) tools alot for timber and plastic. If you use something like FS Wizard it will tell you the material removal rate (MRR) so you can compare different settings for feed&speeds and tool types. You also need to consider if you will use parallel bits, upcut or downcut bits... all depends on what finish you want. You need to learn about the chip load and the mm/tooth as if these are not right then you either wear your bit out fast or you choke the tool... The mm/tooth cut is the size of the "bite" of material the tool takes as it moves along. Each tool is designed for a maximum bite. Peter


https://app.fswizard.com/

[joeavaerage]

Hi.
single flute and two flute tools have large gullets and thus can transport chips away from the cutzone easily. They are often used with wood and plastics, and quite widely used for aluminum
'Sticky' grades of aluminum (1000's, 3000's and 5000's) can clog up tools, and therefore single and two flute is preferred for those grades.

When it comes to plastics, they can be a difficult proposition. Some like polyethylene and variants of it like HMWPE and UHMWPE form strings rather than chips and can be a real bastard to machine.
Polypropylene similarly forms troublesome strings rather than chips. Other plastics are very heat sensitive and the chips can and often do weld themselves into a lump, and to the tool or the parent material.
Acrylic forms nice chips, but is heat sensitive, almost requiring flood cooling. ABS is even more heat sensitive. If you are going to get BUE (Built-Up-Edge) where chips weld themselves to the tool, then ABS will be it.

When making small parts in plastic my go-to material is Acetal. It forms nice chips, is not overly heat sensitive and the resultant parts a moderately strong and reasonably tough. If cost is no object then Teflon is good.
It forms nice chips and leaves a silky finish. I use it for epoxy molds. If you need tough then glass filled plastics are worthwhile, glass filled PEEK is especially nice, shame it costs as much as it does.

Three flute tools are most likely used on aluminum, while four, five and more flute tools on steels. A tool with four or more flutes has narrow gullets and will clog up easily. For harder grades of aluminum
like 6061 and 6063 and 7075 the chips are likely small enough that they will not clog in four flute tools. I regularly use four flute tools in aluminum without difficulty, mind you I ALWAYS run flood coolant with aluminum
to assist with flushing chips away from the cutzone.

Four, five and more flute tools tend to have a thicker and stronger cylindrical core, and that strength is required for steels and stainless.

You need to find a balance between chip evacuation and tool core strength. Unless there is a particular need then most plastic, wood and aluminum can be done with two flute tools
which are widely and readily available cheaply. If you need more tool strength then three or better four flute is the better choice. I use four flute tools on a wide variety of metals and plastics,
and almost always with flood coolant. I refuse to put wood anywhere near my machine as the wood fibres react with the coolant and turn into almost a gel that blocks everything in sight.
A real PITA.

Down-cut tools are a little specialist, and therefore more expensive. They are really only warranted and indicated with laminates and other soft materials where you wish to avoid 'feathering' the topmost edge of the cut.
I would not bother with down-cut tools until you have explored the strengths and weaknesses of regular two flute up-cut tools.

Often with tools you may find that one of your regular two (or three or four) flute tools will work with a new material, but may not be optimal. If you do not need production speeds and/or mirror finishes then just use
your regular tools. When you do need production speeds and/or mirror finishes be prepared to pay a fortune until you find the right balance of properties.

Craig

[joeavaerage]

Hi,
this is probably not really important to you if you are cutting wood and plastics but if you ever attempt to cut steel then this will help.

Many end mills are square ended, usually with a centre cutting grind. The issue is that the very outermost tips of the tool are square, and while really sharp are both tender
and wear prone. With soft and easy materials that is probably not an issue, but with steel and stainless it is.

You can buy endmills which are nominally square but have a small radius ground into the very tips, often called Bull Nose tools. This extra process costs, and commonly you will pay a 10% premium for a radiused tool.
The advantage is that the cutting at and around the tip is distributed over a longer path and therefore very VERY much less prone to wear. The downside is that as the cutting is occurring over a longer
path the required torque goes up, so if you have a torque limited spindle you may not be able to exploit these tools. If however your spindle has the torque then pay the extra and get a radiused tool.

I buy 1/8th with 30 thou radius Destiny Tools Raptors and can get six hours in steel with them. The same size tool, but square ground I can get about one, maybe two hours out of. I buy these from the US. Whats going
to happen to the price I don't know, but I certainly cant see them staying the same.

For some while I've been buying four flute Winstar endmills for steel form a New Zealand supplier, CarbideNZ in Palmerston North. They are Chinese made but of very fair quality.
In most cases they are just square ground. A little while ago I bought some local made tools, NZ Carbide, Auckland, and they have a 0.5mm radius. they have been a real eye opener, and despite the cost will be buying more.

Even more recently I had a bloke wondered into the workshop whom has been a pro CNCer for many years. He was all over my machine, very interested. He was so keen, especially when he realised that I am
electronically trained so that I may help him with his stable of CNC machines, has has four Matsurra's, one a huge five axis behemoth, he came back later in the day with a new 6mm endmill for me to try.
It is a Sandvik but branded SECO four flute but with a 1mm radius. He swears by them, and I've been giving it hell in stainless and steel ever since. The radius means the tool is just that much tougher, I've probably had
eight hours use of it already.

They have an intriguing double relief grind on the cutting edges. The first relief grind looks to be a little shallower than any regular singular relief grind I have seen, but about 1.5mm back from the cutting edge the relief
grind takes on a steeper angle for the remainder of the grind. This has two advantages that I can see, it one allows a little more volume of carbide, and therefor strength in the vicinity of the cutting edge. Secondly the
steeper grind at the tail of the relief allows a slightly wider and cleaner entry into the gullet of the flute thereby assisting chip evacuation.

As I posted above, its all about finding the balance of properties, and these 601 (6mm diameter, 1mm radius) Sandvik/SECO are the best I've ever encountered. I now need to see if I can buy more of them. I seem
to recall him saying they were about $38NZD each, which is pretty fair for quality carbide in New Zealand.

Craig