CNC End Mills

H

herromynameis

Joined
Feb 21, 2022
Messages
25
Hey friends, I've been looking for a good reference on the essential end mills for CNCing fixed blades. I see countless end mills on makers' tool changers, but have a feeling there is a smaller essential list, similar to grinding belts. Everyone has their version of, "Get yourself a 36 ceramic grit, 120, 220, etc." I'm curious how you would boil this down to maybe 4 or 5 to purchase immediately - For example if I was to guess - A beefy profiling cutter, a refined profiling cutter, a rough beveling end mill, and a fine bevel finishing end mill. Thanks in advance fellas.
 
It depends on what EXACTLY you want to do. What profile including minimum radius. Are you going to do any slotting? What machine are you using? Coolant? What are you cutting?

For cutting steel my go-to source is Lakeside. I have no complaints about how well they cut or last, their prices are excellent, and they are made in America, which is a must for me. For roughing their stubby corncob mills can't be beat.
 
Hey Diemaker thanks for the response! My plan is to mill 1095 annealed 10" max length tactical style fixed blades on a Tormach 440. I would be bringing them from profiling to beveling, all the way to kydex sheath work. The initial plan is to run fairly slow as I have to be fairly quiet, and use TiAlN coated carbide and clear chips with air. Your question about profile radius makes me fully realize why my question is difficult to answer, but I think I'm learning the answer is - "use the thickest and shortest end mill that works". You've solidified Lakeshore as the go-to brand to me now and I'll absolutely use them. I guess I'm looking for more detailed knife-centric advice on the types I need for the different processes. So far my list is as follows for hard critique:

-Profiling (Including weight reduction holes): TiAlN lakeshore carbide 4 flute cutter (or can I just use the side of a ball end mill to save a tool switch)
-Beveling: TiAlN lakeshore carbide .250" ball end mill (Trying to figure out if another size is needed for smooth finish)
-Drilling: TiAlN lakeshore carbide
 
If you are slotting when you profile then IMO you don't want more than 3 flutes unless it is a corncob, which is far better and you can go with 4 flutes. Do get two of the stub corncob, Fireplug, end mills for roughing, you won't be sorry. If you are profiling without slotting then start with 5 flutes, even if 1/8" diameter. They have a thicker core so they are significantly stiffer, and 25% more flutes to distribute the wear. The shorter the better, the less they stick out of the tool holder the better, and the shorter the tool holder the better, especially with less robust machines. Since you are designing things then don't do fractional internal radiuses. Instead of .125" go with .14" or so with a 1/4" end mill. It is just a lot easier on the tool and it will leave a nicer finish. Avoid using ball nose end mills if at all possible, using bull nose end mills that have a large corner radius instead. Feed mills might be a good way to rough the bevels.

Annealed 1095 is soft but if you use enough air to do the job it is noisy. I always use coolant when cutting annealed or other soft steels, generally because I use 1/4" or smaller tools. It certainly keeps everything cooler, adds lubricity, and is better for flushing the chips out. If at all possible I think you are better off using coolant, unless you don't have the guarding to keep it contained.

What software are you using to program with?
 
Ah great great points, Diemaker, thank you. I'll grab all these, thank you sir. I'll also try to find a way to incorporate coolant per your advice. It's curious you mention bull nose for beveling, because it seems most people default to ball nose. I trust you're right. I'm interested in trying to minimize tool swappage as I won't have an ATC immediately. I was thinking about trying to manage multiple tasks with a single end mill, and it looks like in Aaron Gough's video he might actually be using one single bull nose for most of it like what you're referring to - Profiling, weight reduction milling, and even beveling. I've linked it below if you feel like calling me a fool.

Aaron Gough's Video

I'll be using Fusion 360 then sending it through Pathpilot.
 
Diemaker said:
Since you are designing things then don't do fractional internal radiuses. Instead of .125" go with .14" or so with a 1/4" end mill. It is just a lot easier on the tool and it will leave a nicer finish. Avoid using ball nose end mills if at all possible, using bull nose end mills that have a large corner radius instead. Feed mills might be a good way to rough the bevels.

Annealed 1095 is soft but if you use enough air to do the job it is noisy. I always use coolant when cutting annealed or other soft steels, generally because I use 1/4" or smaller tools. It certainly keeps everything cooler, adds lubricity, and is better for flushing the chips out. If at all possible I think you are better off using coolant, unless you don't have the guarding to keep it contained.
Click to expand...
Great advice. When I worked in machining, I generally programmed internal radii at .01" or so larger than the end mill size. Otherwise, it just pauses in the corner and vibrates. You can even see a better finish.


Wondered about the coolant myself. It's much more than just chip clearing.
 
I am fully aware of Aaron's work and have watched many of his videos. He is somewhat active on a machining forum I watch. There are many ways to skin a cat and how we each do it is often a bit different. For roughing softer metals I find corncob mills to be by far the superior route, often even for aluminum. Yes, it is an extra tool but they cut with far less pressure and don't lift nearly as much as finish mills do. While this isn't an issue for the machines I use it often is the determining factor as how fast I can remove metal without the part moving as holding the part is often my limiting factor. Even if you don't have a tool changer the control should have multiple height offsets. Hopefully you can program the machine to go to a tool change location and hold with an M0 so you can swap tools then press the green button to proceed. Some controls will allow this, some won't. My only experience with Tormach is their bandsaw.

A major problem with ball mills on a flat nearly horizontal surface is you are cutting near the center of the tool. Not only is the surface speed of the tool very low but the tool geometry is often poor as there is no room to grind in the proper shape. With a bullnose mill those radiused edges are out on the periphery of the tool so you avoid the ball shapes limitations on surfaces the bullnose will work on, like bevels. You will be able to cut faster and the tool will last many times longer.

I figured Fusion, I have been using it when it was still beta and love it. For the price it can't be beat.

I have tried cutting steel dry with air blast and with full flood coolant and find my tools last longer and I can remove metal faster with flood coolant, same with plastic. I rarely use tools larger than 1/4" and have never had problems with thermal shock. I know the coatings need heat to work properly but they seem to last longer with coolant in my applications.
 
Wow, very well explained on the ball mill, Diemaker, I totally get it. It's a no brainer. I'll take your word for it on the corncobs too. They look downright mean and I'll plan this for my ultimate setup.

Yea it sounds like you can't go wrong with flood coolant. I'll try to incorporate this immediately or at least work towards it.

That's a good point on tool change location being programmed in, and I don't think I can do without a power drawbar right away to make it somewhat easy.

D davek14 I'll make that note on radiusing, thank you.
 
herromynameis said:
It's a no brainer. I'll take your word for it on the corncobs too.


D davek14 I'll make that note on radiusing, thank you.
Click to expand...
How much stress is on an end mill is determined by chip load, at least partially. A corn cob cutter kind of shreds the chips and makes for a smaller chip, reducing chip load.

On radiusing - ya, the only way for an end mill to cut a radius the same size as the cutter radius is to pause in that corner. With a slightly larger radius, it's at least circular interpolating (actually moving to cut that radius) a little bit.


Diemaker - the only time I've had trouble with thermal shock is with a carbide insert cutter. Even those will load up without coolant.
 
You must log in or register to reply here.
Back
Top