Cutting aluminum - Share feeds and speeds

[louieatienza]

Ah, ok, so Fusion360's answer to this is their "adaptive" CAM ops. So I guess that's where you do the deeper (full depth?) thing with smaller stepovers like Louie was saying.

https://forums.autodesk.com/t5/compu...g/td-p/5860958

But playing with it, I can't get the helix entry to work (the setting is there, but it's still plunging).

There should be some setting for helix angle, or helix radius... I'm not sure as I do not use Fusion360. You might be able to do a helix down as a "drill op" then rest machine using "adaptive clearing" starting at the hole.

However, I should note that trochoidal milling is not really necessary for something like a slot (especially in aluminum), unless the material is very hard. For a slot, it would be better, and faster, to use a tool that's smaller than the slot width, and use an inside profile strategy spiraling down the slot's border. This way, except for the first pass which is shallow anyway, you avoid full engagement.

This idea also holds true for a narrow pocket such as the example above. Because of the many position moves, this would slow down the actual machining time. A better solution would be to create a rectangular "boundary" inside that pocket, no wider than 1.5D of the tool, cut down to the pocket depth with a inside profile strategy spiraling down, then rest-machine using high speed (adaptive clearing) toolpath. In this way, the tool will retain engagement a LOT longer, which means faster cut times since it does not have to "retract and restart."

[Kosh]

There should be some setting for helix angle, or helix radius... I'm not sure as I do not use Fusion360. You might be able to do a helix down as a "drill op" then rest machine using "adaptive clearing" starting at the hole.

yes, but that setting is not working. Searched F360 forms and found it is a known bug. There is a workaround (a stock boundary setting) which makes it functional. I have it working now.

So, sounds like your algorithm is "half and half" ... half of bit dia for DOC, and half of DOC for RDOC.

[louieatienza]

yes, but that setting is not working. Searched F360 forms and found it is a known bug. There is a workaround (a stock boundary setting) which makes it functional. I have it working now.

So, sounds like your algorithm is "half and half" ... half of bit dia for DOC, and half of DOC for RDOC.

For rDoC, it will depend on your spindle power/machine rigidity. I'd start at .125D (12.5%) and go from there. It actually doesn't matter if you have flex or backlash, as these are roughing strategies. So I guess it's half and quarter.

[louieatienza]

Here's a part I made recently for a friend. The slots are .065". I used an .0625" 2-flute endmill at 14ipm and .030" DoC. What I employed was a inside profile strategy, spiraling down to the cut-through depth (.0875"). Because the slot is slightly wider than the tool, I avoid full engagement. The trick is keeping the swarf out of the slot to avoid re-cutting. Flood would work great, but I'm not set up for it; rather I just keep at it with a brush, which also recoats the surface with my lubricant of choice, WD-40.

[louieatienza]

A link to my YouTube page, showing some of the "evolution" of my aluminum cutting techniques...

https://www.youtube.com/user/AtienzaLouie/videos

[Kosh]

Ok, I re-did my CAM ops in F360 to use 2D adaptive strategy and take Louie's approach. Here's a video of the simulation.

Aluminum CNC Controls Bulkhead CAM ops

[louieatienza]

Ok, I re-did my CAM ops in F360 to use 2D adaptive strategy and take Louie's approach. Here's a video of the simulation.

Aluminum CNC Controls Bulkhead CAM ops

That looks pretty cool... I would do all the drilling ops first. Then you can use screws to hold the part down before doing the other ops; makes for a tighter setup. Also eliminates the need to create tabs. I even drill holes on the drop-offs and screw them down as well, which avoids having it move and fouling things up.

edit: Nix that... Though I'd do that profile cutout last. Once all your through holes are milled out, you can use those holes to hold the part down, either with flange screws or with strips of scrap material bridging the holes. Also for the stepped or counterbored holes, if you're using the same tool, it's probably faster to do each hole first, complete, then move to the next. Moving at each Z level is usually only done with very thin walls between pockets where milling individually would cause warpage.

[FoxCNC1]

it is indeed. So I have a question because I personally dislike using tabs. What is the best way hold down a part that doesn't have holes we can use to screw into?

[louieatienza]

it is indeed. So I have a question because I personally dislike using tabs. What is the best way hold down a part that doesn't have holes we can use to screw into?

You can't! Unless you make a vacuum fixture. But the way I do it would be to mill every other feature, and save the profile cut out for last. Use a larger diameter tool, and profile down, leaving on the side and bottom. With a 1/4" endmill, I'd leave .01" on the side and about .020" on the bottom. The part will still be held strong. Then, using a 1/8" endmill, do a finish profile pass, cutting through that .020" you left on the roughing pass. I machine a lot of Mic-6, and I leave the plastic film on the bottom of the part, and if my setup is accurate, I can cut down and actually leave the plastic film to hold the part! In the cases where I have to leave tabs, I make them as thin as possible, and use a chisel to pop the part out. If the part is flat, it's easy to trim those parts flush with a router and a piloted bit.

But if your part is relatively large, you can cut it as I described, and since the 1/8" endmill is very small compared to the part, the part usually doesn't move as it completes the cutout. If you're doing it on a mill, then you may have to dream up a fixture so you can flip the part over and clamp it down somehow, and accurately locate the part. Or you can use slightly thicker material and face-mill the back to remove the part. Or fixture the part that it drops down on the cutout pass (I normally don't like this because it leaves the part unsupported). I've even used spray adhesive with good results (3M #77)

If they're of no consequence, I try to engineer holes in most my parts that I can fix them down.

[ColletandBit]

it is indeed. So I have a question because I personally dislike using tabs. What is the best way hold down a part that doesn't have holes we can use to screw into?

You can always go the double sided tape route... if you're brave enough.

I've always wondered if superglue would work (a la Clickspring videos). https://twitter.com/clickspring1/sta...212928?lang=en

[louieatienza]

You can always go the double sided tape route... if you're brave enough.

I've always wondered if superglue would work (a la Clickspring videos). https://twitter.com/clickspring1/sta...212928?lang=en

Use super glue on a substrate mainly for thin sheet aluminum, works for stacked thin sheet. Soaking in acetone or lacquer thinner releases it.

[Kosh]

You can always go the double sided tape route... if you're brave enough.

I've always wondered if superglue would work (a la Clickspring videos). https://twitter.com/clickspring1/sta...212928?lang=en

I think I'll just screw my stock down in the corners, there is enough room and stick with the tabs. Because I'll be "chamfering" all the hole edges as well, it'll be easier. Point taken on
making the tabs thinner.

Now, I have used superglue to hold down shell when CNCing it for inlays. It works really well. The issue is getting it off. I've used acetone as a bath to remove it, but what I've found
is that only the small surfaced areas (which is fortunately the actual inlays themselves) will release easily. Ie, the acetone will only penetrate so far. Perhaps if you left it overnight it would
work better, but that stuff tends to evaporate as well.

What I have found works well with shell is just PVA glue. I used that to attach to hardboard blanks, and then I just put them in a bowl of water and boiled it in the microwave, they came off easily.

But that won't work for alum for multiple reasons...

oh, another technique I heard about, maybe this would work. Superglue the alum to a sheet of 1/4" hardboard, then after machining, flip it upside down and run it through a drum sander until the hardboard is gone.

Will have to check out the click spring stuff.

[ColletandBit]

I think I'll just screw my stock down in the corners, there is enough room and stick with the tabs. Because I'll be "chamfering" all the hole edges as well, it'll be easier. Point taken on
making the tabs thinner.

Now, I have used superglue to hold down shell when CNCing it for inlays. It works really well. The issue is getting it off. I've used acetone as a bath to remove it, but what I've found
is that only the small surfaced areas (which is fortunately the actual inlays themselves) will release easily. Ie, the acetone will only penetrate so far. Perhaps if you left it overnight it would
work better, but that stuff tends to evaporate as well.

What I have found works well with shell is just PVA glue. I used that to attach to hardboard blanks, and then I just put them in a bowl of water and boiled it in the microwave, they came off easily.

But that won't work for alum for multiple reasons...

oh, another technique I heard about, maybe this would work. Superglue the alum to a sheet of 1/4" hardboard, then after machining, flip it upside down and run it through a drum sander until the hardboard is gone.

Will have to check out the click spring stuff.

I think he uses heat to break the superglue bond

[dgage]

I think in the video ColletandBit shared yesterday, the guy mentioned using 5-min epoxy, which he then used heat to break the bond fairly easily.

[Kosh]

OK all, I did a "proof-of-concept" run yesterday in 1/4" MDF using the same o-flute bits that I'll be using the aluminum. Turned out pretty good! Just a few adjustments to make for fit.

A couple questions for ya'll:

1) for the lip around the edge and the counter cut, it's just cutting like a regular wood. Ie, goes to depth (1/2 of bit diameter), and the plows through. Should
I be slowing down the feed rate on that one?

2) for the 1/8" holes, I just have it tap drilling with the 1/8" o-flute bit. I've seen others do a "spot drill" operation first with a v-bit to define the point before using
drill bits, is that necessary in this situation?

Thanks!

[ger21]

OK all, I did a "proof-of-concept" run yesterday in 1/4" MDF using the same o-flute bits that I'll be using the aluminum.

Rule #1:
NEVER cut MDF with a bit you'll be using for aluminum. The MDF will dull the bit much faster than aluminum will, so you'll already be starting with a dull bit.
For best tool life, keep your bits separated based on material they'll be cutting. You should have separate bits for wood, MDF, plastics, and aluminum.
If you use a tool for plastic or aluminum that's been previously used with MDF, your finish will not be as good as if you cut aluminum only.

[Kosh]

Rule #1:
NEVER cut MDF with a bit you'll be using for aluminum. The MDF will dull the bit much faster than aluminum will, so you'll already be starting with a dull bit.
For best tool life, keep your bits separated based on material they'll be cutting. You should have separate bits for wood, MDF, plastics, and aluminum.
If you use a tool for plastic or aluminum that's been previously used with MDF, your finish will not be as good as if you cut aluminum only.

Understood, and I usually do that, just wanted to make sure they were same bits for this small project.

[FoxCNC1]

^ great advice as always Ger

[Kosh]

OK, so last night and tonight I finally got around to making that bulkhead out of aluminum. I just received my pro linear motion upgrade from CNCRP, and I have to bust the machine down now and rebuild it. I figured this was a good time to get WD-40 all over the spoil board as I'll making a new one once I rebuild it.

I basically followed Louie's guidelines and it cut very well. I actually stopped it after about 3 hours worrying the bit was getting hot, and was pretty much cold to the touch. Seemed to have a good chip load too. However, close ups of the cut quality at the end here, would be interested in feedback on whether they are smooth enough and how to fix if they aren't. The chamfer seems a little rough too... moving too fast? (445 mm/min).

Overall, it came out well, esp for my first time in alum! No broken bits!

[louieatienza]

OK, so last night and tonight I finally got around to making that bulkhead out of aluminum. I just received my pro linear motion upgrade from CNCRP, and I have to bust the machine down now and rebuild it. I figured this was a good time to get WD-40 all over the spoil board as I'll making a new one once I rebuild it.

I basically followed Louie's guidelines and it cut very well. I actually stopped it after about 3 hours worrying the bit was getting hot, and was pretty much cold to the touch. Seemed to have a good chip load too. However, close ups of the cut quality at the end here, would be interested in feedback on whether they are smooth enough and how to fix if they aren't. The chamfer seems a little rough too... moving too fast? (445 mm/min).

Overall, it came out well, esp for my first time in alum! No broken bits!

I think that came out pretty good for your first part! As to the edge finish, could be a number of things... maybe a tad too fast for your finish pass, slightly too slow spindle speed for finish pass, workpiece possibly could be more secure, looseness or flex somewhere, tool runout... biggest thing though in my opinion is tool stick out. The closer the collet is to the work without interfering is best. Use stub endmills whenever possible.