CNC Tool Libraries and CAM Templates

With so many threads mentioning the benefits of tool libraries and CAM presets for manufacturing and how much overlap there is in terms of machinery in the FIRST sphere, let’s all try to help eachother lower the barrier to entry for advanced manufacturing.

My proposal is for teams to state what CNC machinery they have access to, what CAM system/workflow they use, what are the typical tools used (and maybe even links to purchase them), and what is all included in their CAM presets. I’ll start:


CAD/CAM Workflow: Onshape>STEP>Fusion 360

Typical Tooling:

We call this the Cyber CNC Tool Library and use these tool numbers with all students and mentors CAMming parts. We figured out how important standard tool numbering is the hard way…

You can download and use this library in Fusion 360 from here. Use this guide to help import the library. I suggest you re-order and number to suit your teams needs.

Almost all of our tooling is HSS as it is easy to work with and cheap. We tend to break tools regularly when teaching students so HSS suits our needs well. We also aren’t cranking out TONS of parts, just a couple of each usually, so the slower feeds and speeds don’t bottleneck us too much.

I’ve also linked the tools in Mcmaster, but that is not necessarily where we order them from.

This is obviously not exhaustive, and we are planning on adding a chamfer tool and possibly a few others as well (hopefully based on this thread)! We also don’t have any router-specific tooling in the library yet, but the intention is to use the same tool numbers and library throughout our shop.

CAM Templates:

We call this the Cyber CAM template and are still messing around with it. It should have reasonable speeds and feeds for all of the Cyber Tool Library tools. It includes:

  • Spot-drilling all holes less than 1/2" (we might make this smaller in the future)
  • Auto-selecting and drilling of all of our drill sizes in the tool library
  • A printed note in the UI to screw parts down after the drilling operations
  • A manual stop in the program to give the machinists time to screw the parts down without stopping the program
  • Adaptive clearing options for all endmill sizes (with “rest machining”)
  • Bearing bore options for 3/8" endmill (pretty much our most commonly used endmill for removing lots of material)
  • A 2D contour with a 3/16" endmill to cut parts out of their plate
  • A 2D contour with the spot drill (what we currently have for chamfering parts, not ideal)

You can find and copy our latest CAM template here. Again, my suggestion would be to cater this to your own teams needs. This is a fantastic video going over how to create, save, and use CAM templates.

I follow the belief that deleting CAM operations you don’t want is quicker than adding ones that you need which is why this might seem like a lot of different options. I also used “rest machining,” which assumes material has been removed from the next smallest tool down. If you are only using one size endmill make sure you uncheck this option on your adaptive clear routines.

To make all of this I modeled a simple part that has pretty much every typical feature a standard 103 robot part may have. I then used that part to make a simple CAM template.

The part:

Let the template sharing begin!

Other resources and recommended reading:

CNC Routers for FRC Robotics “Megathread”
CNC Tooling for FRC “Megathread”
OMIO Tips, Tricks, and questions
(Will add to this over time)


This is awesome! I totally agree that standardizing tool numbers is important, the tool numbers I use at work have influenced a lot of the number scheme for 1678.

It would be awesome if you could post a link to this thread into the CNC router mega thread and would prefer that the OP get the credit for linking it and not myself.

1 Like

Fantastic idea. Done and done!

I hope too that those using the metric system share their settings as well. The robotics team uses imperial, but at work we are setting ours up in metric as we do a good deal of European work.

We have a few templates for machining aluminum and polycarbonate. I will try to clean those up and post them here soon. Templates and tool libraries are a boon for fast and reliable plate work in FRC.

1 Like

We haven’t been able to figure out a good solution to have our tool library synced across all team members accounts. Our current solution has been to create all the tools in a part file, save that part file to the team project, and open that file whenever you want to do CAM. Fusion lets you access tools in other open files.

If anyone has gotten cloud/shared/synced libraries and templates setup (not just uploading the files to the could and installing manually) please let me know.

Here is our setup.

We use the short .125 to drill every size hole besides .201 and find this is faster than a hss drill bit.

We also add in a recommended ramp DOC and use a slotting speed feed rate so no matter what a student cant break the tool. We manually crank up the feed rate if doing an adaptive.

In case your wondering we start numbering at 10 because these mills get used at work during the day.


That’s a perfect solution! We just keep these files on our Google drive and students download them to their own computers or computers within the school that have fusion (hense the timestamp). It takes only a few minutes to import, but once they do we can be confident about how the presets will interface. I agree, having them all synced over multiple accounts would be fantastic, especially as tools are modified or added.

That you use the 1/8" endmill for nearly all hole boring is a really interesting idea. That surely would speed up total cycle times for plate work. Why don’t you do this for 0.201" size? Tubing, on the other hand, might not be as simple.

Fantastic idea to keep the feeds/speeds for slotting for all mills. That definitely might save some tooling expenses. We usually teach students to lower the FR when trying a new program for the first time, but that doesn’t always happen.

Really interested to hear your tooling and rates for polycarbonate. We have been having a really hard time finding the right speeds, feeds, and tooling that doesn’t produce an awful finish or melt. I’m sure we have our speed too high, but we only have a fixed-speed spindle for the time being (minimum 12k rpm).

We put hundreds (or thousands?) of .201 holes on our robot so we invested in a nice short, carbide tool. This lets us drill at 10k rpm, 100ipm and go all the way through a 2in tube. I’m sure it saved hours of run time over the season considering it drills almost 10 times faster than an hss bit. We only occasionally have to drill a .25 hole or a .159 and this is when the .125 FEM comes in handy.

1 Like

Do you happen to have video of your hole boring process? Would love to see it.

1 Like

I second this and would also love to see a link to the tool.

Heres a video of us drilling a 1 inch tube. (just imagine a 2 inch one)
I wouldn’t be surprised if its faster now. I also really love using the .125 end mill for most holes. Its so convenient and reliable. But as you can see having the drill really speeds up tubes :slight_smile:.


I’ll post our full feeds and speeds next week when I get into our shop, but we have been cutting polycarb with both Huhao and Ozzy Boards 4mm single flute carbide cutters at 50 IPM 20k rpm and 0.125 DOC. We get an almost clear edge with only an air blast. Without an air blast, the chips are warm but still don’t melt.

1 Like

Hella money, Kenny. Any reason you do 1/8 and not something like 4mm? Also link to tool?

That’s a thing of beauty. Definitely interested in knowing a bit more about the tool.

In terms of your 1/8th endmills, I’m assuming you’re only going through the near side of tubing with that? Are you required to do tubular parts in 2 operations then?

I don’t think there is any particular reason besides that we are familiar with it and it works out for our hole sizes and radii. On 3309s router we use a 4mm single flute. But we run 3 flute on the 4414 mill. I do not have a link that will have to be JJ lol.

1 Like

I just checked last years CAD and I think we only used the .125 endmill on a tube 4 times. In all of these cases we were able to use out 1.25 inch long .125 endmill (see JJ’s Screen shot of our tools). Because we had the long end mill we were able to do it in 1 op (a lot slower). That being said, the .125 tool is mainly used on plates. We try to use .201 holes every where we can so we can rip with the drill. (which I dont have the link too).

1 Like

Do you use the .201 drill for 3/16" rivets? If so, you don’t find that to be too loose?

looks like its a 3 flute, I think all our endmills are 3 flutes. Only every had problems with a .25in EM chip welding when ramping aggressively.

I think one of our mentors that works at haas brought us this tool from work, It was used but only slightly compared to our standards.

Never with rivets, but sometimes with 10-32s, planning on testing a .196 this offseason. In my experience the loose fit of .201 makes up for oversized tool and powder coating (probably more like a .196 after paint)


We actually just started using templates in F360 and have had cloud syncing work without too many hiccups, although we have a setup with Fusion Team so I’m not sure if it’s possible to do without that. With Fusion Team (and everyone on a team hub) make sure “Enable Cloud Libraries” is checked in Fusion’s settings (under General > Manufacture). You probably will have to re-create your templates, and in my experience, it’s often taken a weird combination of rebooting Fusion and opening several different folders to get them to actually show up under “create from template,” but once they show up they work great.

1 Like