Mmh, interesting. I thought the Carbide trim router was just a rebranded (or cloned?) Makita, but indeed it says 12.000 min RPM on the site. If anyone has the Carbide router and a tachometer to measure the min RPM, or knows where the knob vs RPM table can be found, it would be interesting to know.
Yep, I had mentioned that a few times when people were looking at which router they should get.
1 Like
My use of “hard” versus “soft” is unrelated to the seed type (so it’s technically wrong), I meant it in Janka hardness/density way. Which is also not a good way to define two categories, since there is a continous range of janka/density values…I just go by the feeling of how hard/dense/heavy a given wood seems to be, and maybe double-check its janka value to compare it to other woods I have cut before, and that’s about it.
3 Likes
3 Likes
@Julien Does your simplified spreadsheet work for V bits? If it does then what should the inputs be for a 90deg vbit like the #301 ?.
Does it work for ball mills also?
If the spreadsheet does not work - is it possible to add in whatever is needed to make it work?
I was quite surprised how poor the default Carbide Create recommended S&F were for my DeWalt router as it cannot go below 16.5k rpm, yet they give much slower rpm that are just not possible - I have been running it at the lowest speed but not been increasing the feedrate by nearly enough to get the right chipload - this must be the reason for very hot bits that I have been experiencing.
I wish that Carbide Create would fix it so better default F&S are given for those with a Dewalt !
BTW, I have nearly finished compiling a spreadsheet table of different woods and their Janka values (over 300 so far - some are very obscure). I found many tables on the internet - all of which had some surprising omissions – so I have been combining them. It may be useful to add this in a sheet to your spreadsheet so all info is in one place ? I am happy to provide it - or make a simpler version with just woods that are commonly available for the hobbyist if you wish.
2 Likes
Hi @Hooby
the worksheet does not have any specific tuning for Vbits and ballnose endmills, that’s a good point, I should add something in this regard. The basic principles still apply, but I’ll see how I can correlate the usual recommended feeds and speeds for Vcarving with the guidelines I already have.
I feel you about the silly recommended RPMs in CC, I and several others raised this issue many times… What you can do though is just multiply everything by a given factor (RPM x factor and feedrate x factor) and you will get the same chipload with a usable RPM.
Good idea about the consolidated janka table, do share it and I will integrate it! It will also help me correlate them with unit power values when I start measuring those for various woods.
1 Like
@Julien Here is the consolidated spreadsheet of many wood Janka hardnesses that I have collected. There are 393 of them - some I have never heard of. Also I left a few duplicates where different sources think they have very different Janka values - Its up to the user to decide which is the best one!
If there are any important ones that I have missed then please add them.
I would like to also have Plywood, Baltic Birch Plywood, Hardboard, Particle Board etc added in but I have yet to find Janka values for these (presumably because they are all made differently, but some sort of ball-park guidance would be great!) - any ideas?
I have marked the commonly available woods with an * - so you can use the filter to just show these so it is much more manageable. Feel free to add or remove others.
As a completely wild-ass guess I have “suggested” that any wood with a Janka of 700 or more can be generally regarded as “Hard” for the purposes of your simplified S&F calculations. I have absolutely no idea whether that is a good value or not - My feeling is that it may be closer to 1000 or so - especially since I have seen MDF at 1000 to 1500 which surprises me - I would have guessed it much lower and in the “Soft” category. I bow to anyone’s opinion on where a practical boundary for soft/hard would be since I have no real experience in this at all. Please offer improved suggestions !
I have added it all as a new sheet in my copy of your simplified spreadsheet for my own convenience - but what I attach now is a standalone spreadsheet so you can add it or not as you see fit.
Wood_Hardness for CNC.zip (17.7 KB)
3 Likes
thanks ! I will be away from any computer for the next few days but I will check this out in detail when I’m back home.
In this article, Bob Warfield also sets the limit for “soft” woods (density not seed) to a Janka value of 1000, so it sounds like a reasonable limit.
What I need to do, based on advice from @gmack, is measure the unit power of various woods, and see how it maps to the janka values.
Or, maybe we could just experiment with the top 10 woods used by hobbyists, and experimentally determine the ideal chipload for each one, and call it done.
3 Likes
Nice! - can I add it to mine too?
IMO you really need to know K factors to calculate all the appropriate milling parameters - chipload doesn’t do that. I’ve tried to make that easy on the workbook’s “Working Spreadsheet” by entering measured HF Spindle currents or Router powers during operations.
Yes of course! …
@gmack
Hmm, I’m sure you’re right… but IMHO this is for noobs like me and your suggestion may be too much for Julien’s simple spreadsheet aimed at basic Shapeoko users? Speaking for myself, I think all I need right now is a much better way of setting F&S that is superior to the default and often misleading ones set in Carbide Create. This will also lead me to better understanding before I get in too deep.
Your excellent advanced spreadsheet is the place to go for advanced users with exotic requirements and so on?
2 Likes
That’s what I’m after: a beginner version that grants a workable (albeit not technically ideal, or you could even call it “wrong”) feedrate , based on very few parameters. Then it’s easier from there to learn a smarter way, involving unit power, deflection, etc…
just a matter of not drowning in too many things to learn at once
3 Likes
That’s not my intention. I was hoping that it would help people (including me) better understand what I consider to be the basics. Maybe this will help with that.
Since you’re a retired woodworker, I imagine that you have experience using routers. With router bits less than 1” diameter, you probably use the maximum speed supported by your router (22,000 – 30,000 RPM) because you can advance (“feed”) the router or workpiece faster without pushing harder (increasing the “feed” force). My default router table “feed rate” seems to be around 100 inches per minute (IPM) and my router’s maximum speed is 25,000 revolutions per minute (RPM). So, the workpiece advances 100/25,000 = 0.004 inches per revolution. So, with a two-flute router bit (or endmill), the workpiece advances 0.002 inches per flute/tooth (IPT) - that’s the “chipload”. If the workpiece shows signs of burning, I decrease the depth and/or width of cut to safely enable a feed rate increase. A typical 10-inch combination blade for a table or miter saw has 40 teeth and spins at 3450 RPM. A 100 IPM feed rate produces a 100/3450/40 = 0.0007 IPT chipload. Recent experience suggests that chiploads of about 0.001 IPT are acceptable for almost everything that folks use Shapeokos (and Nomads?) for (so enter 0.001 in cell D10 of the workbook’s “Working Spreadsheet”).
Properly operated power tools do all the cutting work, the operator (or CNC machine) just positions them. Positioning them properly requires that the operator or CNC machine counteract the cutting/milling forces generated by the tool. (Most of the force produced by routers is perpendicular to the feed direction - i.e. toward the fence on a router table.) The amount of force produced by the tool can be calculated from the magnitude of power it uses when cutting/milling. The magnitude of that power can be calculated from the material removal rate (MMR) if the material’s K-factor (cubic inches per minute of material removal per horsepower (HP)) is known (and entered in cell J15). It can also be approximated from the measurement/entry of the tool’s input power when not cutting/milling (cell D32 of the workbook’s “Working Spreadsheet”) and when cutting/milling (cell H32). Note that other sheets in the workbook show known(?) K-factors and your Janka hardness values – thank you for that!
The maximum amount of allowable machine force used for the calculation of the cutting/milling parameters can be entered into cell J13 of the “Working Spreadsheet”. The default value of 18 lbf is reportedly what the standard X-axis stepper motor can provide. The usable value will be far less than that due to the lack of machine rigidity. That lack of rigidity causes the cutter to be deflected from the intended position due to force exerted by the cutter. Deflection vs force is easy to quantify with a luggage weight scale and a ruler or calipers when the machine is on with a stationary unpowered router. I’d be reluctant to enter more than 3 lbf for starters in cell J13.
The cutting force on the endmill will also cause deflection/bending. The amount of allowable deflection (at the end of the endmill) is entered into cell D13. Too much deflection will break the endmill, but 0.003 inches is likely plenty safe, at least for 1/8” endmills and larger. (That’s probably more that an order of magnitude less than machine flexure induced deflection.) Other required information about the endmill is entered into cells D4 – D9.
Entries in rows 1 - 3 of the “Working Spreadsheet” aren’t necessary but may prove useful for documentation and sharing purposes. (I hope you do both.)
If you use a HF Spindle, leave/make cell J4 blank and enter the spindle’s info into cells G5 – G8. If you use a router, leave/make cell G5 blank and enter its voltage and current ratings into cells J4 and J5 respectively. They’re more indicative of actual router output power than the advertised router power. Leave J7 at 50% unless you know otherwise. Enter your router’s maximum speed into J10.
Some manufacturers specify endmill maximum operating speeds as the tangential speed of the cutting edge expressed in Surface Feet per Minute (SFM) rather than RPM. If SFM is entered into cell E17 when cell C17 is empty/blank, the resultant spindle/router speed will appear in cell J17. Recent experience suggests that maximized cutter or spindle/router speeds are best for virtually everything that folks use Shapeokos (and Nomads?) for. I usually don’t use endmills from manufacturers that don’t provide speeds and feeds information, they may not be safe.
The desired depth and width of cut (DOC and WOC) are entered into cells J21 and J22 respectively. IMO, a good/safe starting value for DOC when cutting slots (i.e. DOC = WOC) is the endmill diameter for all but the hardest of woods. Since MRR (and force) decreases proportionately with width of cut, DOC can be increased accordingly as the WOC decreases. I.E. a DOC of twice the endmill diameter with a 50% endmill diameter WOC seems appropriate.
The entered WOC, endmill diameter, and required chipload are used determine an IPT (cell D11) for the feed rate calculation that compensates for the “chip thinning” when the WOC is less than 1/2 the endmill diameter. That feed rate, shown in cell C24, can be over-ridden by an entry in cell E24.
I hope this helps. Try it, you might like it! Help me improve and/or explain it? Feedback from anyone of any type is welcome and encouraged.
2019-08-04 Speeds and Feeds Workbook.zip (168.3 KB)
4 Likes
@gmack
thanks a lot for the explanation- that helps a lot! I will work through this over the next few days.
I think there is more than enough justification for both yours and Julien’s spreadsheets. They both move us all into deeper understanding and better cutting results.
I have to say though, that the folks at Carbide3D (@robgrz) should incorporate the basic learnings here to improve the F&S defaults in Carbide Create as they are improving it. All it would take is to have a drop down parameter in the job set up to specify whether you have a DeWalt, Makita or Carbide3D router and then deal with the rpm and feed speeds accordingly. The pain, uncertainty, confusion resulting in prematurely ruined cutters and spoiled jobs for new and inexperienced users could be substantially mitigated!
The highest speed of the Makita and Carbide3D is 30,000 RPM and the DeWalt’s is 27,000 RPM. From a purely technical point of view there’s never a reason to use anything other than those speeds if the endmills allow it.
1 Like
Yes - so I now understand - but Carbide Create recommends speeds at the low end of the router’s capabilities and in many cases far lower than the DeWalt can possibly go. That is my concern with the defaults that CC gives - they are just non-helpful in those cases.
For instance for Hard Wood using the #201 .25" cutter for an outside profile CC gives a rpm of 8333 - which is quite impossible for a DeWalt which can only go as slow as about 16,500 rpm. I bet most new users just shrug their shoulders and go with it (as I did) and then saw their cutters overheat and the wood burn (especially MDF at those speeds and feeds even though they put the rpm up at a still impossible 12.5k). It would be a brave person to then set the router at max 27,000rpm and the feedrate at some unknown higher number without any guidance. So as a new user I gradually increased both and it is still clear that I was nowhere near optimum.
These excellent recent discussions and spreadsheets have been invaluable and timely to get my understanding and results far better and to treat the CC defaults with a lot of suspicion when the suggested rpm is less than 16k
2 Likes
IMO, you would do well to disregard what GWizard advises too. But you can use it to vet my analyses by forcing it to use locked speeds and feeds. Beware that the K-factors used therein are generally quite inaccurate though. Thanks for the feedback! 
1 Like
I’ve seen many posts where Dewalt users always operating at max speed were complaining of burning through their brushes very quickly.
Regarding the feed and speed of Carbide Create, I understand that they were developed for the Nomad and they are carrying on and CC does not make a distinction for the machine you use. The Nomad spindle speed is from 2000 to 10000 RPM so if CC recommended 25000, the Nomad users would have to correct the F&S instead of the Shapeoko users.
This is definitely something else that should be fixed in a future version of CC.
3 Likes
All the more reason to use a Makita, which runs faster and quieter anyway. Apparently @Vince.Fab has had good luck using one for years(?) milling aluminum at 30,000 RPM. Someone apparently posted speeds and feeds for Shapeokos here. It’s not clear where they came from though!.
1 Like