Hey guys… any suggestions for cutting box joints on a vertical jig. I’ve had complete blow outs at standard feeds and speeds for 5/8" baltic birch with what ever bit I’ve tried. some success with 1/8" DCSB at 30ipm at 20k rotations but complete blowout with similar set up for 3/8" compression bit… I’m going to modify the jig to accomodate a spoilboard on either side of the birch and add more horizontal clamping for stability… any ideas/ suggestions appreciated.
Cutting baltic vertically is hard… have you tried any trochoidal toolpaths?
You can make those in Fusion.
I use them in my dovetail setup: One Bit Dovetails
My first thought would be the plywood. Very thin layers that will just chip off without support. I would agree with the thought of spoilboard on both sides for support. I’d bet solid wood wouldn’t do that as easily.
Is it possible to generate trochoidal toolpaths in Aspire?
Nope, Fusion 360 is going to be your best bet for that.
Sounds like a great opportunity for someone to write a Vectric gadget. You would probably get more than just a few folks to actually pay for it.
I have been doing quite a few box joints lately with Baltic Birch in both 12mm and 6mm thickness. I have not tried doing so using fusion 360 (would love to see an add in that would work in fusion 360), however I have been having great success using the “Box Creator” gadget in Aspire.
Works well using a 1/8" DIA bit with the panels horizontal rather than vertical. I have had reasonable success with just a standard upcut bit but keeping the depth of cut to .200" or less. 18000 rpm and feedrate 60 to 80 ipm. A bit slow but it does keep the quality up (not running a production shop so time is not a big factor for me).
Two tricks for the gadget.
First make sure to set the allowance at about .010 otherwise the parts are to tight to go together. I will use less for small boxes <6" and add some if the box is larger >16".
Second the box creator makes the fingers only to the depth of the thickness of the material. This does not leave any room for error in the fit and glue up. I will set my material thickness to about .015" thiker than it really is, run the Box creator, then change my material thickness back to the true thickness. This way the fingers are just a little longer than the thickness of the material and easily sand flush after glue up without sanding through the outer vinier.
Vertical spoilboards and improved work holding seemed to do the trick… also went back to the 1/4" spiral down cutter… 140 ipm and 18000 rpm… thanks for all the suggestions!
Those look great!! That is definitely some sturdy vertical workholding!
To do it without backing boards, you need good toolpaths. For joints I really like the JointCAM software. Its toolpaths always take into consideration cutter direction and do a scoring pass when needed for clean cuts. Making through dovetails on my AVID CNC router, designed with JointCAM Software - YouTube
If you just have simple in and out toolpaths, use a sacrificial backing board on each side and it will also fix the problem.
JointCAM is pretty solid. Once I got my head around how they do the axes I was able to get it to do some neat stuff. (for reference I have my XY reversed)
Ya, the terminiology and orientation of everything took a bit to figure out. The simulation of what the joint looks like is really helpful. Also, the guy who writes it is very responsive to bugs. I found 3 or 4 minor things while it was using it heavily and he would generally fix them and put out a release within a couple days.