Is this bit the same as a standard down cut?

[Pan (Andy photenas)]

Hi guys I was wondering how this bit differs from the Standard spiral bits the sell out blind?

[wmoy (Winston)]

Not sure which “standard” endmills you are comparing this to, but the 251 is a regular downcutting endmill, just like many others on the market.

[TDA (John Torrez)]

Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.

I’m with Winston here. There’s not really such a thing as a “standard” tool. Downcut is one aspect of tool geometry (helix direction). There are tons of other ones like:

• Rake: Angle of attach of the flute
• Helix angle: How tight the helix is
• Margin: One of the ways the back of the flute is ground
• Relief: another of the ways that the back of the flute is ground
• Core: The amount of material left after grinding flutes
• Core taper: Change in the core across the length of cut
• Flute volume: The amount of room in the flute for chips

There are a lot more than that. Those will change how a tool cuts, the force to make the cut, the amount the tool will deflect, the finish of the cut, usable RPM, etc.

On top of that there is also the grade of the carbide used. And it’s not even close to as simple as “sub-micron”. To give you a rough idea here’s the listed specs of a number of sub-micro grain carbides that are in the K20 ISO spec:

Chinese YG7 T.R.S= 1.9GPa HRA=90

Kennametal KFS06
T.R.S.=3.44GPa HRA=93.3

Ryotec (Mitsubishi) TF15
T.R.S.=4.0GPa HRA=91.0

Those will not deflect, wear, or finish remotely the same.

One of the issues is that almost no one is going to tell you most of those features as it could let someone copy their tool. So in general you only get the bare minimum (number of flutes, helix direction, tip, micron “grade”).

If you want some examples of how some of these change the cut I go into it a little here:

Best practice for tiny endmills

Hi, I’m using .5 mm endmills to cut .15" deep, .5 mm wide slots in hardwood. I’ve seen a few recommendations for spindle rates, depths and feeds here and there but still I snap these things off almost immediately. Can anyone give me a good starting point for best practice on these?

Hope that’s useful. Let me know if there’s something I can help with.

[Pan (Andy photenas)]

Is there a way to learn what type of endmill I should be using on say a lot of small boxes with minimal sanding?

[WillAdams (William Adams (Carbide 3D))]

To reduce sanding, a downcut tool such as the #251 or the #46200-K .125" 2 flute down-cut included in:

Amana AMS-119: CNC 3-PC Starter Pack for Shapeoko

is a great option (and note that that pack which also has a tool similar to the #251, but coated) is described as suited for woodworkers).

[gdon_2003 (Guy Donham)]

As @wmoy said it is standard 2 flute down cut bit. I use it all the time. The only limitation with down cut bits is deep slots the slot can be choked with saw dust. A down cut bit pushes the saw dust down and traps it there. So for deep slots use an up cut bit if possible. The other issue with the #251 1/4" down cut bit is if you have a loose collet or defective collet the bit will be pulled further and further down into the wood due to the nature of the down cut. So make sure you tighten your collet up well with two wrenches on the Makita/C3D router.

The #251 is my go to bit for 1/4" and it works well. Just remember the limitations of any down cut bit. You get a cleaner surface but the sawdust can be a problem. There is cases for both down and up cut bits and make the correct choice for a given situation.

[TDA (John Torrez)]

@Pan

Is there a way to learn what type of endmill I should be using on say a lot of small boxes with minimal sanding?

Part of it will come with experience. However, I’ll try to give some general idea of a few. This will change depending on your goals though.

As an example you said you are cutting small boxes and are concerned about sanding. There a few things I can take from that but there’s going to be options depending on variables I don’t know. To start with I don’t know the material. You say sanding so I’m going to assume that you are talking about wood or MDF. I’ll go into 3 aspects based on minimizing sanding. Deflection, helix, and edge.

Again, this isn’t an exhaustive list, just some examples. All of the below is like for like and assumes no other issue or limit. These are going to be simplified versions and there are exceptions or work arounds that I will not be addressing.

Deflection
Deflection is when the tool or machine are put under enough load they will deflect (bend). This can result in chatter in the cut from the flute(s) being pulled in and out based on the load on tool. From a tool perspective the easy thing to look at to minimize this is a more rigid tool. A tool with more mass left in the tool will be more rigid and less prone to deflect/chatter. So we can look at the tool’s cut length, and core.

Cut length is fairly straight forward. The longer the cutting length the more material had to be removed and the weaker the tool.

Core you will have to guess at based on visuals as pretty much no one will tell you. But an easy way to estimate it is to look down the tip of a tool. If you imagine, or in the case of a picture draw, a circle of it’s cutting diameter (touching the edges of the flute(s)), the more of that circle filled with carbide the more “core” it has left.

Helix also effects this as the tighter it is the less overall mass there is.

I should probably also mention stickout here. While it’s not specifically a tool feature stickout can be limited by the cutting length, carry out, or necking of a tool. The short version is that the more length of a tool sticking out of the collet the more it will deflect. So you want as much of the tool inside the spindle/router as possible without bottoming it out or the collet clamping on something other than smooth, full diameter shank.

Helix / cut direction
The helix is the twist of the flute. The tighter the twist the more it will effect the cut. So when looking at this consider that a higher helix tool will transfer more of the cutting force into the Z. Additionally, it will be pulling or pushing on the material in that direction. That means that you are more likely to chip out or fray material in either the top or bottom (if cutting through) and it takes less chipload (feed) to do it the higher the helix. It also effects the chips as an up-cut will pull chips out the top of the cut and a down-cut will force them to the bottom.

While there are tricks to help with this, in general it means that a down-cut is more likely to recut chips and leave more finishing work on the sidewall and floor of the cut. An up-cut or down cut can chip or fray the top/bottom surface if the material is too weak to resist the force or there’s not enough shear. Which side depends on the direction.

There are also 0 helix or “straight flute” cutters. These have their uses but they are very hard on the machine and cut as you are always engaging and disengaging the entire edge at once. There’s also compression cutters which I won’t get into a lot here other than you have to make your pass depth deep enough to get to the down-cut area to take any advantage of them.

This is one where you are going to be picking where to get better results.

Edge
This is going to be a lot harder to tell. Where things like the rake, edge radius, and relief matter. Probably the best advise would be to find manufacturer(s) you trust and look at what the tool is spec’ed for. There are cutters that are more “generic” or “universal” where they are typically listed for cutting multiple dissimilar materials. There are also be application specific cutters where you will see things like “soft media”, “wood”, “metal” “aluminum”, or “plastic”. They will typically be tuned for either similar or extremely specific materials.

As an example, a good version of these types of cutters for soft material would have a more aggressive rake, a smaller edge radius, relief set to reduce edge contact and help with wear, etc. In this example that would make for a better wood or plastic cutter but a poor or lower tool life metal cutter.

Something like the example tool above can leave a better cut, use higher RPM, and take less force to cut. This assumes though that you’re setup for and running feed and speeds to take advantage of it. It may also cost you something else like tool life.

Keep in mind that even with all the above you still have to have proper chipload (feed) and surface speed (RPM) or you can get a poor cut no matter what tooling. It may also be that the combination or machine, setup, and material makes it to where you can’t take advantage of it. Another thing that you probably noticed in this is that in some cases these are compromises. And another compromise is going to be the time it takes to evaluate and make use of the above. It might not be where your time is currently best spent and there’s a lot you can do modify how you are cutting with current tooling to compensate.

Hopefully that at helped a little. If there’s something I can help with let me know.

[Pan (Andy photenas)]

I’m going to need to read this a few times and then process it! I really appreciate your in-depth answer and will study this until I understand it exactly. Thank you!