New to CNC; waiting for my SO3 to arrive. I want to make a giant cribbage board with 1/4" for the pegs. I have drawn the cribbage board with all the peg holes and track line using FUSION 360. Wanting to know what would be the best way to make the 200+ holes? Can you use a .25" uncut end mill and “drill” all the holes? Suggestions?
Thanks
Pocket Clearing works great from Fusion CAM. I make battery holders with 19mm wide 22mm deep circles easy peasy. 
edit: I use the .125" square end mill 
-Hank
Any thoughts on using the drilling option within Fusion and using a .25" end mill? Or would you suggest using the 0.125" end mill and create hundreds of .25" pockets?
If you want to straight drill them you will need to make sure your endmill is a center cut, and you will need to peck drill them since there is no way for the chips in the middle to get out.
I would use an 1/8" or 3/16" end mill and helical mill them. Just spiral the bit down in .030" deep passes per revolution.
Entirely up to you there. Both work great. I usually have other things happening to clear in passes so the .125" is my go to. 
Test on some scrap 2x4. When in doubt…test it out.
-Hank
Any thoughts on using a 2 Flute straight plunge bit?
Two flutes is probably the best, but plunging it straight in 1/2" deep might cause some issues.
On the other hand, give it a try and see what happens.
Wanting to know what would be the best way to make the 200+ holes? Can you use a .25" upcut end mill and “drill” all the holes?
A drill is ~4 times better going down than across. An end mill is ~4 times better going across than down.
Drilling with an end mill is commonly called a “plunge”. Although an end mill is relatively inefficient for drilling (compared to a drill) it is often the best choice when one does not have an automatic tool changer. The time to change the tool weighs the time to drill a few holes.
With a large number of holes - time wise - it makes sense to switch to a drill as things will overall be faster. That said, many people appreciate minimal tool changes and will accept the extra time to complete a job.
Depending on the end mill diameter and material, one commonly doesn’t plunge all in one go. One has the CAM software generate multiple operations that accumulate to the requested depth (often called layers).
The general guideline for plunges is no more than 1/2 the diameter of the end mill per layer. Often, one has to do a bit less because of the nature of the stock (material).
To learn about end mills please see:
Many CAM packages are fussy about their holes. Some packages will allow a 0.25" end mill to make a 0.25" hole, others require a smaller end mill or making the hole 0.251". I’m not a Fusion user so I can’t speak to how it behaves specifically.
If one can use a 0.25" end mill for 0.25" or 0.251" hole, be sure to use “peck drilling”. The end mill will occasionally withdraw, removing most of the accumulated material in the hole.
Smaller diameter end mills will cause the CAM software to generate not only layers but also a pattern to remove all of the material in a larger hole (a “pocket”).
The highest volume end mills are 0.125", 0.25", 0.5", 0.75", 1.0" and so forth. Yes, there are odd sizes but these tend to cost more (low volume) and be harder to find.
mark
The issue with using a drill bit in the S3 is that the RPMs on the router are too high.
If you got a SuperPID so you could slow the router down to 5000 RPM, then you could probably get away with 1/4" and smaller drill bits.
Anything larger than 1/4" and even 5000 RPM is going to be too fast.
I was explaining basic machining principals.
The SO3 can have a spindle - that’s up to the builder. If a spindle is used, drilling become possible.
As I indicated, most CNCers - especially if they do not have a tool changer - prefer to use end mills since they avoid tool changes. Yes, this also avoids the need for slow RPMs and using drills.
Anything larger than 1/4" and even 5000 RPM is going to be too fast.
I run 0.5" end mills at 10K RPM all of the time… End mill diameter and the RPM they can be run with largely depends on material being worked and to a lesser degree the end mill material and coating.
With some stock materials - not on an SO3 or a Nomad - I’ve had 0.5" or larger end mills running properly at speeds of up to 40K RPM (and 60K RPM is possible). For jollies, we use an IR gun to read the end mill temperatures - over 200 degrees C. Yeah, these were seriously coated!
mark
I was explaining basic machining principals.
The SO3 can have a spindle - that’s up to the builder. If a spindle is used, drilling become possible.
Yes, I get that you can change the spindle. Most S3 users will have the DeWalt 611 router.
I run 0.5" end mills at 10K RPM all of the time… End mill diameter and the RPM they can be run with largely depends on material being worked and to a lesser degree the end mill material and coating.
I know you can run end mills fast. That’s why I said “drill bit” and not “end mill” in my comment.
I run 1/4" end mills in my S3 with a DeWalt 611 at high speeds all the time, they work great. But I was talking about drilling, with a drill bit.
I know you can run end mills fast. That’s why I said “drill bit” and not “end mill” in my comment.
Fair enough.
mark
I’ve done something like this and used Fusion 360 as well, just with 1/8"
I oversized the hole slightly larger then my bit to allow Fusion to generate plunge gcode. That worked fine since I was using brass rod for the pegs.
Having just recently used the drill function in Fusion for a recent project I think @twforeman has the right idea with peck drilling.
Thanks for all the input; Just waiting for the arrival of my machine then will test things out and post. Have new tool path set up for 1/4" end mill with peck drilling engaged using Fusion 360. Just sitting here by the curb waiting…