I don’t want any expensive endmills yet since I’m just starting and will probably break some. I’m looking to buy a bunch of them cheap on aliexpress for now.
I’ll be cutting 12"x12" 1/4" aluminum and mostly milling out large letters, but sometimes smaller letters too. The finish on the inside/bottom of the letters doesn’t matter so much because it will be filled in and won’t be visible in the finished product.
I have a bunch of 201 flat endmills, but from my research I might prefer a ball endmill for cutting letters since it’s apparently better around turns.
Also coating seems to be important. TiN, DLC, ZrN?
Can anyone link me some good endmills on aliexpress? I’m looking into stuff like this but not 100% sure what to go with. Seems I could research for endless hours
I cut quite a bit of aluminum, mostly shapes out of thin sheet. When it comes to endmills, single flute endmills are the only way to go for aluminum. I’ve found multi flute endmills eventually clog up with chips despite your best efforts. Coated endmills definitely help, but not essential. I’ve had pretty good luck with some of the cheap ones found on amazon. Also, its super important to keep your cut channels clear of chips so it’s a good idea to keep some compressed air handy to blast the chips away.
I’ve had very varied quality on endmills from Aliexpress, even from the same vendor.
I found a couple of local (in country) tooling suppliers that sell from their websites, here’s one
they are not expensive and the quality is consistent, you should be able to find a decent local supplier near you too with a bit of googling.
The DLC coated bits are harder to clog up than the uncoated so I pay a little more for those as they tend to outlast the uncoated by more than the price difference for me.
I’ve used the un-coated ballnose from that supplier in Aluminium but was careful with the roughing passes and fed fast and shallow in the finishing toolpaths using Isopropanol lubricant with the ballnose.
(Well crap, my hypometric precursor device is blown…)
I like the single flute diamond coated from 2L. I still have and use the first one, 1/8", I bought a couple of years ago. Not cheap but not expensive either.
Ditto on the 2L. I use the 1/4" and 1/8" single flute from them as my go-to aluminum tooling. I have tried both the diamond and not and I think the diamond helps enough to justify the slight price increase but the not diamond coated has worked quite well too.
I have before, but if I am using a ball end, it is most likely a tapered ball end mill. The ball end mills are two flute, and I usually switch to those after roughing with the single flute square end mill.
I have run across a single flute ball end mill only once, and if I could find it again, I’d buy a couple of them to try them out.
Not for the standard Carbide Compact Router — it doesn’t have a sufficient clamping range. A 6mm collet is available from a 3rd party:
While this will work for ER-11 collets, it’s better to get a 6mm collet there as well — these are widely available. Two vendors I’m confident of ordering from are Precise Bits (@TDA is active here) and Maritools (I bought a full set as well as a wrench from them and they’ve worked fine for my modest needs).
I should have mentioned I’m currently using a dewalt router. I have a collet set but all imperial / fraction of inch. Do you think the 6mm will work in the 6.35mm collet or should I buy metric exact fit?
Also wondering is there any complication with using metric bits? Its as easy as setting the bit measurement in the program right?
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.
Just as an upfront we don’t sell a 6mm collet for the 611. So I don’t really have a horse in this race. Additionally, for the angle and kerf you can’t clamp our 1/4" down to 6mm. Even if you could I wouldn’t recommend it on any collet as you are likely to pickup more runout. Far from ideal in metal machining.
Generally speaking keep in mind that any runout you have will in the worst case get added and subtracted to different flute’s chipload (for multi-flute tools).
Won’t comment on brands or quality of tools for obvious reasons. However, per above if you do have runout single flute tools will be a lot easier to consistently run. You still have to worry about the initial load on plunge (so ramp if you can). But they have far fewer issues as the chipload isn’t variable across the flutes and cutting depths.
Pretty amazing resource it really helped me. I ordered a bunch of cheap upcut and downcut endmills at 1/8" and 1/4" for now. I have some coming in soon from amazon and a bunch from aliexpress that will take 30-45 days. I’m sure I’ll have a few questions about feeds and speeds for you guys since math isn’t anything I’m even remotely competent in I’m willing to learn though. Once I feel comfortable using the machine I’ll order some better endmills.
Silent shop vac came in today, so tomorrow I’ll start leveling the bed and get moving forward towards my first project.
No problem, I didn’t really have the time to go through the rest of this thread in detail yesterday. So while it might be late I’ll try to hit some of the other points briefly.
This primarily means that you will be deflection limited. Doesn’t mean you can’t do it but you are going to have to watch your cubic material removal rate (chipload and depth per pass).
Higher rake tooling and tooling that doesn’t leave land will typically give you better results. An easy check for land is to see if you can follow the grinding pattern of the blank into the flutes of the cutting tool. Land is usually left for strength but can increase the cutting forces.
This will help but plan on doing a clean up / spring pass at the end to clean up the edges. You will probably have better machining time and tool life this way than trying to cut so low of a chipload or pass depth to keep from needing the final pass.
Part of this depends on the tool but in general isn’t true. As long as you have proper gashing at the tip of the tool it will not work better in direction changes. You are cutting inside the previous cut so you are only moving your chipload in a direction with the edge of the tooling.
In economy tools, ball ends may actually be worse as it’s much harder to get good rake in the ball without multiple grinds and diamond wheels.
Coating can help but avoid anything with an “A” in the coating (TiAlN). This will typically bond to the aluminum.
DLC is a catch all for carbon coatings. Some of them are pretty good like TaC (Tetrahedral Amorphous Carbon) some are very much not and almost act like and abrasive. It depends on the method, layer thickness and the like.
The other problem with DLC coating is they need fairly decent chipload to keep the heat down or the coating will just evaporate as they are only good to around 350-450c. It will still help smoothing out the grind (any properly applied coating should) but it will disappear from the leading edge and compression point.
I’d avoid the down cut in general but especially when slotting. They are a pain in aluminum, typically have higher cutting forces, and make it more likely to recut chips.
You might want to “bin” these some for things like:
Land - (mentioned previously)
Helix - which is higher the tighter the twist is.
Rake - how aggressive the leading edge of the flute is. Hard to come up with an easy way to check for this one. It’s basically how extreme the angle of the flute is from center.
Core - This is how much material is left from grinding the flutes.
Any tool with land will cause more cutting force if the land engages with the material after the cut.
Helix could go either way. The higher it is the higher the shear and the more force is directed up into the spindle. That could be good if you’re deflection limited in your X and Y. Like for like though (core, rake, etc) it will be a weaker tool. No helix (0 helix, straight flute) is the highest cutting force.
The more aggressive the rake the less force it takes to make a chip with it. It’s also typically weaker though as there’s less material at the leading edge. In a lot of cases if good or bad will depend on the carbide grade.
The more core left in the tool the stronger it is to things like tool deflection which can get extreme in some cases.
The other usual general advise.
Don’t buy features you don’t need e.g. longer cutting lengths. Every part of the tool will be used, either for you or against you.
Make sure you are using hard mounting (clamps, screws, blue tape and CA). Do not use double sided tape. You are cutting very small slices out of a material that is causing much higher forces than woods or plastic. You don’t want your material moving around “a lot” relative to your chipload.
If you can get away with it use a cutting fluid of some kind. Even if you are just brushing or spraying it on it will buy you some forgiveness.
Pay attention to your metal grades. It’s going to be a lot easier to machine a 6000 series than a 3000 or 1000 series in general. Additionally all your numbers will change as the minimum requirements for your chipload will change.
Hope that’s useful and not too late. If there’s something I can help with let me know.