I guess you could put transducers on the frame of the Shapeoko at different/strategic locations and measure amplitude and frequency of the vibrations. You could have a controller adjust speed and feed if possible or make recommendations through a display to increase or decrease those parameters. This could be a nice project for those Arduino enthusiasts.
1 Like
I think Vince has basically discovered that higher RPM based feeds give him the best finish because it forces resonances up to higher frequencies likely with lower amplitudes. Lower frequency resonances probably are more detrimental to finish quality.
Probably little need to experiment much, if you can run at higher RPM, and a suitably higher feed.
5 Likes
So just max out RPM as long as the machine can handle the associated feedrate ?
Then what’s the deal with the oldschool surface speed equation that calls for a specific RPM depending on the surface speed that a given (metal) material likes best ? i.e.
RPM = (SFM x 3.82) / Diameter
1 Like
I believe that SFM has to do with thermal characteristics — how much heat is generated by friction, how much heat can be carried away by a given chip.
One thing I really think we need to work out is what the optimal toolpath strategy for machines is (presumably adaptive clearing / trochoidal milling) and how that affects this sort of thing — there being a separate HSM calculator at: http://brturn.github.io/feeds-and-speeds/ seems to underscore this dichotomy.
1 Like
Well, I’m not prepared to provide a unified theory of speeds and feeds at this point.
Although my feeling is that many of the historical suggestions relied on machines that had lower spindle speeds and were also substantially more rigid than the SO3.
And I personally wouldn’t just run the router at maximum speed, I’d likely balance the RPM with noise tolerance and feed rate comfort, but shooting for a higher RPM than is often suggested.
I sure hope I’m not sidetracking your work here, though, I’m just providing some personal theories and honestly I probably should have kept my mouth shut and allowed you to carry on on your own unified theory rather than possibly contaminating it.
2 Likes
There was an interesting thread on this started by @The_real_janderson not long ago. Does SFM Matter?
Your thread, here, is most interesting, can’t wait to see a Unified Theory of Shapeoko 3 Speeds and Feeds.
Meanwhile, my current approach is to leave my speed at 30k and adjust other parameters until it sounds nice, haha, calibrated ears.
2 Likes
I 100% agree with this approach. crowd-sourcing will be very complicated, especially with everyone’s machine at varying levels of modification. Providing a reasonable value to start with and let the owner push from there gives flexibility to the user and the creator of the source of knowledge (yourself in this case).
Also, to the SFM argument, it just seems like that doesn’t necessarily matter to what we do. Like @Vince.Fab mentioned, we run more Datron-style milling with high RPMs and a focus on chiploads rather than SFM.
2 Likes
@cgallery
by all means do provide your theories and experience, I am basically still just a newbie trying to find my own way through the hazy topic of feeds and speeds, and trying to make sense of the multiple bits of wisdom scattered around here!
I like my router as quiet as possible and I’ve been running 99% of my jobs between 12 and 15k, but that was mostly out of convenience, and I now realize I should go and check the high RPM territory for a change.
@Griff
I just re-read that thread, I read it earlier but it did not stick. Bottom line as I understand is “sure, you can have a look at SFM if you want to, but you can just as well ignore it and you’ll be fine in most cases”.
Very interesting that your baseline RPM is 30k, yet another hint that I should look at changing my RPM habits.
I’ll continue my quest for the “Oversimplified view of feeds and speeds that can still be good enough for newbies that refuse to take numbers for granted”
3 Likes
I see SFM as ballpark data point.
Long time established numbers that get you within range of what should work.
Most companies offer it with their tooling.
When in doubt aim for this if you have nothing else to go off.
The thing is our machines are not built uniformly. RPM and feedrates can reach pretty decent speeds but the rigidity is seriously lacking out of the box for alloys. So you scale back accordingly till you’re see finishes that work.
You may find your machine can’t even hit the SFM numbers before even being able to make a cut. Physically impossible with the stock or modded hardware. Again, just a place to start or aim given nothing else to work with. I find SFM to be helpful particularly with drilling where data can be scarce.
2 Likes
I for one am also looking for the Shapeoko cookbook. I want to stand on the shoulders of the pioneers.
I find it interesting that our software, Carbon Create does not have some tables of F&S based on the material we want to mill, the database has fixed values that you can change manually. Even VCarve has fixed F&S and the values are not material and machine specific well maybe not exactly machine but a range like machine levels that could be selected.
F&S is a major factor in the results you get but it seems that everyone has their own recipes and F&S are at the intersection of engineering and art form. I was reading from the CNC Cookbook where they state that chipload is not an important factor for beginners but …
Chipload: Beginners can ignore this. Others may use it to make sure they’re in a familiar range or to specify the chipload based on Manufacturer’s Recommendations for the specific brand of cutter you use. G-Wizard is fairly conservative, so again, Beginners can ignore it.
2 Likes
If we were to try to do this scientifically, then what would we even measure, besides broken tools and finish quality? Tool/cutting temperature? Noise? Vibration? Gantry deflection?
1 Like
Don’t get me started on Carbide Create’s default values 
The fact that it still has Nomad-style RPMs as recommanded values for some materials after all these years is beyond me. The look on my face when I first saw the “4687 PM” and had no clue what to do with it back then, with my Makita router starting at 10.000RPM
I agree that beginners can safely ignore all of this and go with the recommanded settings, I know I did. But sooner or later there is the urge to understand
3 Likes
Honestly, I would not even go that far. Finding a deterministic method that gets me a cut that sounds good, looks clean, and does not take ages, every time, would be more than enough.
3 Likes
This thread is a great read… It did make me feel better that I’m not the only one who doesn’t know the way to calculate F&S but it also made me feel hopeless in that NOBODY knows (or agrees on) the right answers. I am a relative beginner, but one thing I think I can add is that “fastest is better” is definitely not always true… In cutting some aluminum recently (building a computer case) we had the spindle of the dewalt going top speed (our thought being aluminum is harder than wood… faster must be better) and we had what I’d consider reasonable feed rates, and the friction got to the point that we were melting the aluminum out of the way instead of cutting it… We resorted to cooling it with WD40 while cutting, which helped, but we didn’t actually get GOOD cuts until I saw someone recommending spindle speeds even lower than the dewalt would go, so we ended up cutting at the lowest spindle speeds, and got much better results, and were even able to increase feed speed. Sorry I dont remember any of the details of the feed speeds, but they were not based on anything but trial and error…
My only other comment is that I can’t wait to see what might come out of this thread in the end, and I caution not to let a desire for perfection get in the way of compiling a useful table that may not be 100%… There are so many reasons listed in this thread that show why the answers will be different for everyone (different build qualities, different mods, etc) that having one number that is best for everyone is impossible… Having a living document of what range works with what is probably the most that could be expected.
Thanks for sharing all your hard work and I’ll try to take better notes next time I try something so I might someday have useful information to share too…
2 Likes
Thanks for sharing Steve. Indeed aluminium is much less forgiving than wood, so you need to have at least a good starting point for chipload & depth of cut values, otherwise all kinds of unpleasant things happen. This is precisely what I am trying to get out of this exercise/thread. I’m actively working on writing that specific chapter of the Shapeoko e-book/beginners guide I mentioned in another thread, but before sharing a draft I need to put my action where my mouth is, and test the process/values myself.
2 Likes
Steve, can you provide some ideas of the type of aluminum you guys were working with, and what kind of spindle speeds and feed rates/cutting depths you were using? Specifically, what speeds and feeds were causing melting, and what worked better for you?
1 Like
I too increased the speed of the spindle trying to get better results but this thread set me straight, the speed of the spindle is proportional to the horizontal speed (feed rate), the depth of cut and stepover (Radial) as well as the number of flutes. You change one, you need to adjust the others to compensate. At a given depth of cut, doubling the spindle speed means that you double the feed rate. As Julien indicated above, the chipload for a given bit seems to be the constant. The question is determining the proper chipload for your bit and the CNC as you indicated, many of us have made some mods to the original Shapeoko setup that increased one or both stiffness and spindle power.
Chipload= feed rate (IPM)/ (RPM X number of flutes)
Maybe the chipload table should have the basic number for a completely stock Shapeoko and one for the most advanced setup so someone would know the upper and lower limits of the range.
1 Like
My suggestion based on experience with cutting plastics (which can cause melting issues similar to aluminum)…
(1) Start with the tool manufacturer’s suggested chip load, right in the middle if there is a range.
(2) Now, pick an RPM that you can tolerate noise-wise and won’t be too hard on your spindle. The higher, the better, to a degree. Higher spindle speeds = fewer problems with resonances.
Determine your feed rate with those two parameters [(1) and (2)] in mind, BUT, halve the DOC recommended by the manufacturer to compensate for the lesser rigidity of our machines.
Then, you can experiment with increasing DOC until you’re happy with overall performance. Or leave it at 1/2 for a simple one-off item.
In summary, I think a lot of people tend to play with the feed speed to compensate for lower rigidity. Instead, play with DOC.
That is the Phil technique.
4 Likes
The more I think about it, the more I like this approach. I was already bought on the fact that max achievable DOC is the major difference between the Shapeoko and more rigid machines, but I am still following an “in-between” approach of reducing both the DOC and the recommanded chiploads.
My revised best guess for “starting point/ minimal chipload” is currently :
| MDF | Soft wood | Hard wood | Acrylic | Aluminium | ||
|---|---|---|---|---|---|---|
| soft wood + 25% | <= hardwood + 25% | <= Acrylic + 25% | <= Aluminium + 25% | <= baseline | ||
| 1/16" | 0.0006 | 0.0005 | 0.0004 | 0.0003 | 0.00025 | half of 1/8" |
| 1/8" | 0.0012 | 0.001 | 0.0008 | 0.0007 | 0.0005 | half of 1/4" |
| 1/4" | 0.0025 | 0.002 | 0.0015 | 0.00125 | 0.001 | baseline |
I would be quite interested to see how Steve’s chipload relates to this reference, or what everyone else has to say on these values.
2 Likes
Running a minimal load doesn’t guarantee the best cut performance or finish, but it should prevent many of the issues people have.
1 Like