Finished up all the parts today and got them shipped out!

Nothing too exciting or unique today finished milling out the final set of parts without any issues, then moved from there over to deburring and tapping the holes. I use an Exacto knife for most of the smaller burrs and a file for the larger ones, I'm sure there are better tools out there for quickly removing burrs, but I'll have to do some more research into it. 

For the final cleanup, my boss instructed me to remove only the larger burrs and throw them in the tumbler to finish them off. The tumbling leaves a hazy look to the part, almost as if it was lightly sanded, they turned out quite lovely and only need a quick rinse in soapy water and drying before they were ready to ship out!

I've also got two more jobs lined up, so I'm glad I was able to get this finished up today so that I can focus on those the next couple of days. Getting a bunch more hours at the shop and still enjoying it very much, each day seems like an hour each time I work and am always surprised to find my shift over so fast!

Today I got the rest of the parts all programmed and started running them one by one.

Unfortunately, due to the time-consuming stepdowns at the very end, the whole operation takes about sixteen minutes per piece, and there isn't a whole lot I can do to speed it up. Also, I do I run the risk of breaking a tool or the part itself. I also used a little playdough like clay to reduce the vibrations of the slitting saw when cutting the small side features. I'm honestly shocked how everything lines up so perfectly with the CAM programming, and I'm having almost no tolerance issues.

One strange thing I am encountering is when trying to get off the part from the block of aluminum in the center, in the corners wouldn't quite match up, and I would have to work pretty hard at it to cut it out completely. My boss checked it out himself and also isn't quite sure what's going on; its a brand new 1/16" endmill and is cutting two thou per side under what it should. It's pretty consistent in how much it's leaving, but I'm too afraid to program it with the negative stock to leave to compensate for it. One of the only things it could be is if the cutter is wearing out from some of the other toolpaths it's doing, but there aren't any signs of similar error elsewhere. The quick and dirty solution to this issue is to have it cut down five thou deeper than it did before, so instead of cutting the corner with an Exacto knife, I only need to cut the side of the block.

While working on the parts, the Haas VF2ss started to leak coolant all over the floor (turns out I forgot to clear the chips from the coolant conveyor) and had to pause to mop it all up. 

Unfortunately, I ran out of time for the day, so I had to leave the last set of parts for tomorrow. My goal is to get these shipped out by the end of my shift tomorrow, which will require me to debut everything, throw them in the tumbler, wash and dry them, and package it all up.

Today I got to make another fixture plate and started programming the final operation for the parts I've been working on the past few days. 

For the fixture plate, I took a piece of scrap aluminum and faced the top, then drilled the three holes to match the three on the block of the part to locate it. The whole operation took about seven minutes to program and two and a half to run. F

From there, I started working on the 3rd operation for all the parts and had some difficulties at first when trying to clean off the flat surfaces. After looking at some of the other toolpaths, I noticed that the manufacturing extension was now available. My boss bought the whole Fusion360 package when it first came out, and up until this point, it was all locked, and I didn't have access to any of it. Because of this, I was able to use the deep and shallow finishing toolpath to clean up quite a bit of the part.

There was also a small slit in the part that met up with a hole I drilled on the 4th axis, so I had to cut it with a slitting saw and a contour toolpath. I've never used one of these before, so I was a bit cautious and took it slow at ten inches a minute and three times the width in its sidecut. 

When I went running the program, I quickly ran into an issue where the bottom of the saw blade would collide with the steel hard-jaws if I let it run as it should. My boss suggested I move the fixture to the edge of the jaws and relocate the work origin on one of the holes using a gauge pin and dial indicator, which is what I needed up doing. From there, I was able to go through the rest of the toolpath without issue until I got to the cutting out sequence. 

The way I machined the part was to leave a block of material in the center to locate off of and have a secure fixturing spot in which I could cut all the features. The piece is a pyramid-like shape with a thin band lining the parameter with nothing in the center. The way I would get it off the block was to cut from the underside and cut away at it from the opposite side until it would just fall. It's tough to explain how it works, but the long and short of it is that you cut away small amounts of material and finish it at the same time, taking tiny steps down until it comes loose. For the longest time, I couldn't understand why it wasn't coming loose; I had the tool cut past the bottom of the flap where it should have just fallen off. I finally figured out that the endmill I was using was a 0.06" endmill and not a 1/16" (0.0625"), which made a surprising amount of difference in the rigidity of the part, being held up by just four thou. 

Finally got all the parts finished up on the 4th axis! After getting all the toolpaths down on yesterday's part I was able to copy them over to each set.

Each part was 10-15 minutes and I got the coolant aligned perfectly to get each of the tools working so I could walk away and program the rest.

The final operation for these is to place them face down on a new fixture plate and cut them out of the holding block which I'll do on Monday.

Today has been probably the most frustrating day I've worked in the shop yet, I broke three semi-expensive endmills and had some weird luck.

There weren't very many features on the part, but the ones that they do have are tiny, going all the way down to a 0.008" groove to cut out. I programmed the part around those features and didn't worry about trying to clean up any of the larger faces (I'd get those when I send it through the final operation. So I would take the 1/2" endmill and clean up the areas around the features, then with the smaller tools come through and mill them out. 

My troubles started when I ran a 1/32" (0.03125") square endmill to pocket out a small cavity and snapped the endmill. I didn't think my speeds and feeds were breakneck, and I was shocked that it caught so quickly, I used an adaptive cleaning operation and had its ramp down to its final height, then spiral out from the center. I asked my boss about it, and he pointed out that the height of the pocket was over 100% of the tool diameter, which I didn't realize until then that it was. I was trying to get the endmill to cut about 120% depth of cut with an 18% sideload at 12 inches a minute. The hole itself was about 0.023" deep (80% tool dia) and should easily be able to handle that; however, I forgot to take into account that I had stock to leave on the top face above it (10 thou) and so couldn't take that kind of stress. I ended up just leaving five thou on that top face (I would clean it up on the final operation) and receive ten thou step-downs. 

After cleaning out that small pocket, I then used a trace toolpath to get the 1/32" endmill to follow a specific path around this button like feature. Unfortunately, I thought I could take the endmill deeper than it could go and snapped the second one of the day, at this point I was got frustrated and had to take things way down, I was very caught up in getting these parts done that I took things too fast to get lower run time, but what I didn't think about was the amount of time I was spending trying to save those few seconds and ended up wasting over an hour if I had just let it take its time. Thankfully everything went much smoother after this and got the rest of the toolpaths done without much hassle, except for breaking yet another 1/32" endmill when I forgot to adjust the speed on a different pocket (it didn't break the first time because I manually lowered the feedrate on the machine). 

I also had a very small 0.008" feature to slot out so I used a 10 thou endmill (oversized is acceptable) and took 1 thou step-downs (4 in total) till I reached the bottom. 

My boss noticed that something about the part was out of line and wanted me to check with a dial indicator along one of the flats of the parts to see if it was true. Something I didn't realize was that the locating pins didn't actually stick out far enough and the chamfers on both the holes and locating pins shifted the part ever so slightly; the weird thing was that by some stroke of luck, the fixture plate in the A-axis was perfectly level (within 0.0001"). So I somehow messed up getting it level, but since the part wasn't perfectly straight, it worked out to be almost dead accurate. Another stroke of luck (if you can call it that) was that most of the features on the part where about thou or two undersized, this confused and concerned me. Still, after going it over with Wayne, he explained that due to the runout on the machine, tool holder, and endmill, most manufacturing companies would make their endmills undersized to compensate for that. Still, he said that if everything were in perfect alignment, you would get the tool perfectly aligned and get a small part, which was the case for this.

Overall it took a stupid amount of time, and I ended up staying an extra hour to get the first batch of parts done on the 4th axis operation. Since I got most of the kinks out, the rest should be pretty much smooth sailing as I only need to copy and paste the toolpaths over and program the final operation.

Working on the Pocket NC again, programming the final features that I've been putting off since the beginning. 

The part that I'm working on has a flowy feature that connects two pocket holes (as seen in the image above). The difficulty is getting the ball endmill to finish up that face leaving a decent surface finish.

I started by just trying out a couple of the multi-axis toolpaths in Fusion360 without much success. I'm relatively new to 5-axis programming and have only done simple exterior features; I have not done anything like this, so I am not even sure really where to begin. I ended up just googling how to do it and found a helpful thread on the Autodesk forums talking about this specific issue; they even had a download for it. 

I copied over the preset of the multi-axis program into my CAM setup and modified a few of the settings and generated it; I immediately got a very complicated jumble of toolpath going every direction possible. I simulated it, and just as expected, the tool crashed multiple times in the stock it was supposed to avoid and barely got any of the surfaces I selected. I ended up just restricting the endmill to a specific orientation and limited it to a maximum of 10deg tilt to prevent it from going on the other side. It turned out pretty decent, and the simulation shows it gets most of the material I wanted removing, there is one section toward the end where the side of the tool rubs up against the wall where I'm not super pleased with, but I'm sure I can figure that out. 

Today I worked on getting the 4th axis set up and dialed in on the Haas Minimill.

My boss showed me how to load the collets and dial in the position using a gauge pin and indicator. Using a 5/8" round gauge, I swept the dial indicator along the six inches of stick out and taping the base with a rubber mallet until it was within one-tenth (0.0001") from end to end. It took a stupid amount of time to get the 4th axis base locked in and still am a little frustrated.

From there, I used an edge finder on both sides of the rod, then divided the values by 2 to get the Y-axis origin, then did it again to ensure I didn't make a mistake the first time and got the same result as before. After that, I was able to load the mini fixture plate in the collet and tried facing it with an endmill to ensure I had a flat workpiece aligned with the machine but didn't get a perfect surface finish. My boss ended up tossing it on the lathe and cleaning the face it manually. 

After loading it back onto the minimill, I retook the edge finder and touched off the outside face for the X-axis origin. After that, I loaded one of the parts onto the fixture plate and secured it down; I then took the dial indicator and swept one of the flat faces to set the A-axis rotation origin. 

The final thing that I need to do is setting up the tools and setting the heights off the centerline of the X-axis line. I'm able to do this by using a 4" gauge block off the minimill table, the height of the 4th axis machine is precisely four inches above the face of the table so I can use that as a reference height. 

I also made sure to mark the top of the fixture plate and set up the CAM to have the engraving side always facing me; this ensures I don't make mistakes when loading the parts on the machine. 

I started running the finishing toolpaths on the Pocket NC today.

I'm disappointed with how the flow toolpaths turned out when cleaning up those chamfered edges, the machine had this weird pausing as if it was stalling (it wasn't) and left some pretty lousy finish marks. Maybe I programmed it wrong, and there is some smoothing I forgot to enable but very unhappy with that toolpath, I may try it again with swarf as I got great results when finishing the inside pockets. 

The swarf toolpaths for the side pockets turned out surprisingly well, and I got a very decent surface finish on all of them. I used a 1/8" endmill but should have gone with the 1/16" as it can't quite reach those corners, meaning it left some material there and looks a bit off if you study it.

I also cut out three of the final features using a 1/16" square endmill and a contour toolpath ramping down. Still not sure how to get that last feature at the top where it slopes into the top pocket (see picture above), and any suggestions would be much appreciated!

Today I worked on finishing up the first operations on the final set of parts and making a rotary fixture plate to attach them to. 

I was able to get the first operation done on the final set of parts without any issues and started moving over to the fixture plate. I spent a couple of minutes coming up with the design in fusion360 and then programmed the CAM and sent it off to the machine. The fixture plate is a small 3/4" block on one side, and 2"x1.5"x0.5" plate on the other with three holes matching the ones on the parts to bolt them together. I'll be using a square chuck collet to hold the fixture plate and using 1/4" pins on either side with a bolt in the middle, giving a very secure workholding fixture. 

Unfortunately, I completely forgot that the center hole needed to be threaded, and accidentally milled it out too large and had to scrap the fixture and start over. I also was cutting the clearance on the sidewalls of the fixture plate when drilling it out and caused the 1/4" drill bit of rubbing against the sidewall, leaving a mark and the tool to deflect. I changed the design a bit and added a small radius around the hole to allow the drill sufficient room to drop down without interference. I then flipped the fixture plate over and manually removed the last 1/4" backing to bring it down to its final height. 

Once I finished the fixture plate, I removed the vice and cleaned out the machine to prepare for the 4th axis to come down. There wasn't enough time to dial it in, so I'll be working on that tomorrow. Overall it's coming along nicely, didn't get as far as I thought I would but making steady progress.

Today I finished up all the programming for all the first operations on the four sets of parts I'm working on. 

The sets of parts are very similar in shape, so I was very quickly able to copy and paste the toolpaths with a few minor modifications to get it all working correctly. I'm getting into a groove with the Haas Minimill setup and programming, where I'm making very few mistakes and gaining quite a bit of speed. 

There are only two more operations per part that I need to work on, the fourth axis angles; for that, I will need to make a rotary and flat fixture plate to secure the pieces on. I'm a little nervous about using the fourth axis on the Haas Minimill as I'm not sure if it works the same as on the Pocket NC where I need only change the orientation of the toolpath for the machine to recognize and move to it automatically. 

The current process for the first operation of each part is to cut the stock down to size from a more substantial bar, align it in the vice (put small markers using old carbide on the jaws) and tap it in place on the parallels, then set the machine running. I wasn't able to finish the last set of parts today but have the program finished so I can get those running first thing tomorrow morning.