First attempt at aluminum failed, please help

I recently started using a new Nomad 883 Pro. I got a 1/4" thick piece of aluminum and I’m trying to make a bottle opener.

I kind of winged the toolpath parameters using some settings I saw on Shapeoko’s wiki. 12 inch/min feed, 6 inch/min plunge, 0.012 inch stepdown, 2 flute 1/8" square end mill 30deg helix AlTiN coating.

Excuse my lack of experience, this is literally the first time I tried to cut aluminum on this machine. The plunge seems to make a louder sound, the machine seems to jerk slightly, the regions where the plunge happens seems to have a rougher cut, it looks bad, like a nick. In the picture below, where A and B are.

C happened after the perimeter was done, the cutter tried to plunge all the way to the bottom, the spindle completely jammed and stopped. I halted the machine by turning off the power completely, as it was trying to do a profile trip with the spindle not moving at all.

What did I do wrong? What should I change? Is my end mill toast? Did I fry my spindle motor?

It seems like the feed rate is fine and not noisy at all but the plunge is terrible. Also, how can I prevent that super-plunge that jammed up the spindle?


Welcome to the forum!

No, you haven’t damaged your spindle; the stock is shot and you should check the end mill for damage (it’s probably OK). This is what learning is all about! We’ve all been there! :blush:

The super plunge will take some research. There could be an issue with your CAD or how you set up MeshCAM for the part. Thankfully, this isn’t hard to figure out… it will just take some time.

No need to apologize! We’re here to help!

Winging feeds and speeds leads to (potential) disasters! Take your time, think, be careful and things will be fine.

The feeds and speeds from one type of machine are not transferable to another! Spindle characteristics, fixturing, and many different factors affect feeds and speeds.

Also, you stated important facts about your machining but left out the RPM of the spindle. When stating a feeds and speeds, one must identify the machine, the spindle (which may be implied by the machine), the feed characteristics and the RPM. If the RPM cannot be stated specifically, tell use the setting of the spindle/router (“11”, “warp factor 6”, “ludicrous speed”).

Without the RPM it’s hard to be perfectly clear about what happened here. That said, the SO3 tends to run at RPMs that are higher than the Nomad is capable of. With that in mind, a feed and speed winged from the SO3 would tend to “push too hard” on a Nomad… and what you are reporting would be expected to occur.

Can you please take a screen shot of the MeshCAM parameters? Also a screen shot of the tool definition (so we can see the RPM)? Also a screens shot of the MeshCAM tool path.

You stated you’re machining Aluminum. Can you please tell us which formulation specifically? There are many and they all have different characteristics. More detail is helpful, 6061 is good, but something like 6061-T6511 would be best.


The aluminum should be 6061, it’s this , sooooo all it says is that it’s 6061, and cheaper than McMaster-Carr

Here are the toolpath parameters that caused the failed project

the spindle was 7500 RPM, that’s a Nomad default, I didn’t think I should touch it.

I think on the next attempt, 10000 RPM, and show the plunge down to 4 inch/min?

The part has 2mm supports in places, I think the “super plunge” happened with 2mm left and right where one of the support should have been.

I tried using FSWizard but the output seems to be less conservative than the Shapeoko settings, so I thought I was in the clear.

On a side note, I noticed that MeshCAM 6 has a folder for “carbide” with “materials.csv” and a Lua script for the Carbide Auto Toolpath Wizard. The materials.csv file does contain an entry for aluminum but it’s been “deactivated”, any idea what’s going on here? Dare me to change that to activated and give it another go?

The actual file is hosted by Onshape

If you don’t want to make an account to view, then download

Here is a screenshot of my path preview

Two quick things:

  1. Plunge should rarely (only in really soft materials) be more than 1/4 of the rated chip-load for horizontal feed-rate.

  2. I can see that because of the posts you’ve left for yourself that you’ve got lead-ins along the posts, but they’re not for EVERY depth of path, so it’s trying to plunge through a LOT of material before it does the actual cutting path, and as a result you’ll also have some pretty deep cuts that are probably more than the recommended 1:1 depth/diameter ratio for the rated feed-rate, and they’d need to be slower to not overload the spindle & axis motors.

The support posts are actually probably causing more problems than they’re worth in this instance, and you’d do better to just model some small tabs at the bottom of your geometry.

See this picture for the problem areas:

It was trying to plunge to these lower paths, and crashing on the attempt, and based on your photo I’d say that’s the case across the board with the issues in the part.

@UnionNine, to model the tabs as part of the geometry, you will also need to model the rawstock and the outer perimeter of the kerf. Otherwise, the tabs as part of the geometry, MeshCAM will happily machine right around thier ends. You’d need to do something like this

For this shot (thank you, @frank26080115 for the link to the model) I’ve modeled a parallel contour at .15" from the part perimeter to allow the cutter a little clearance, and made .02" high supports at the bottom.


But, the true solution to the problem you point out, @UnionNine, is to reduce the machining margin to just larger than the tool radius. Here I used .065" as the margin. MeshCAM takes the cutter axis out along the supports to the machining margin, so you want to minimize that lateral travel. The finer the calculation tolerance, the closer the machining margin can be to the actual cutter radius. MeshCAM always wants to make the margin at least as large as the cutter diameter, so that is something I always need to override…


Good suggestions Randy, but just don’t forget, also slow the plunge-rate :wink:

Thanks everybody

The design is a “copy by eyeball” of but I wanted to take a shot at 1/8" end mills first before snapping 1/16" end mills, so I remodelled it completely, and without pockets

So on the next attempt, increase RPM to 10000, 0.065 inch margins, 12 inch/min feed and 3 inch/min plunge?

You should check out some of the feeds & speeds articles in here and elsewhere to determine those numbers empirically, rather than just guessing at it—so you understand the chipload and know what you’re doing :wink:

So I did look around the forum

@ApolloCrowe gives out TPS files with his tutorials, which is great, thanks, but I didn’t see one for aluminum

This guy @zymurgy here First aluminum job is using 8000 RPM 16 in/min feed 8 in/min plunge, faster than my numbers, but with a smaller stepdown and much less complicated geometry. He claimed to have gotten the numbers from G-Wizard. @ApolloCrowe call the numbers aggressive

@mitchell says 5 and 1 works but is slow. @robgrz suggested 10-12 for feed. @WillAdams links to the same Shapeoko page I was reading

Plugging the numbers myself into FSWizard gives me 20 inch/min feed. From all that I’ve read around here, calculator software cannot be fully trusted yet, at least not for the Nomad, and experience trumps all.

I’ve :v: hacked :v: MeshCAM to give me the Carbide Wizard option for aluminum, with the highest quality setting, it’s telling me 12.2 inch/min feed, 1.52 inch/min plunge, 0.01 inch stepdown, spindle RPM will be 7500

What do you think of those numbers?

I ran 6061 number through G-Wizard and all of those are believable.

There are many correct solutions for feeds and speed. Many are equivalent, some have interesting affects on the finish.

Reasonable roughing (rather than hogging) numbers at 7500 RPM is 13 IPM, plunge of 6 IPM. 0.015 cut depth.

I would definitely rough things first, then finish. Fine finish is 4 IPM, plunge 2 IPM.

Using AlTiN coatings adds 2 IPM to all the numbers.


I would like to suggest the 1/16 cutter over the 1/8 for waterline type cuts like this. Less material to remove.

Your posted numbers should work well and eliminate the step-out from the high plunge rate you saw in the first cut test you posted.

12.2 inch/min feed, 1.52 inch/min plunge, 0.01 inch stepdown, spindle RPM will be 7500

In early testing I was cutting 10IPM 1.5 plunge .015 step down and 10k RPM with the 1/8 cutter.
with the 1/16th cutter that i prefer now, I would slow the feed to 8.5 ipm.

I have a stack of materials to test cut on the PRO so you can expect to have a full set of tested feeds and speeds soon.

Have you tried our fixturing wax?

1 Like

The only reason why I’m avoiding 1/16" cutter right now is I’ve got a fear of it breaking, I figure I make a sacrifice of wasting a bit of time and material to lessen the risk of snapping a end mill entirely. Am I wrong?

I am using that roll of double sided tape that shipped with my Nomad. I didn’t want to mess with wax, as I am on carpet lol I wouldn’t know how to get it out if it dripped. Funny story, the first time I used hair spray on my 3D printer bed, there’s now a dark spot on my carpet where I sprayed it…

I hope I get some updated materials.csv and any updates to the Carbide wizard Lua script. I am not understanding where the “Power” column of materials.csv is derived from. I will eventually need to add my own values for materials like grade 5 titanium.

The “power” for aluminum is set as 400 inside materials.csv, but I don’t know the unit or what property it maps to. Is it tensile strength? shear? hardness? Inside the calculation, this value is used to recommend the DoC and predict the deflection on my cutter.

I finished the cut but the surface is very rough, any tips? I accidentally left the RPM at 7500, or perhaps it’s because the end mill got dulled up, or maybe the feed rate of 12 is too fast?

Also, how do I clean up a AlTiN coated end mill that got a bit sticky? I… uh… cut my finger on it already lol what’s the right way to do it?

By the way, the geometry of the bottle opener is a perfect fit, but the size of this thing doesn’t have enough leverage for a comfortable bottle opener, it works, just a tad small and there’s no comfortable way to grip it

I… uh… cut my finger on it already lol

Been there. Done That. :joy:

There is no practical way a high quality end mill will be dulled in one or two uses with the materials you’re working.

AlTiN coating is not recommended for Al work - it attracts the Al being cut; use ZrN or TiB2 coating. If that end mill doesn’t clean with a stiff brush, the Al is probably welded to the end mill… the end mill is toast. Is it? If so, it also confirms that the parameters are “off”.

Could you please post the the MeshCAM parameters window?


The old parameters were actually 6800 RPM, 12 feed, 1.5 plunge, 0.064 margin. I think touching the wizard overrides the RPM

I made a new cut, 9500 RPM, 10 feed, 1 plunge, and using the Carbon3D factory stock 1/8" carbide end mill, and also no supports (the tape was enough)

could still use improvements but I’m done with this bottle opener practice project for now.

There’s still a small nick where plunges happen. How can I tell MeshCAM to do plunges farther away from a surface? Also I noticed that MeshCAM refused to generate a roughing tool path, why? How do I tell it to do two waterline passes, where the first one is maybe 0.03" away?

EDIT: also, Carbide Motion crashed on me once… I think my vacuum cleaner generated too much EMI on the USB cable. Like… really guys… put a try-catch around all your hardware IO calls and attempt a resume for me. I’m going to order a short dual ferrite double shielded cable soon.

@frank26080115, good-looking workpiece! (BTW “Hecho in Mexico” real-sugar Coke?) About the dual waterline passes on a 2.5D part, see for an idea. (Also

Whether or not MC will do a roughing pass is a balancing act between the calculation tolerance and the machining margin. The absolute minimum theoretical machining margin is the tool radius, but realistically the practical minimum machining margin is about 110% of the tool radius, and that is if you have the calculation tolerance pegged (.0001"/.0025mm depending on your units)


The Cola goes with Fallout 4 these few days.

I read those forum posts, are you suggesting the “fake ball mill” method?

I don’t understand why CAM software is so expensive when Slicers for 3D printing is about the same complexity but plenty of them are free. A few slicers have a feature where the Z start point is randomized to avoid Z-scarring. We need a revolution here. Isn’t CAM tool path generation just the inverted version of slicing?

CNC is a pretty mature market, and up until the desktop mills came out, had a very expensive cost of entry. Perhaps that’s why programs cost big $$$ - it hasn’t adjusted to the new norm yet? Mind you products like Fusion 360 are priced very aggressively so things are starting to shift.

I feel like the 3D printers wouldn’t have taken hold if the printers + the software weren’t affordable and easy to use.

Just a tip, check out Vetric cut2d. It costs $149 and provides a lot of customizations for cutting - for example, you can ramp in your cuts if you like. And you could run 3 cuts in 1 gcode file - a roughing pass, a profile pass that gets to near the bottom of your stock, and then a 3rd and final profile pass that has different parameters from the previous one. Really easy to use and flexible.