Where to get Endmills: Poll

I'm by no means a pro, but this is all of the information I have gathered AND experienced in the real world. This stuff can be and usually is the difference between a rippled finish and a near mirror finish. It's a lot, but I tried to get to the point with everything. Make your own decisions, but please give it a read.

What kind of aluminum cutting?
For hogging out material, I use diamond coated O-flutes.
For finishing, I use variable flutes.
For drilling small holes up to 5mm, I use a carbide drill bit.
For drilling larger holes, I use a chamfer/drill mill AFTER drilling a pilot.
For chamfering, I use a chamfer/drill mill.

Avoid certain finishes:
TiAlN - Aluminum content will bond to the work piece.
AlTiN - Aluminum content will bond to the work piece.
TiN - Most are made cheaply now and flake right off.

What coatings work:
TiCN - Very low friction, but needs active cooling.
Diamond (2 types) - Incredible durability, but more expensive.
Nothing - Much better than having a coating just for the sake of having a coating.

Flute Count:
- Higher is better for finishing.
- Lower is better for SRR.
- More flutes for anything other than finishing requires a higher speed proportional to the flute count. So 2 flutes at 100 (arbitrary value) would be 4 flutes at 200. This means you need a tougher machine, which is why a lower flute count will favor our hobby machines more.
- Higher flute count end mills are stronger, but have less space for chip removal per flute than a lower flute count.

General:
- Cut as deep as you can in each pass. Take a shallower cut into the material if needed. (Less X/Y. More Z.) This goes into HSM (high speed machining.) The 0.3mm stuff you see on the promotional video for the Mini Mill is a good way to kill tooling and surface finish if you aren't using multiple tools. Cutting deep also preserves tool life by using more cutting length, which in turn, preserves surface finish.
- Use the necessary tool! I've so far used up to 6 different end mills in a single 3 axis job.
- Look into SFM (surface feet per minute).
- Look into SRR (surface removal rate).
- Look into HSM (high speed machining).
- CLEAR CHIPS CONSTANTLY!!! Recutting chips is a tool killer and heat generator (which then becomes a welder). You can use mist coolant, flood coolant, or even just an air blast.
- "Coolant" methods are primary for chip removal.
- Longer end mills exaggerate every issue. Use as short of a tool as you can. (Check out stub lengths.)
- 100% width cut passes suck! Try to avoid it at all cost.
- Cutting aluminum is the same as cutting acrylic and similar plastics.

I use three sources:
Lake Shore Carbide - very wide range. I get my stubs, larger drills, variable, and chamfer from here.
2Linc - diamond o-flutes and nice engravers
Drill Bits Unlimited - You kind of have to know what to get as some of the inventory really is cheap crap. The smaller o-flutes (no coating) are tiers above anything from eBay/Ali. I also get my small drills, small o-lutes, corn/diamond cut and small (sub 2mm) 2 flutes from here.

 

There are a few other things I forgot to mention. I'll directly answer your questions after this.

Ramping:
End mills might not seem to have an issue when plunging into woods, foams, or plastics, but they are meant for side cutting. They hate plunging and hard materials will show this. That's where ramping comes in. The idea of a ramp is to keep the end mill cutting sideways while gradually increasing depth. Depending on the tool, ramp angles range from 2 degrees to 10 degrees. If you have no choice but to plunge, do so very slowly, peck, AND make sure you clear the cut material away.

Corner Radius Tools:
It might not seem like much, but the tip of the tool is what experiences the most cutting force. On a standard end mill, the tip is a very sharp point. This means that most of the cutting force is directly placed on that single point. With a corner radius, that force is spread out among the radius of that edge. This greatly increases tool life.

Depth to Diameter Ratio:
This really depends on the flute profile (count and angle), but a tool can not effectively clear material after a certain depth. You also will not be able to aid in chip removal with coolant due to the fact that you can't actually get it into the cut. In this case, you have to make a cut much wider than your end mill to allow material and coolant to work around the sides of the end mill.

Work Hold Down:
This is probably the most important out of EVERYTHING. If you can't hold it, you can't fully utilize your machine. The cutting force can be surprisingly large. If you just can hold it, your only option to use a smaller end mill.

Expensive vs Cheap End Mills:
It doesn't matter if you break them. I don't know if we can break a 1/4" on our machines, but 1/8" isn't an issue. Due to that "safety" feature, that's the size where you can really push the limits of the end mill. The way it reacts is going to directly translate to identical, but larger versions of that end mill (or anything sharing that flute profile.) You'll see that many manufacturers charging $100 for what you see in the links for $20 is stupid. They won't realistically last any longer or produce a better finish. The Chinesium end mills are a different story. Just don't. When I saw Lake Shore mentioned on NYCNC, I thought to myself, "yes! I was right!!!"




If your cutting 12mm thick aluminum, you'll be there forever with a 1/8" (3.175mm). If you can hold the work piece down and have space for a larger 1/4" (6.35mm) end mill, go that route. It will sound a lot more terrifying and will put a much higher load on the machine, but you will get it done much faster.

How are you holding the piece? Are you holding the finishing product or do you plan to hold the material and simply use tabs? If you can hold the finish product instead of the surrounding material, then you should make a rough wide cut around it. After the rough wide cut, come back with a finishing pass of at least 0.5mm. This is what will kill the waves caused by the initial chattering. To achieve the wide cut, you can spiral into a spot and HSM at various depths around the part. The second way is a full width cut. This is the tool killer and machine stresser, but it's faster. You essentially make two rough cuts, and outer and inner. The outer would be done at full diameter, while the inner can use a step over. Doing both outer and inner at the same time per depth allows for chip removal. going outer at full depth, then inner at full depth is a welding situation due to no chip removal beyond the first 1/4" or so.

I wouldn't use a single tool. You'll find that the end mills can effectively clear material away until they are pretty much dead, but the surface finish goes down gradually from the start. Dedicate one for MRR (I said SRR in the last post. It should be material removal rate. I'll edit that.) Dedicate another for finishing.

I have the 1/4" version of that particular variable flute you linked to. It is supposed to be good for MRR, but I use it strictly for finishing. I know my machine can't run hard and fast enough with three flutes for MRR. The wheels begin to lift out of the track. There's a good chance that yours may as well. That's why I simply stick with the o-flute for MRR.

As for speed, I run the same o-flute that I keep mentioning at 900mm/min with a 2mm step over and 2mm DOC (depth of cut) at 20k rpm. I was limited to a palm router...and then I killed it with aluminum. (Sparks started flying from the commutator. It was quite interesting.) With a 3mm o-flute, I believe I got to 500mm/min with a 0.4 step over and 1mm DOC at 22k rpm. (I honestly forgot as I jumped up to the larger mills with HSM ideas around this time.) My last safe recording (not HSM based) was 500mm/min with a 1.2mm step over at 0.6mm DOC at 22k rpm. All of this is under flood coolant, which removes chips and keeps it cool. Everything changes when you remove coolant.

One major thing to keep in mind is that the ideal chip load isn't always attainable. There are plenty of factors from every single machine that make the same exact process different. We have to compensate by going a little higher in rpm or lower in speed. The type of chip removal setup plays another huge role. WD-40 is NOT a solution to anything other than to break rust from a squeaky door hinge. It doesn't hurt (much) to start a little slower and slowly ramp it up. Keep an eye on the end mill itself. Is it still straight, or is it causing flex in the gantry? Once you've hit that point, you can do the rough math and see just what kind of load the machine can handle.

If someone else wants to jump, please do! I'm not one to provide direct answers, just the information to get to it. From my perspective, knowing how and why something works is way more powerful than knowing that it works.

 

Will do Gary!

I can't talk without showing something though can I?

This piece ultimately became scrap since I nicked it from the other side, but it shows pretty much everything I talked about. Keep in mind that it is a bit dirty and oxidized from sitting for months. It also reminded me of another detail (see below). For reference, the holes are 4mm in diameter. The channel around the part is 8-9mm (can't remember exactly) to compensate for chip removal with a 1/4" (6.35mm) end mill.

This part was made with:
- O-flute for clearing and rough finish
- Chamfer for...chamfering
- Drill for...drilling
- Variable flute for finishing

But it also shows:
- use of multiple tools
- work hold down method. Showing a little skin isn't bad.
- direction of cut. Notice how the scrap is wavy, but the part is smooth.
- depth of cut
- wide outer pass to create the channel for chip removal


I'll add a few extra details about each aspect to the main post.

- A deeper cut means less lines on the final part. A finishing pass is one way to compensate for this. I make my finishing passes at full depth. This eliminates possible alignment inconsistencies in the finish. (I have pictures of this too.)
- For work holding, you can use a vacuum or a clamping force, but some parts are too skinny. In this case, I used a skin. The skin was later removed when the part was finished from the other side.

Direction - Climb vs Conventional:
Some materials don't care what direction the end mill moves. Some will cause the end mill to chatter. Some will flex the end mill. Each material is different and has it's own requirements. Just like everything else, direction of cut plays a big role. they are normally distinguished by clockwise and counter clockwise, but that may be confusing if you have inner and outer cut surfaces, just like the part in my picture. A conventional cut essentially scoops the material ahead of the end mill. |(think of using a shovel to scoop sand.) A climb cut tries to walk over the material. (Think of pulling leaves with a rake.) You would think that scooping (conventional) is more efficient, but that's not always the case. During conventional cuts, the end mill stays relatively straight IF it and the machine can handle the load. When working in harder materials, this translate to slower feed rates which means more time and more rubbing instead of cutting. Climb cutting has it's flaws too, but the benefits in aluminum outweigh the negatives and can easily be circumvented. Climbing causes the end mill to flex away from the material. We compensate for this by applying a finishing pass, sometimes multiple finishing passes. However, we don't have to slow down with a climb which means less heat, which ultimately means greater tool life. I admit that I'm a little fuzzy on exactly how a conventional cut interacts with any material, but that's the general idea.

 

And a bit of a tangent... I think that's all I can offer.

Here can see just how much I rely on the O-flute, but I have used down to a 0.8mm 2 flute in aluminum with good results.

To keep as much as you can in their original packaging. It just makes it so much easier to find and identify. Try to keep extras of what you use the most. One slight parameter mistake is instant game over. Take a look at the broken drill mill. This is also when I learned about coatings. The replacement was bare and has an insane amount of hours worth of aluminum and carbon fiber on it.

I have a few more. A good one for me has been the corner radius TiCN. I have three little 1/8" ones in the pictures, but also have a larger 1/4". I want to say they all have a 0.010" (0.25mm) radius. In CAM, the difference in flat vs corner can change the way the entire program creates the gcode.

The last pic is a dishonorable mention to TiN, AlTiN, and eBay. The small TiN O-flute is a cheapy. I have tried multiple from different sources and they all broke instantly at the cutting tip. Maybe the sellers try to hide inferior material behind a pretty gold coating. Notice the welding on the AlTiN. Once a tool welds, you can chip the welded bit off, but it will never be usable again. What you see is the bare carbide after the cutting edges and coating we're destroyed. The ball nose is just there since it came from the same eBay seller.