Okay, so I have a set of Lakeshore Carbide 1/4" 6 flute countersinks https://www.lakeshorecarbide.com/100degreecarbidecountersink-sixflute.aspx that I’m looking at using to countersink some screws in 6061-T6 aluminum. I use Fusion 360 pretty much exclusively for my Shapeoko 3 XXL, and I’m trying to figure out if there’s any opinions on the correct speeds and feeds as well as machining operation for this task. I do hole boring all the time using the bore operation with great results using a 102z endmill.
There is the drill operation in fusion to plunge, but is that the correct operation? And does anybody have any recommendations on plunge FPS? Obviously plunging is going to engage all of the cutting surfaces at once so I’m concerned as to how to proceed. When I’ve done chamfering in the past, I’ve taken a couple of passes, but I know the countersinks are a little different.
Also, my typical chip load of .001 will be a little different I think in this operation, which is normally what I default to for aluminum machining. Any help would be greatly appreciated!
@cqualley you are not going to be able to run your router at a low enough speed to effectively use that style of countersink, you would be better off using a drill press with the countersink mounted in it as a second op.
I suppose that makes sense, I was figuring if I ran it at 10k, 60 ipm would net a .001 chip load. But, I guess with a drilling operation that would result in all the flutes being engaged at one time, so maybe that’s not an option? The drill press is not an option I want to explore, kind of why I bought a CNC after all. Any other suggestions on end mills that would be capable of countersinking on the Shapeoko?
My other thought was, is it possible to run it more like a chamfer operation? there’s not a straight plunge but more of a spiral entry in to the material? The hole will already be drilled in a pervious operation, so my thought was to basically chamfer the edge of the hole.
@cqualley The style countersink you have is best used at low speeds, I would run that at around 200-250 RPM, which this style of machine is incapable of doing. Even in an industrial VMC that style tool is going to be ran within a low RPM range in order to produce a good result.
You could chamfer mill the hole, but would need to look at other tooling, the style tool your currently have is meant for plunging and applying an axial load rather than side milling and applying radial load. Harvey Tool offers a fairly large selection of chamfer mills and would likely have one that suit your needs. If you were dead set on using your CNC to do the chamfer that is the route I would recommend pursuing. A second option is to helically interpolate the chamfer with a small ball mill, but this would not be very efficient from a time standpoint.
Ultimately a drill press (or often times a knee mill) with a countersink is the most efficient way to deburr a bore using a machine, you could also look at hand deburring the hole with
a machinists scraper.
CNC’s are great tools, but something that may take 30 seconds on a drill press to do will likely take significantly longer on your machine. By the time you factor in the amount of time that a tool change takes, resetting your Z offset if you do not have a Bitsetter, and running that portion of the program you may be looking at several minutes to chamfer one hole.
I use a variety of chamfer mills for countersinking, but most are 1,2, and 3 flute. Typically, I use appropriate size tool, and peck drill. I’ve never bothered to optimize any of it, its a quick operation, I just use some modest feed per rev. Most tool suppliers will give you data on vertical feed rates/SFM for such a tool. RPM=SFM * 3.82/Diameter. IPR=FPT * number of T.
As others have said, that’s not really a tool for high RPM, it seems that Lakeshore does have a set of chamfer mills however
In Fusion you can either use a 2D contour toolpath or a 2D chamfer, you need to set up the cutter as a chamfer mill to use it with these toolpaths. Typically you roll around the edge of the hole and stepover or step down until you’ve reached the final chamfer depth.
I run a 2 flute chamfer mill at 20kRPM and stepping in 0.5mm per pass moving at 800+mm/min in Aluminium and it works OK for me.
Yeah, I guess I don’t know why I thought they would work honestly. I’ve heard a wide range of different suggestions for these countersinks as far as RPMs go—everywhere from 200RPM on here to 6k on other sites. Whatever the case, too slow for the Shapeoko, so I’ll use a different method, maybe by hand. As far as chamfering, I have a couple of chamfer end mills that I use on aluminum, but I think the comments are probably correct that it’s more work than it’s worth. Maybe this is just a job for the drill press.
The Shapeoko can do a fantastic job of putting a nice clean chamfer around your parts and that can really finish a part well.
If you’re countersinking a couple of holes then the question is whether the tool change in the Shapoko is easier than using your high quality countersink in the drill press.
Yeah, for sure. I guess I’m not afraid of a tool change honestly, it’s 30 seconds for me. I just finished an aluminum part and ran a nice chamfer around the outside, it definitely produces a much better finish.
Yeah, I might give one of the lakeshore ones a try too. Honestly though, I used one of their 1/8" variable 2 flute zrn end mills for the first time today and it clogged with aluminum chips within 20 mins, even with a continuous air blast. I’ve used my Carbide 3D 102z end mills for hours of aluminum cutting with identical speeds and feeds and never had an issue once. So, I can’t say that was a great experience the first time using one of their end mills.
Understandable. Tools have a wide variety of design parameters and use considerations. Advanced performance in one scenario or another, but certainly always with some trade off.
I’d surmise most industrial tooling doesn’t consider a very light duty hobby machine application.
For instance, a variable helix is I believe designed to reduce resonance. This allows for a heavier cut. Assumably the tool is designed to take this heavier cut, and performs best under such a condition. Maybe you just need to push it harder. But maybe the machine can’t provide optimal application.
I have a variety of specialized 1FL from a single manufacture that I’ve played with a lot. The cut quality varies considerably at the same woc/doc/chip load. The highest performance of them hasn’t been great for me, I haven’t been able to load the tool enough without machine deflection. Meanwhile, a shop I contract with uses them exclusively for the purpose, and they provide a beautiful finish.
Yeah, that’s entirely possible that it’s just not designed to run slower. I looked at the feeds and speeds for their variable tools after you mentioned that and, in general, it lists aluminum at .003, which is considerably faster than what the Shapeoko can handle. I’m typically shooting for around .001 on aluminum with very good results (on most end mills that is).
Oh well, lesson learned I guess. The issue I have with some of the manufacturer speeds and feeds is they’re pretty much all triple what the Shapeoko can comfortably handle, but this time the chip load must really matter. The flutes have a deep design which seems to make them more likely to get clogged, but probably not as big of a deal with larger chips I guess.
The manufacture recommendations can give you an idea of what the design intention is between product lines. For instance, I tend to gravitate towards tools geared towards high(er) speed machining.
I email every tool manufacture with my application and questions. Some of them will be hesitant or unwilling to provide details, some kind of “There are too many variables” “secrete sauce” lazy answer. I don’t buy from them. Most of the reputable manufactures will be happy to help. I haven’t gotten any magical advice on strategies relating to a hobby grade application. But a lot of good information about what the tool expects, and under what condition it was designed to perform. They will often get you going in the right direction.
They’re pretty cheap and we don’t have as much choice of vendor in the UK as you guys in the USA have.
Single flute definitely seems to be the key part in not getting clogged and I’ve used these down to 2mm and they work really well. With only one flute it’s quite a bit easier to find an RPM and feed rate that the Shapeoko likes which also has a sensible feed per tooth.