First Experiments with new Nomad 883

The Nomad 883 arrived yesterday. I got it set up and tried some simple cuts. I did the wrench, which
I guess must be the ‘hello World’ of the CNC area. It turned out ok, but did not quite cut all the way through,
I think this is a zeroing issue. Anyone else see this same thing? Since the example starts with the NC file and
not an STL I do not see a way to adjust the depth of cut which is what makes me think I did not zero the Z axis

I also tried cutting a Thompson silhouette that came from a downloaded DXF. At fist the stock origin and the
part origin were different, and the Nomad started cutting above the stock. I fixed the origins to both be on the
top left side of the stock, and part, and then it cut the part out fine.

The third cut was a simple design I did to cut out a square piece from one inch stock with a couple steps around the outside, some raised letters in the middle, and a small pocket on the top. This turned out great. So I tried making a small box that was an 80 X 80mm square that had a 15mm pocket cut in the top to form a small shallow box. It was running fine until about half way through the Nomad jumped about 40mm to the left and continued running the program. It looked like the zero point suddenly shifted because it looked like the correct cuts were being made but the place the cuts were being made suddenly shifted 40mm to the left. This is not repeatable, just seems to happen once in awhile. I do not want to use the metal vise until I find out what causes this shifting behavior. Has anyone else seen this?

I had reasonable luck with the tape, as long as I used lots of it, and had very flat stock. I found that a cookie spatula is great for removing the stock and finished part from the machine when it is done cutting.

I was pleasantly surprised at how quiet the Nomad is. The quality of the engineering is good, much better than what I found with my Replicator 2. No problems downloading and setting up the software. Only issues are a few parts where the tape came loose, and that issue of the Nomad suddenly jumping to the left and trying to finish the cut over there. Has anyone found better tape than what comes with the Nomad, or are you using the hot glue method?

Pictures of first three parts below. Nothing fancy, but it feels great to have parts on day one!

1 Like

We received our Nomad in February, started with zero CNC experience. Carbide 3D has put together a really nice setup, there is still a learning curve (if you are starting from zero like us) but climbing that hill has actually been a lot of fun.

Regarding the “jumping” you described, that has happened to us as well. Our diagnosis was that the bit was trying to remove to much material. We were either going too fast (feed rate) or the depth-per-pass was too high. We adjusted those settings and the problem was fixed. Can’t really explain it, but its the noise the machine makes that tells us if we are pushing it too hard.

1 Like

The important concept here with the feeds and speeds that I didn’t get at first is chip-load. It’s all about optimizing your chip-load.

Generally speaking, you want to have your machine taking as large of a cut “per tooth” with the cutters as you can with your machine’s limitations, because if your cutter is just rubbing against the material instead of cutting it, then you’re burnishing instead of cutting, which builds up heat and wears your tools out faster. That subsequently makes the machine do more work in the end once your tools get dull, and also decreases finish quality. If you’re taking too large of a bite though, and your chip-load is too high, you’ll break the tool, stall your spindle, or over-drive an axis stepper motor (which is what you’re experiencing).

The limiting factors on chip-load are:

  1. Tool strength: you push too hard against the tool and it can snap, which for us is more likely to be a problem with micro tools and dull tools, as the Nomad can’t push too hard in the grand scheme of CNC machines. I’ve snapped a 1mm long-reach ball-mill, but only because my fixturing job wasn’t ideal and I had misaligned the material slightly relative to the stock as-shown in the CAM.

  2. Machine rigidity & axis drive strength: how hard can the machine drive on each axis? This is where we’re most often going to run into trouble, because the steppers used on the nomad are good steppers, but they’re still just not that big! I don’t know exactly what the delivered force is after you take out mechanical transmission losses, but they can be overloaded if your feeds are too high, especially when they’re trying to accelerate or decelerate quickly (because inertia). Also, there’s inherent elasticity in the belts on models driven by those rather than lead screws, and in the case of the So3, it’s riding on plastic v-wheels.

  3. Spindle speed: the reason the saying is “feeds 'n speeds” is that these two factors do a dance to determine chip-load. The faster you can spin the spindle, the more aggressively you can drive the tool around, because the higher spindle speed is reducing the per-tooth chip load on each revolution of the tool. We are somewhat spindle-speed limited, because we want to run in the nomad’s sweet-spot of about 5krpm for most cutting tasks. It can run up to 10krpm, but it’ll generate a lot more heat and wear the bearings out faster than if you run it at a slower speed. We’re not production shops, so what’s the rush?

Therefore when you’re trying to figure out what your feeds and speeds should be, you want to find out what the ideal chip-load is for the material you’re cutting is with the cutter that you have, and then using the spindle speed available (which is up to ~10krpm, but shooting for 5 to 8krpm) and figure out the feed rate from there. Once you’ve gotten the feed rate calculated, you evaluate that feed-rate and think about if it’s faster than the machine can and/or should drive, which has a max speed 100ips on X & Y (inch per second) and 50ips on Z, and remember, inertia with going into and out of the stops.

Realistically, you should typically keep actual cutting feeds well below 50ips, otherwise the machine will be less accurate going through the material, as the steppers will be more likely to lose steps when trying to decelerate into stops and corners and accelerate out of them while still engaged in the material. This is especially true of material with non-uniform properties (wood and composites) that offer varying resistance to the tool. You can go fast in foams, waxes, and soft plastics, but use any feed optimization functionality your CAM provides for easing into and out of corners smoothly.

You can cut lightweight polystyrene foams and balsa at ~60ips I’ve found, but even for soft hardwoods like poplar, I don’t do roughing passes faster than 45ips, and I only go that fast with feed-rate adjustments turned on in my CAM planning so that it slows down going into and coming out of corners so it isn’t jerking around.

If you think the feed is going to be too fast given the speed that you’ve calculated with and the material you’re cutting, then you can slow the spindle speed down to decrease the feed-rate accordingly to maintain optimal chip-load, and that way you’ll be less likely to over-drive an axis motor.

And, sometimes you have to take smaller bites and take a little extra tool wear because of the machine’s limitations. Since the spindle is a 50w brush-less system, too high of a chip-load will stall it in certain materials because the spindle can’t offer enough torque, even if the tool is designed to cut more aggressively.

Hopefully that’s some helpful background theory to get better cuts with your Nomad (or Shapeoko3) :smiley:



Thank you for the info on chip-load, it is very helpful as I am learning how to effectively use the Nomad.

I used the settings that came from running the ‘carbide tool path wizard’ after selecting ‘wood-soft’ and ‘tool #102’. The feed rates the wizard generates are shown in the attached screen shot. The tollbooth wizard picks a feedrate of 68in. I did try it again using 50in and got better results, but the cutter still jumped out of the programmed path near the end of the cut as it was rounding a 90 degree corner. Should I try again at even slower speeds?

What settings for depth per pass and feed rate should I be using for pine and plexiglass-acrylic? Should I just add a custom tool with the settings you suggest and then use that instead of the tool path wizard?

I have much better luck holding wood stock using hot melt glue than the tape that comes with the Nomad. Removing the glue is a bit of an issue, but at least the part does not come off during the cut. Do you use hot melt glue or have you found a better tape?

What is an effective way to hold down plexiglass-acrylic?

I feel I am getting close, if I can get the right speeds for pine and plexiglass-acrylic and a more effective way to hold stock then I can hopefully get more consistent results.



Hi Steve,

Getting straight into the specifics now I see :wink:

I would recommend reading this article about the chip-load from CNC cookbook for more background on the concept of chip-load when you have some time, then consult this article about end-mills from Make magazine if you want more helpful diagrams and descriptions, and lastly when you’ve got some serious reading time, dig into Michal Zalewski’s excellent treatment on hobby CNC and resin casting.

You’ll have many questions answered you didn’t even know you would have, as you go about learning this stuff :slight_smile:

Ok, to answer your questions:

  1. Should you try slower speeds? Possibly. More importantly, the “tollbooth” wizard probably isn’t optimized for your material and the stiffness limitations of the Nomad, just some fine-tuning to do there probably. Also, there’s a fair bit of difference between different woods, and as soon as you hit a knot all bets are off. Check out the Janka hardness scale, and also this bit about guesstimating feeds based on it, as well as running your own sweet-spot tests based on the wood you’re trying to cut with a given tool.

In your case, instead of just reducing speed as a first-step, I’d be inclined to reduce your step-over. When you have the tool trying to turn a corner and then “plough-cut” through that much material without any momentum, that’s more likely to overload the steppers than if you keep a greater depth and maximum speed, and just take 1/2 to 2/3 of your tool’s width per pass. Try it, and see if it works better for you.

As one tertiary thought, you may want to try setting it only to climb milling rather than “use parallel path” for your roughing pass if you’re cutting soft wood, or just conventional milling if you’re in a particularly hard wood. I say this because in climb milling the tooth is engaging the most material at the beginning (which will take a bite out of softer wood that would otherwise want to yield and rub instead of getting cut) and conventional milling engages the most material at the end of the cut, so it induces less vibration in the tool and work piece as it cuts. Your mileage may vary, it may help or may not matter depending on your wood, fixturing, etc.

  1. Should you set up your own custom tools with suggested settings instead of using the wizard? Yes, and no. You should be figuring out what works with your available tooling in your available materials, and making note of it, but you may not want to make different “tools” for each different material, instead just get used to entering different values into MeshCAM to get the desired results in each material with the base tool definitions you have.

So basically, create a spreadsheet that is divided up per tool and per material, and note what’s working well and what needs tweaking, after you look online and find good starting points like these Onsrud tables for their tooling.

I use Fusion360 which has HSMworks embedded in it for much of my work, so my tool library looks like this:

Individual tools have a lot of different details that I’ve programmed in:

And I’ve created a holder profile to approximate the ER11 collet nut, so when it simulates toolpaths it takes into account the holder so I don’t bottom it out into anything:

But, even with all that pre-programmed in, I still end up adjusting feeds and speeds based on the ideal chip-load in the material with a given cutter. If you dig around on the internet you’ll find tables like this one that give general recommendations for starting points on different materials.

Acrylic, Aluminum, and Hardwoods are all within-range with 0.004" chip-loads, which at 5krpm and a 2-flute cutter works out to 40 ipm feedrate.

The settings given in the toolpath wizard would put the chip load at 0.0068" per tooth, assuming 5krpm. That’s a bit high for all three of those materials with a 1/8" tool, but would be better (but not quite enough) for a 1/4" tool.

As for depth per pass, machinists with bigger equipment generally try to get a 1x diameter depth when plough-cutting at rated chip-load, and feed is reduced by 25% for 2x diameter, or reduced by 50% for 3x diameter.

Since our machine is belt-driven and isn’t that rigid, I would recommend starting at 0.5x diameter for depth in most materials, with 1x diameter being the goal for roughing passes. I generally leave 0.005" to 0.01" of material to remove with the finish-passes—more for softer materials (Poplar, Acetal), and less on harder ones (aluminum).

I’ve used both tape and glue, and the tape works well as long as the materials are non-porous/minimally porous and clean—free from oils/moisture and dust, and you’re not cutting too aggressively where you’re going to pull the work-piece up.

In order to ease part removal when working with the glue, you want to apply a thin bead around the edge of your block of stock material, not under the middle, because you want to be able to apply a bit of rubbing alcohol after a job to it to get it to release—I haven’t looked into why rubbing alcohol makes the hot-glue release, but it does as long as it’s wetted. Once the alcohol evaporates the glue returns to full-tack strength if you haven’t removed the piece fully yet.

Tape should work well for plexiglass, especially if you’ve got a nice clean spoil-board to tape to, and don’t make your cut-depth to great. Try pressing and holding the tape for 10-15 seconds before letting up, to make sure you’ve really make a good connection between the tape, work-piece, and spoil board.

Alright, I have to get back to some actual work, so good luck!



Thank you so much for your help, I really appreciate
it. I am going through all the links you provided, and will then do some more experiments based on your recommendations. There is a lot of interesting stuff to learn, and that is part of the fun. I will let you know when I have made some more progress.




I changed the feeds and speeds for pine based on your suggestions, and the information I read in the links
you provided. The values used are shown in the attached screen shot.

When I used roughing, the cuts came out as expected. When I tried a cut without roughing, the cutter left
the expected path about half way through the process and went right through the design where it was not supposed to cut. The design is a 2.5D rectangle with a pocket cut in the middle. I thought I should be able to do this without roughing, but it caused the cutter to jump off the path. Why would this happen?

In the finishing section should I use the same value for ‘step Down’ in the Waterline function that I use for ‘step over’ in the first ‘cut along X’ finish pass?

I found some carpet tape at home depot called, ‘Roberts Double-sided carpet seam tape’ and it seems to work much better than the tape included with the Nomad. It seems to work about as well at the hot melt glue, but is easier to clean up and remove.

I am now experimenting with cutting some Acrylic. If that works you may here cheering coming from the northwest :smile:

Hi again Steve,

Roughing is very important—it’s probably better explained as “bulk material removal” because that’s the process by which you’re going to get rid of 95% of what you want to cut. If you don’t have those passes clearing the way, then you’re engaging the cutter a LOT more when you go to do the finish pass, likely more than the .5x to 1x diameter-to-depth ratio I mentioned. The point of the finish pass is to remove just the last few bits remaining with minimal forces on the tool and work-piece so neither deflect under loading.

If you’re trying to just cut out a profile, then you will want to use “Waterline” finishing but with an appropriate step-down and feed-rate (it uses the same value from the parallel pass section of finishing options) so that you’re not biting off more than the machine can chew. You’re definitely not being aggressive with the 0.428mm step-down, so I’m not sure without seeing the tool paths what it was trying to do, but it may be because of your angle limits or something that it went straight for a pencil clean-up and dove right in…

Glad to hear the double-sided tape is working better, I"ll have to see if I can’t track some of that down here where I live :smile:

After reading about feed speed based on the info from @UnionNine, I reduced the feed rate to 35in, and set the stopover and depth per pass to half the cutter diameter. This yielded better results and allowed me to complete the lighted sign project I had been waiting to do since ordering the Nomad. The photos below show the sign both on and off. The name is cut to a depth of 3mm in 6mm thick plexiglass. The base is pine, and of course needs some stain.

I initially used the speeds recommended by the ‘Carbide Auto Toolpath’ in the tools dropdown menu. That caused problems, and after significantly reducing the speeds things started working better. I wonder if the AutoToolpath Wizzard needs to be revisited with different numbers. It seems like new guys would try that first so they should have know good parameters…

I still see problems with the the parallel finish pass. What I am seeing is that in some parts the roughing and waterline do not cut in a particular area, so when the parallel path starts it is taking a bite which is the full thickness of the wood and that is too much for the Nomad so it stalls then takes off in the wrong direction. If I do not do the parallel cut things work, but I am left with material I wanted removed. Anyone see this sort of issue or have ideas on what to check?

It seems like roughing and waterline should take away material so the parallel finish is just removing a small amount. For some reason this is not happening with some parts and the parallel cut tries to remove way too much material at once.

The sign in the photos below was the practice piece, now I can try something more interesting. The light comes from LEDs in the base that shine up through the acrylic.

1 Like

Hi Steve, it’s hard to say why it’s leaving material behind without seeing the settings and the toolpaths. Can you post those for us to scrutinize? Also, did you import an STL or generate one from a 2D file?


After watching the machine cut, and looking closely at the simulations in Meshcam Pro, I found that the problem was that the part had an angled surface sloping downward in the z-axis and the roughing pass was not using ‘3D roughing’. The surface angling down into the z-azis was not roughed, and when it was time for the parallel path it tried to take the entire depth of the angle in one bite, which was too much and caused the machine to stall and jump. Now it seems obvious why it is called 3D roughing. :slight_smile: I finished the design of a knife and it is being cut now. I will post the results in another thread. Lots to learn…

I have to ask this as im in dis belief that these values would hold up for cutting aluminum on a nomad 883.

if i’m calculating this right, the formulas would recommend with an 1/8" flat mill -5000 rpm @ 40 ipm W/ .063 doc

in my tests, I am lucky to get 5ipm w/ .01doc @ 9000rpm w/1/8" flat mill

maybe works better with higher tooth engagement?

The formulas don’t take into consideration the spindle power and the machine stiffness and axis-motor power available, so hypothetically, yes those calculations might work out for optimal cut characteristics… but aren’t what this machine can do.

The nice thing about CNC Cookbook’s feeds & speeds calculator is that you can include the spindle power (wattage), and you can ‘de-rate’ the values to reflect what the machine can do.

For longevity of the useful life of your tooling, you’ll want to try to keep to the optimal chip load for the cutter and material combination in as deep of a cut as the machine can push, because you want to minimize tool burnishing (rubbing) against the material, in particular because the heat from rubbing is the number one enemy for the tooling.

@davidgjohnson I have been meaning to get to some aluminum projects soon (making a set of church keys with the company logo on them) so when I do dial in my feeds & speeds in aluminum I’ll post them for you here :slight_smile:

thanks, I look forward to it.
im using the following:

9500 rpm
.01 doc (started at .04 worked down)
.05 stepover
5 ipm feed
2 ipm plunge

1/8 flat mill 2-flute, 45*, zrn coated
using cutting fluid and I still get stalls on 6061 (85 bhn)

@davidgjohnson @UnionNine Mark has given me these numbers for Aluminum with a 1/8’’ 2 flute endmill:

10K RPM, 15-20 IPM, 0.02-0.03 DOC. Plunge at 6 IPM.

This is roughing speed. Finish is much slows for a fine finish - 6 IPM, 0.01 DOC.

I have tried 10K, 16IPM, 0.02 DOC for contouring on 6061. It works fine for me. Finishing wasn’t great, I didn’t add a finishing operation and also maybe because I didn’t clear out the swarf well - going to try the air nozzle solution from the other post. Mark also suggested a DOC of 0.03.

I stalled the spindle trying to cut a hole of about 0.150, didn’t have enough space for chip remove I guess. I switched back to my old feedrate of 8K, 12IPM and 0.01 DOC which worked fine for the tight space.

@cjm27 what cutter are you using?
I cannot get close to those values…
the plunge will stall me for sure.

I thought the zrn-coated high angle 2 flute would help with the issues you mentioned.
it hasnt seemed to help.

I have the Lakeshore Carbide 2 flutes ZrN coated corner radius endmill. I forgot what flute angle it was, but I think our cutters are similar and it shouldn’t be the problem. I have been using WD-40 for lubricant, and your cutting fluid should work better. If there isn’t anything special about the programs you are running (I do a lot of slotting, which is pretty demanding), I don’t see much difference between our setups.

Mine is a Pro, but in the end it shouldn’t make that much difference. Any chance it’s a problem with your machine?

I have tried WD-40 as well
using 6061 (85 hardness) from McMasterCarr.

I purchased some MIC6 (cast aluminum) to try at some point because it is much softer.

I just went back to your previous posts and saw the 6061 part… So I went back and edit the reply.