Milling Brass - Mess Mitigation - Success/Failure - And Questions

[Ziggy]

Hello

This is my first foray into cutting metal with the Onefinity so please forgive my lack of experience.

I don’t see myself cutting metal very much. However I wanted to make some brass inlays.

I didn’t want to ruin my spoilboards with cutting fluid. I also didn’t want brass chips getting into the lead screws if I could help it.

So I did a little work in Fusion and came up with an – admittedly – probably overkill solution.

My idea is to have a flat(ish) tray where I can screw down sacrificial plates to which I have glued sheets of metal. In addition, I wanted to keep the chips that shoot up out of the lead screws as best as I can so I made a shield that attaches to the Suckit arms.

Here is the tray.

Here is a piece of brass Superglued to a 3D printed spoil plate

I reasoned that once the milling is done that I could immerse the 3D print and brass into acetone and let it sit overnight. More on this later.

I posted a couple of videos of the milling operation to YT.

This brings ups a question/concern. Is that “clunking” sound normal? It seems to happen when there are sudden movements. Normally I have dust collection running so I wouldn’t have heard it. Is there a setting in Fusion CAM that tells it to make the transitions more gently?

Also, I think I have my ramp too steep.

Here are the videos.

Video 1

Video 2

Takeaways:

The idea worked for the most part but wasn’t entirely successful.

I realized that I didn’t need to make such a large hole for the chip shield since I would be using shorter milling bits and the spindle would never need to pass through. I’ll make one with a hole just big enough for the collet. Easy enough.

The biggest failure is that the spoil plate failed. I think using an upcut bit caused the top layer to lift and it ruined a couple of my parts. (See Below) I will try printing another with 100% infill and using a downcut bit, If that doesn’t work I may search for a different substrate.

The part on the left was fine. the part on the right lifted and the side of the cutter ate away part of the “C.”

Soaking the parts in acetone worked but also had some downsides. It caused the PLA to warp and twist to the point I was afraid it would bend my parts. So I had to pull everything out and gently cut around my parts. After letting them soak overnight they came out clean.

To be honest, I don’t like the fumes of the Superglue and I don’t like the mess of the acetone. I am considering using Hideglue to attach the workpiece to the spoil plate. That can be soaked in water to release the part… theoretically. My only worry is that the hideglue might not be strong enough to deal with the milling especially after being squirted with water based cutting fluid.

So… any ideas or suggestions?

Also, please let me know if that clunking sound is normal. It is a bit worrisome.

[AndyP (Badger)]

I have come across someone who makes steel clock hands and superglues the steel directly to a piece of machined Aluminium and uses a solvent to soften the superglue once the hand is cut. I haven’t tried it myself.

[Hermsen.BJ (BJ Hermsen)]

I found that super glue did not mix well with cutting oil and/or the heat that soaked into bread when I tried that…but it may have been me and my feeds and speeds

[SurfinGump (Forrest)]

I purchased a mist coolant block and nozzle (https://www.amazon.com/gp/product/B07HT1Y4BK), which I attached to the laser mounting screw holes, and used isopropyl alcohol (IPA) as my coolant/lubricant. While it primarily functions as a coolant, I like to think it provides some degree of lubrication as well.

The brass blanks were sourced from Send Cut Send (highly recommended). I secured them into a jig made from a scrap piece of wood, using a combination of blue tape and super glue. As long as I didn’t flood the piece with too much IPA and kept it to a barely noticeable “fog,” the tape and glue did an excellent job of holding the brass firmly to the MDF jig.

One of the advantages of using IPA is that it evaporates extremely quickly and doesn’t damage the wooden jig. By keeping the airflow at about 20-25 psi, I found it was enough to blow the brass chips clear of the bit.

The downside, though, is that the brass chips still get EVERYWHERE. Even with a dust boot and the misting nozzle working together, tiny pieces of brass seemed to fly into every corner! I had to be meticulous about vacuuming and cleaning up after each carving, and often during the carving process as well. Despite my efforts, I still ended up with brass splinters (ouch!) for days after, even when I thought I had thoroughly cleaned everything up.

Given the constant cleanup required and the fact that I was working on extremely detailed 3D carvings on relatively small pieces (~4-inch tall blanks), I’ve decided to scale back on these projects. Mass production of these intricate 3D carvings is simply too time-consuming and prone to scratches caused by the bit and/or chips getting in the way, so I’ll likely only do them for special occasions moving forward.

I hope this post helps someone considering brass carving! Photos, videos, and details on feeds and speeds to follow below.

Toolpaths:

3D Roughing 1
Powertec 1/8" 2FL Up Cut End Mill
1 mm Boundary Offset
0.5 mm Machining Allowance
3D Raster mode
Avoid machine areas: checked
Raster angle: 0 degrees
18,000 RPM
750 mm/min
750 mm/min plunge
40% stepover
0.0295 INCHES pass depth

3D Roughing 2
BitsBits 4TEB10-062-2FL - 1/16" Tip 5° Tapered Ball Nose
1 mm Boundary Offset
0.1 mm Machining Allowance
3D Raster mode
Avoid machine areas: checked
Raster angle: 45 degrees
16,000 RPM
2000 mm/min
1000 mm/min plunge
8% stepover
0.025 INCHES pass depth

3D Finish
Lakeshore Carbide 020ENG14-20DG-DE-N3 (20.0°, Tip 0.508mm - 6.35 mm)
1 mm Boundary Offset
3D Raster mode
Raster angle: 0 degrees
18,000 RPM
2000 mm/min
2000 mm/min plunge
8% stepover

[Machinist (Bill Blades)]

@SurfinGump

I had to be meticulous about vacuuming and cleaning up after each carving, and often during the carving process as well. Despite my efforts, I still ended up with brass splinters (ouch!) for days after, even when I thought I had thoroughly cleaned everything up.

Wow, welcome to my world when I cut aluminum (which is why I generally don’t do it very often). And when I use cutting fluid, it doesn’t clean up as well but it helps the cuts tremendously.

@Ziggy

Also, please let me know if that clunking sound is normal. It is a bit worrisome.

I don’t believe that’s anything to worry about, it sounds pretty typical to me. The cutter is always under a certain amount of preload when cutting, and that sound may just be the cutter ‘settling in’ to it’s new temporary stopping point.

@Ziggy

and using a downcut bit

Downcut bits may be great for wood, but in general, they create more cutting pressure on the workpiece. I think surface finish will suffer and the additional cutting pressure/heat may tend to warp the part. Your mileage may vary on the downcut bit though, as I learned as a machinist that brass doesn’t always play by the same machining rules as other metals.

[Ziggy]

Thanks for all the replies!

It is really appreciated. Especially the advice about the downcut and the tool paths.

These are all thru cuts on 20 gauge brass. Basically this project is just a “first pancake.” I am using it to learn.

[Arzt (David)]

My first efforts with brass caused brass dust to enter the spindle (had to rebuild the bearings after a few workpieces). I’ve since added an air port and continuous air (“purge air”) to prevent that.

Extremely small (single flute) cutters seemed like ways to get fine detail, but 0.01 and 0.005 tips broke. Amana’s engineers said tips that fine require speeds and feeds that my spindle can’t do. (Speeds like 60k and feeds of 1-2 IPM).

So I went to a “Maker’s Space” At a local college, and picked up some ideas. First, I abandoned those extreme tips, going to 60 degree 2-flute V-bits but only for clean up, A 1/8” straight mill hogs out most material.

The most important (and, in retrospect obvious) tips concerned the hold-down. For a clock dial, the engraving has to be equally deep at 12 as it is at 6 (etc). That requires me to mill a flat surface on the spoilboard just before securing the workpiece. The spoilboard has to accept screws, tolerate milling, and tolerate oils without swelling. It’s also good to be able to use several times. That introduced me to Delrin. That’s a brand name of acetal resin plastic. The Delrin brand is ridiculously expensive, and has some properties we don’t need, so I buy generic acetal plastic from McMaster-Carr. I can tap threads in it to accept plastic screws, and secure a brass sheet to it. The acetal sheet itself is secured to my main spoilboard with countersunk holes (beneath my brass). A final leveling is performed just before securing the brass.

I’m still searching for brass sheets in alloys of 360 or 353, which are supposed to be the most machineable (they contain some lead).

[AndyP (Badger)]

Great notes, thank you

[Ziggy]

Thanks so much! I actually looked for Delrin and also found it expensive.

I started to just go to Big Lots and buy some cheap plastic cutting boards.

–

Is your spindle air cooled? I am curious how the chips got inside.

[Arzt (David)]

No, my spindle is water-cooled (Mechatron). When cutting anything, if I look closely, I’ll find dust everywhere (wood, MDF, brass, etc). So the brass dust is more destructive than the others, but who needs any of them in our spindles? The dust was entering through ventilation holes that exist around the collet, even without a specific air flow to favor that direction. Purge air is a specific flow against that direction.

Though it was new to me, the company said they would have recommended that feature if they’d known of my intention at the initial purchase. It requires a flow of 100 l/min, which is about 3 cubic feet per minute (CFM). So it required a compressor that can deliver 3x that, at a pressure of 90 psi.

Why 3x? because the compressor will fail if it has to work for long periods without resting 2 minutes for every 1 minute of action. My (DeWalt) compressor pushes 14 CFM at 90 psi. Be careful of sneaky claims about the CFM Some sellers claim they produce amazing volumes, but they don’t tell you that the force behind that massive flow is 10-15 psi. Once you connect anything to a compressor, the resistance becomes a factor.

[whiskey]

Check out Winston Moy on YouTube. YouTube.

He does a lot of projects in brass and aluminum. He uses the shapeoko, but the principles transfer over to the onefinity as well.

[Ziggy]

Thank you! I watched the video you linked. I’ll catch more later.

I did some experimenting over the weekend and I had some success and a bit of failure.

I managed to break 3 bits but luckily they were cheap bits.

The first thing I changed is that I printed my “waste board” with solid infill. Then I also printed small sides so it looked like a very short box with no top.

After gluing my brass to the waste plate, I mounted it as normal. Then I squirted a little bit of water based cutting fluid in the “waste box” and then filled the rest with water. Essentially my brass was now submerged.

This worked wonderfully and there was no problem with chips going everywhere.

However it was still a bit of a failure.

No matter what I did the small parts would not stay stuck to the waste plate once the bit made it through. The parts would inevitably come unstuck as the bit was making the final passes breaking through the other side.

I was completely coating the brass piece in CA glue and then clamping it for 24 hours. (I even tried Hide glue but that didn’t work either. The reason for the CA or the Hide is that they are soluble in acetone and water respectively.)

So… after ruining three bits and a bit of Amazon brass, I finally relented and added tabs. This worked fine.

–

One possible problem is that I was using a single flute down-cut bit. As pointed out earlier in this thread a downcut may not work well. The downcut bits seemed to cause impacts as they cut (vibration) that I think were what was breaking the CA bond. I didn’t have any 1/16" upcuts to try. (Some on order now.) I tried keeping a reasonable chip load but ended up raising the RPM and lowering the feed in a effort to not be as “jerky.” I also reduced my depth of cut to .002 and had a ramp angle of about 15 degrees.

Now that I think about it, I am not sure if the CA failure was the bond to the brass or the PETG / PLA. (I tried both.) I may go dig a few failures out of the trash to see. Hmmm.

I do not know how double-sided tape would work under water. The stuff that I have is strong but gummy and fouls the bit. I just bought some other thinner stuff but it doesn’t seem to have much holding power.

Part of me now is thinking that if I want to retain the water bath I might just print thicker waste boards and then screw the parts down while keeping the tabs. That said, I don’t know how the water bath would work with a upcut bit. It sure was nice to just be able to dump the chips rather than worry about them getting into my lead screws. Plus, my cheap bit cut like a dream.

More experimenting to come.

Thanks for all the replies.

[Ziggy]

Cutting Copper and Brass Sheets - #MaterialMonday

This was helpful. Maybe I should go back and see what kind of brass I bought.

Also, that wax sounds interesting.