May 2, 2018 at 8:20 am #59258
1/8″ 2 flute down cut end mill cutting 6061 with air jet cooling. I’m figuring 25mm/sec with a .8mm to 1mm DOC at 20000 RPM. Am I about to screw up? Feed calculations say anywhere from 29 to 50 mm/sec but I have nevsay cut anything with my MPCNC at more than 30mm/sec no matter what depth. Anyone have numbers to share?May 2, 2018 at 9:15 am #59265
I would not use a down cutting bit with metal or plastic. The main thing is getting the chips out, that does the opposite.
Only go that way with thin sheet goods cutting all the way through into a spoil board to avoid the material lifting.May 2, 2018 at 12:16 pm #59277
My bad, it is an up-cut bit. I only use my down-cut bit with stringy wood. I never really thought about using it for thin stuff though, good call. Otherwise, do my parameters look ok? I’m thinking my main constraints are deflection from machine rigidity, and the feed rate where the machine doesn’t stall or lose resolution. I can cut 1/4″ lexan with no trouble at 30mm/sec and 1mm DOC at 20kRPMs using a single flute up cut bit.
I’m cutting some motor and idler mounts for a RailCoreZL 3D printer. I have got to give that new E3D tool changer setup a try and the RailCore (core xy) seems to be a great base for that. I could buy mounts from 713maker, but there’s no fun in that!May 2, 2018 at 12:22 pm #59280
Instead of moving so fast with your cuts you really should cut slower and deeper. I honestly can’t give much aluminum help, it is very machine sensitive, every machine will be different. Just do test cuts.
You are wasting money on bits with such shallow cuts, and you will gain accuracy with slower moves. All the issues happen with direction changes, the faster you do that the more the issue happens. 8-15mm/s is nice. Only go faster than 15mm/s if you are cutting full depth and you feel there is room for more speed.May 4, 2018 at 1:16 pm #59430
Well, I slowed down to 15 and went deeper, obviously didn’t slow down enough because I broke a bit in no time.
Slowed down to 10 and tried a chip buster and it was trying to gaul and the cut looked nasty. Tried to slow down the spindle and it began to bog, so I stopped.
Went to an alTin 1/8″ down cut 2 flute. Slowed down to 8mm/sec and and reduced my plunge speed to 4mm/sec switched to climb milling. Better, but not good enough, although I was re-cutting some of the lesser quality cuts made by the chip buster. Messed with speed and feed. Seems it likes a little faster speed…keeps the spindle from bogging…but that requires a faster feed or I see signs of melted chips…however faster feed starts to chatter. I’m zeroing in on a sweet spot and enjoying the ride.
I’m thinking a single flute will work better but I don’t have an alTin coated one. Maybe it is time to dip my toes into the trochoidal pool.
Time to place an order for sharp stuff!May 4, 2018 at 1:27 pm #59431
I’m thinking a single flute will work better but I don’t have an alTin coated one.
Single flute would be my suggestion, the coatings should not do anything at our light duty use case.
I would suggest starting with sample pockets using the peel pathing. Slot cutting is the worst case scenario, tricoidal helps but get some good pockets first so you understand how your machine deals with aluminum. A pocket using peel keeps the load to whatever your stepover is, a slot engages both sides of your bit, so at least twice the load. Avoid slotting whenever possible.
I can’t picture a burr breaker working very well. I have never used one and got them for the Carbon Fiber people. With aluminum you are just trying to take the largest bite your machine will allow and getting the chip out before you recut it. This takes all the heat with it and prevents work hardening.May 4, 2018 at 2:33 pm #59435
Tom, I have seen a couple of your posts over on the RailCore FB page. I too want to build that printer using the MPCNC. Hopefully start on that project later this year.
Have you looked at Kevin’s YT videos on cutting aluminum? Here was is last and his settings are in the description. He gets good results on his machine.May 12, 2018 at 2:18 pm #59879
Thanks for that video johnny. I’m having a great time building the printer and Tony helps so much. I’ve been wanting to tackle milling some aluminum for quite some time. I’m going to get the bed from 713maker.com, and possibly the idler carriers, but I’m determined to make my own motor mounts.May 14, 2018 at 8:20 am #59940
Broke 3 bits yesterday but I learned a few valuable lessons. #1 At the RPM that the DW660 turns, a single flute bit is mandatory….and so is an air jet. #2 Start with a new bit unless you are damn sure the used one is sharp. #3 Proof your gcode program before cutting with your only new single flute bit. That way you don’t break it when you fail to enter the correct z offset.
1 user thanked author for this post.May 14, 2018 at 8:34 am #59943
And I’d like to point out that Kevin’s settings would have worked very well had I not wrecked my machine with incorrect beginning z offsets. If we learn from failures, I’m gonna be a genius by the end of the week! Right now I’m pouting like a 2 year old. (So says wifey)May 14, 2018 at 11:27 am #59955
You will get there no doubt. If you haven’t yet, either build a speed control(rheostat) or buy one off amazon. They are cheap enough and work well enough until Ryan get his speed control figured out. Just search Router Speed Controller on Amazon, they are around $20 and get the job done. Its not a set and forget type thing but will let you make slight adjustments to your router speed mid cut.
1 user thanked author for this post.May 14, 2018 at 3:12 pm #59996
I’ve got the rheostat but I’m just guessing with it. I started following the thread on the PWM speed control and it seems promising.May 20, 2018 at 3:10 pm #60288
Well, No tools broken this weekend! First try on Friday night was a failure. Went sailing Saturday. Woke this morning and tore down the MPCNC. Tightened up ALL bearing-to-conduit bolts and made sure all conduit had to be pushed into each tri-bearing setup. Shortened my Z legs by 4cm reducing my Z from 80mm to 40mm. Re-thought my feeds and speeds and went to cutting. This time using conventional milling instead of climb milling. First attempt was the best yet but my pocket depth and feed rate was a little aggressive so I backed off 5% on feed and 10% on stepover and I finally produced a working part!
1 user thanked author for this post.May 20, 2018 at 3:43 pm #60291
Nice, looks pretty good.
I know it is frustrating that I don’t just have a set of numbers that just work but I am sure you see know how simple and easy wood is compared to metals. In metal every mm of size counts and a 5% speed change actually makes a difference. I am super pumped that you stuck with it and made it happen.May 20, 2018 at 4:39 pm #60296
I know it isn’t the prettiest thing, but it is dimensionally correct, which is just awesome. I have one more to make. I believe the biggest change came with the steps toward making the machine more rigid.
Do you usually use conventional or climb milling?May 20, 2018 at 5:02 pm #60297
Well, if you are slotting you are doing both. Try to avoid slotting…but usually we want to cut out our parts so slotting is a necessary evil as tricoidal can take a lot longer. You can try to maximize your tricoidal by take a much deeper cut/slot to minimize the cut time.
Climb should be a better cut on anything other than slotting. Make sure you are using a finishing pass, that should give you really great dimensional accuracy and pay attention to the chips on the roughing pass, you want them as large as possible.May 22, 2018 at 8:36 am #60365
Made two more yesterday and I have more aluminum on the way.
I use EstlCam so the choice of climbing or conventional is global per program. So to get a combination of both, I’m going to have to do 2 programs and either run them separately or figure out how to combine the gcode. No big deal.
I tried going deeper on my trochoidal cut slotted holes and got a slight dog bone shape. It was a new bit so that may have been the issue…any insight someone can share on that? I think I have my regular slotting settings good, so I may go away from trochoidal . Got some scraps from my screw ups (aka learning experiences ) to practice.May 22, 2018 at 8:43 am #60369
I am not saying conventional is better for slotting. Slotting is both no matter what you chose for the Gcode. I engages both sides of the tool, so it is slow and machines stressful. No need to make 2 different codes.
I tried going deeper on my trochoidal cut slotted holes and got a slight dog bone shape.
I am unclear what this means. Tricoidal is not really a slot any longer but just a, ummmm, for lack of a better term a long pocketing operation. It should be consistent for the length but it is a complicated cut and has a ton of customization settings. This might take awhile to get right. I am unclear about what or how it came out dog boned, but if your slots works don’t bother with tricoidal.
If you have a slot cutting fine use that 100%, make sure to also use a finishing pass and you should get really really good dims. Tricoidal is a different beast.
You must be logged in to reply to this topic.