When designing pieces that are meant to fit snugly together, what kind of wiggle room do you normally give?
For example I am designing a slot and tab style container, is there a rule of thumb for making the slot slightly larger or the tab slightly smaller so that they still fit but don’t need forced in place?
For other CNC machines I’ve seen suggestions of around 0.005" (call it 0.1mm). It’ll depend on the device’s actual accuracy of course.
You can wing it by slightly altering the tool bit diameter you give the CAM software
I usually do what @mooselake suggested and leave .005" of nominal clearance for parts that are meant to fit together as you’re describing, but the machine I use at work is not a Maslow and allows me to hit very tight tolerances. For a Maslow, with a published accuracy of 1/64 (.015625") I’d probably cut out one of the parts with the tabs first, then gradually increase the width of the mating slots in .005" increments until I was happy with the fit. Not sure if this works for your specific application, but maybe it does.
This will highlight the tolerances on both the tab and the slot, which will both come into play with the desired fit. Then you’ll know more about your particular set-up as well. Maybe try it in the middle for best results? I think someone mentioned that on another thread.
A simpler alternative: If your making the parts out of wood, you can always stay on the safe side and program a nominal .005" gap and then hit it with a little sandpaper until it fits nicely. When machining parts, it’s a lot easier to take away material than it is to put it back.
Worst case 1:
-tabs undersized 1/64
-slots oversized 1/64
= sloppy fit
Worst case 2:
-tabs oversized 1/64
-slots undersized 1/64
= doesn’t fit
In my opinion, case 2 is easier to fix if you need a nice snug fit. Especially if you can leave the part set up in the machine to test the fit before removal.
Just to clarify for the less-mathy inclined here. 
Is the suggestion then:
Confirm your actual tool bit diameter. If you have a tool bit that is .5 inches wide normally, you go into your CAM software where the tool bit diameter needs to be defined for creating the tool path, and reduce the .5 to a smaller size by .005" - such as .495" using our actual .500" bit example.
Or should we use the other published Maslow 1/64 number, meaning that an actual .500 bit minus the .015625 maslow fudge gives us a .484375" suggested tool bit diameter software setting for our CAM software.
It sounds like the first option of using a small amount of fudge aka .005 reduction in actual size for the software gives you a chance for a second pass or sandpaper right?
For the “second pass”, would you take the first CAM output, and then reduce the tool bit software setting another .005" to get a little more bite out of the board? Aka, actual is .5", first pass tool setting is .495", second pass is .490"?
Since we are here talking about fudge and multiple passes, what’s the cheapest set of sheet goods that people are using to test out designs before throwing down the baltic birch 3/4" boards? OSB? MDF?
I appreciate all of the knowledge being shared in this forum, and want to make sure the shorthand doesn’t go over my head. Thanks!
wouldn’t you want to make the first cut leave the pieces too large, and then
trim them to final size?
you example leaves the parts small, and if you do the same thing to both parts,
the undersizing combines to leave you with 0.02" of space.
@Orielbean I’m referring to the width of the slot and mating tab. For example, if you want to fit a .500" thick tab snugly into a mating slot, try designing the slot width at .505" so that there’s a tiny bit of clearance for the tab to fit into. If that’s not enough clearance, add another .005" and re-machine the slot at .510" and so on until you find the right amount of clearance for your machine and application. How you add those incremental increases in clearance is up to you. “Tricking” the machine by changing the programmed tool diameter is clever, but you could also just modify the files and tool paths. If you’re anticipating this type of fit in your parts, you can draw several slot sizes in your 3D model so that you can easily re-write toolpaths and re-machine larger and larger slots. Cut some small test parts and see what clearance is best for you!