CNC Routers for FRC Robotics


We normally cut with a 6mm end mill so we are not getting into the micro machining levels where run out really kills small tools. The smallest we go is maybe 4mm but that is for rest machining. Tool life seems to still be pretty good as we easily get a season off a single bit and that is usually cutting 2 robots worth of parts. However with students… we often crash and lose the bit before its life is fully up.

Balance wise, we haven’t noticed any chatter, nor any poor surface finishes. We do try to keep the setup as clean as possible such that we don’t introduce more errors. We have only done some cursory runout and tramming checks but nothing strenuous. Once we started using them, we found that they worked well enough for what we were trying to accomplish.


Runout is most significantly a problem (IMO) when using multi-flute endmills. One flute will wear out much faster than the others and cause cutting/chip clearing/rubbing issues prematurely. However this isn’t really a problem with routing because I generally use single-flute tools. With only one flute there is never a wear imbalance.


I agree but I have seen issues on some lighter duty routers where runout can cause a uneven chip load in aluminium forcing them to dial back their feeds into a sub optimal range.


My team is in the market for a cnc, and I was wondering what your guys’ recommendations for a budget of $5000-$7000ish. We are looking for a bigger cutting area along the lines of 2’x4’ or 4’x4’. We would be using it to cut gearbox plates as well as plate for our base, so it has to be precise and sturdy. Anyone have any thoughts?


The Laguna IQ series is very capable, but has poor customer support. All quality American routers with good support cost a lot of money, so you’ll have to decide what’s most important to you. You should be able to get the 4x4 version for around $7000 iirc.
The Omio X8 is not a bad choice even inside that budget range, but it’s not large enough.
Somebody else with more experience with American brands can chime in here.

One a separate note, I recently placed an order from Cowin CNC in China for a 2’x3’ router for $2350 + $600 shipping. It should be more capable than most routers, but I’ll need to wait a few weeks for it to arrive.


Did you quantify the run-out? Why was it a problem with a single-flute cutter? And can you clarify on what you mean by ‘light duty’ router?


Why wouldn’t runout be a problem with regards to chipload on a single-flute endmill?
I do agree that single-flute endmills are significantly less affected by vibration when it comes to breaking, but 0.001" of runout on an endmill that’s only supposed to do 0.002 IPT is a 50% variance.


If you imagine run-out as the tool being clocked slightly to one side, such that the cutting edge is 0.001" behind where it should be, the point is that on every pass of that flute it is 0.001" behind where it should be (or ahead, or to the side, or whatever). Each revolution, the machine still moves forward 0.002" and the cutter takes a 0.002" chip, not a 0.001" chip.

On a two flute cutter, you would have one cutting edge forward, and one back, so one would be doing all the work, and the other none.


What this guy said.

Some sort-of funny things could happen with the single-flute. The depth where the eccentricity pushes the cutting edge out will cut a little wider. The depth where the eccentricity pushes the cutting edge in will cut a little narrower. However, when routing a part I’m not expecting much better than ±0.005in, and 0.001in sounds like a crazy-high run-out number… but maybe my Kress spindle has spoiled me.


These specific cases were in machines with wood routers as spindles. They can have a lot of runout (especially when loaded) compared to a proper spindle due to the bearing setup and the lack of a ER collet. Some are better than others but you can often get a significant cutting performance increase just by moving to a proper low runout spindle.


I suppose. Even when I had a DeWalt router as a spindle runout was tolerable, at 0.0004in.


In my experience, moving from a router to a spindle did yield a very large performance increase, but I wouldn’t attribute it to runout.

The biggest difference I saw is that router power ratings are generally just wrong to start with (marketing HP vs. HP), cannot run slow enough, and do not have the torque/power at low speeds, to avoid bogging down compared to a spindle at low speeds. They can still cut, but only because they rub, rub, rub, and build enough pressure to force the cut. This can look like “runout rubbing” or something similar. If you want to run at a higher speed (RPM), you need a higher feedrate (IPM), and more horsepower. Hobby/Prosumer gantry mills do not have the stiffness to effectively use a high horsepower spindle and keep the accuracy we’d like for most of our parts.

As an aside, these machines are generally not very stiff. It’s been awhile since I ran the numbers and am on a work computer not my home… but I calculated cutting forces (resisting lateral movement of the cutter through the material) in the neighborhood of 40-50 lbs on GWizard for a 1hP cut I was dialing in a year or so ago. On our CNCRouterParts mill, if I put a force gauge on the tip of a 1/2" bit (relatively rigid) and measured deflection at that load, I got ~0.010" of deflection, versus something closer to 0.001" on my Tormach (again, ballpack). One thing I got feedback on from the folks at CNC Router Parts is that most efforts to make the machines stiffer, or use encoder feedback, yada yada… are not as important as upgrading the CAM platform to allow for things like finish passes, when you are chasing pure accuracy.


While I do agree the HP ratings of a wood router are wildly different you really should be running close to maximum spindle speed when using a single flute cutting tool. The other issue with wood routers is the Variac variable speed control means you loose a ton of torque when you turn down the speed. A proper three phase spindle+VFD even without a encoder has closed loop functionality (even in “open loop” mode) that will try to maintain a constant speed since it can measure back-EMF.


While I do agree the HP ratings of a wood router are wildly different you really should be running close to maximum spindle speed when using a single flute cutting tool. The other issue with wood routers is the Variac variable speed control means you loose a ton of torque when you turn down the speed. A proper three phase spindle+VFD even without a encoder has closed loop functionality (even in “open loop” mode) that will try to maintain a constant speed since it can measure back-EMF.

Yea, certainly didn’t mean to make that sound like “anyone running high speeds is wrong”, but I think there are instances where lower speeds can be beneficial too.

I’ve been running a 3/16" Amana O flute for awhile and found it to be a reasonable compromise between rigidity, minimum radius on parts, etc.

The manufacturer recommends 600-1000 SFM, which is roughly 12k to 20k, and I end up running ~15k (half of my 30k spindle) at the lower end of the recommended chipload. I found a pretty big performance increase being able to cut at full sheet thickness (0.08 to 0.125 Al5052), and unscientifically “seems” to work a bit better with the 3/16 bit than the 1/8" bit. Also, while a minor thing, we directly drill to 3/16 for our hole patterns, so it saves a collet swap to go from a 3/16 bit to a stub length drill bit.

To expand on the “unscientific” stuff… the 3/16" bit has at a slightly slower speed has a bit more margin than the 1/8" bit across the board. At the full sheet DOC, you have a little more room to get chips evacuated. We have had issues (need to fix, just low priority) with our air blast/cooling setup (FogBuster), where every now and then the magnetic mount vibrates loose, or we snag a hose, etc. All fixable stuff, but the margin is the difference between failure in 30 seconds or failure in 5 seconds. Same thing with if we are slightly off with a hold down screw and clip the edge of one, or any number of other mistakes, where the 3/16 bit has survived a surprising number of times.

I probably should look into running a smaller bit again and dialing in the process/failure modes, which would bring the spindle speed up among other benefits, and I bought a few 4mm bits to play around with as a step between the 1/8 and 3/16 options.

Out of curiosity, if you are running max speed, what are your speeds/feeds/bits/cooling setups in aluminum?


I can do 40 IPM/.25" doc/full WOC with a 6mm single flute endmill at full speed (~22k I believe) no coolant or air blast. I suspect I could do the same with a 3/16" endmill if I was using the fog buster.


I’m curious, do you think a big part of getting a DOC that large is the width of the bit? We typically stick with 4mm endmills for convenience, but on large jobs blasting through full DOC would really save some time.


We have a new CNC Router (OMIO X8) and will begin training students in September. From our limited use of a CNC mill last year and working with the CNC router this summer, CAM and CNC router setup time far out weigh CNC cutting time. Our goal is to minimize setup time at the expense of cutting time.

With this said, we plan to standardize on a 4mm single flute carbide end mill for the majority of cutting. We plan to use a circle mill operation for small hole (.1875 - .25") drilling and a pocketing mill operation for larger “inside” pockets (slots, bearing holes etc). We will use a contour operation with tabs for “outside” operations.

The idea is to save setup time by only zeroing once and eliminating tool changes.

Comments on potential issues or better methods appreciated.


This mirrors my sentiments about CNC machining. Standardization and quick setup is the key to making parts quickly in FRC.
I’m not sure what “circle mill” is, but a helical bore works very well with a 4mm endmill. 0.02-0.04" stepdown per helical revolution is a good number to hit.
Learn how to use CAM templates too. We used one on 1072 this year with Fusion and it made our programming time decrease drastically.


Probably not, I’d stick with 4mm-5mm. Since most FRC work is full WOC contours I’ve found 4-6mm to be optimal. Any larger and your really loosing any benefits of the additional rigidity of the tool by the large WOC and the cutting forces become too high for the machine to take advantage. Unless your machine is really rigid like ours it’s unlikely you’ll get any significant cutting time improvement. In this case I was doing some pocketing and wanted to see what it could do.

Another thing that helps a lot is a pressure foot. It holds down the sheet and helps stabilize it which is especially useful with thinner materials. It reduces the amount of tabbing needed to hold parts down which save cutting time. The more consistent fixturing rigidity allows us to up our feeds and speeds.


I found an interesting DIY pressure foot design:
Add in some kind of an adjustable pressure system (pneumatics?) and it could be quite effective.