CNC Routers for FRC Robotics


So, in preparation for getting the Omio up and going, I’ve taken a crack at generating the CAM to cut out a couple of parts. If anyone would like to spot check what I generated and see if it even vaguely makes sense, I’ve made it available here:

I would LOVE for someone to take a look at it. It simulates all the right shapes, and doesn’t look like it’s going to break any tools, but I’m sure I could be more efficient somewhere.


assuming this is aluminum

Couple comments:

Looks like you’re using a rather wide tool for this work IMO. Your feeds/speeds might be more favorable with an ~1/8in tool. Smaller tools usually have more favorable cutting parameters on routers than larger tools. They also let you fit parts closer together when nesting a large panel of parts.

Your DOC looks really shallow. I think you can go deeper per pass. Like 2x at least.

Much of the machining is full WOC, yet you run a very small stepover for the helical boring operations with the same shallow DOC. I think you should go full DOC with small (10-20%) stepover in the helical operations. This approach takes advantage of radial chip thinning to improve your MRR and spreads wear along more of the tool than many smaller step-downs will.

If you don’t have GWizard, I think you should get it. The cost-savings in good tool utilization is well worth it IMO. For a part like this on *my *router (800W spindle, stiffness-limited to maybe 400W) I would run 28krpm, 32ipm, 1/8in single flute carbide tool @ 0.3in stickout, 0.07in DOC (1/4in plate in 3 passes, with a little plunge into the spoil board).

Hope this helps, and good luck!


Hm, interesting about smaller tool, I thought that generally a slightly larger part would let you run faster as it could hold up to a bit more.

So like 0.06+ for DOC per pass? asid61 had suggested 0.03, so I was sticking to that.

Much of the machining is full WOC, yet you run a very small stepover for the helical boring operations with the same shallow DOC. I think you should go full DOC with small (10-20%) stepover in the helical operations. This approach takes advantage of radial chip thinning to improve your MRR and spreads wear along more of the tool than many smaller step-downs will.

I might need some clarification there - I thought I had the WOC fairly small as well with a small stepover. This is the first time I’ve done this, so a little of that went over my head… Are you saying it should helix it’s way down the .25 and then cut the rest out stepping over at the full .25 down?

Generally, other than being evidently too conservative, does it look okay-ish?

PS - thanks so much for looking at this!


You should start at 0.03" per pass, but you must increase it until you know the limits of your machine and tool. Otherwise, you’re practically throwing money away.
That second part is absolutely correct- helix down to 0.25" (well, 0.28" or 0.29" once you account for material thickness and flatness tolerances) and then do low WOC passes to take out the rest of the material. Look at page 24 of this manual:


Ooooooo, this guide book looks really good. This is the kind of thing I’ve been looking for to really get going.


Any vice or clamp recommendations for the Omio? I know they sell a few, but I was curious if there were any for holding bigger sheets at all. Obviously for big jobs just screw the sheet down to waste board, but I’m always looking to see what you guys have found that works for you. My current plan for most jobs is M6 screws holding an MDF wasteboard to the slots + .201 holes in the aluminum to secure the plate down with #10 wood screws holding the plate to the MDF. (M6 because that’s the size the Omio clamps come with, and #10 because we use #10 screws everywhere and have a lot of .201 bits around.)

Also, if you need to cut multiple identical parts on a small CNC, is clamping two sheets together and milling it out together a thing you can do? I assume so. ie., need to make a bunch of some part out of .125, so stack two together and clamp them down and treat it as .25 in CAM? And/or .25 + .25 and treat it as .5?


You can use screws with a washer and put those around the edge of a sheet to hold it down. Faster and easier than drilling holes into your stock.

As for cutting multiple layers, I would personally avoid cutting like that since it’s a bit too jank for my tastes. You might run into problems with tolerances cutting multiple sheets at once.


Hm, I don’t think I’ve ever seen that done before, do you have a picture or something? I’m curious to see this.


Kind of like this:

I use #6 brass woodscrews and regular steel washers (because brass washers were hard to find). Typically it only takes several per plate.


Interesting. I never would have thought of doing it that way, I was clamps / screw down all the way! This is really useful.


On thingiverse there are STL’s for many variations of clamps. I printed in PETG. They work. However we use a waste board bolted to the T-slot. Use .75 drywall screws to hold plate down. Cam to drill holes first. Then insert screws. This will help with chatter on thin stock. Continue with rest of cuts.


We just got our Omio X8 router in yesterday, and a couple of us put it together today. We assembled everything, but we haven’t yet had a chance to run anything to make sure it works. The router was ordered by our school, and apparently the administration didn’t get an email from Omio with any details (from what I’ve seen, they’re supposed to have emailed some specific version of Mach3 and config files and/or some other guides for how to set everything up).

I was hoping someone who got that email from Omio could forward it to our public team contact email (, with any private details in there removed. We’d really appreciate it, as we’re trying to get the router running tomorrow so we can start milling parts during build season.

Also, I didn’t get a chance earlier to thank everyone in this thread who provided very valuable feedback in our choice of router, tooling, feeds and speeds, and basically everything else I know about CNC routers at this point – so, thank you to everyone who posted in this thread!



Let me know if you have any questions!


I’d start around 0.06 and go up from there.

Yes, for a .25in part helix down, then start clearing things out. Here is a video of this sort of operation on my mill. That is a .25in tool taking a 0.75in DOC in 6061 with 10-20% ish sort of stepover.

Do not sandwich parts. Chips can, and will, get driven between the parts and cause some serious recut and z-height issues. I’ve done it, I’ve learned how to get away with it, but I do not recommend it. The only time you’ll save is setup time, and setup is a small fraction of a job time, typically.

On a more general note: I replaced my dust collector with a much nicer OTS solution from HomeDepot.

It has a little suspension to it.

It does a wonderful job collecting chips. This is what things look like after some cutting. Only a few chips stuck to the light oil on the stock remain.

We also started screwing down sheets with metal roofing screws. The neoprene gasket prevents marring on the metal parts.

This cutting was done at ~24ipm, 24krpm, 0.080in DOC (full sheet depth), in 5052 H32 aluminum.


Just to be clear, those specs you are listing are a for a mill. Could similar specs be achieved on a router? I assume your 0.06 advice is for use on a mill like the specs? Depending on what kind of machine he has and the size of bit he is using, I might start a bit lower.


To reiterate and or/clarify:

On the mill we’ll comfortably do 0.25in-0.75in DOC with 0.25in tools. We always use GWizard to optimize feeds, speeds, and HSM parameters. This is usually 4-5krpm, 30-50ipm, and around 20% stepover in 6061T6. Typically we’ll use a very fine water-based coolant/air blast. It is worth noting that we run out of spindle power on the Tormach 1100 before we run out of tool performance using the end mills that 95 gives away.

On my router, with an 800W spindle derated to 400W for stiffness, I’ll comfortably run 24ipm, 24krpm, and 0.1in DOC in 5052H32 with a 1/4in long single-flute 1/8in Onsrund cutter. Typically I run this dry or with an air-blast. I’ve run up to 32ipm in 6061T6 sheets. I have used the same tool for dozens of hours of this type of cutting.


Alright, so thanks to @RoboChair, we were able to get our software installed and start running our Omio X8. However, we came across a weird issue: we were able to jog the axes and such through Mach3, but when we ran the spindle test G-Code command, the motor didn’t seem to start spinning.

The display on the CNC controller showed the RPM we tried to set it to, and the spindle seemed to make noise like a motor running, but it didn’t turn the bit we had attached. Has anyone had that issue, and what could we possibly do to fix it? We’d like to be able to get everything running early in build season, so any help is appreciated.


It was plug and play for us, make sure the spindle power cable is threaded on all the way, the screw fitting isn’t the best. The control box should be showing some number at 400.00 or below when you turn the spindle on using Mach3, 400 is ~24,000RPM.


We got our new Omio X6 today!


It’s adorable