Home Workspace | Clamp Project v2 | Pocket NC

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. 

Home Workspace | Palette Knives

Huge thank you to @oakblades for sending me some handmade palette knives!

These are going to be useful for around my workspace for those small hard to reach places. They both look absolutely amazing and you can really see the care he put into these! Each one has a serial number, these are 3858 and 3859.

Home Workspace | New Endmills... Again | Pocket NC

I've been super busy with work these past few days and haven't had much time to continue my education on CNC machining.

Since the new 1/4" collet came in for the Pocket NC, I can now use more significant tooling. I don't have any endmills for cutting aluminum specifically, so I'm in the process of picking up some new ones. I've been talking to Wayne (the local CNC shop owner) and asking him about the different aspects of the bits I could get. The one thing he keeps stressing to me is rigidity, which I haven't heard other machinists talk about much, but it makes a lot of sense. 

His premise is that you only want to get enough cutting length for what you're going to use. In this case, I will only ever use 100% of the tool diameter in the length of the cut/stepdown. So if I have a 1/8" endmill, I only want to have 1/8" LOC (length of the cut, or flute length) to get the most rigidity I can from it. Similarly, the flutes are also super important; the fewer flutes you have, the less stable the tool is and can be prone to deflection; however, the more flutes you have, the less chip evacuation you will get. So there is a balance you want, and he uses and suggests three flute endmills. It provides enough space for chips to evacuate with air coolant properly, and still have enough rigidity to prevent deflection.

Home Workspace | Infrastructure Part II | Pocket NC

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.

Home Workspace | Infrastructure | Fusion360 & Pocket NC

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.