I’m still quite new to the Shapoko3 so I’m hoping someone can help me understand this better.
I ordered some Amana tool downcut end mills (46225-K, 46202-K) for a couple of projects and I have been hesitant to use them because I have unsuccessfully tried to calculate the appropriate feeds and speeds for them and was worried I’d break a tool.
I summoned the courage to try the feeds and speeds from the Carbide Create end mill library but I got a lot of chatter (cutting into maple). I tried backing off on the rate by 20% n Carbide Motion as this video suggested but that didn’t seem to resolve the chatter.
I’m looking for some help to figure this out so I can continue to use these end mills.
I’m new here also, but have a question that might get you to the answer. What is the IPM, RPM, and depth of each pass?
I ask, because even if yo change RPM and IPM, going too deep will cause chatter. If you haven’t already, try increasing RPM, slow IPM and reduce the depth of cut by at least 60%. Finally make sure your router is secure and perfectly level. Any movement will cause chatter.
Feeds and speeds are confusing at first, for me the major source of confusion initially was that the recommendation you may find on the internet seem to vary wildly, and more often than not are not directly applicable to a stock Shapeoko.
Using the suggested values in Carbide Create is usually a good place to start, but then again there are many specific cases depending on what cutter you are using, and geometry you are cutting. My take on feeds and speeds for a Shapeoko is in this section of the ebook.
What geometry are you cutting ? I suggest trying pockets first, they are easier on the machine since only a quarter of the cutter section or so is engaged in the material. Find feeds and speeds that work for pocketing for you, then when you need to do profile cuts (slotting), dial down depth of cut.
Downcut endmills are great to reduce tearout, but they are not as efficient as upcut endmills when it comes to chip evacuation, then tend to push chips down so if you are slotting the chips may end up being packed at the bottom of the cut, possibly leading to chatter, the deeper the cut the likeliest this will occur.
If you don’t feel like going through the whole F&S section I linked above, here’s a summary:
Set the router to the highest RPM you can bear (say, 18.000RPM)
In maple, aim for a chipload of 0.001". Since chipload = feedrate / (nb of flutes x RPM), for your 2 flute Amana cutters, that chipload would then call for a feedrate of 0.001" x 2 x 18.000 = 36ipm in this example. You can experiment and go to higher feedrates, but don’t go much slower, as some point the chipload will become too small and you would rub the cutter rather than cut anything, which is quite bad.
Aim for depth per pass = 50% of tool diameter for pocketing, and a bit less, say 35%, for slotting. Again, it is quite possible to go deeper, but it’s a safe place to start. So basically, start with 0.04" depth per pass for the 46225-K, and 0.08" depth per pass for the 46202-K, and see if that gets you a good cut. If it does, then you can incrementally try deeper cuts.
use dust collection to make sure chips are getting sucked out of the cut.
It does look like a dark art, but it’s an illusion created by the large number of variables that come into play and interact with each other, and by the fact that no two machines are exactly the same. It’s of course 100% science, BUT everyone has a different need (and willingness) to deep dive into the details of the theory. What I find most interesting in this forum is that you will find a whole spectrum of users, from those who set feeds and speeds by ear or experience alone, to those using a variety of calculators (@gmack’s, @spargeltarzan’s) to optimize their cutting parameters, and they can all produce excellent results. Statistically though, it seems that most of the former mainly cut wood, while many of the latter mainly cut metals
I live happily in the middle-ground zone: I just keep my chipload in check depending on the material and cutter size, apply a few rules for DOC/WOC, dutifully make notes of what cutting parameters have worked for me, and that’s it. If this was a business for me I would most certainly put more effort in optimizing my material removal rate.
Or, it may be that this is indeed an arcane art and I just think I have a good enough understanding of it all, when in fact it goes over my head
@Julien To answer your question I was cutting what amounted to slots 1/8" wide in a geometric pattern. (It’s a company logo with is a bunch of connected lines). I will review my settings and then post latter this evening with what I was using.
Depending on the material I always cut 2…a test piece to dial in my feeds and speeds…then the final piece.
But I carry the ways of an old school wood worker…always plan to screw up.
so also lets be clear, F&S are a range of values, not a narrow “point”. The size of the range varies by material, wood is extremely forgiving, aluminum a lot less so, steal, well… narrow.
So early on I was confused wondering what the perfect F&S was for something. Then I realized that as long as I was in the range, I was good… and could focus on all the other things
For wood, if you go outside the range on the fast side, you either snap the bit or get malformed cuts. If you go on the too-slow side the wood can get burn marks, but mostly you just make fine dust.
What I did learn as rule of thumb:
Crank up the RPM. Higher RPM means less forces on the machine (vwheels, belts etc) and less forces on the work holding.
Depth: Conservative is half diameter – but at max RPM you usually can go to full diameter easily. Of all the tradeoffs, bump the RPM (so router speed) up and you can cut deeper.
Plunge: Since I got the HDZ I stopped worrying about that… and most cuts are not that plunge heavy so normally I stick to defaults (10 ipm or so) mostly since it doesn’t matter. For V-carves, it does matter, and I might go to 20 ipm. For some really bad plunging bits (surfacing bits or my new 1/2" amana cutter) I would go to maybe 5 ipm.
Feedrate … I admit I am pretty conservative there but the nice part is that this is the parameter you can dynamically bump up or down in Carbide Motion… so even if you start conservative, you can hit that “+” button all the way to 2x faster depending on how the cut is going in reality.
For a 1/8" bit I often start at 45 ipm (so I can dynamically go all the way to 90)
lately for designs where I care about the surface finish I’ve started to decrease stepover a little bit for pocketing operations (and trading feedrate up). Especially with Carbide Create, a perfect 50% stepover can leave artifacts while 45% or even 35% ends up much smoother.
Also as much as all the math can say you can go all the way up to feedrate X… unless time-is-money, going below that is lower risk in terms of something going wrong (workholding coming lose etc) and also, if you care about cut quality, staying away from the upper edge of the range is often a good idea.
a Dewalt router on 3 is ~20.000 RPM , feedrate of 508mm/min is 20ipm, stepover was 50%D, so your chipload was 20/ (2flutes x 20.000) = 0.0005", which is ok-ish for a 1/8" cutter but is getting uncomfortably close to the rubbing zone as far as I am concerned. So I would crank up that feedrate (which is counter-intuitive, I know…)
Depth of cut was 40% so that is ok. To play it super safe since you will be increasing the feedrate, initially reduce depth per pass further until you are confident it will work.
Something like 50ipm at 1mm DOC should be quite fine.
Every insight I have to offer about how to approach feeds and speeds is in that ebook chapter I linked above, and then at some point (not the same point for everyone) the important thing is to stop worrying and start cutting (and, yes, occasionally breaking endmills)
Imo running chipload that small is definitely not ok unless you are checking and adjusting run-out religiously.
1/8 end mills can be “touchy” due to the stiffness of the shank (and core) compared to 1/4 tooling. Stickout is a huge deal and deflection can cause chatter even when cutting parameters are perfect.
Feeds and speeds are fun. Learn what you shouldn’t do then start conservative and work your way up.
3 Likes
Griff
(Well crap, my hypometric precursor device is blown…)
12
Hey Vince, I’ve tried a few Amana 1/4” shaft/1/8” cutter end mills recently. I know by experience now they can be pushed harder then regular 1/8” mills. You smart guys have any real numbers on this?
Its really depends on how long your flute length is. The longer the length, the less the tapered shank will matter.
Its not too hard to come up with numbers but its different with each tool. I have an Amana 51777-Z 1/4 shank tapered 1/8 single flute down-cut that would probably rip…but it only has a 5/16 cut length. Ive also run some tapered Datron 3mm SFs at some seemingly impossible speeds and feeds. Again, a very stubby cut length.
Its still safe to start at straight shank speeds and feeds then slowly increase.
Millalyzer, the SFPF Workbooks, and GWizard account for that. Bigger shanks enable more stickout and provide more collet holding force. A 1/4" shank is 16 times as stiff as a 1/8" shank. so flexure of the exposed portion of the 1/4" shank can basically be ignored.
I followed you advice and reviewed the section of the ebook you pointed out and used the simple Excel calculator you created. I was able to create Winston’s threaded waste board from Fusion accounting for the difference between the Carbide 3D 3 flute #251 and my 2 flute Amana 46202-K. It turned out great!
A couple of questions came up during the updating of the feeds and speeds and the subsequent run in Carbide 3D.
The chip load in Fusion 360 didn’t match the spreadsheet value or if I used the spreadsheet calculated value it in Fusion it changed the feed rate. Does Fusion not account for chip thinning like the spreadsheet?
When I loaded my file in Carbide Motion the run time said it was ~8 minutes but Fusion’s simulation showed the runtime at ~30 minutes. Just trying to understand what caused the discrepancy?
Indeed Fusion360 Feed per tooth / Feedrate combination does not take chip thinning into account. Which is strange, since it knows the width of cut. However, WOC is defined two tabs “later” in the workflow (the user is expected to fill in the parameters from the leftmost tab to the rightmost tab) so I can only assume that they did not want one parameter depending on something else not yet entered which would then alter the original value. I mean, imagine you entered 100ipm for feedrate, proceed to fill in other parameters, enter e.g. 0.01" optimal load, go on about your business, then you may not realize that your feedrate value has been automatically bumped to a higher value “behind your back”. Now, they COULD have just added a “chip thinning” checkbox so that only users who explicitly want it (hence know what they are doing) would have it.
Runtimes: there are typically discrepancies in estimated runtimes between various software (there are even discrepancies between what CC estimates and what CM estimates). Actually it’s not easy for the software to provide an accurate estimate, mainly because of two factors that the software does not know about: rapid feedrate and accelerations. Those two things are static GRBL parameters configured at the controller side, and neither Fusion360 nor CC can know what value they have on your machine, so they resort to using a default value. For Fusion360 estimates, at least you can adjust the rapid feedrate value used for the estimate: right click on a toolpath => “Machining Time” (or something like that), then adjust the rapid feedrate value, to what $110/$111 value is on your machine. Still won’t be perfectly accurate. When I care about machining time estimation, I tend to use different tools to give me their estimate about a specific G-code file. For example, this online G-code viewer will print out a time estimate.
Maybe we could convince @fenrus to make another one of his nifty browser-based tools to provide a better estimation, where folks could manually enter their specific GRBL params, upload a G-code file, and voila.
