Does anyone have a good calculator that can help with speeds, feed, DOC, RPM and other settings that I can put into Carbide Create? I am wanting to move to a shallower cut with more ipm and I am having a hard time finding concrete information with out having to decipher it. Most are ‘claiming’ could run up to 120+ ipm at a cut depth of 0.050" on soft woods and then 0.040" on hard woods. It just seems like that would scream. I use Bits Bits and Carbide 3D cutters (2, 3 and 4 flute on endmills mainly). 4 flute has only been tried once and it was not as successful and I believe it was spinning too quickly (haven’t had time to try it again). Thanks!

1 Like

We had links to various chipload calculators on the old Shapeoko wiki, including the CNC Cookbook one whose author, Bob Warfield guest blogged at:

and see the various discussions here:

and the videos at:

There is a spreadsheet for this at:

but see:

1 Like

Hey Will, would you recommend the G-Wizard calculator as well as the spreadsheet above. So after looking and doing some math, I came up with the following items. I have Shapeoko 5 Pro.

Do these sound crazy for a 1/4" carbide bit as they do to me:

Hardwood (oaks, walnuts, etc.):

    110 ipm at 0.030 DOC (15k-18k rpms) - 3 flute

Softwood (pines, white poplar, etc.):

    30 ipm at 0.040 DOC (15k-18k rpms) - 3 flute

Also, curious on if you have any experience with 4 flute (1/4" - carbide). To get the chips out I have had to slow down the spindle which slows down the ipm you can run. Just picking your brain on that while I am here. I only ask because I have some that I would like to use if I can get the chips out without causing too much force/issues.

I never managed to get the G-Wizard calculator working for me, mostly because I mislike Adobe Air. Some folks swear by it:

while others swear at it.

I just the Carbide Create defaults, and if it seems like a cut isn’t taxing things, will use feed rate override.

@TDA wrote up a system which I used early on:

which I would suggest as a testing/verification methodology — it includes one important consideration for machines which do not have positioning known to the controller, backing off a tested feed/speed so as to have an adequate safety margin.

1 Like

I downloaded G-Wizard and have been overwhelmed with the info and emails from them and have not had time to really try it.

I read the section on Feeds and Speeds in the workbook last night and really want to give the more simple spreadsheets a try. So far I have just been using the defaults, but have not done appropriate adjustments based on DOC and WOC so I want to do that.

BTW @WillAdams I read the section on toolpaths as well and there is some outdated information in there based on the newer CC releases. If we notice something specific like that is there a process for us to notify and/or make some suggestions?

If you mean at:

that would be @Julien

My spin on it is at:

and I’d be delighted for any feedback or corrections (one page actually has an intentional error, to prove that no one needs it/bothers to read it).

Yes, it was the first one since that is what was linked early yesterday. I will look through your version as well. Now you have challenged me with that intentional error. I may be too much of a noob to identify it.

If you spotted outdated info in the ebook let me know the specifics, I’ll try and fix them.

1 Like

Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.

This is a remarkably hard question to give a simple answer to. The problem is that you have a huge number of variables that can change what you should actually be running at. I’ll briefly go into some and link to other posts I’ve made to keep this one from being too long.

The thing I would say is the most important to understand digging into feed and speeds is chipload. The simple version is that chipload is the thickest part of the chip removed from the material per flute per rotation. This combined with surface speed is ultimately what all feed and speeds are trying to get to. As an example if you have a feed and speed of 100IPM (2540mm/m) at 20KRPM for a 2 flute in a given material that is a 0.0025" (0.0635mm) chipload (Feed / RPM / Flutes). That chipload number will mean more to the cut than anything else and can be scaled with RPM up and down for the machine and surface speed.

What chipload will be good for a given material will depend on not just the material but the tool geometry. A few simple examples of this would be rake and helix. The rake of the tool is how aggressive the cutting flute is. The higher it is the lower the forces to cut a material. It comes at the cost of flute strength though. The helix is the twist of the flutes. The more there is the higher the shear forces and force direction changes. This can help to drive more of the forces into the Z and cut material cleaner. However, it comes at the cost of tool strength and if the helix is too high for your material you will start to tear out since more of the forces are moved to the Z. To summarize those examples in their own example. Let’s say we are cutting wood. It will cut better and with less forces using a higher rake tool. You also want at least some helix as that will increase your shear and spread the load to the Z. However, you want to avoid high helix tools as the material won’t be able to hold itself together with too much force in the Z.

After that you have material considerations. Woods are notoriously more problematic as they aren’t consistent. For simple examples again you have hardness (janka), the grain (tightness and direction), and moisture content. Every one of those will change the correct chipload for the material. The hardness is a fairly obvious issue but I don’t think most people realize the true range. Pines are around 350-700lbf, maples 700-1500lbf, oak 1000-1500lbf, hickory 1300-2000lbf, and rosewood 2200-2800. That’s not the top and bottom and I’m chopping part of the ranges. Then you have the grain which will cut differently and have parts that are hard and softer so how “tight” the gain is effect how you can actually cut it (e.g. maple generally cuts cleaner than oak even with the same hardness). The moisture content also changes the cutting dynamics with dryer wood preferred for consistency and tool life. Plastics and metals are more consistent but both still have minimum chiploads you need to hit to keep from melting and to actually cut and not grind.

You then have machine and tool force limits. Assuming there’s not a material limit you are then going to run up against cutting forces. First the tool obviously has a limit before the force on the flute breaks it. You also have a tool deflection which is how much the carbide is bending from the forces of the cut. The tool deflection is also effect by geometry and carbide grade. Those forces also have to be resisted by the machine and it will also deflect (all machines do). How much deflection you can get away with will depend on your tolerances and finish requirements. Eventually it will be enough to cause chatter and/or enough deflection will break the tool as it snaps back to it’s normal position as it slows during cuts.

After all that you have modifiers like runout (how much the tool is spinning of the center axis of rotation). Which can functionally add and subtract an unintended chipload (feed) in multi flute cutters.

All that to basically say there’s not really any great calculators out there as they are pretty much all missing data that changes where your good/best cut will be in YOUR material, with YOUR CNC, and YOUR tooling. So in general it’s better to try and find a decent minimum and work from there.

To answer some specific questions here:

No, you will regularly see industrial machines run well over double or triple that at 0.50" pass depths with good 1/4" tooling. Can you? That depends on a lot but you will reach a machine deflection limit before those machines.

Keep in mind chipload here 110IPM at 18KRPM on a 3 flute is a 0.002" (0.05mm) chipload. That’s barley the rule of thumb minimum for soft material and it won’t maintain it in direction changes. The 30IPM is obviously under it (I’m guessing 30 is a typo).

A IPM range without RPM and flute count means nothing as it’s ultimately chipload.

If a tool “screams” or not is usually related to surface speed, chipload, and geometry. So it will scream in general if you just have much too small of a chipload. However, it will also scream even at a good chipload if the RPM is too high for the geometry. There’s also cases in extremely high aspect ratio tools where you are just screwed noise level wise no matter what.

The short simple version would be that you can treat them proportionally. Until you reach the material limit this comes down to force. The force is mostly cubic material removed per flute per rotation. So if you chop the pass depth by half you can double the feed. It’s not exactly a 1:1 as the helix plays into it but it’s pretty close.

Here’s some of my posts I was talking about to keep from making this one longer.

More on chiploads and surface speeds. Origin/consistency of chipload recommendations - #285 by TDA

More on runout. Precision collet upgrade worthwhile? - #12 by TDA

Deeper break down of some tool geometry and material effects. Best practice for tiny endmills - #15 by TDA

I’ll end this the same way I did on chipload thread. Don’t get bogged down in the optimal or perfect. There are pretty big margins with decent tools in soft material. That not to say you can’t get some more knowledge and get a better result though.

Hope that’s useful. Let me know if there’s something I can help with or expand on.


It was mostly in the toolpath section about paths that are not available in CC. Some of them are now, at least in Pro.

I will look for the specifics later.

Would it be possible to talk on the phone more about this sometime? If not that is okay with me, just thought I would ask.

Way to put me in a tough spot Dave…

Don’t want to get too much into this as I don’t know Carbide3d’s feelings towards us (we sell competing bits). I also don’t want to be doing anything that’s advertising or marketing here… And I don’t want to leave this hanging either… So I’ll just say I’m in the support chain for PreciseBits.


I am going to go out on a limb here and say that the educational value you provide to help Shapeoko users advance their skill sets outstrips the concern over bit revenue for C3D. But I appreciate your consideration over the issue and can also understand any concern from C3D.

On one of my university exams in computer programming, the professor had intentionally made an unsolvable task based on the parameters given, just to see how many really understood programming logic. Over half of the students failed that part of the exam.

Most of the time people don’t give feedback if errors or mistakes are found, the sole focus is to find a solution to their problem, even if that entails fixing the error so that they can have progress.
I have done that myself numerous times, not a good practice I must admit.

So to say that nobody has reported an error to You yet, means that no one has read or needed it, might be a bold statement.

The page in question was written because it was insisted that a “manual” was needed which was mostly made up of statements along the lines of:

Click Connect Cutter to connect to your machine.

I would like to think no one really needs to read it, and I doubt anyone has.

That said, I’ve found (and reported) at least one typo in pretty much every ebook I’ve ever read (and I also found a typo in my second edition print copy of The Fall of Arthur and got a nice note back from the editor that it will be fixed in the third edition, and have had multiple letters printed in national and international magazines noting corrections, as well as a fair number of other books) — this includes Frank Herbert’s Dune, and I waited until it was on sale for $1.99 before buying it to re-read — you’d think if almost 20,000 readers of the ebook are reading so closely and care sufficiently that they would highlight a passage that they would notice and report errors — it’s not much more effort to do the latter.

1 Like

I suspect that meant people feel reporting an error would make them seem ungrateful or like they are being critical.

Others may just not have the interest/time/desire to be bothered.

And some may just skim and never notice.


This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.