I have checked my spindle and it seems fine. Looking for some guidance on getting these made with decent reliability.
I would like to know others success and endmills that work as it seems single flute endmills are not that common.
Hopefully I given enough information to get me going.
With a 1/32" 2-flute, that video from Winston’s MaterialMonday series recommends 10k RPM at 6ipm, DOC 0.006"
So you are in the right ballpark for feeds and speeds.
What workholding method are you using ? for thin material like that you need to hold the whole surface underneath the stock, you could possibly be getting vibration of the stock otherwise (leading to tool breakage)
Have you tried a small air blast to remove chips from the cut ? It should not matter much at this low depth of cut, but recutting chips is never good, and I suppose you are doing slotting (profile) cuts so it is still possible that chips pack in the slot
Hello, thanks for the reply. I use masking tape and instant gorilla glue.
My problem could be a bad batch of endmills. I have carbide 3D cutters arriving today, so we will see how that goes. I have used the included chip fan and I have a compressor that I blow the chips out with.
Can you recommend any other endmills, just that I’m in Canada and the way things are they are taking a month to arrive.
Also is it worth getting fusion 360 for adaptive cutting?
One more idea to double-check: did you surface your wasteboard or do you see any uneven depths when cutting the first pass? If the wasteboard surface is not quite aligned with the machine’s XY plane, you may get subtle variations in cutting depths from one spot to the next, which could mean larger depth of cut than programmed (and eventually tool breakage if the actual depth of cut is much larger than it should be). This is a long shot, and most probably not the case since you were taking very conservative passes already, but worth checking in any case.
I’m on the other side of the pond so I have no tips, hopefully some of our Canadian members will chime in
Since the hobbyist license for F360 is (still) free, there is no harm in testing it. Adaptive clearing toolpaths are definitely a very interesting feature (not as a solution to your problem, but in general)
Do I understand right that you’re cutting out shapes? How big are they?
One thing that might help is to do multiple passes with different tools. You could do an initial cut with say a 1/8" or 1/16" endmill (which will also allow a much higher feed rate so save you a lot of time) then come back and finish small details the bigger endmills can’t reach with the tiny endmill.
This not only reduces distance cut but should also reduce plunges, which might be harsh on the tool.
I am cutting 2D shapes, simple flower petals. 2"x2"
C145 tellurium copper, no one carries it. Special order, but it sounds like bar stock only. Anyone have a source or is it go my another name, or something similar? I will try 1/16 ball nose to start then switch the the 1/32 flat and see how that works.
If the part is cosmetic, have you considered easier to machine and obtain alloys like brass? You could even consider coating the easier-to-machine material in a copper paint. If you really want, maybe you could copper-plate a piece made of another material.
I think because machining copper is kinda weird and specialised. A quick search shows options on eBay and Alibaba though.
No. C145 is more for industrial purposes. I got it from McMaster. If this is for jewelry stuff, or something that will be handled, I’d probably avoid the alloy for something more pure in case of any Tellurium leeching out. Generally, you’re just going to have to suck it up and use a less-optimal jewelry grade copper alloys.
Things to look out for:
If you f* up your speeds and feeds, you may end up annealing your material.
Look at your tool with a magnifying glass periodically to make sure they’re still sharp.
Also keep an eye out for if the edges of your cuts suddenly become infested with burrs. That’s usually a sign that things are less-than-optimal. Maybe you’re heating up the material, or your cutter got dull.
I like to use Harvey Tool’s charts as a reference (example: https://harveyperformance.widen.net/content/rptnkylsjh/pdf/SF_72000.pdf?u=1i9tm9 ). For a 1/32" endmill you should be targeting a chipload of about 0.0003". Start with a depth of cut of a couple thou, then increase as you gain confidence. For those small tools you should be at max RPM.
If there’s any dust lingering in the cuts at all, try to vacuum or brush it out between passes if you can safely do so. Otherwise, throw on the chip fan and pray.
