CNC Routers for FRC Robotics

This post isn’t going to machine itself. Let’s begin.

The topic of this thread is CNC routers and all associated topic content. The intent of this thread is to create a highly comprehensive discussion about CNC routers and how teams use and abuse them. This is to provide an easy reference to any and all interested teams who want to do the same.

Let me start this off with saying that a CNC router is one of the most powerful tools for FRC teams that money can buy. If I had to sell all of my equipment except for one machine, that one machine would be our CNC router. Every team would benefit from a CNC router. Regardless of what you currently have (even if you have a shop full of VMC’s), CNC routers will still add some serious productivity boosts. This is my personal opinion and it is fine if yours differs from mine.

Why is a CNC router such a powerful FRC tool?
–Rapid prototyping with a 4’x4’ bed to work with allows quick development of mechanisms with very accurate dimensions that can be changed and redone quickly.
–Machine any square or rectangular tubing reliably, repeatedly, and rapidly. Includes bearing holes and rivet patterns.
–Fantastically easy sheet machining in polycarbonate.
–Easy machining of sheet aluminum(with appropriate CNC) for parts such as the following, bellypans(lightened), gussets, thin gearbox plates, and sent sheet metal component flat patterns.
–Machining of plate aluminum(3/16"+) is not hard at all(with the right machine set up) allowing you to make the following parts, drivetrain side plates, drivetrain gearboxes and similar, chain sprockets, certain types of gears, and much more.

Every CNC router is a different machine and behaves differently than any other model. Unfortunately this means that it can be very hard to find good advice about feeds and speeds for a given machine without tracking down someone using a similar setup and tooling. Unfortunately this also mean that the only machine I can give that kind of advice for is the VeloxCNC routers, mostly the 50x50 model. I’m going to leave a lot of the specifics of feeds and speeds out because it would be a lot of work to put it all up here and you will get more benefit from my CNC router video series.

What machine should you look at buying if you are interested in owning a CNC router?
This is going to depend on a few factors that will be team specific.

How much space can you make?
We all have limited room for equipment and it can be hard to find a place for a large CNC router. Our VeloxCNC takes up about 8 foot squared and it is a large chunk of space. I suggest you buy the biggest machine you can support within your space. It is worth the sacrifice you make for the space and you could very easily work a storage system into the stand/table your router sits on so the space is used effectively. For FRC type work there is not much benefit to a 4’x8’ bed size because almost nothing we build requires any part with a dimension over 4 feet long. If you have plenty of room, go for it. DO NOT get a machine with less than 4 feet in at least one dimension as it will seriously hobble the utility of the machine. 4’x4’ machines are a perfect fit for the work we do and allows us to machine half sheets of whatever material we want.

How big is your budget?
This is the hard part of giving advice for what machine you should look at. With any major piece of shop equipment it is worth spending as much as you can reasonably handle on it. Every additional dollar gets you more machine than the previous. It is always better to plan to save up to get the bigger or better machine than to get a cheaper machine now. Pick the machine you want and need, then find the money to make it happen. It’s a lot easier to convince sponsors to give you additional funds when you have a very specific plan for what you are going to do with them.

What are the important points for a CNC router that will be cutting metal?
Rigidity! You want a solid machine that can both drill and mill. To accomplish this you need a rigid gantry design and minimal cantilevered loads on the machine. Raw motor speed and power are not as important, but you do need a spindle that can handle the loads.

What machine do I recommend and are there any others I would want to avoid?
Begin personally biased opinions here-> I LOVE our VeloxCNC. It is solidly built and handles everything I throw at it admirably. The gantry on our 50x50 is built like a tank with thick plating and doesn’t budge easy and the 2 acme screws it uses on the Y axis make it really easy to maintain square. Furthermore, Velox is the only company I’ve seen that shows their machine tackling a serious block of aluminum in their demo videos. As for machines I would say to avoid, stay away from the desktop models as they are rarely stiff enough to even machine aluminum.

What flow process does 1678 use to make their CNC parts?
Once we have the CAD of a given part we convert the faces to be machined to .DXF format to use with our CAM software. Occasionally we have a part with a lot of features that is difficult to generate effective toolpaths for with our usual software and we instead generate the toolpaths in SolidWorks with a CAM plugin called HSMxpress(the free version). Our default CAM software is Vectric Cut2D Pro and I highly recommend it for a number of reasons. Mainly, it is a very straightforward program that is dirt simple to learn and use: I like to describe it as the MSPaint of CAM software: easy to use and easy to do all the basics but lacking many of the complex features of more expensive software. That said, you don’t need PhotoShop to make a picture of a circle. It’s most powerful feature is definitely it’s best: the auto nesting feature. Drop a few dozen parts into the program and hit “Nest” and it does all the work of nesting your parts with minimal material waste. Afterwards, we generate our G-code for all the parts we are going to run. We’ve developed a tool library that is segregated by material type where our cutters have all of their settings tuned for that specific type of material to make tool selection easy for our students. Then the G-code is loaded to a cloud storage location and our operators can download the new code and run the machine.

Running our machine
Our machine can be broken down into 2 main areas of use: the sacrifice table and our tube jig. Most of our work is done by using the 2 layer particle board “sacrifice” to hold down stock with screws and machine the majority of our parts. We also machine the whole thing flat so we can get good depth control on 3D parts.
At work I use PVC foam instead of wood and run a water based oil emulsion coolant, it is a lot more expensive but ambient humidity was enough to mess with the flatness of the wood. Off to the side in the second image you can see our tubing jig which uses a number of toolmakers vises we got from to support up to 4 inches of tubing in width.

The tubing jig has a set work offset in our controller software for the router (Mach3), so all we need to do is load a tube already cut to length and run program.
We run an air line to the router from our compressor and we use a mister nozzle that runs WD-40 when we run aluminum to keep the cutter lubricated and cool while clearing the chips it makes from the cut path. We also run a shop vac with an extended line and a Loc-Line nozzle down to our work area to suck up the excess chips. At a minimum you should run air, but coolant of some kind is highly recommended.

When running aluminum it is important to use end mills with fewer flutes to maximize chip clearing. We prefer to use single flute cutters, but 2 flute also work well. Please save yourself the hassle and buy good quality end mills and drill bits. For drill bits you want split-point 135 degree short length bits. Chisel tip drill bits take much more force to drill with and your spindle and Z-axis will thank you for using split-point drill bits. We don’t make our router drill any larger than a #11 drill bit for 2 reasons. The first is that it is easier on the machine and second is it improves the accuracy of your drilling by minimizing spindle deflection from the plunge forces.

CNC Router Video Series
Please look forward to seeing some more videos by me and 1678 popping up over the summer! I am going to be making them for a couple of reasons. One is to make it easier to train my students how to use our machine. Second is to enable the FIRST community to have a technical resource to learn the various methods we use to make our router easy to use for our operators and not have to learn it via trial and error. I’m really looking forward to doing this and having a bunch of videos with various topics related to running a router for FRC. Please let me know if there are any specific topics you would like to see covered.

Part examples run on our VeloxCNC
This is a 3/16" thick gearbox plate we used for one of our shooter designs this year machined out of 6061-T6 aluminum.

This is a belly pan machined out of 0.090" 6061-T6 aluminum.

This is a battery pan made out of 0.063 5052 aluminum.

If you have a CNC router please write a post about your experience with it, any troubles you’ve had, your recommendations, and any particular praise you have for your machine. I want to see lots of input from teams of all walks about their experience with CNC routers.

Best Regards,
Devin Castellucci
Team 1678


Thanks for putting this together! This is a great resource.

Where do you buy your cutters, if it’s not a local supplier? And is McMaster a good place to get cutters?

Also, what are your thoughts/experience with buying a used CNC router? Is this a potential way for teams to get a good product at a cheaper price, or is it asking for an expensive paperweight?


Great start Devin. Looking forward to additional posts.

My team received a ShopBot table top machine with a 2’x3’ base. We installed a 1/4" diameter 2 flute cutter at 10,000 rpm, the slowest setting and have clear cover. Its great for safety and reducing dust and machine sounds.

We mounted an MDF board on an alum T-slot base and installed wedge nuts under the board to allow bolts to clamp the work piece. On top of the board we attached 2 pieces of material, one vertical and one horizontal to create a defined 0,0 point and x,y orientation.

Our vac is set to blow to keep the cutter cool. I’m not interested in using a mist because we are in a very small room with no air movement. Plus I’ve used a hand held DeWalt router at 6,000 rpm on thick alum without a problem.

We are novices learning how to use the machine and trying hard not to break it or snap a cutter. Right now we are learning the CAM software and trying to understand how to keep the cutter above the wood clamps while moving to the cutting pattern. We are trying things out on plywood before switching over to alum.

  • How are you holding your work piece?
  • What is the term for cutting a profile path but not cutting all the way thru the piece in a few places as a way to keep the part from moving?

Build Mentor

This thread is perfect timing as 558 just placed our order for a VR-3636. Could you please provide more info on your cutter selection, speeds and feeds and what CAM software you are using. We are excited to get our into the shop and start making chips.

Your tubing setup is excellent and something we will absolutely have to look into, thanks for getting this discussion started.

Hi Devin,

What spindle are you using? Is it VFD? Speed range? Just curious.

The CNC Router I have access to currently has an off-the-shelf Hitachi router as its spindle, I don’t believe it can go down to a reasonable speed for milling aluminum without damaging cutters.


I believe you are referring to Tabs

At AndyMark, we use a Shop Sabre router, with a 5’x14’ bed to cut large sheet stock for production of a lot of parts (mostly FIRST Tech Challenge fields), but also use it to cut prototype and production parts for FRC teams 3940, 1529, and 45 during the build season. Our Shop Sabre was purchased before I started, so I can’t go too in depth on specs, but it has an 18,000 rpm max (not sure the HP of the spindle, but I believe it is around 3-5 range).

We use Vortex for most of our tooling requirements for the router. They aren’t always super reliable on dimensional stability, but we check the bit diameters on our Haas and adjust the CAM as necessary. Each cutter manufacturer is usually pretty good about offering suggested feed rates and spindle speeds based upon your machine capabilities, as well as the materials you are using. Vortex has a handy chart that I find myself going back to every time our engineers give me a new challenge.

As for CAM, we run Mastercam for Solidworks 2017 here. I used Mastercam in high school on FRC 173, and Mastercam has graciously provided teams with the ability to obtain a free copy (possibly copies, I didn’t look too deeply into the offer) this season as part of the Virtual KoP! I believe the offer might have expired at this point, but you could probably contact them directly and work something out. Our local Mastercam reseller worked with us here at AndyMark to get the proper posts for our machine based upon some code we had from the manufacturer, and it has been a breeze to use since. Mastercam also has easy tools to change feed and speeds and calculates rates for you based upon your inputs.

AndyA and I own/operate a side business doing machining/fabrication. We came into a Torchmate Small Shop Machine for the right price and have used it extensively for personal, robotics, and professional projects.

(CD has a 5-image limit, so I’m just going to pop images in as links)


We have successfully routed the following materials:

5052 H32 AL
6061 T6 AL
Glass-Filled Nylon
101 Copper
Commercially Pure Zinc

It’s a great tool to cut FRC-typical materials!

The vertical forces associated with cutting steel were too much, elastically deforming the deck and z-axis of the machine.


Get it, learn it, love it. Worth every single penny.

We run .001-.002ipt and up to .125in DOC for aluminum, and .004-.010ipt and up to 0.500in DOC for other materials. YMMV depending on tooling, machine stiffness, and spindle power.


We use a Kress spindle, available from Tormach, which has a great mounting system, enough power, and has great run-out.

This is a newer version than the one we have. The collets work nicely, are inexpensive, and provided by Tormach in the US.

We started with a 2+HP DeWalt router, but it didn’t hold up to the usage very well:

We use an MDF deck, like most. The first thing we do with a new deck is to run a program that cuts the entire deck surface down. We slightly oversize the MDF deck so that as the machine clears out its working area, two nice square edges are left that we can justify stock against. The prep program also makes a hole pattern in the MDF for threaded inserts. These let us reconfigure our workholding rapidly and square smaller pieces of stock to the router’s axes. We’ll use flanged head sheet metal screws where additional workholding is needed, and have cut pockets right into the deck to hold odd-shaped parts.

Bolts used to square up a piece of stock:
Co-Cut 1/4in 6061 AL and gasket material for a race car’s cooling system modification:

But what about when the part is completely cut out? We take one of two approaches depending on the part(s) being made. We might bridge the parts, which is the practice of leaving small bits of material connecting everything together. It’s low-effort during cutting because the whole program can run dark, but requires a little cleanup afterwards. This works great for thin metals and plastics and any thickness of wood; basically all materials that can be ground/sanded quickly.

2017 bumper parts router and bridged together: They took just a few minutes to part on the bandsaw and sand flat on a belt sander.

The other practice we employ is to run one program which cuts all of the holes for a part, we then pop screws into each hole, and then cut all of the larger features. This is nice for thicker metals and plastics.

Cutting another race car cooling system part, holes first, then profiled in a second program: 1/4in 6061T6, cut dry with an air blast to clear chips and a 1-flute plain carbide bit.

Robot parts cut with the same technique and tool:

Chip recut is the #1 cause of terrible router experiences from what I’ve seen and read. Get those chips out! This isn’t a big deal in wood, I’ve used down-cut bits with great success. It is a moderate concern for plastic, but a simple vacuum setup will typically suffice. For aluminum 0.125in and thinner we cut single-pass, no recut to worry about! For deeper aluminum cuts, and very deep plastic cuts, we employ an air blast to keep chips clear.

We almost always use a dust collection system with all of these setups.

We generally do not use any coolants or lubricants and have achieved good success this way.


I am very interested in the tube fixture and how you machine the tube with the router.

We have a CAMaster Stinger I SR-24 and have been very happy with its performance. We are able to prototype and make changes to systems quickly, which has lead to the teams seasons getting better every year.

1 Like

Awesome thread!

We invested in a CAMaster Panther unit as one of the new shop tools for the season, and it’s been invaluable (that plus laser cutter). It took our cad->part turnaround time from days to hours/minutes.

I’ve been running aluminum (6061) on it at ~100ips, 12,500rpm (1/4" Onsrud upcut spiral O flute bit) with some pretty impressive results. The only real issue this year was the spoilboard warped a bit because it wasn’t bolted down properly, that’ll be fixed in the upcoming weeks.

Any chance you could share any more details on the tubing jig? That’s the next project on my radar. Had floated a bunch of concepts on how to hold down tubing but nothing as solid as your setup. Thanks!

With a CNC router you should basically always be running max speed (usually 24K RPM) with the least amount of flutes (Onsrud single flutes are a popular choice). Due to the lack of rigidity of a CNC router vs a CNC mill it’s all about taking the smallest chip per tooth (high-RPM) while still clearing chips without re-cutting them (single flute). If you look at Datron CNC machines they are specifically designed to run a 60K RPM with a single flute in aluminium to achieve maximum cutting speed.

Are you sure you’d sell the Webb for another cnc? Now if were talking about a 5-axis cnc I’m all for it.

What Devin and co. could do with a 5-axis VMC legitimately scares me.

– is where we get our single flute cutters. We buy our regular end mills from MSC industrial.
–Do not buy a used CNC router unless you have experience with them already and have someone very trustworthy selling it to you. CNC’s a complex machines and it’s hard to tell if something could be wrong with it without doing a bunch of test runs.

–I really suggest you get a compressor and aim an air jet right at your cutter, a shop vac on blow is NOT enough air flow. You might consider getting a blower with a drop hose(4-6" diameter) if you want to force ventilate your space to outside of the room.
–We use screws to hold our work down, when holding parts down we use brass screws in case we hit a screw it is less likely to damage the cutter.

This will get covered in my video series, I will make sure we post a link to our working tool library that has all our default feed/speed info.

–Dewalt router spindle that you have to select from 5 speeds. I will be upgrading to a proper VFD 2.2kW spindle this summer and will make a video on the process.
–You should be going over 600 SFM in aluminum at minimum, probably over 1k.

Feed/Speeds> I love CNC Cookbook, they have great content. Also check out they have some good CNC advice.

Spindle> I have found the Dewalt to be okay, but I agree that there are many better spindle choices out there and that’s why I plan to upgrade ours this summer.

Work Holding> Your whole section is spot on! I personally don’t bother too much getting our stock perfectly square and referenced but I think that just comes down to preferred approach. We also have a Tube jig that I think serves the purpose you are using your square edges for, correct?

Chips> Also great advice!

Hey Devin,
Would you be able to eventually do a quick walk-through of how you set HSMworks for large plates/ multiple parts, from start to finish?
BTW, 299 has been really grateful for your help with our new router!

Edit: and do you run your router on the highest speed like Marcus suggested?

I should be able to do that. It depends on the cutter, we only start slowing the spindle down when the cutter is about 0.2" or larger. When we run drill bits we go much slower, a #11 gets 13-16k spindle.

Has anyone played in your cam software with varying the z-depth while cutting to improve tool life and help clear chips?

This is used on high volume wood production.

I think what you are referring to is called radial chip thinning, high speed machining, dynamic motion, or adaptive clearing depending on the CAM software. These strategies work very well and are well suited to less rigid machines like CNC routers.

This website doesn’t exist.

Here is the website I believe Devin was referring to in his post.