tag:buildsbygideon.com,2013:/posts BuildsByGideon 2020-08-05T03:26:58Z Gideon Harris tag:buildsbygideon.com,2013:Post/1581209 2020-08-05T03:26:58Z 2020-08-05T03:26:58Z Home Workspace | Making Chips | Pocket NC

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".

Harris Family
tag:buildsbygideon.com,2013:Post/1580977 2020-08-04T21:10:49Z 2020-08-04T21:10:50Z Machinist Apprentice | Polycarbonate Plates & More Watch Pieces| Day 39

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. 

Harris Family
tag:buildsbygideon.com,2013:Post/1580770 2020-08-04T03:27:22Z 2020-08-04T03:27:22Z Home Workspace | Finishing Toolpaths | Pocket NC

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).

Harris Family
tag:buildsbygideon.com,2013:Post/1580683 2020-08-03T20:56:10Z 2020-08-03T21:18:37Z Machinist Apprentice | Hole Tapping | Day 38

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. 

Harris Family
tag:buildsbygideon.com,2013:Post/1579351 2020-07-30T22:12:09Z 2020-07-30T22:12:56Z Machinist Apprentice | Finishing up the Stainless Steel Part | Day 37

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.

Harris Family
tag:buildsbygideon.com,2013:Post/1579085 2020-07-30T03:33:12Z 2020-07-30T03:33:12Z Home Workspace | Pocket NC CAM Workflow | Pocket NC

Made a little more progress on the part for @jaelen_hsu. I've been swamped lately with other work, so I haven't had a tremendous amount of time to work on this project.

Currently working through the best toolpaths for this type of part, I am taking my time and set up all the settings for each endmill and toolpath to make future workflow fast and easy. Taking advantage of sketch geometry in my CAM setups to make boundaries easier to select, which opens me up to many more toolpath options. 

I played around a bit to find what the best types of toolpaths were ideal for milling out these small areas and found that the 2D adaptive and pocket clearing worked the best. But I'm curious to know what other people may use, and would be very interested in everyone's thoughts on how it might be done most efficiently. If I get permission from the owner of the model, I will share the file during and after finished with the part with videos showing the operations in action. 

For this, I am doing an adaptive clearing for the front and back of the part using a 3/16" square endmill, then a bunch of pocketing and adaptive toolpaths for making the smaller features using a 1/16" square endmill.

Harris Family
tag:buildsbygideon.com,2013:Post/1578922 2020-07-29T21:24:34Z 2020-07-29T21:24:34Z Machinist Apprentice | Stainless Steel Toolpaths | Day 36

Today I got to finish the majority of the steel plate I've been working on the past couple days. 

Unfortunately, I'm not able to show very much of the project since it's under an NDA. I was able to finish cleaning the top face of the part and came in with a 1/16" square endmill to do an adaptive clearing and contour the small pins on top. Due to how they were located, there a tiny amount of material that couldn't get cut with the 1/2" endmill.

Two features on this part are critical, one hole, and a pocket, which needs to be in tight tolerance to one another. For this, my boss had me boar them out vs. drilling it, which would allow tolerances of plus or minus five-tenths (0.0005"). I didn't think it through properly and started to do this with a six flute square endmill, but stopped the machine quick when I heard a low rumble then crunch. It turns out that with that many flutes, there isn't enough room at the bottom to clear the chips properly, and so isn't ideal for cutting down. Thankfully I was leaving a few thou on the walls, so no real harm was done. I came in again with a four flute endmill and got the holes to within three tenths (0.0003").

From there, I used a quarter-inch four flute endmill to cut the part out of the stock using 0.03" step-downs at 30in/min. I did get a bit of chatter when it was cutting the backside of the piece, but I think that maybe because the flood coolant couldn't reach the end of the tool, and so was dry cutting. I then took a 1/8" ball endmill to clear a bunch of the material away to get a chamfer along the edges. I had to use a ball endmill because there were some smaller features that only a ball endmill could reach, and so would have to do the entire contour of the part with a 1/16" ball. There are some tricky areas to this part, which I may recreate to show some of the difficulties I had to deal with. 

Overall the part is coming out looking beautiful, and everything is within 0.0005" (well above acceptable tolerance!), and the finishes are immaculate!

Harris Family
tag:buildsbygideon.com,2013:Post/1578367 2020-07-28T21:01:19Z 2020-07-28T21:01:20Z Machinist Apprentice | Fixture Plate & Stainless Steel | Day 35

Today I worked on making the fixture plate for the stainless part I am working on (see previous posts).

I got the steel plate to within 0.0005" of its final thickness, which well below what the allowable tolerance is! From there, I drilled the holes in the steel plate to bolt it down later. 

For the fixture plate, I shaved down the top face to ensure I had a flat workpiece, then drilled the holes for threading. I realized too late that I accidentally cut them with a 1/4" drill bit to make 1/4-20 threaded holes, which is much too big for the thread size. Thankfully I was able just to shift the x-axis origin over a bit and recut it with the correct drill bit (#7 drill). I then hand threaded each hole while it was still in the vice using a vertical block my boss made to ensure you cut it vertically. 

I then bolted the steel down on the fixture plate and got the gcode loaded in the machine, this was the part I was nervous about, and triple checked my programming to ensure I didn't have any errors. I set the Haas minimill off, and right away, a hear a dull crunch sound, thankfully I was right there to stop the machine. What had happened was I accidentally set the origins to be slightly different for the fixture plate operation and steel one. It was only about a quarter-inch off, so I didn't realize it in Fusion360, but the tool dived into the material, thinking it was air. 

Unfortunately, it's a more complicated issue than you might think, and I spent a while trying to figure out how I would change the origin since the setup stock wasn't off of solid models and so nothing I could measure. After discussing it with my boss, I relocated the work origin to one of the holes in the steel plate and swept it with a dial indicator. From there, I was able to get the part off and running; I was only able to get through about half of the first tool operation before I ran out of time for the day. 

Harris Family
tag:buildsbygideon.com,2013:Post/1577979 2020-07-28T03:21:21Z 2020-07-28T03:21:21Z Home Workspace | Swarf & Viewpoints | Pocket NC

First off, I want to say a huge thank you to @aye_cnc for helping me through some of the issues I was encountering on the Fusion360 CAM workflow. If you haven't already I, highly suggest checking out his page where he is posting a lot of exciting content on the Pocket NC! 

My previous post on the PNC project was about having issues with the finishing toolpath on the part where I couldn't get the right orientation and selection to get the interior pockets cut. Alex contacted me shortly after and offered to give me a hand, which I gratefully accepted! 

He recorded himself working through and creating sketch planes for each of the pockets and face orientations to select when setting up the toolpaths. I uploaded the video he sent in my previous post, which I am sure you will find valuable! I didn't even know some of the tools he used existed in Fusion360 and will be using them! One of those is the 3D sketch option, where you can turn a 2D sketch into a three dimensional one, very useful for creating sketch guidelines and templates! 

With the sketch outlines, I was able to create the finishing toolpaths very quickly and easily, without having the pain of trying to select geometry on different planes.

I honestly haven't used the constraints very much in the sketching area of Fusion360. After seeing Alex's video, I will be familiarizing myself with each one, for the speed and accuracy it brings!

Harris Family
tag:buildsbygideon.com,2013:Post/1577821 2020-07-27T20:54:50Z 2020-07-27T20:54:50Z Machinist Apprentice | Stinaless Steel Plate Project | Day 34

Monday back to the grind! Today I worked on getting the steel plate down to its final overall thickness. I absolutely love the look of finished stainless! Its got that nice dark look to it with an almost matt shine.

Since this is stainless steel cold rolled (formed through rollers without heat), it's got a lot of tension built up in it, and so when you release the pressure by shaving one side of the plate down, it will bow ever so slightly in that direction. Because of this I need to remove a thin amount of material from both sides to let it breathe. 

The overall part thickness is about 0.46" (can't give exact dimensions), which is too close to 0.5" to use half-inch stock due to the tension in the material. So my boss bought 0.75" stock and had me shave it down to its final thickness by shaving both sides evenly, starting at 0.05" then as it got closer to the correct height, down to 0.02" stepsons, for better accuracy and to ensure a perfectly flat workpiece.

I had to face the material using a 1/2" endmill, which he explained was to reduce the amount of shock and heat it would generate. If you were to use a larger endmill or flymill your contact would be much higher, thus more friction, and so more heat. The run time for each stepdown was 7 minutes each and had about a quarter-inch to remove, so it took about three hours to do. 

While the machine was running, I got to program the rest of the part. It's got a somewhat unusual shape which can't be held in soft jaws because it needs to be contoured, but does have a few through holes which I'll be using to bolt down to a custom fixture plate for it which I'll go more into tomorrow. 

Harris Family
tag:buildsbygideon.com,2013:Post/1576682 2020-07-24T21:14:08Z 2020-07-24T21:14:08Z Machinist Apprentice | Stinaless Steel Part Programming | Day 33

Today I finished cleaning up the front of the shop and office area, then started programming the CAM for a new contract that came in the other day. 

The part is a flat plate in stainless steel with a few threaded holes and locating pins built into it. The stainless we are using is cold rolled, which means there is a lot of surface tension in the material. Just like the small stainless buttons, I worked on a couple of weeks ago, when I removed the part from the soft jaws, it sprung out at me. The same thing will happen with this plate, and so my boss instructed me how to work around it. I was to take 0.02" off of the top and bottom of the stock, then 0.05" facing step-downs evenly until I got the actual height.  By removing the small amount of material first from both sides, it would release the tension in the material and prevent it from bending later on. 

Since there are the locating features on the top face of the plate, it means the overall height of the stock has to be higher to match the highest point in the model, which requires a ton of material removal to leave just the pins. Wayne wanted me to use a parallel facing operation to cut down the material, avoiding the pins. Still, unfortunately, there isn't an option in the facing toolpath to avoid certain areas. So I played around with a few different toolpaths to see what would work best and leave an excellent surface finish. I found that the 2D pocket clearing worked the best, I was able to avoid the pins and have a decent looking path. 

The part has a unique shape, and so I'll be making and using a fixture plate for it and locating pins, which I am excited for!

Harris Family
tag:buildsbygideon.com,2013:Post/1576538 2020-07-24T03:05:55Z 2020-07-24T03:05:56Z Home Workspace | Multi Axis Contours | Pocket NC

First off, I want to say thank you to everyone who commented on yesterday's post with the PNC pocketing issues. I was able to solve the problem I was having by changing the operation from a 3D pocket clearing to a 2D pocket clearing. The ramp down was still the same, but it didn't take roughing step-downs and went all the way to the bottom then retracted up in one motion. 

I then started getting into some of the multi-axis portions of the CAM, which got a little complicated. The part has quite a few unique angles that require simulations 5-axis work. For all the flat, curved faces, it was pretty easy to do with a flow toolpath. However, when I got into the contouring for the pockets, I ran into some issues. Typically you would use a swarf toolpath and simply select the top and bottom 2D contours. Except this part doesn't have specifically defined line segments on the interior of the piece, and so you only have one point of contact (the outside parameter of the pocket). I'm somewhat new to simultaneous 5-axis programming; any insight would be greatly appreciated!

I am also using the Pocket NC simulator to check and see the toolpath functions as it should in Fusion360. I ran into some issues when trying to post the gcode where it would keep giving me errors "<post name>.failed", until I figured out it was with the 5-axis flow toolpath, I narrowed it down to the maximum tilt the machine would allow and lowered it from 180deg to 15deg.

Harris Family
tag:buildsbygideon.com,2013:Post/1576440 2020-07-23T20:57:14Z 2020-07-23T20:57:14Z Machinist Apprentice | Deeper Cleaning | Day 32

Today I spent the entire day at the shop scrubbing the floors to get them to shine!

I was initially tasked with finishing the corner of the shop, where I didn't have time to do a few weeks ago. Still, after doing that with some heavier cleaning supplies (scotch bright and degreaser), it looked too clean compared to the area around it, and so went through and cleaned the rest of the floors. There is quite a contrast with the before and after, and I thought what I did a few weeks ago was good, it was nowhere near what it was today. 

The downside to using the scotch bright is it removes the seal on the floor but was already scratched up so bad it didn't make a huge difference. My boss is going to have me redo all the floors by sanding, polishing, and sealing when the shop gets slow. 

Wayne also got another contract, which I'll be working on tomorrow. It's a large 7"x3"x1/2" plate in stainless with some unusual geometry to work around. 

Harris Family
tag:buildsbygideon.com,2013:Post/1576269 2020-07-23T03:06:49Z 2020-07-23T03:06:49Z Home Workspace | Ramping Issues on a New Part | Pocket NC

I'm trying something a bit different from the Pocket NC since I have limited time, and that is to restrict it even further by only allowing myself 30 minutes each day, which will give me time to think about it more and ask the community. 

This part is the first of a set that I am teaming up with @jaelen_hsu to make. I'm using the er40 fixture setup on the PNC with a 1" round aluminum stock. It's got quite a few interesting angles and is going to be a challenge, which I am very excited about!

While programming it (started with adaptive clearing to remove the bulk of the material), I did a pocketing operation with a 1/8" endmill to clean out those holes. However, I noticed that the ramping on it was quite long, and once it reached it's pre-defined stepdown, it would retract and do it all over again. I recorded a short video showing what's happening, and I haven't had a huge amount of time to play around with it. But I do know it's not directly related to the ramping section in the linking tab. If anyone has any insight on this issue or a better way to clear out those pockets, let me know!

Harris Family
tag:buildsbygideon.com,2013:Post/1576189 2020-07-22T21:41:27Z 2020-07-22T21:41:28Z Machinist Apprentice | Aluminum Threadmilling Troubles | Day 31

Today I was able to finish up making the parts I started earlier this week and get those deburred and cleaned up. I noticed a small mark on the wall of the part which was where the endmill lead out of the contouring toolpath. I should have had it lead out along the line of the wall instead of coming at a 90deg angle horizontally. I was thankfully able to get it cleaned up pretty easily with a light sanding.

These pieces have a couple of holes on them that needed 2m-0.4 threads, which I wrote about having some CAM issues last week, which I solved on the software end of it. However, when I went to go and mill out the threads, I found that they where much too tight, which I kind of figured might happen. I talked to my boss about it, and he suggested creeping up on the thread size by increasing the tip diameter offset one thou at a time. Which I did for about four thou and still nothing, I didn't go higher than this because when I simulated the highest offset value I put, the tool was almost rubbing against the walls of the 1/16" hole. I'm honestly not sure why the thread milling wasn't working and ran out of time to play around with it and had to thread them by hand. 

If anyone has an idea what the reason could be, I'd be much appreciated! Tomorrow I'll spend a few hours on the thread milling and tap drilling with some scrap pieces of aluminum. 

I also had some weird issues with the laptop my boss picked up to work on. The screen would flicker quite a bit, and after googling the problem and updating the windows software, it would get worse! It mostly occurred when running Fusion360 and having a few tabs going taking up a lot of the CPU, and would get to the point where I could only see the screen every couple seconds due to the noise. I called up Dell customer support to see if they had any ideas, but there was quite a bit of confusion over the phone and could hardly understand what they were saying, so I decided just to spend a bit more time researching the issue. After trying a dozen different things, I finally found something that fixed the problem, at least for now. Under the device manager, I deleted the graphics card and rebooted the computer. I then updated windows to get the backup file of the graphics card, and that worked!

Harris Family
tag:buildsbygideon.com,2013:Post/1575965 2020-07-21T21:49:27Z 2020-07-21T21:49:27Z Machinist Apprentice | Aluminum Parts | Day 30

Today I worked on making a set of 6061 aluminum parts! Not sure what their purpose is, but they have a flat top face with radius edges, and some features on the bottom.

Since there is the radius on the top face, the part has to be done in a two-part operation using soft jaws. For the first operation, I did an adaptive clearing using a 1/2" square endmill to remove the bulk of the material, then a contour to clean the sides up, and a boaring operation to locate the part when flipped, and finally a scallop toolpath using a 1/8" ball endmill. I pulled the part out after it finished and noticed there where facets on the walls of the piece. I wasn't expecting this because I've run the same settings on the stainless with excellent results. I played around with the settings a bit and couldn't find the cause of it. Even the simulation had tiny facets on it. I tried using smoothing and adjusting the tolerance in the CAM, but no matter how much I changed them, I couldn't get it removed.

I started on the second operation but only got through a few toolpaths before I ran out of time for the day. Unfortunately, I also broke the drill bit I was using when I had a 0.0625" carbide drill peck down 0.05". Since I was using the Haas minimill which doesn't have a tool height probe, which means I had to use a single tool to do all the visible finishing by itself, because if there were any slight difference in height, it would show up on the finished product. So the finish quality isn't as good as I would have liked, due to the toolpath marks. 

My boss also got me a 3D connexion space mouse for Fusion360, which I had no idea how much of an impact it made until I tried it! It's always been one thing that kind of frustrated me about 3D modeling programs in general, its always tricky to orbit around the design, but with the space mouse, it eliminates that almost completely! 

Harris Family
tag:buildsbygideon.com,2013:Post/1575626 2020-07-20T21:14:06Z 2020-07-20T21:14:07Z Machinist Apprentice | Threadmilling Issue Solved! | Day 29

Finally figured out the issue I had last Friday with the single flute thread milling!

(if you haven't already you can read about the issue in my previous post) 

It turns out the problem was due to the shoulder diameter on the threadmill itself. By default, Fusion360 decides what the width of the shoulder diameter is, regardless of what it should be; however, they do allow you to add the shank and cutting diameter. I looked around for some time, and even went back to the old tool library to see if maybe they had more options to input data into the tool settings, but alas, no. 

I was able to fix the problem in a sort of roundabout way; in Fusion360, there is an option to add custom tools called Form Mill's. The basic idea is you sketch out a 2D half of your endmill, then select the center axis where the form would wrap around to create the tool. Huge thank you to @saundersmachineworks for the video on Form tools, made it super easy, and only took a few minutes to sketch and create the custom tool. Now that I had the custom tool I found the pitch diameter offset by taking the thread size 2mm (2mm-0.4 thread), subtracting the hole size, 1/16", and dividing it in half (for both sides) to get the correct number. I then simulated the toolpath and watched it as it cut through the material, and it ran perfectly! You can see above the two tools in video and drawn out, one on the left sketch pad is the custom form tool, and the one on the right is the tool library input one. 

Harris Family
tag:buildsbygideon.com,2013:Post/1575619 2020-07-20T20:41:12Z 2020-07-20T20:41:12Z Machinist Apprentice | Threadmilling Troubles | Day 28

I was in a bit of a rush the other day and didn't have time to write up what I did. I got a new part to work on from my boss and one of the things he wanted me to try thread milling for the tapped holes. 

I thought it would be a relatively easy toolpath to program after watching a few videos's on it. However, I very quickly ran into an issue when making the tool itself. Unfortunately, there isn't a lot of information online about actually creating the tool, only some of the settings that set the offsets. I played around with the tool settings a bit and input the data I got online from this threadmill, and finished setting up the toolpath and everything seemed fine until I simulated it and saw it only cut into the material and left a very light trace where the tool barely touched the material. I spent a very frustrating two hours on it trying to problem solve but with no avail. I thought it might have to do with the tool diameter offset but I played around with that and didn't get any results. 

My boss then pointed out that the shaft of the cutter might be rubbing against the walls of the hole and thinking it's cutting it when it's not. I played it through and had it show color differences so I could see if the tool was rubbing or not. Turns out it was and I tried again to change the settings around with the threadmill but got similar results. I found that Fusion doesn't allow you to dimension the stickout of the teeth on the endmill. It's very difficult to describe the issue, but if it works I'll go into more detail and visual examples. At this point, I ran out of time and had to leave it for the weekend. 

I saw my brother (@bladesofbelaq) who is also a machinist and asked him about the issue I was having and we discussed it for a while. He then realized that the issue might not be with Fusion, but rather the tool itself, not being the right size for these threads. He pointed out that the threads are only going to be cut with the sharp edge of the threadmill and never with the stickout of the teeth. 

Harris Family
tag:buildsbygideon.com,2013:Post/1574218 2020-07-16T20:33:05Z 2020-07-16T20:33:18Z Machinist Apprentice | Shop Cleaning and Re-Organization | Day 27

Today I worked on cleaning the shop after focusing only on making parts earlier this week. I'm delighted I had the opportunity to organize the tools beforehand as I know where everything is and where everything needs to go!

Not super interesting today, mostly sorting the tools I wasn't able to get to before and setting up new bins for the taps. There are quite a few different kinds of threading tools, some spiral, two, three, and four flute ones, and even some with drills! My boss also got another part for me to work on, which I'll be doing tomorrow, so I'm very excited about that!

Harris Family
tag:buildsbygideon.com,2013:Post/1573811 2020-07-15T21:11:40Z 2020-07-16T20:33:13Z Machinist Apprentice | Threading & Shipment | Day 26

Another full day of preparing these parts for shipment!

The last set of parts needed to be threaded (40 holes in all) each was a blind hole, and so I had to go down twice to be sure I hit the acceptable length. An interesting technique I haven't seen or heard of before but is built into the design of the hand taps. There is a hole at the top of most tap holders; its purpose is to slide a gauge pin into a vertical clamp of some sort, which in this case was the old manual CNC mill. You then slide the hand tool into the pin, and it creates a perfectly straight and stable way to hold the tap handle and still rotate and move it up and down. It's difficult to explain, so I'll upload an image of the setup I was using to thread all the holes.

After that, I gave all the parts a bath in soapy water, removing all the dirt and grime from sanding and deburring, then a rinse and spray down. From there, I packaged each part with toilet paper to ensure safe shipment! Since I've spent most of my time working on those parts, the shop has gotten somewhat messy again and will be spending the majority of tomorrow cleaning and reorganizing the tools.  

Harris Family
tag:buildsbygideon.com,2013:Post/1573376 2020-07-14T21:25:10Z 2020-07-16T20:33:08Z Machinist Apprentice | More Deburring and Cleaning | Day 25

Today was more deburring, cleaning, and prepping parts for shipment. My boss did the final piece, which is a unique shape requiring three operations to mill it all out and didn't have enough time before it's due to have me do it. 

Removing copper burs is the bane of my existence; this specific piece has over 30 edges on it and ten parts total. Not to mention, copper is very resilient to any sort of tool you throw at it and takes several passes to clean up each edge. If you're not already aware of what a burr is, it's typically melted or pushed away material that the cutter (in this case endmill) didn't slice but simply shoved it to the side. I'll put up an example I found online of a more exaggerated version (before and after).

Part of the design included a section with three thin flat walls that were extended out and open on one end. If you tried machining it without any modifications, you would have a lot of trouble getting an excellent finish and staying in tolerance due to the fragility of the wings. The way he overcame this was to make a temporary wall on the opposite end and fill the pocket with a hard plastic molding material, then you can come in later and remove the partition with better rigidity and structure without the worry of the walls buckling in. The casting material is a Quik-Cast Polyurethane two-part resin and takes only an hour to cure with low shrinkage.

Harris Family
tag:buildsbygideon.com,2013:Post/1572846 2020-07-13T21:04:25Z 2020-07-13T21:04:26Z Machinist Apprentice | Deburring, Cleaning, & Tapping Copper | Day 24

Nothing too exciting today, I finished tapping the set of 101 Copper parts I worked on last week and got those ready for shipment. 

I also programmed the other side of the second set of parts that needed a small corner stepdown and got to do that on the Haas VF2ss. The second operation setup on these parts was pretty easy and only took a couple of minutes to program. Since there were only ten pieces, my boss said just to do each one at a time and put them in diagonally to make each part be in the same spot as before. 

I did the entire operation with a 1/16" square endmill, first to pocket out the soft jaws, then to cut the corners on the part itself. I programmed the corners of the part to cut out a little bit larger than the edge of the part to allow it to sit snug against the side walls. However, after running the program, I accidentally broke the tool when it took the corner at 100% engagement and 29in/min, I then talked with Wayne, and he said that it wasn't necessary as the corners on the parts where rounded. So the 1/16" would already clean the edges properly. I reran it without that pocket and got a lovely finish. 

After that, I did a dry run the copper toolpath to cut through the aluminum soft jaws to prevent things from overloading. When that was complete, I cut the ten parts and got them all within one thou of each other. 

Harris Family
tag:buildsbygideon.com,2013:Post/1571813 2020-07-11T03:12:36Z 2020-07-13T20:41:33Z Machinist Apprentice | Copper Parts! | Day 23

Today I got to machine the 101 copper parts I mentioned previously. Unfortunately, since these are more detailed pieces, I am not able to show the entire piece and have to blur some parts out. But as you can see, they turned out nice!

In preparation for this part, I did some research on milling copper, and for the most part, a lot of people say it's one of the more delicate materials to cut as its got a gummy like consistency and can wad up on your tools. I also read that you want very sharp tools when cutting it to prevent the material from just being pushed rather than sliced through it. I also found that it's super shiny and picks up every little detail; even with the finished product, you can clearly see the path of the tools but can't feel any deviation in the finish. Because of this Wayne had me do a spiral toolpath in the little pocket on a ball endmill, he said if I used a flat or bullnose endmill and cleaned the bottom face unless I had the tools measured correctly, you would see a slight step between the endmills even if you couldn't feel it. I had to use a ball endmill to get the corner radius at the bottom of the pockets.

Overall it wasn't too difficult to program, and the entire machine time for ten parts (each about 1" square) was one and a half hours. I needed to make 20 of these, but the second set required a larger hole size, so instead of reprogramming the whole thing, Wayne just had me run the same program but switched out the drill bit. When I ran the second batch, I remembered a second before the tip of the drill hit the material that I forgot to set the tool height, and thankfully no harm was done. If I let it run, it would have rapid into the stock thinking the drill was shorter. 

After that I de-burred the parts and started threading the holes on one set, I ran out of time though and will have to pick up where I left off on Monday. 

Harris Family
tag:buildsbygideon.com,2013:Post/1571356 2020-07-09T21:24:53Z 2020-07-09T21:24:53Z Machinist Apprentice | Shipping Parts & Programming 101 Copper | Day 22

Today I finished up the second batch of larger pieces and got those packaged up. Since these are such small parts, Wayne had me put them in old plastic endmill boxes with a little bit of toilet paper to keep them from getting damaged. I think the issue with the weird height differences for the smaller parts was due to the slight radius in the bottom of the softjaw pockets, which allowed them to be moved around every so slightly, and so getting different measurements if the clamp position was changed. For the larger parts, the tolerance was within 0.0005" of the design, which isn't too bad at all!

The rest of the day, I spent working on the next set of parts using 101 Copper. I am just about finished with the programming for it and cut the soft jaws to hold it in place. I also got to use an edge finder for the first time, which I used to find the back wall of the vice to use as the origin in the CAM setup. The copper will be cut to width when putting it in the vice, so making sure it's perfectly aligned for repeating the process. 

I'm starting to get into a groove at the shop and feeling pretty comfortable with all the Haas mills! I know where all the tools are, how to program and set up one and two operation parts and get them ready to be shipped out! I'm still not as careful as I should be with freshly cut parts and accidentally brushed against the side of the soft jaws when taking them out.

Harris Family
tag:buildsbygideon.com,2013:Post/1571037 2020-07-09T03:23:45Z 2020-07-09T03:23:45Z Machinist Apprentice | Finishing up the Parts | Day 21

Today I finished up the second operation on the parts I was working on yesterday.

After finding the center of the hole and relocating the G54 to it, I was able to run the second program to finish up the parts. I had a few test pieces that I made before so I could toss these if they didn't turn out any good. It turned out alright, though the surface finish wasn't the greatest, and Wayne noticed the chamfer wasn't entirely centered on the part. As it turns out, I forgot to enter the new G54 home, and so was about six thou off. He also suggested surfacing the top and leave about 0.03" on top to connect the parts; this would allow the tension to be released and make the pieces easier to bend the bow out of it. 

I edited the code and reran it on my main piece, which turned out very nice. Unfortunately, while measuring it, I noticed that it was consistently five thou off on the height, and after discussing it with Wayne, I added that offset to the code to lower it by that amount. However, after putting the parts back in and running it once more, I must have miss measured the first time, and all the parts came in under four thou of the drawing. Since this is on a time limit, he said to use them as is, as the tolerance had to be within ten thou, though he would typically get it closer. I'm not sure how I miss measured it the first time, but I have a sneaking suspicion that the one I referenced wasn't flat against the bottom of the soft jaws. I finished up the rest of the smaller pieces and set up the jaws for the larger parts, which I'll be finishing up tomorrow. 

Overall a bit frustrating with the tolerance mishap, but I'm delighted with how their surface finish!

Harris Family
tag:buildsbygideon.com,2013:Post/1570552 2020-07-08T03:03:44Z 2020-07-08T03:03:44Z Machinist Apprentice | Finishing First Operation and Cutting Soft Jaws | Day 20

Today I got to finish up the rest of the parts on the first operation. There are two sizes of these parts and did all the first operation in one go before cutting the soft jaws since the location was a known one and easy to set the stock in place. 

My boss also solved the issue I had yesterday, where there would be a small cap on top of the part that should have been cut off when facing the material but wasn't. Wayne thinks it might be due to the released tension in the stainless stock, and rerunning the facing operation, that seemed to solve it. Each part I loaded ended up with the same small cap on top and had to rerun the first toolpath on each one. 

After making enough of the first operation parts, we moved over to the soft jaws. For that, Wayne had me put a 1/32" parallel to separate the two jaws, to give it some clamping force when the parts are in. I then faced the aluminum and located the center for the soft jaw milling operation. It came out a bit rough, and after consulting my boss, he reran the program after deburring the edges. From there, the parts fit in pretty nicely, though there was a slight radius in the crevises of the pockets which I didn't see on the used endmill I loaded. Thankfully it doesn't look like it will be an issue as the fillet on the part matches the radius on the inside pocket. From there, Wayne put a 1/16" pin in the locating hole, and I used a dial indicator to find the center to set the G54. I ran out of time for the day and will finish the final operation tomorrow!

In between runs, I started programming the other parts, which will be made in copper. I unfortunately, I won't be able to share any images of the elements themselves as they are proprietary, but I'll do what I can to share pieces of it. It's got a lot of nifty corners and crevices, which were a bit of a pain to figure out how to do because of interior radiuses done in metric.

Harris Family
tag:buildsbygideon.com,2013:Post/1570244 2020-07-07T03:26:59Z 2020-07-08T02:40:36Z Machinist Apprentice | My first Operation on the Haas Minimill | Day 19

Today I got to run the milling operation on the Haas minimill that I programmed last week!

I loaded the new soft jaws into the vice and faced it. I then used a couple of parallels to space the two apart so I could cut a groove down the center to fit the raw 1/4" stock in the middle. From there, I loaded all the tools and found the center to set as my G54 (work origin). While loading the endmills (each bit has to be manually measured in using a height gauge block), I accidentally sent the z-axis crashing down on the material, breaking the 1/16" ball endmill and leaving a small fragment in the stainless stock. Thankfully there was no lasting damage, but it made me jump when it happened and left me a bit on edge for a while after. 

After loading and setting the tool heights, I started the operation. Everything went according to plan and got through all the toolpaths without a hitch. I did set the peck-drilling process to take 0.0004" by accident, and so that took quite a bit longer than intended. Once the first operation was complete, I loosened the vice only to see the part practically spring out at me due to the released tension in the material. Right away you could see it didn't look the best, it has significant facets which the contouring toolpath should have cleared up, and you can see the top face somehow has a little cap on top of it from what I am guessing is a tool height issue. 

I edited the toolpaths to correct these issues by changing the tolerance and added smoothing (allows the toolpath to roll around instead of point to point), which I posted the code again and set the machine running. I also re-measured the tool height offsets on each of the tools to ensure everything was correctly aligned; this time, it ran much better and had an excellent surface finish (I forgot to take a photo). However, there was still a small cap on top, not as tall as it was before, but even noticeable, and I'll have to do some digging to figure that out. 

Harris Family
tag:buildsbygideon.com,2013:Post/1568505 2020-07-03T17:16:24Z 2020-07-03T17:17:16Z Home Workspace | New Vice Fixture | Pocket NC

My boss gave me the day off for independence day so I thought I'd write about my new Vice Fixture from @pocket_nc!

After talking a bit with a few different people about my old clamp system, I designed a couple of months ago; they pointed out a few flaws. The main flaw with it is the rigidity of the design, the only point of contact with the stock is the lower half maybe 1/2" in total, and the rest is free-floating; this causes vibrations to go through the stock and leaves imperfect surface finish quality. 

I talked with my boss about it and mentioned @pocket_nc had a circular stock fixture to hold round rods of material with an ER-40 collet. It's got sufficient clamping force to hold it securely in the vice and provides much more rigidity. I was convinced that it was worth it very quickly, especially since I didn't have to do as much work calculating where the stock was in the machine. My boss also mentioned that you could take 3" round stock and put it on a lathe to cut one end down to 1" (the largest diameter the clamp can hold). With a piece of circular stock cut down to 1" on one end means you can pretty much mill out whatever size part you like on the machine with relatively stable work-holding.

It came in on Tuesday, and I was dismayed to find the tool to tighten the fixture, not in the package. I contacted Pocket NC, and they responded within an hour, apologizing for the mistake, and shipped a new one right away. The next day I received it, not even 24 hours after I got the package. I love the people at @pocket_nc; they are always super friendly and have fantastic customer support!

Harris Family
tag:buildsbygideon.com,2013:Post/1568240 2020-07-02T23:54:02Z 2020-07-02T23:54:02Z Machinist Apprentice | More Fusion360 Programing | Day 18

Nothing too special today, much the same as yesterday programming another similar part and double-checking my speeds and tool orders. 

I also figured out the issue I was having with post-processing to Haas machines. The error I was getting was related to the program name; it requires that you only have numbers, and a minimum amount (in this case 4) and no letters. However, you can change the name after generating the G-code when you save the file. 

I also started programming one of the parts that were to be made in Copper but didn't make too much progress due to some complicated features in the part I wasn't sure how to mill out. It had an interior pocket with the edges filleted to a metric value. I attempted just to use a metric ball endmill to get that corner, but I kept getting weird finishes in the simulation. 

Harris Family
tag:buildsbygideon.com,2013:Post/1567769 2020-07-02T04:25:59Z 2020-07-02T04:26:50Z Machinist Apprentice | Fusion360 Programing | Day 17

Today I was focused on finishing the CAM for the part I worked on yesterday. 

After talking with my boss, I decided to scrap what I did and start from scratch. I did it pretty messy and wasn't very easy to make quick changes. I also had oriented the part the wrong way and had the first operation on the underside of the piece instead of the top. The reason for doing the top of the piece first was purely for aesthetics, and if things didn't look quite right, it's better to have that on the underside where it wouldn't be as important. I figured that since this is such a small part and for the client, they would want accuracy over aesthetics he said it should be dead on regardless, and so work the side that would have the best finish. It would also make clamping these in soft jaws much easier as I wouldn't have to mill out a groove for the pin on the bottom.

Since this is a two operation part, I decided to make a solid model for the stock rather than try and create a box around it in the CAM setup section. Having a pre-designed object would help with locating the part after flipping it over by drilling a hole through the center, then probing it from the other side. 

I'm pretty pleased with what I came up with and need to double-check some of the toolpaths, but I think it's just about ready! I also did have some issues with the post-processor, giving me an error when I posted it to Haas. It wasn't very clear as to what this issue was, and so I'll have to play around with it a bit more to find out why. 

Harris Family