What's new
What's new

CAM Tool libraries- What's your setup?


Oct 13, 2014
Kelowna, Canada
We're only 1 month into running our new VMC, and the tool library in Fusion 360 is already getting annoyingly messy.
Tool #8 is several kinds of endmills, as well as a tap, so I'd like to figure out something before there is 1000 tools to try and re-organize.

My Okuma has a 32 tool ATC, and its simple to detach T8, and insert T849 in whatever ATC pocket.
I don't hate the idea of keeping a standard tool library in the machine that matches CAM, but just renaming the tool when you insert something different is also fine.

What's your preferred way to keep everything organized?
Keep a CAM library only? CAM and machine with matching libraries?

For a CAM library, do you just do 1-50 indexable mills, 51-100 endmills, 101-150 drills + taps, etc, or larger series of 1-100 indexables etc.?

Looking forward to hear how everyone else does it!
I have tools by material and don't bother with the numbers apart from the standard tools that I never remove from the magazine. When I set up a repeat job I first check what tools I need that are currently in the magazine I then change the numbers in CAM to match the magazine.

There are so many different ways to do it and they all work. Just go with what you are comfortable with.

For me it's CAM library only.
I have a 21-tool carousel, with 3 tools standard - a 2" facemill, a 1/4" spot drill, and a 1" insert cutter. These tools find their way into > 75% of the aluminum and steel gadgets I make. Since I'm doing one-offs and very short production runs, I pretty much need to reset my tool carousel for every part (making a transmission case with 1/4-20 tapped holes, 3/8-16 tapped holes, 3/8 reamed pin holes, snapring grooves, root fillets, etc. fills up the carousel pretty quickly).
I also take the nonstandard tools out of the machine after a run, so they don't get gummed up with coolant/chips while being unused.
Another note: I can't necessarily depend on having the exact same 3/4" endmill in the exact same toolholder with the exact same tool length I used last time. The shop is primarily for the students' use...so occasionally I find my latest favorite extended length endmill in the Scrap Carbide box :rolleyes5:

Long and the short of it is, I haven't bothered with a CAM library.
Being that this is a process problem, it's important to include how your shop handles tooling independent of CAM...

Are you a job shop that keeps standard tools in a shared tool library? i.e. you transfer tools between machines and already have these tools touched off? Then it would be good to maintain your tool database within CAM, and simply give these tools your internal numbering system. I believe in fusion you can provide whatever tool number you want, so long as your machine allows a large range of tools, such as your Okuma. I know Haas is limited to 200, and umbrella style tool changers can only call up a tool up to your capacity, but can apply any of the tool offsets 1-200 for that tool. Below is a link for a job shop from the Practical Machinist youtube page that I think does this right... multiple machines with a central tool library.

Skip ahead to 27:40 for the section on tooling
SB Solo

Are you building tool assemblies at each job? Then throw the numbering to the wind and don't worry about tool numbers in your CAM library. Keep default tools, and adjust the numbers in your CAM as you go.

Do you have a hybrid system? A small selection of pre-built, commonly used assemblies? Have a numbering range that specifies whether it is a pre-built tool or an on-the-fly assembly that needs to be touched off. This makes it clearer to your machinists whether a tool needs to be transferred from your tool crib, or assembled and touched off. In this case, assign a range to pre-built assemblies, and another range to the on-the-fly tools.

In any case, if you have a central tool library, you may want to include a macro call for changing tool offsets from a centralized file, this way you only need to change this file once, and all your machines can access it. Another option is to manually change each tool offset in each machine anytime a pre-built assembly has changes applied to it. My experience is limited to Haas controls, but if you are experience enough with programming, you can make it so that these changes are automatically sent to the machines, without having to run a macro on each tool. I know most modern machines allow for writing macro variables over your network.
Last edited:
Thanks for the replies everyone. Its good to know that there isn't one absolute correct way to do it that I'm ignoring.

Jrfiggz, that video looks promising, thanks for posting it.
This is the only VMC in my shop. No sharing tools.

I'd mostly like to avoid running to check the tool mag for every operation at the computer, and think the fewer tool edits we do at the machine, the fewer fat-fingered screw ups we'll have.
A simple option may be to utilize the MTConnect data off of your machine. I am not familiar with Okuma controls but it does seem that the app store has an MTConnect app... The MTConnect standard includes tools in the machine, which can help you to pull this data from your computer that you are running fusion 360 on. It seems like the only data point for your tools you won't be able to get is the Tool comment, which I imagine might be helpful for readability. The cool thing about MTConnect, is that it essentially creates an HTTP endpoint that you can type into your browser, and it'll give you the relevant data points. I'd check out the Okuma app store, and download the MTConnect app... it seems there is a bit of a set up process, but if Okuma support is good, this is a viable option.

Another option is if you have anyone familiar with creating applications in C#, VB, C++, or ASP.NET you can likely create an application for your Okuma that integrates with fusion to pull tool data, including the tool comment. Fusion supports add ins, and if you code it up properly, you can do everything without ever leaving fusion.
For us, we're a job shop and have 6 vmc's with 3 Okuma Genos M560v's.
What I do in Mastercam is just post out tools in numerical order starting at T1.
Since we're constantly using different tools, we're always swapping out tools in the machines.
I don't register the tools in the machines... IMO it's a complete waste of time and too much of a hassle.

So basically, every program I write is T1, T2, T3, etc...
The way I do it, 20 tool carousel.

T1 is spot drill.
T2-T8 are for drills and taps.
T9 is my chamfer mill
T10-T15 are for endmills. Usually I'm only aluminum or only steel all at once. Smallest to largest- T10 is often a 1/16", up to T14 at 1/2".
T15-18 are for larger endmills or weird tools, again in order of diameter.
T19 is my facemill.
T20 is kept empty for touch off tools (no probe, so wiggler and/or dial indicator).
@Mtndew what do you mean by you don’t register tools? I’m inexperienced with Okuma controls and curious to how tooling is loaded in
I don't register or mount tools into the library that is on the Okuma control.
I just hand load them into the spindle for each job. And we run 1-5pc jobs all day every day. So there's no sense in using T848 for a #3 center drill.
Mine are T1-T32 but rarely ever use more than 20 tools for a job.

Now if you want static tools to remain in the magazine that's all fine, but then you're juggling tool numbers when you have to replace one of them with a different one.
To me it just creates more hassle than what it's worth.
I have a 11 tools that live in my mill and rarely change unless I need more tool slots for a special job

Tools 1-5 are for a specific product I use all the time. #1 being a 1/4' endmill for brass/aluminum, working downwards, 1/8, 1/16 and 1/32 ending with tool 5 being a 3/8-16 roll form tap. Tool 6 and 7 are 1/2" Aluminum end mills one long, short one long, my usual go to for moving more material quicker, Tool 13 is a 1/4" spot drill, then 14 and 15 are drill holders. Tool 20 is a face mill, typically setup for aluminum.

I have 21 slots, the rest are used for job specific tooling... and sometimes I just change it all for a specific job. tooling #'s are saved in the tool crib in camworks, same with material specific feeds and speeds for those tools