I am building a bunch of fancy furniture lol, its out of plywood but it still takes the time. I am working on tolerances and trying to get prefinished ply (birch to fit snuggly.) I am onto the 1/8" Compression bit and ran some work tonight but still not happy with my rule of thumb. I heard you just add .01 inch to the female inserts, but it seems like vertical panels into horizontal need more. Just want to start a conversation and see if anyone has advice on how to get as close as possible joints with ply and how you offset your line work to ensure tight fits?
On my old machine I had a diy vacuum hold down system. I used it more to hold sheet material flat when cutting speaker cabinets. I would set my files up not just to mill the slots but also the end that would be inserted into the slot to a specific thickness. Generally the thickness of your material is going to vary enough that a one size fits all file will not give you super tight tolerance. This was the only solution that I could come up with that gave me consistent joints without having to measure and adjust my file each time. The MDF I was using was around 0.76 at the time. The files were set up to be zeroed from the table surface to 0.74. Slots would be milled about 5-7 thou over. Basically perfect every time with just a little room for glue. This only works if you have some sort of vacuum hold down, which can be done super cheap if you are just trying to hold material flat. Lighthouse Brand Vacuum Motors
On the left side click the link for Shopbot motors and I think there are links to their forum where Brady Watson did a ton of work figuring out DIY vacuum hold down solutions. To just hold sheets flat an old shop vac can work well. You just want a little 1/8" or so hole on the inlet side for leakage to help cool the motor.
Cut a slot with your bit, and measure it with calipers. I bet it isn’t 1/8", and probably a little bit undersized. There are several ways to handle this, but the easiest is just to put the measured diameter (ie: the width of the slot) as your tool diameter. This may help a lot with precision. I find that some fairly new bits are a good .003-.004" off. Some of it has to do with feeds & speeds.
Once you have done that, cut test pieces and modify tolerances until it fits. You can start out with doing this, but if you switch to a new bit you may find out that things don’t work again, so doing the first step will help you a lot.
Hey I do a bunch of work with plywood and utilize dogbone joints for a lot of plywood projects. Here is a quick run down of things I’ve come across over the last few years:
1- Adding 0.01" to your female (pocket) can be a great starting point. Ultimately, the quality of your material will impact how well this works.
2- Speeds/Feeds: I have noticed that if I increase my speed up to 180+ IPM, my pockets do not retain the same level of precision that they do if I run my machine down in the 120-140 IPM range. I am using a Pro4896 machine with a custom made MDF vacuum table. When I step down to 120-140 IPM, I also try to reduce my spindle RPM’s to maintain an appropriate Feed per Tooth.
3- Test Joints: When ever I switch to a new material, I cut two test parts that are the same as each other, basically it looks like I am cutting box joints. But each “opening” has a different measurement and then I write in the measurements on the part that I initially 3D modeled them at. So say I am working with a 1/2" thick plywood, I will make one where one cut out is 0.490" wide, the next is 0.495" then 0.500", 0.505", 0.510" and then 0.515" . As I’ve made two of these, I will then test fit them together to see which dimensions fit together the way I prefer for that project. If I find that one set of dimensions is a tad too loose and another is a tad too tight, then I will make another set of these test joints but then go in intervals of 0.015" to see if that improves the fit.
4- Endmills: When I am working on products that require a really tight fit, I set some endmills aside where I track the number of sheets that each of those endmills have cut. Once they hit 5 full sheets, I then put them in a different group of endmills for either development projects of production work where the tolerances don’t have to be spot on. Around the 10 sheet, I notice my pockets/tolerances seeing a real impact for the wear on the endmills. I use a bunch of 1/4" 2 flute downcut endmills.