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.

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!

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. 

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!

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.