DIY Numpad: Machining Madness

I've spent the last week testing out different things to see how I could improve my ability to machine acrylic. Since I didn't want to have to buy new lead screws (which would mean spending more money and waiting for them to ship), I first tried to fix the ends of my lead screws. To prevent a screw from whipping, it needs to stay under some critical speed that is a function of it's length and the boundary conditions of the ends of the screw.

My screws are rather poorly installed, with only one end being fixed to the stepper motor and some part of the middle inside the anti-backlash nut. The other end was not fixed at all and there were no bearings to take the axial load from cutting. This was never a big issue before since I never ran my machine faster than 48 IPM during cutting. But now since I wanted to push 70-80 inches per minute without things resonating and stalling, I would have to fix this.

For the y-axis lead screw, the longest one in my CNC, I designed a few bearing blocks that could attach to the 8020 running under it. I started off with one to fix the far end of the screw in a simply supported way. This didn't really do much, and the axial load was still all taken by the motor.

Before adding more bearings and designing a system to tension the leadscrew, I tried adding some lubricant to the the lead screw and nut to reduce the sliding friction of the plastic on the metal. I read some posts online recommending adding just a little is actually very important to proper operation (which makes sense since the screw should have minimal friction with the nut, like with ball screws). I put a few drops of some generic anti-seize/rust-removing lubricant and the difference was like night and day. The x-axis no longer made any resonating noise at all when running over 80 IPM and y-axis ran much smoother too. (also the little rust that built up on the screw in some places was cleaned off by the lube and the nut running over it.

Next, I designed another bearing block to go on the motor side, so that I could tension the screw and take off the axial load from the motor.

I cut this out with my new end mills I bought a week earlier. I realized I lacked 1/4" endmills and bought two 1/4", 3 flute carbide end mills for general work, a 1/4" 2 flute carbide end mill for aluminum, and a 1/8" 2 flute carbide end mill. These were my first "real" end mills, in that they weren't from generic cheap 10 packs; I got them from drillman1 on eBay, with the two flute ones being Kyocera branded.

1/4" 3 flute carbide endmill

Cut from MDF.

The cutting went smoothly and I installed the block the next day:

On the other side, there is a bearing and a nut tightened to pull on the screw, and on this side the motor coupler acts as the nut and is pressing against the bearing. I only had normal bearings, not axial bearings or thrust bearings, so the coupler rubbing against the bearing was not ideal. However, this wasn't a big issue.

I tested this out for a bit, but still get resonance. During a test cut at 80 IPM, the y-axis lost some steps during some high-speed changes in direction.

Test pockets.

I was testing different feeds and speeds to see how I could get the best finish in acrylic. I realized that using conventional cutting for 2D contours left a much better finish on the walls:

Inside wall is rough while outside is smooth in a climb cut.

I tried two end mills: the single flutes I got a while back, and the two flutes I got last year for cutting aluminum. Both were cheap 10 packs so I could afford to test with them. Everyone says to use o-flute or single flute cutters to be able to run at the relatively high RPMs of a router (~10K RPM lower limit for me) and low feed rates of hobby machines. I was having serious trouble with chip evacuation and kept getting melting with my single flute. A little bit of plastic would get stuck in the flute and just ruin things. This is why I tried the 2 flute and higher RPMs; the two flute had a low helix angle and worked pretty well for getting chips out of the pocket and cavities.

Yesterday, after doing all that plastic testing the day before, I decided to do some practice for cutting out the acrylic cases for my numpad. Using the same 1/4" 3 flute end mill from earlier, I ran an adaptive tool path for roughing the pocket: 0.15" stepdown, 0.06" optimal load, 72 IPM. I tested this in some extra 1/2" thick acrylic I got when the seller accidentally sent 4"x4" squares instead of 5"x5".

Adaptive roughing.

Plastic chips!

It went really well, except for the lost steps in the middle of the program. I had to bump up the spindle speed to around 18K RPM to get the cut to sound good. I was afraid of heat generation from the higher surface speed, but it wasn't a problem at all. I had real chips (tons of them)! I kept a constant blast of air on the cut, but it wasn't really necessary; the chips pretty much ejected themselves out with no problem.

To try to further combat the lost steps without making another bearing block, I moved the motor side bearing block to the other side:

At the expense of table travel (I wasn't planning on making anything that big in the near future), this created a fixed end condition that made the screw whip much less. I just realized I should swap around the orientation of the bearing blocks to put the section in between in tension, but this worked really well. I still should put a bearing block on the motor side, but that can wait for now.

Today, I got around to really testing out making a numpad case in the 5"x5" stock. With all the fixes and things I learned for cutting the acrylic, I felt confident I could make this work.

This needed to be a two-sided setup since I needed to cut out the holes for the screw heads on the back side, then cut out the pocket, lip, and perimeter on the front side.

Back side.

Front side.

I aligned the two sides by drilling out the screw holes deeper than the bottom and using pins to align after flipping. I could only align the two holes along the bottom right faces since those were the only ones symmetric around my flip axis.

Screw heads opened up and holes drilled.

After flipping and cutting the pocket (1/4" for roughing, and 1/8" for getting the corners and finishing the walls):

The edge of the floor has a lip since I forgot to
re-zero the z-axis after swapping 1/8" cutters.

When doing the finishing with the 1/8" end mill, I started with the single flute cutter I had, but it created a really poor surface finish and the cutting wasn't consistent (edge didn't perfectly line up in some places. Swapping over to my new 1/8" end mill and running the program again gave a much cleaner result.

After these steps I realized there some sort of alignment issue but I couldn't really tell what exactly was wrong. I tried to test fit a plate and PCB into the pocket, but the corner holes didn't exactly line up. I just continued on since this was just a test.

Still using the new end mill, the lip for the plate and the edge cut went perfectly. Despite going only at 48 IPM and running at around 12K RPM, I had no issues with melting through the whole depth of the cut. I'm pretty much never going to go back to my old end mills; these may be more expensive but you get what you pay for: the quality and sharpness of the new 1/4" and 1/8" far exceeds the generics from China.

When the lip was being cut, I realized what the issue was. The two pins I used for aligning the bottom edge weren't enough to keep the stock perfectly aligned. The bottom was well-aligned, but the top could still skew a little. This caused the holes on the far side to not line up:

Right side holes are mis-aligned.

Case backside with the PCB inside.

However, everything else fit perfectly. I can still use this case to test cutting out the top side USB hole. (I plan on aligning the case vertically but still need to figure out how to set up my work piece origin in a reliable way.) Next time, I just need to add another alignment hole to drill out on the other side. The frosted finish of the outside is really nice and has just the right amount of diffusion.