I haven't had too much time to work on the Pocket NC today, but I did want to get one thing done. And that is better organization, I would continuously have tools floating around my workspace and would often lose them. 

I saw a video by @saundersmachineworks, where he showed all his systems for organizing his tools using Kaizen foam. He's got a fantastic system, and I highly suggest watching it ("Ultimate Machine Shop Toolbox & Organization" on youtube). The basic idea is to lay your tools out on a piece of foam, then outline and cut out groves to fit each one snugly; this allows you to quickly look over and make sure you have all your tools in place and helps with putting them back in their proper spots. 

For mine, I've got calipers, both clamps, the setup Allen wrenches, a few files, the collets, and the metric screws that came with the Pocket NC. I also stopped by Wayne's shop (local machinist), and he graciously gave me an ER11 3/16" collet after talking to him about my difficulties with the 1/4" tooling. 

Finally getting the clamp piece finished up on the Pocket NC

I just got a new 0.25" 3 flute endmill, which I used to do the adaptive clearing on the central part of the clamp. Unfortunately, after setting it up with Pocket NC's recommended speeds and feeds, I found that it stalled quite a bit and even would stop spinning entirely. I had 10% of the tool diameter side load, 90% stepdown, and 0.0008" inch per tooth, which related to 12 in/min and 8,500 RPM. The above video shows what I kept running into, I played around a ton with the speeds and feeds and still got the same results. I then took it way down and cut at 0.0005" width of cut, 9,500 rpm, 25 in/min, and 0.2" stepdown, which finally worked. Overall I'm kind of disappointed that the 1/4" endmill can't do more than it does, and I'd say is equal with a 1/8" if not inferior. 

I then used the 1/8" endmill to do the rest of the pocketing and finishing, which only took about 20 minutes total. I'm so glad I had preset toolpaths ready to go, it sped things up, and I was able to get bunches of toolpaths sent off together. I wasted a considerable amount of time trying to figure out the proper settings for the 1/4" endmill that the project took about three times as long as I would have liked. 

I had a 1/4" chamfer bit, which I used for the first time to clean up the edges. I love 2D chamfer, it's so easy to program, and the finish quality is outstanding! After all the finishing passes where complete, I went back to the 1/8" square endmill to cut it off the base. I wasn't sure what toolpath I should use for this, and after looking around I found the 3D swarf was the best. I didn't want it to make a 3D motion, so I locked it in place by setting the tool orientation. I had it take 0.005" step-downs and leave 0.005" stock to leave so I would be able to come in later and part it off by hand. It worked out well, and I was left with a very thin onion skin that I could nudge the piece, and it would move side to side seemingly forever. There was virtually no cleanup necessary except to knock off the edge with a single sweep of a file. 

The quality difference between this and the first one is incredible, not to mention the speed and efficiency with having preset toolpaths ready to go. The main reason for redoing it was the bottom face of the clamp, which wasn't very flat on the first go. 

I've spent the past few hours generating toolpaths to machine out the clamp piece to use as templates for future projects. 

I had no idea until I started trying to optimize the operations of how much time I wasted. I would typically use 3D adaptive clearing as my coverall for machining, including finishing passes. I would usually use the rest machining to prevent re-cutting material, which worked, but if I made any edit to the previous toolpaths, it would give an error to all the rest. 

I'm nearly finished and have a bunch of toolpaths each for a different purpose (as seen above). I would watch a few tips and tricks video's from @saunders then use some of the information I got to imbed into the programming. It's been super helpful, and I cut the overall machine time from 3-4 hours to 57 minutes! I'm still working on optimizing the order in which I do things and splitting things up to get the most accurate part.

One of the tricks I found interesting where for the finishing passes. Instead of doing one operation to clean the bottom and side faces, you would split them in two. I would generally do this, but the thing I didn't think about was not letting the endmill doing the floor touch the side faces; this will prevent the side of the bit from rubbing against the side face and leaving a poor finish. The way you do this is by adding roughly one to two thou on the radial stock to leave. 

Now that I am taking my time and making the best toolpaths, I'm looking at the simulation, and it had helped tremendously with removing wasted time and preventing mistakes like tools plunging into stock. These new toolpaths do require a lot more tool changing (6 times, I think), but I think it will be worth it for the outcome and speed it will bring. I've also separated each group by the endmill, so I need only export for each tool.

I'm super pleased with what I've come up with so far and need to order a few 1/4" endmills to fit my new collet and toolpaths.

Since my mishaps last night, I realized I had to take a step back and set plans in place for setting up cam easier and more accurate, also known as infrastructure.

I would typically set up my part in Fusion360 and generate toolpaths as I went, exporting and running each one. I did this mostly to make small changes easier when I was first learning how to machine parts. However, its very time consuming, and I often make mistakes (like yesterday), leading to sub-optimal outcomes. 

Today I am working on replacing my old system with a library of tried and true toolpaths I can duplicate for other projects. The first part of this process is putting all my tools in my tool library; this allows me to quickly select the endmill I want to use and have all the settings already programmed into it. It would also give me the propper feedrate, rpm, and tool number without having to re-enter in the information each time I set up a new CAM setup.

The other half of the coin is setting up the toolpath settings; I can duplicate my known toolpaths to new CAM setups and quickly generate them, which I can then make small changes for the different parts I machine. I'm setting these up with some baseline guidelines, so I know they work, then change them depending on the situation. 

I'm also shuffling through some of John Saunders' older videos on programming tips to embed into the toolpaths, as well as recommended finishing processes optimized for accuracy and efficiency. 

Going to start by saying the remake of the clamp piece didn't go too well, and I ended up having had to walk away from the computer before making any more mistakes. 

The first of many things that went wrong was getting the stock for the clamp. I had some 10"x2"x0.7" 6061 aluminum I got from Wayne (local machinist) and wanted to cut it down to a 2.5" bar stock to fit in the vice setup. I did pick up a bandsaw the other day but didn't have any blades for it, and none of the local stores had them in stock. So I opted to cut it manually with a hacksaw, though after 5 minutes and making a dent in it, I am ashamed to say I took it over to the drill press and drilled tons of holes in a straight line to use the hacksaw then to cut the remaining material. It worked but was not a pretty sight. 

I then did a few adaptive facing operations to ensure the CAM setup knew precisely where the material was, and this is where the second thing that went wrong happened. As soon as I started the machine, it sounded horrible, and I could not for the life of me figure out why, toward the end, I noticed it left a groove that was rounded over and not cut square as it should. I then took a closer look and found that the tips of the endmill where gone, I have no clue how that happened, but they were cut off somehow, so I had to toss it and use a four flute bit I got from @designtheeverthing and continue from there. 

I was able to get through an adaptive clearing toolpath on the top without much issue and then went to the side faces. I drilled out the holes for the locating pins and the center hole to attach it to the bed before removing the bulk of the material from the other side. Unfortunately, the size of the hole was more significant than the 1/8" drill bit I was using; I did a pecking toolpath to make its way down to the bottom. However, when I inserted the pin into the hole for a test fit, it had quite a bit of wiggle room, which I am not entirely sure why. The stock did move a bit when it was drilling, which may be part of the reason, but since it's a drill, it can't cut sideways, so maybe not. There is way too much room for the pins to be useful, so that put a damper on the whole part, making that it is effectively useless to use locating pins. 

I was then working on finishing the inside faces of the hexagon shapes where the nuts would sit. I stupidly sent the endmill crashing into the material with a pocket clearing toolpath eating away more material than it could handle, and the sound it made was horrible. I paused the machine, but since the endmill was still spinning, the sound continued, and this was the first time I ever had to use the emergency stop on the Pocket NC. After that, I had to stop before I made any other mistakes.

I went into the project without a plan and just layered toolpaths on top of each other and in no particular order, then exporting the g-code for each one similar to what I did with the previous clamp piece. Very unorganized and ended up with 20 code files. 

I need to take a step back, organize my toolpaths and set default feedrates depending on the tools, so I don't have to manually enter in so much information each time, and export my code with a bunch of toolpaths instead of one per file. The very frustrating situation, but I've meant to reorganize how I do my CAM systems. 

Today I started doing some test cuts and dialing in the new clamp I made this week. 

I started by inserting the new clamp on the disk into a few CAM setup files. I then took the bar stock I had for this project and modeled it up and located it in Fusion. I knew I needed some adjustments as if the clamp was even a hair off; it would throw everything else off as well. I did a facing operation on the front face and dived into the material by about ten thou when it should just skim over the surface. I let it cut a small amount before stopping the machine; I then measured how far it cut and divided it by two to see the offset of the hard stop in the design. I then reran it, making small adjustments where necessary; it doesn't need to be perfect but close enough to ensure I wouldn't run my endmill into any significant amount of material. 

After getting it within about five thou on both sides, I noticed there were slight stepover marks that you could feel as if the stock was at an angle. I took another square piece of stock and aligned it vertically with the aluminum in the clamp and found it was at a slight angle that threw the tool off when doing horizontal passes. You can really see how far it's off in the picture where I have one lined up properly with the base of the clamp and the other in it. 

I figured this might be just due to the clamp not being perfectly flush with the base disk; however, after doing a few facing passes on that, I still had the same issue. I'm honestly pretty lost as to why it's doing this, and if anyone has any idea what it could be, advice would be much appreciated. One thought I have on it is tool runout, I don't have a dial indicator, so I don't have any easy way of checking if that's the case.

I'm going to be redoing the main clamp piece again, so that may fix the issue, but I would like to know what caused it for this piece to avoid it in the future. 

The last thing I need to do to get the new clamp in place is to drill and tap the holes on the new bed.

I was planning on using a 1/16" square endmill to boar out the holes in the disk. However, none of my tools were long enough to do the job. So I opted to use an actual drill bit this time; I first spot drilled where the holes would go then pecked my way down with a 1/8" drill bit. I wasn't entirely sure how easy it would be, but I was pleasantly surprised and only took a few seconds to make all three holes.

I then took the 4mm x 0.7mm tap I bought last week and hand tapped the center hole; this is my first time using a threading tool, and it was surprisingly easy and only took a couple of minutes. I then test fitted the main clamp piece, and it fits perfectly! I used the locating pins provided by Pocket NC and dropped those into place as well, a very nice fit for it all!

The reason for tapping the center of the disk as if I ever wanted to make another clamp/vice system it would make my life easier knowing its exact location.

I had most of the part already machined out the night before, so all I needed to do was poke a few holes for the locating pins and cut it off the stand. For the holes, I used the 1/8" endmill I used to do the rest of the part with and did a pecking drill operation. I really shouldn't have done it with an endmill as it made the hole quite a bit wider than I wanted, and there is a bit too much wiggle room for my liking. If I thought about it, it makes sense, since endmills have side cutting capabilities, any kind of vibration would cut into the walls of the cylinder, whereas a drill bit would only cut down.

After milling out the holes, I then moved over to parting the piece off the base of the stock. This was much easier than I thought it was going to be, I created a sketch on the face of the side I wanted to mill from and made a rectangle in which I could restrict the path of the endmill. I then used an adaptive clearing to remove the material from underneath. Unfortunately, about halfway through the cutting operation, I forgot the stock wasn't perfectly square in the clamp, which caused the endmill to dive into 1/6" of aluminum thinking it was air; this flipped the stock partway out of the clamp. I did get it on camera, and you can almost hear me jump when it happens. 

Thankfully I was able just to loosen the clamp a bit and get it back in place, and after that, it was pretty uneventful. I came in from the four different faces and cut each about 0.8" down then for the last operation left about 0.05," which I would cut off manually. I did this rather than having the endmill cut it all the way off in case the part fell and scraped up the finish on the piece.

I noticed that the holes for the set screw and pins didn't go all the way through the bottom of the part, so I took it over to the drill press and finished the job. I then used the small files I picked up last week to deburr the edges and clean off the bottom, where I parted it off the base.

I then took a piece of bar stock I had that this project was based around and drilled two 0.25" holes on the drill press to match the holes on the new clamp. Since the clamp screws I'd be using are smaller than the 0.25" holes, I had no problem aligning them appropriately to fit. After tightening the clamp screws, it was not going anywhere, super stable!

Since I also now have the new bed/disk that came in today, I removed the old clamp and installed it. It fit perfectly, and I only need to machine a few features on it before its ready for the part I just finished! I just rested the new clamp on the table to see how it would look in its final state.

After coming up with the new clamp design last week (see previous posts), I finally got around to machining it. Not going to lie, I was a little bit dreading since my last aluminum project failed. 

I designed the clamp fixture to match some 6061 stock I had already to make it easier on myself. I decided to use the recommended speeds and feeds for cutting aluminum by Pocket NC, and it seemed to work pretty well though a bit slow. I'm using a three flute 1/8" square endmill at approx 20 IPM. The local machinist was giving me some tips on machining it and told me to move the endmill farther into the tool holder; he said you only want it 0.01" more than what your most extended depth is to get the most rigidity out of it. That alone improved the sound of the milling by quite a bit.

I was also looking into coolant systems for the Pocket NC and asked around one of the Facebook groups, where I heard someone using it and ruining one of the belts in the table/bed. The machinist suggested I use coolant, even a light misting every hour would make a world of difference; however, after talking to the people at Pocket NC, they urged me not to. However, midway through the operation, when I was sending a few videos of it running to the machinist, he suggested I try coconut oil on a brush and lightly dab the part about to be milled, just a drop or two. I tried it and holy smokes; it improved the sound tremendously, and I even cracked the feed rate up by 20% without any change in noise.

After doing a 3D adaptive, I did a few pocket clearing and facing operations to cut the holes and clean the sides. I, unfortunately, I wasn't able to finish it due to time restrictions, but I will pick up where I left off tomorrow. Overall very pleased with the outcome thus far.

While I was out today, I also stopped by a local machine shop to discuss better ways of milling out small parts, primarily the pendant that I worked on a couple of weeks ago. 

He suggested that instead of having the two pegs for the part to stand on, it would have better rigidity to have a thin flap of metal surrounding the piece. It would also help with cutting the pendant loose; for my system, I would simultaneously cut off the part and finish the face, which was quite difficult and left a bunch of imperfections I couldn't remove later. He also suggested using putty to fill in the first side milled out; this would prevent vibrations, which could cause a bad surface finish. You can see in the images of how he milled out similar parts.

In addition to all this, he mentioned that it would be easier to get the side's filleted with a square endmill vs. a ball endmill. The reasoning behind this was you would need the ball endmill to reach farther down past the part and would interrupt the metal flap around the piece. I initially thought he meant to do step-downs with the square endmill, which would leave steps on the finished part, but rather mill it to flow over the sides.

Another great piece of advice he gave me was for the tooling itself. He was saying that you only want as much flute length as you're going to use, and any more than that would be pointless and give you less tool rigidity. I've heard this from Saunders and a few other people as well but forgot it when ordering the new endmills. He also gave me a Harvey tool catalog which he said would explain the purposes behind coating and the best endmills for the material being used.

After giving me this very much needed advice, he gave me a bunch of new stock I could use to mill. Mostly 6061 aluminum but also a bar of 7071, and aluminum & bronze compound, some more acrylic, and black material that I forget the name of but reminds me of micarta.