I’m still learning and wondering how the open-source feed/speed calculators compare to the paid ones. What are your go-to calculators?
I’m also working on a mac, which limits my options. HSMAdvisor is PC only and GWiz is ending mac support (and their interface isn’t great). I could run windows on my mac with VMWare or VirtualBox, but I’d rather not if the other options work well enough.
It…really depends on what you are milling and whether optimizing machining time is paramount for you, e.g when you use your machine for production of parts for a business.
At one end of the scale there is “mostly milling wood as a hobbist” (=me), and you really don’t need fancy calculators then.
At the other end of the scale there is “producing batches of aluminium parts as a business, with tight tolerances”, and then it becomes less obvious how to optimize the feeds and speeds aggressively while still having control on tool wear, deflection, etc…
If you have Excel for Mac, you could start with the community versions we have:
GWizard: you will fnd a good number of threads here where folks shared their views. I bought it early on 3-4 years ago, used it a couple of times, and failed to understand how to deal with the seemingly incoherent results it was giving me, never used it again, but of course YMMV and I think the consensus here is that it may be more useful on much larger machines, than on Shapeokos and Nomad.
HSMAvisor: only heard good things about it, but I never used it.
On a Nomad, I would think you don’t really need (or could justify the cost of) a paid calculator anyway?
For a Nomad, no, not really. I tried so many of those tools but they don’t work well because they don’t take the jelly-like construction of the Nomad into account (it’s rigidity-limited long before it’s power limited).
The process I ended up finding that worked for the Nomad was:
The one exception for me was Millalyzer. I haven’t tried it’s “give me feeds and speeds” options much but it’s fantastic for understanding what the different variables actually do and for the price, it’s a steal.
Oh and Julien’s book is amazing. It’s Shapeoko oriented to a degree but everything discussed there is relevant to the Nomad as well.
I’m not sure how good it is I’ve not yet purchased the licence for it) but the tool database in Vectric VCarve Desktop (so I assume their other CNC software) products, where you can ‘play’ with the settings for each cutter and watch the chip load change accordingly.
I think that could be useful to set starting parameters, at least.
Granted it’s only available on Windows, though.
I bought GWizard, because Carbide3d seems to be promoting the “CNC Cookbook” heavily and I thought it can be trusted. I now consider that a mistake. GWizard does produce “something” — you can get numbers out of it. But those are not numbers that you can take and use with your Nomad. I ended up stalling the machine or burning/melting stock on various occasions. Also, there is a “tortoise/hare” slider which I have no idea how to set, it will take your numbers into ridiculous ranges on both ends.
I have no idea why Carbide3d promotes this tool, in my opinion it is useless with a Nomad.
I then started testing HSMAdvisor and after loading a power profile created by someone for the Nomad, got considerably better results. The numbers you’ll get are at least in a reasonable ballpark, and for some materials and endmills are very close to what I found by experimentation. But I don’t feel like I can trust this app. I found it is overly sensitive to tool stickout and will produce good numbers for longer tools, but go over the top with shorter ones. Tweaking the “aggressiveness” slider often produces no change in feeds/speeds. It also sometimes produced numbers that I know are way too aggressive and will stall the Nomad. I tried fiddling with the power envelope, which didn’t change things much, making the torque several times smaller did make the numbers more reasonable. I ran out of time, but I intend to go back and try talking to the author and reporting my results, perhaps things can be improved.
I do believe that HSMadvisor is the better tool. Even its materials selection is more reasonable: I really don’t need to choose from 54 kinds of pine wood, but I do want to see acrylic (cast and extruded) and epoxy or polyurethane modeling board, preferably in several densities.
More generally, this is far from what I expected from these tools! I wish Carbide3d would dedicate some time to work closely with the author of HSMAdvisor to produce a good “Nomad 3” profile that would reliably produce usable numbers. I think this is a major stumbling block, and not just for beginners — even people who get experienced with some materials need to start from scratch with others. And if you nail down your feeds/speeds for a specific endmill in a specific material with an adaptive toolpath, you will still stall the machine in a slot.
I know that some people think this can’t be done — but I really don’t think this is rocket science. Given a well-specified machine, perfectly described endmills, and a range of reasonable materials, these tools should really be able to produce conservative numbers for us, numbers that we can use right away, with no voodoo or hand-waving. The tools should also “know” that wood will burn and acrylic will melt and not suggest feeds/speeds when this is certain to happen.
Also, I will take issue with this:
On a Nomad, I would think you don’t really need (or could justify the cost of) a paid calculator anyway?
Having paid 3k for a Nomad, why not pay $50 for a calculator? It makes perfect sense! Especially if you work with smaller endmills and risk breaking a $25 endmill. The reasons for using the calculator are different with the Nomad: it’s not to optimize mass production, but to get a good starting point in a new material with a new setup. But the cost is very much justified. Or would be, if the tools actually worked.
Which Nomad do you have, what are you milling, and what HSMAdvisor machine and power profile are you using?
The spindle or the motion?
I have the Nomad 3, I’m milling HDPE, softwood (pine), acrylic and modeling board. The stalls I saw were spindle stalls, which resulted in motion stalls.
I used the Nomad 3 profile, which now that I looked seems to have been created by you 
Here’s an example of a failure scenario:
It’s a 6mm two-flute endmill, and I’m getting ready to use an adaptive toolpath with a 40% radial engagement. HSMadvisor will tell me that going 12mm deep at max feed is just fine. It’s so happy that even fiddling with the “aggresiveness” slider won’t change the suggested numbers.
In reality, going 12mm deep with 40% engagement is an instant stall (tried it). I normally use 6mm with a feed of 1750mm/min at 24k.
My statement “Like the SFPF calculator it apparently uses material K-Factors for its calculations. A recent earlier update added K-Factors for wood, but they’re 2-3 times higher that they should be IMO. But it so happens that the one just added for acrylic (and most other plastics), should be “close enough” for most woods [especially since they’re likely crude approximations anyway]” was apparently too generous for softwood (it’s much farther off) (https://community.carbide3d.com/t/speeds-feeds-power-and-force-sfpf-calculator/16237/52.)
You might want to consider monitoring spindle power as discussed here.
Well, I am not really interested in maxing things out — what I want from a calculator is to provide a reasonable safe starting point and tell me when I’m doing things that are not reasonable. If there was a global “safety vs speed” slider, I’d slide it all the way to “safety”. But there isn’t, the included “x1/x0.75/x0.5” slider doesn’t do what I’d expect.
12mm DOC with a 6mm endmill is clearly not reasonable for a Nomad, and I would expect something to go red on my screen and tell me that I’m doing stupid things. I still don’t know how to achieve this.
Another great addition would be a warning for melting/burning material: especially with acrylic this is a very important factor.
what I’d love is a web page or something like that where one can upload the gcode for a design, and the page then calculates based on the actual toolpaths what the range of the various IPT/forces/etc is maybe with a drop down for various materials… and then suggestions for how to tweak the feedrates for the various passes.
A spreadsheet is all fine for precalculation, but if you end up, say, slotting half the design the spreadsheet does not know that… which is obviously very different than a finishing pass with 25% stepover.
The gcode has that information in it…
You’re absolutely right – unfortunately it’s not rocket science. That would make it so much easier.
Thing is, the physical limitations of small machines are somewhat different from the professional equipment which the textbooks are written for. Furthermore, they are certainly not well specified (how much backlash today? proper belt tension? how much wear in those puny plastic nuts? chip evacuation?), neither are many common endmills perfectly described - some major grinding shops don’t even give you the rake angles, which is really the minimum needed for accurate forces.
Nevertheless, if your calculator is at least consistent, you can use your known-good operation (e.g. adaptive ap 6 mm, ae 2.4 mm, fz 0.036 mm), and use the values (forces, torque) that your software computes for this as your personal limit (which should, for example, yield slotting ap 2.3 mm, ae 6 mm, fz 0.036 mm):
Yes, the material model may not be perfect, or the tool rake angle somewhat different, but they’re equally wrong in both cases, so the comparison may well hold.
Vericut Force does precisely this. Granted, it’s not a website; you may need to run it overnight and it’s not much cheaper than a 3-ton CNC (per seat, of course), but there you go.
While appreciating the complexity of the problem domain, I still think I don’t need all this precision as a hobbyist.
I want a safe, reasonable starting point, and if there is a big margin between that point and the maximum that my machine is capable of, that’s fine. I’m not running a production shop where every minute counts. If I want or need to, I can tweak the values later and test the limits. But I’d like to start from a good place.
Also, some reasonably simple heuristics would go a long way. If you are milling acrylic, the tool should not suggest speeds/feeds that will melt the material, and this doesn’t require complex modeling.
I think we are not very far from that point, and if HSMadvisor’s author put his mind to it and focused on that exact problem for a couple of months, we’d be there. In fact, I’m wondering why Carbide3d doesn’t make a deal where they pay the author for developing a good machine model of the Nomad, so that people don’t have to struggle with the biggest problem in CNC world when you are new to it (“what feeds/speeds do I use?”) when buying a Nomad. I suspect this problem is solvable for the cost of around 2-3 Nomads.
If that’s all you’re after, it’s easy:
That should be a reasonable starting point for just about any material and endmill you can use a Nomad to mill.
If your endmill manufacturer doesn’t provide recommended feeds and speeds for your endmill and material, you should consider replacing the endmill/manufacturer with one that does.
The Nomad is very picky, so Carbide3D has prepared a set of endmills that work for it as well as a set of feeds and speeds that use those endmills in a variety of materials commonly milled on the Nomad.
Those feeds and speeds are embedded in Carbide Create, where Carbide3D seems to expect newcomers to remain for at least a little while.
So Carbide3D has a reliable solution for feeds and speeds that works for them. I imagine that’s why they don’t invest in calculators.
Not to say it wouldn’t be nice if they invested in a calculator but I doubt it will happen. They don’t even have a chip clearing solution for the Nomad (despite apparently being aware that it’s necessary, as they have one for the Shapeoko).
Well, I wish this was possible — even when buying from otherwise good an reputable companies like Nachreiner, you don’t always get feeds/speeds for all endmills and all materials.
I suspect this problem will resolve itself the same way several others did: by Autodesk eventually implementing a “good enough” solution in Fusion 360 and eating everybody’s lunch.
The suggestion wasn’t to buy from “good and reputable” companies, it was to buy from companies that provide feeds and speeds.
For example if you want a 6mm endmill for milling HDPE (from your earlier example), DIXI Polytool sells a variety of them (e.g. 7301, 7042, 7562 and thoroughly-specifies feeds and speeds (example). On the cheaper end of the spectrum, CncFraises also sells endmills appropriate for plastics and they specify the feeds and speeds (on a sheet of paper they send with the endmills).
I really doubt it. Fusion 360 doesn’t make features for hobbyists (it removes them), it makes features for machine shops. In a machine shop “safe enough not to break the machine” isn’t really a consideration, what they want is a delicate balance between machine utilization, tool life and job runtime. That’s a much more complicated problem to solve and I don’t think anybody even tries to solve that problem automatically at the moment.
Some CAM packages (SolidWorks/CAMWorks, SolidCAM/InventorCAM) do try to manage feeds and speeds to some degree but their recommendations don’t work for the Nomad.
MeshCAM also has suitable feeds and speeds when running in the Carbide 3D license mode — it’s what most folks use w/ a Nomad.
Forty plus year machinist here. There are Speed and Feed Calculators available, but as a 5+ year owner of a Shapeoko, you also learn there are Speed and Feeds that the Shapeoko can and cannot handle. Meaning I have found that Carbide Motion is a great starting point, and with the feed override…I can quickly find the sweet spot. So I ask, what’s wrong with CM? (I am honestly confused)
I’m guessing you mean Carbide Create (the toolpath-maker which has preset feeds and speeds for Carbide 3D’s machines)?
I can’t speak for @jwr but for me using Carbide Create regularly isn’t an option, as I need the features of a full-featured CAM package (e.g. parametric design).
Pulling the feeds and speeds from CM and putting them into a CAM package certainly works but CM only has feeds and speeds for Carbide 3D’s endmills, which are limited in variety and somewhat costly/difficult to obtain in Europe.
And you misunderstood my point. The Speed and Feeds calculator for YOUR machine is built into CC. Meaning, you are not going to find a machine specific F/S calculator online. Pick a material, draw a simple piece of geometry, read the speed, feed and DOC information. Take this info in which ever CADCAM program you desire. Bada Ping Bada Boom.
Just to clarify here, current versions of Carbide Create no longer use calculations, but instead a set of curated feeds and speeds developed/tested by @wmoy — there was at least one version (433? 434?) which was supposed to be optimized for trim routers — but we are instead using the hard-coded values now.
I believe MeshCAM might have a calculator, but folks would want to check on that w/ support@grzsoftware.com
