Small details bit tool breakage

I am trying to carve tiny details in small pieces of hardwood (playing around with bloodwood as well good ol’ Maple).

I am using G-wizard, but my bits break every single time. I’m trying to adjust the speeds and feeds, but I don’t know what I’m doing and it’s not working. Also, it takes about 6 hours to do an incredibly small section of the design. To carve my entire design would take five days (at least), and it’s only 1.5" by 1.5." Obviously, I am doing something wrong.

Below are my settings. Some of you are going to wince at these numbers, probably - others will get a good laugh! But once you get off the floor, have pity on this newbie and please tell me what I need to change, read up on, or whatever. I’m here to learn…

Bit: 0.051" micro carbide 2-flute end mill
Depth per pass: .001"
Stepover: .007"
Feedrate: .05"
Plungerate: .007"
RPM: 9000
Max depth: 0.035"
Offset direction: Pocket

Also, I notice the spindle gets pretty warm (almost hot), which I’ve been reading can mean it’s rubbing - too slow. So I’m guessing I need to increase the feedrate, but I don’t know by how much. And I’m frustrated that G-wizard’s settings don’t work. I mean, I bought it for this exact reason. I wasn’t; expecting magic, but the amount of time it takes if I follow their recommendations seems extremely excessive, and even at those slow speeds, the bit breaks within minutes.

Any help is appreciated. . .

What are you using for CAM?

Why are you not roughing w/ a larger endmill, doing clearing passes w/ a medium-sized one, and only switching to the small endmill at the end?

Carbide Motion

Good question about the larger end mill for roughing. I guess two reasons. First, most of the details are very small - I don’t think I could go much larger to rough anything out on some of the design. I certainly could for some of it, however.

Second - and this is a bad excuse - I don’t really know how to clear passes with a larger endmill using CM. Can CM even figure this out? Which paths to do first, and then when to switch to a smaller endmill? I was playing around with Meshcam for a few weeks, and it seemed like that program could figure this out for you . . .

But then I thought while I was learning I should just stick with Carbide Create and Carbide Motion. Trying to keep it simple while I get the basics down (Meshcam seemed more complicated). MAybe I was wrong to do that? I can always go back if that’s the way to go…

I also downloaded Fusion360 but that was WAY above my head.

Where are you getting your bits? I cut very hard woods such as purpleheart, wenge, padauk, katalox, Bolivian rosewood (pau ferro) and bamboo quite often with bits much smaller than that ( 0.0472", 0.0394", 0.0315", 0.0276", 0.0236", 0.0197", 0.0177", 0.0150" and 0.0120") at more aggressive feeds and plunges without breaking them on a regular basis.

For instance, I run:

Bit: 0.015"
Depth per pass: .020"
Stepover: 40% or ~0.008"
Feedrate: 20 IPM
Plungerate: 15 IPM
RPM: 25,000

Unfortunately, since I am doing 2D work, I use Inkscape and, so I can’t help you on the software side of your issues.

Also regarding the roughing with a larger bit vs finishing with a smaller bit; is this a 2.5D contoured pocket type engraving, or a 2D flat engraving? If it is a 2D pocket, you can rough with a large bit, then do an inside profile with a smaller bit to get the sharp corners. So, for me, I will clear a pocket with an 0.063" bit, then do an inside profile with an 0.0315" bit. You can go with a smaller bit that is no smaller than 1/2 the diameter of the larger bit without the smaller bit missing material in the corners.

I’ve been trying bits from various sources. The bits I’m using now come from DrillMan (on Ebay) - he was highly recommended by some folks on here so I thought I’d give him a try.

Where do you get yours? Those sizes sound awesome for “down the road” stuff I’d like to attempt…

I am doing 2D work right now. I was hoping to cut channels in a darker wood and then cut a reverse out of a lighter hardwood for an inlay. . . not easy to do with these sizes, I’m discovering. Might also try colored epoxy in light wood if my idea doesn’t work. . .

I just downloaded Inkscape the other day but didn’t delve too deep. Also seemed above my skillset - steep learning curve, from what I could see, but I am willing to learn how to use it. Don’t know much about makercam. I’ll look into that, too.

Thanks for the advice in your last paragraph. That sounds exactly what I need to move forward. Many thanks, MadHatter (and nice username!)

P.S. I also cannot go above 10000 RPM with the Nomad, so your 25,000 makes a difference, I suspect!

MeshCAM automates multiple endmills — for Carbide Create, it’s a bit trickier — you have to lie to CC about the endmill diameter or add additional geometry to leave a roughing clearance.

If you want to do inlay, you may want to consider Vectric Vcarve which has especial support for it.


My bits are also from Drillman1. I have bought a few from other sources, but of the ~200 or so bits I have bought, most were broken due to “operator head-space and timing issues”.

I started with Inkscape before I even received my SO3 so I would have things lined up to cut, and (as I previously said) I do 2D cutting, it works fine for me. I recently bought Vectric V-Carve and although I bought it mainly for the diamond drag engraving feature, I do plan on using it for actual v-carving one of these days.

It definitely doesn’t hurt to try out different software as long as it works with your machine. Sometimes, regardless of how much you try, you just don’t get one program, but another seems to suit you just fine. For me, Inkscape is similar enough in feel and commands to PowerPoint and Visio ( that I have used at work and home for 15+ years) that I was able to pick it up with no problem, so I use it mostly even though it looks like V-Carve has some pretty cool design features.

Interesting. Thanks! I’ll check it out.

Definitely cutting too slow in feed and plunge rates. Not sure what you are putting into G-Wizard but when I did it, for Sugar Maple (the harder of the maple options), I get the following:

For Slotting, where you have the full diameter of the mill engaged (a worst case scenario):
DOC: .0003"
RPM: 19000
Feed / Plunge: 3.52 IPM / 1.8 IPM
Turtle slider at 15% for very conservative.
If you adjust the RPM numbers up, you get faster Feeds / Speeds as well.

You need to cut faster but you also have to pay close attention to deflection limits and use conventional milling. You probably need something better than CC to create your toolpaths, as you should be ramping / helix into your pocket if you cannot use a larger clearance tool. I can cut brass with 1/16", 1/32" (.03125") mills and not break them. The way you engage the material can be just as important as feeds / speeds.


Thanks. That’s very helpful. I don’t think my Nomad spins faster than 10,000 RPM. Maybe I’m wrong about that?

Anyway, I’ll get more aggressive with my cuts.

I think I’m going to invest in v-carve. Seems like it’s pretty great at inlays, which is what I want to do, plus it can obviously do a lot more than what I’m currently using. Or I’ll go back to Meshcam and figure out how to rough out my pockets with a slightly larger bit.

Again, thank you for taking the time to give me advice! This community is fantastic.

Ah, you are using a Nomad. I calculated based on my Shapeoko. That might make a difference but I believe your Nomad spindle should go more than 10000 RPM. I also categorized this whole thread into the Nomad sub category, that way it’s a little more clear to others. I still believe you should be cutting faster.

Always great to see another Nomad coming to life! Believe you are correct on RPMs - unable to go over 10,000 RPM. I am not particularly familiar with hardwood but from ‘feel’ your feed rate does seem pretty slow - 1/20 of an inch/min - probably more rubbing than cutting. It’s tricky to get the right feeds with tiny bits like that as instead of chattering or stalling they just break when pushed.

WRT to breakage - is there a particular action that causes them to break like during plunging down into the material or while in a slot the same width as the tool? Might get some clues from that.

I use to cut copper 1/16" carbide flat whit DOC 0.07mm. Feed 400 mm/min Plunge 170 mm/min RPM 19000 and coolant Trichloroethane whit good ventilation .
A few drops each time Trichloroethane is required , not much is not necessary.

1 Like

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