I'm ready to give up on machining aluminum kinda.... maybe?

I moved it out of the way for the video and used the hand nozzle.

I have a whole dual air nozzle setup I posted elsewhere in the forum.

2 Likes

There are a couple screws holding it down as well.

1 Like

Hmm I have been running 24k rpm with a single flute. I’ve been slowly dialing it in. Pass depth is .35mm plunge feed is 13mm/min and 320mm. I’m uploading videos to YouTube right now I will post them when they are complete. I would just keep trying. Think of it as your light bulb. I can’t imagine you have reached 1000 tries yet. As daunting as that may sound.

On a positive note I’m pretty sure I could sharpen your single flutes for you if you have any that are not completely broken. These are before and afters

this is the manufacturers tip this is them all together

2 Likes

Ok, first, that’s pretty cool. I want to try. Second, I’m petty impressed you’re getting through any aluminum with those. I broke 6 in about 20 minutes and went back to the Kyocera.

1 Like

Yeah the edge cut tools I shy away from.

For this last one skip to 45sec

1 Like

These are all the same endmill. I’m not even using anything for evacuation just the air coming off the bit.

Also these are only 5$ a bit so cheap to learn on.

I have a bunch.

Well I managed to solve 2 of the 3 issues tonight by switching to my other spindle. I no longer get the chatter I was getting, and it doesn’t seem to break the bits anymore when it goes off the rails, just grinds to a halt.

That said, I still can’t cut a 2d contour deeper than 1/8th in, regardless of how many flutes I use, before it goes off the rails at some point. The thing about trochoidal tool path, is I can’t imagine how long that would take for 1/2in thick aluminum on something 12" x 33". I would imagine it would be measured in days assuming i could figure out how to even write the tool path for it

Think of it this way, for slotting (contour) you need to make multiple passes. For trichoidal (adaptive) you can possibly do full depth, or more realistically only two passes. The width does not need to be much larger than a contour either.

Worth a few test cuts.

Still feels like something is wrong. For the same sized machine with the same spindle as before (all things equal) the Primo should absolutely be better/faster. Has anything changed?

It’s better, but both the primo and the burly gave me the same issues with cutting 2d contours over 1/8th in deep. the biggest difference though, is I was cutting .14mm and now i’m cutting .25mm DOC.

I guess I will play with it some

Testing 2 flute 10k rpms 3mm dDOC adaptive for a center slot. So far so good, overall a bit slower but I can probably tweak that still.

3 Likes

How wide is your roughing pass on 2d? Going lower than the width of the endmill is thing to be a real challenge on chips evacuation. I’ve done ok with a second pass at half the diameter down to 0.23, but it was pretty hairy at anything less than that. It’s probably about as deep as I’d go with that. If you’re cutting deeper, I how you’re using more, maybe another full - width pass.

In fusion, no matter what I set the roughing pass width to, the 2nd pass is always like .25mm from the 1st. Which isn’t enough to help and I damage bits as a result

Can you show that panel? That doesn’t sound right at all. Do you have the roughing passes set to at least 2?sounds like it could just be doing one roughing pass, then the finish. At least, that same thing happened to me a lot at first until I figured it out.
On my 2d aluminum contouring, I prefer TWO roughing passes, and finish only at final depth (again, approx 1/4 inch aluminum…might want two lighter final passes for your 1/2 inch, depending on the load). For your depth, you might try 3 roughing passes at 1/2d stepover or two ~1d roughs. It makes sense to me that if I’m full slotting the first pass, a 90% pass should be easy, but I’m a chicken…hence the 1/2 stepover.

What am I missing?
I set it for 1 stepover max of 1.5mm and it puts a .25mm 2nd step over.

I add 2 roughing passes and the 2nd one follows my settings, but you can see the 1st one is still only .25mm


That’s not the first pass, it’s the last one. These work outside-in. The first picture shows a rough and a final, the second shows 2 roughs and a final.
The toolpath lines aren’t differentiated between rough /final, so they look the same. It’s you finish only at final depth, that last pass (0.25mm) will be lower than the rest. Benefit, you use all of the flute at once so it tends to look a little nicer, but it is a higher load, so you might want to use a couple passes or (what I usually do) repeat finishing pass to make sure that deflection didn’t mess with the dimensions.
You’re pretty much there now, i think, with this. It’s gonna help a lot with chip evacuation on contouring.

Didn’t want to clutter up the last post but this is worth considering…
More than 2 roughing passes, the Adaptive strategy starts to look more attractive imo. The time can be about the same, i think slightly longer with Adaptive. Maybe a lot longer now that travel moves have to be the same as cut moves unless you have a full version of fusion. So you take lighter cuts, but deeper. No full slotting makes it more reliable, deeper cuts means removing more metal with the upper part of the flutes for better tool life, and lighter cuts means you can push the speed up a wee bit more. But once you make those tweaks to the Adaptive path relative to the slot, you can compare the machine times. The trick is to create a sketch with an offset of your part (larger) and use that sketch to constrain your toolpath (in the second panel). Sometimes it makes sense to add 10 or fifteen minutes with the Adaptive if it means you don’t have to babysit the part got broken mills, or even if that first full-slot pass just makes you anxious.
I don’t see a bunch of inside corners, though, so as long as you don’t need more than 2 roughing passes, i wouldn’t even bother. But that’s me.

Right, so how do I tell it to make the final pass larger? 3 roughing passes takes a ton of time.

I’m trying adaptive, so far unsuccessfully. I tried 1mm DOC but its going to take 3 hours to cut my small 1in x 4" part. Considering the contour path takes 15min, I don’t find that acceptable. I can send my 12x33 out and have these laser cut and returned faster than i can cut them that way.

Maybe I should just design everything to be cut with 1/4" if I can?