Today I worked on getting out all the kinks of the first operation for these parts.

I got through the majority of the toolpaths with very few modifications. However I did have some issues with the wall finishes, there seemed to be some weird ridges as if the tool was jumping around. I'm thinking it may be some vibrations which there isn't a whole lot I can do about since the location features are very tall and thin and I need to get around the entire parameter.

I also got to try out engraving for the first time using an off-center flat edge chamfer endmill. I spent over an hour yesterday trying to get it to work properly and finally got it to work. I'm honestly shocked by how good it turned out and will definitely be using this again in the future for my own projects!

Overall nothing too exciting today, ran through the first set of parts with +-0.001" tolerance. I'll be continuing on Monday and getting the next three sets of parts all finished up and ready to go on the 4th axis.

Thankfully all the parts are very similar and so I can copy and paste the same toolpaths over, I'm also able to use the same stock setup. I set up some guide markers on the Minimill for where the stock fits in place and so I'm able to swap out parts very quickly.

I started milling out the pockets of the part I'm working on with @jaelen_hsu.

It all started pretty well; I didn't make any changes to the original program I set up and set it off running. It got through the first three pockets no problem, however, when it got to the fourth one, the 1/16" endmill I'd been using, snapped! I had it running at 24 in/min, 10% sideload, and 100% tool diameter step-down (0.0625"). Thankfully I caught it on camera and found that the issue was due to chip welding, what I'm confused about is why it didn't break before, the sound was pretty much the same throughout and no noticeable chatter. 

I decided to speed it up to 30 inches a minute and lowered the sideload to 8%, and stepdown to 80%, and the same thing happened, it ran for a minute or two, then snapped as well. The only other thing I can think of that is happening is lousy chip evacuation, and the endmill is recutting the aluminum and bonding onto it. 

If anyone has any idea as to how to fix this issue, I'd greatly appreciate it! I'm down to my last 1/16" endmill and don't want to try anything I'm not pretty confident with. 

Today I focused mainly on programming the contract my boss got earlier this week. 

I'm not able to show the exact part, so I will do my best to explain the difficulties I've run into and the solutions used. The piece is like a large open frame with a few pin location features on both sides. It's also got some small features on the side faces of the part; this means you will have to rotate or flip the piece each time to access the different angles. There are four sets of four parts each, each very similar in design, so once I get one finished, the rest would take very little time to program. 

Right off the bat, it was a bit overwhelming as I had no idea how to start going about programming this part. The main issue I had was clamping it down after the first operation. Since it's got the long pins on the corners of the piece, it would be challenging to hold it down on a table without crushing it properly. I talked to my boss about it, and he explained to me how to do it; basically, you add a large block fixture to the center of the part where the hole would be, and you would use that as the locating and fixturing point. You could then flip the piece over and secure it down on a fixture plate to mill out the other side. 

Then the question of how to do you machine out the side features on the part came in to play. Initially, my boss explained to me how to to set them up in hard jaws and use a hard stop and similar work origins for each side; then you would only need to reset the tool height to the top face of the part and keep the x & y point the same. After discussing it some more, he thought of a much easier way to get access to those features using the 4th axis that he has set up on the Haas Minimill. Using the rotary 4th axis you could make small fixture plate and use the holes made from the first operation to locate it, this also means you don't have to reset the tool height for each face, thus saving quite a bit of time. 

I just finished up the first operation of the first part and spent the extra time to ensure I can find repeatability with the other parts as far as the CAM setup goes. 

I'll show more of the CAM process as I near the finishing stages of it. I continually realize I have to think outside of the box when machining parts and not to fall back on my understanding of it. Even with the piece I am making on the Pocket NC with the speeds and feeds, it's counter-intuitive to what I originally had in mind and yet made sense if you thought it through. 

Since my last post, I got some recommendations from @designtheeverything about how to improve the milling on the @pocket_nc.

He suggested something kind of counter-intuitive to what I was initially thinking but made sense if you thought about it. That was to increase the speed, keeping the sideload the same and depth of cut the same, on the face of it, if it doesn't work when the machine is running at 18 inches a minute, how would increase the machine load help? Well, the answer goes back to the main issue I was having, namely heat since I had it running slower, it gave the endmill a more extended period to cut those chips. This means that the chips were heating up, and before they could get cut, they transferred some of their heat to the rest of the stock, and little by little, this heats the aluminum to a point where it starts gumming the metal. 

So I decided to do just what he suggested, and bumped the speed from 18 inches a minute to 40, immediately I had to stop the machine due to it stalling, the torque on the Pocket NC wasn't enough to keep up with speed at the sheer amount of material coming at that pace. Thankfully this was an easy fix, and that was to reduce the stepdown from 100% of the tool dia to 30%; this worked beautifully, the sound was pretty decent, a little rougher than I would usually like but it was cutting no problem. I then increased the speed to its max (60 inches a minute), and it improved the sound. 

Today I finished making the batch of watch parts I started yesterday and started working on programming a new, more complicated part. 

Getting the soft jaws cut and the second op going took only a few minutes, and I had all the parts finished within an hour. I then deburred the edges and threaded each of the holes. The tapping of these holes was surprisingly smooth and easy and felt a lot like the threads were already cut, but after testing each one with a thread gauge, they all came out correct. Somehow I broke the just the tip of the tap inside one of the holes, and it felt like a very slight crunch, very similar to breaking the chips when threading the stainless, so I didn't think much about it until I pulled it out. 

Thankfully there were many more taps, so I swapped it out with another one and finished the rest of the holes. From there, I washed each part in soapy water, rinsed, and dried them. After inspecting each one, I found they were all within 0.001" of the design, which is well within acceptable tolerance but not entirely ideal.

My boss got me a new contract to work on, which is going to be the most complicated part I've worked on yet, using 4+ operations and some very unique CAM techniques. The piece is very similar to one @saundersmachineworks skateboard truck but not as organic of a shape. 

Finally, starting to make some chips on the Pocket NC, I decided to get the machine running and make tweaks to the program as went. 

Right away I ran into an issue when I started the machine up, it cut fine the first few passes, but I quickly realized it was cut above the stock in the z-axis. Thankfully it was as easy as inputting the correct b table offset value given in the manual with the machine. After that, I was able to get it running correctly. 

I used the recommended speeds and feeds for cutting aluminum, but had to reduce the rate and chip load some to prevent the metal from overheating. I cut down about a 1/8," and you can notice a slow change on the face of the metal where the heat started to increase and started to become muddled. It also started moving the aluminum rather than cutting it, which you can see at the end came out as strands.

I only had a short amount of time to work on it, but I was able to find some changes I will try out next time. The main one is to lower the roughing stepdown; I think that since it's got so much contact with the material, it's creating more friction and thus heat. I'm going to try the same stepovers and feedrate but reduce the step-downs by half, 1/8" to 1/16".

Today I made some thin plates using polycarbonate and some more aluminum watch parts!

These small plates where an interesting but easy part of making. Since it's plastic, I was able to use double-sided tape to hold it down on the fixture plate I used yesterday. Because of the tape, I couldn't use any coolant (which would only get in the way regardless), so I had to skim the surface with a face mill, then wiped down with degreaser on a rag to ensure the adhesion on the tape would stick.

For the programming side of it, I used a 1/2" three flute square endmill to face the top of the 1/8" thick polycarbonate, flipped and cut it again till it was at its final thickness 0.04" (not actual part height, close to). Then I used a 1/8" three flute square endmill to contour each part, leaving five thou axially to remove later, this was done to ensure the adhesive didn't get on the cutter, thus leaving a lousy finish. I had to account for the tape as well, so I measured the thickness with one side of the paper on it, then measured the paper and subtracted it from the total to get my number. From there, it was as easy as cleaning them up with alcohol and a rag, then inspecting each one. Everything was within 0.0002" (two-tenths), which is well within spec. 

From start to finish, the polycarbonate plates took maybe an hour and a half to complete, which was mostly due to trying to find the stock from the scrap piles.

One of the previous projects I worked on a couple of weeks back wanted a few more watch parts made, and so I got to set up the stock and re-run the old program. It took only 30 minutes to set up the machine, cut the aluminum, and mill the first operation out. I did three sets of two and will finish them off tomorrow. 

Smoothing out some more of the Pocket NC project CAM work, setting all the details in place. My goal is to get this all down on the first try so that I can pretty much-hit start and not have to touch it except to swap tools.

I've also got a public download link (https://a360.co/3hWbbpP) if you're interested in taking a look at some of the toolpaths I'm using to program this part. I should be able to start making chips in the next couple of days, assuming all goes well. I may have my shop work increase, though, so that may throw my timing off. 

I'm also thinking of running this part first in ABS or some other plastic to see how it comes out before doing it in aluminum. Overall I'm pretty pleased with how it's coming along, and I'm pretty confident in the areas I've completed so far. 

I also had some issues originally when trying to post the G-code, where it would fail the .nc code and not allow it to export correctly. I was able to solve this issue by switching the machine type from a v1 to a v2-10 in the post process tab right before exporting the g-code (see picture above).

Today I got to work on tapping and threading holes using the Haas minimill and Fusion360.

Unfortunately, I forgot to take pictures at work, so I recreated the drawing in Fusion to use as an example.

The CAM programming end of it was quite easy and only took a minute to setup. I first drilled out the hole using a pecking method (1/3" of the tool diameter) then came in with the tap to thread the hole. How the tapping works is by aligning the spindle rotation (in this case 500 RPM) with the vertical (z) motion of the machine, matching it perfectly to the thread pitch, when it reaches the bottom, it reverses the spindle and comes back out the same way it came in. It's pretty nerve-wracking because if there is any slight thing off, the tap could easily break.

I tried it first with a set of imperial threads, 1/4-20, 10-32, and 4-40, each of which worked fine, though I did snap one of the taps when cutting the 4-40 hole that was due to my random selection of a 4-50 tool in the program. 

Interestingly, when I moved over to equivalent metric holes, 6-1m & 5-0.8m, it was extremely loose when tested with thread gauges. I have no idea why it does that, and nothing in the program is different except the tool size. My boss says he's had similar issues when using metric taps, and the only solution he found was to convert the metric taps to imperial manually, and it seems to work that way. He thinks its due to the conversion and some rounding down or up inside the machine.  

I also got the day off on Friday which is why there wasn't any post then. 

Today I finished up the steel plate part and got it packaged up.

One area I was kind of nervous about was getting these small tight corners with a few angles meeting all at one spot. The original plan was to come in with a 1/16" square endmill, and adaptive clear out the material, leaving five thou on the walls, then contour it with the same tool. However when I sent the machine running, the endmill snapped right after it touched the material, I am honestly not sure why the chip load on it was well what it could handle, and there were no direct plunges into the content. 

Unfortunately, there weren't any other 1/16" square 4 flute endmills like that long enough to get the whole wall, so I had to revert to using a 1/8" one, this meant I couldn't quite get the corner to how it was drawn but got within ten thou, which is acceptable for this part.

Once getting that corner done, I used a contouring toolpath with a 1/16" ball endmill to finish the chamfer along the edge of the part, using four thou stepovers, which gave an excellent finish. I then took the 1/4" square endmill I used to cut the piece out to finish off the walls of the plate removing the five thou I let behind. Stainless steel makes me very nervous about running anything on, and I quadruple checked each operation I posted. 

I had extra time before the end of my shift so I thoroughly cleaned out the Haas Minimill and typed up a quick checklist reminder for setting up and tearing down at the end of the day.