This is my first “lets see what this thing can do” project on my new Nomad. It’s a variation on a “turners cube”, the apprentice’s challenge of long standing. This is a project that gives you lots of practice with fundamental milling skills. Squaring up stock to size, setting up the workpiece in the vice and the zeros on each axis. You can really see when you make small errors. Even if it’s not your first rodeo It’s a good project for blowing out the chunks on the work flow for a new tool and at the end you have a nice little thingy to show the muggles.
I started by rough cutting a 25mm cube out of a Renshape block. Then I squared it up to 23.75mm using a .250" cutter. The gap in the bottom of the vice was a little wide for the cube so I used a pair of " thin parallel shims" from little Machine shop as parallels. Why the odd size cube? Because I could have done a better job with the saw roughing out the blank. I figured it was quicker to trim up my CAD model rather than cut out a new blank.
I used Meshcam on the STL file to generate the tool path. I used the “carbide auto toolpath” function in the tools tab to set up the cutting parameters for a .0625" ball end mill. My first try had the mill cutting the whole outside of the cube, No need for that, the cube faces where already cut. I went back and selected just the part of the model that needed cutting as the machining area. Much better, now only the part that needed cutting was getting cut. The new toolpath looked good and the estimated cut time was just over one minute. Wow, one minute, not bad.
The blank cube was set in the center of the vice jaw with the parallels underneath. I squished the blank down on the parallels with one hand and tightened up the vice with the other. The axis zeros where set by jogging the cutter close to the workpiece and then backing off until I could pass a 3mm dowel pin between the cutter and the workpiece. ( thanks whoever suggested that!) The appropriate value was entered in the zeroing screen, for X and Y, the pin diameter plus half the cutter diameter and for Z, the pin diameter.
I like to use an a edge finder and I will be using one as soon as we get a way to turn on the spindle while jogging, but the dowel pin method let me set up the zeros on all the axis repeatably with no worry about crashing the tool. Once I got past the fumble fingered pin dropping stage it was reasonably quick to set the axis with a dowel pin.
The NC file was cut on each face of the cube, resetting the cube and zeroing out the axis each time. One thing I should mention, if you cut the ball free while you are machining the last face bad things will happen. To prevent this I sized the holes in the faces so that I would leave about a 1/16" of material attaching the ball to the cube and then cut the ball free with an exacto knife.
I started the project about 10:00 this morning and by 3:00 in the afternoon I was done. Woo Hoo! this nomad thing is a bunch of fun. After seeing what Apollo is doing with dice I’m wondering if they might be good blanks for making “stupid machinist tricks” gifts for the nieces and nephews.
That is a super-cool project, @SWBennett, and a great machining job! Thank you for the comprehensive description of the workflow. I am suspecting that the depth of cut on each face was beyond the flute length of the .0625" bit? Assuming so, it looks like MeshCAM handled the toolpaths so that the shank didn’t interfere with the workpiece.
I’m wondering why you used a machining region rather than selecting “don’t machine top of stock”?
Can you explain a little about the edge finding method with the tool? Particularly how you set the zeros by entering values?
EDIT: Duh, I figured it out… you have to hit ENTER to get it to accept the typed-in value, all this time I was tabbing and clicking off, and it would go back to 0.
Machine geometry only, margin=0 will keep the cutter axis within the boundary of the workpiece. For that matter, with the rawstock shrink-wrapped to the geometry, you can use Machine whole stock with margin=0 for the same effect.
@SWBennett’s way obviously works too, with the extra step of drawing the machining region.
@SWBennett can you please explain this a bit more? I looked closely at your photo but can’t see any sign of the exacto cuts (well done!), and I’d love to know where the supports were.
Why use area to machine? It was the first thing I tried and it worked fine. I’m new to Meshcam, and for now I’m relying on pure blunder craft.
It turns out you don’t need to cut very deep into each face at all and the supports are included “for free” if you’re clever about sizing the holes in the faces of the cube.
I wanted the ball to be as big as possible so it was sized to be the same diameter as the side of the cube. To figure out the supports I thought about a traditional turners cube.
If you look at the corners of the inner cubes you will see they extend into the next larger cube. The size of the inner cubes is set by the depth of the hole for that cube. The amount of overlap for support is the difference between the diagonal of the inner cube face and the size of the hole. Make the hole too big or the inner cube too small and bits will come flying out when you cut free that last little bit of stock.
The supports for the ball are the residual “corners” we had in the turners cube. We can use a little math to figure out where the edges of the hole intersect the ball and we can use that depth of cut to figure out the “cube” size. The math is not too tough, Google “equation of a circle” and bust out the spreadsheet if you enjoy it. Just make the holes slightly smaller than diagonal of that virtual cube you work out. This will get us close. But we still have to account for the tool diameter and how deep the ball end will reach down. It got too tangled for me to want to work out on a Sunday morning. But the bottom line is still Hole too big, ball falls out, hole too small, you spend a lot of time cutting the inner bits free.
About this time the old Jedi designer spirit should be whispering in your ear “use the CAD Luke”. I did a little knoodling with calculator and scratch pad to get a SWAG on the initial hole size then fussed with the model until it looked good and would leave enough material in the edges to stand up to being milled. I used the CAD tool to take a slice through the model to check the support. Still no definitive adjustment for the cutter geometry and all that stuff but It worked out in the end.
One more thing I should mention about the supports, Renshape is pretty forgiving of minor differences in surface finish. I just trimmed with a fresh blade then before taking the picture I carefully placed the ball so that the trimmed spots where hidden by the cube edges.
