Site Navigation

Your Account

Choose Language

These manuals will walk you through the BoXZY experience, from the first un-boxing to using your device for the first time. Please follow each numbered manual in sequence so that you don't miss any crucial information. After you complete 1.3 Using Your BoXZY, you'll be able to move on to the 3D Printing, Laser Engraving, and CNC Milling manuals.

77 Questions View all

Table of CNC feeds and speeds...

I'd like to start milling 6061 aluminum with my Boxzy using MeshCAM to generate the g-code., but I'm hesitant to do that without knowing how fast I can move the router and how deep a cut I can make in a single pass.

I saw a Boxy video that said Boxzy was working on developing a table with this information. Does anyone know the status of that work or has anyone figured out what the appropriate settings are for the bits provided?

Answered! View the answer I have this problem too

Is this a good question?

Score 6
Add a comment

4 Answers

Chosen Solution

You can use Autodesk fusion to determine feeds, speeds and cut depths per pass for the bit you are using, even if you don't want to use their CAM. You should always reduce the given feeds, and pass depths by 50% if you are not an advanced user. For newer users, I don't recommend going slower or faster than 50% of the given feeds as these will give a good chipload at BoXZY's achievable spindle speeds (start the mill around half of full speed and adjust based on results). This is really important for keeping the part and bit cool. The only thing you'll want to personally determine is step-over (vs depth per pass in some cases). Keep in mind the first cut is usually cutting on both sides of the bit, this is the hardest part on the bit. When doing a step-over the machine is only cutting on half the bit and can more easily shed chips (go to advanced information below to know more about how to take advantage of this). Here's a few details:

Brass and aluminum - Material clearing with a 1/4" bit: I wouldn't personally exceed 1/16" depth per pass, 1/32" per pass is safest for quick clearing, go even lower for higher tolerances ( less than 25% of the tool diameter is a good rule for max depth on very hard materials). You can infinitely reduce the depth per pass based on your comfort level without any real issues. Max step-over should be 20% of the bit diameter, I recommend 15%. You can always go more aggressive but it adds noise and stress. I use midway between 3 1/2 and 4 1/2 on the Makita speed control, depending on the hardness. WD-40 should be occasionally applied over the part when milling metal (cover the part, not the bit).

Wood and plastic - Material clearing with a 1/4" bit: I wouldn't exceed 1/8" depth per pass for an internal cut, 1/16" gives really clean results (50% of bit diameter is a good rule for max depth per pass on softer materials). A step-over around 25% of bit diameter works well. For plastic, create a conservative toolpath that will not overheat the bit and melt the plastic. This can take testing and tuning.

The thinner the bit the lower the depth you'll want to cut per pass. I do this by percentage. If the bit is 1/8", I would not exceed 25% of the bit diameter or 1/32" max cut depth in hard materials and 50% of the bit diameter or 1/8" in soft materials . I even then still reduce it a little just to be safe.

- Some more advanced information -

You can use a lower initial cut depth when you are cutting on both sides of the bit and have a higher number for the step-over. Here's an example; I cut a raspberry pi case and I used my max depth to clear the initial cut with two passes, I then used a much more conservative step-over and cut away portions twice as deep as my initial max depth per pass to clear away material and enlarge the cutout (because I was then only cutting on one side of the bit).

You can also reduce the depth per pass and increase the step-over. Example: Do a 1/16" depth cut instead of a 1/8" depth cut and increase your step-over to 40% from the original 20%. This is just preference in my opinion. The cut takes roughly the same amount of time, though it's safer to get more aggressive with the step-over than with the depth per cut.

Was this answer helpful?

Score 4
Add a comment

I spent the weekend educating myself on CNCs and found G-Wizard on the cnccookbook website. Along with the tutorial videos provided, I was able to calculate the feeds and speeds for one of the provided bits. I also have been using the packaged MeshCAM software to generate by G-codes, but now I've run into another problem which I am about to post. The Boxzy interface isn't reading the G-codes. I've narrowed the problem down to Boxzy not accepting G-code commands that do not include spaces between keywords.

Was this answer helpful?

Score 2


I've been going on the CNC cookbook site for months now. A lot of great info, including some tips on cutting aluminum. Not sure whether or not to buy the G Wizard calculator as most of the stuff seems geared to bigger machines. Will definitely download the trial when I pick up my Boxzy.


In one of the video's the BoXZY team promissed to make this information available to us.

Maybe this site can help:


The unofficial forum hasn't seen any action for a couple of weeks now. After looking at some of the material on the cnc cookbook site it is apparent that a lot of variables influence feeds and speeds. Hardness of material, depth of cut, width of cut, cutter size, number of flutes on cutter, etc. I will be giving G-Wizard a try as well as taking notes.


It is always a good idea to check tool manufacturer website for speeds & feeds.

Some tools are designed to specific applications and/or materials.

Things like fixture stability and coolant type are of great importance as well and might be overlooked.

But, I digress.

I guess CNC machining should be considered a form of art ....


Daniel did you ever figure out the MeshCAM issues? I also downloaded the program and like the ease of the interface for a new CAM user but I havent yet been able to generate g-code that can be loaded directly to the Boxzy. I must be doing something wrong. Interested in your trials with it.


Add a comment

I think you would find these links useful.

Was this answer helpful?

Score 1
Add a comment

Quick word on the adaptive clearing toolpath - you want to set your tool engagement to about 40% so that you can take deeper passes while clearing out maximum material from your stock. I was tearing through HMPE with 1/4” passes at 16”/min and the router set at max rpm. It was pretty fun to watch. Great info here -

Was this answer helpful?

Score 1
Add a comment

Add your answer

Daniel Lau will be eternally grateful.
View Statistics:

Past 24 Hours: 1

Past 7 Days: 3

Past 30 Days: 18

All Time: 3,416