When cutting aluminum with out coolant what should a feeds and speeds be and the step down be? Im trying to cut contour and have already broken several bits. Using fusion 360 to program my tool paths usong 2d contour. using a 0 flute spetool 1/8 an also a 1/4. Look on the spetool website and there description is confusing to me.
1st question - what alloy? They are not all machineable. I use 6082T6 or 6061T6. On a workbee with V-wheels I used 10~13 K rpm, 3 mm single flute spiral upcut, 0.5 mm doc, 500 ~1000 mm/min. After upgrading to linear rails I doubled the doc and feedrate, and could probably go faster on the feedrate. Alex. PS, I do usually use air from a collet mounted fan for cooling - helps with chip clearance as well.
The T6 bit means it has been tempered to make it more machineable, but you shouldn't have much trouble with 6061. Are you seeing any signs of the aluminum welding itself to the bit? Profile (contour) is one of the more difficult toolpaths because you are basically cutting a slot, and keeping the cut area clear of chips is essential. Alex.
No the bit seems clean but my slot seems to be holding the chips. I been cutting at 12in/ mum and .121in in doc. I'm going to assume now after reading your comments I'm cutting way to deep and speeds can be adjusted to
For the 1/8" single flute, the numbers Alex gave of 10krpm, 500mm/min ( 20inch/min) and 0.5mm DOC (0.02 inch) are a good place to start, increasing cut depth if all goes ok. How deep are you trying to cut the slot? With a stick-out of 22mm (0.87"), cutting any deeper than 1mm at a time will head into >1% bit deflection. If you have a shorter stick-out, then it would be safe to go deeper each pass, but if the tool is longer, then the depth of cut needs to be more conservative. For a 1/4", 10krpm, 1000mm/min (40 inch/min) and 1mm DOC (0.04") to start should work, and you should be able to push the DOC up to 3mm, possibly 4mm depending on your router/spindle power (and machine rigidity). For the 1/4", bit deflection is not the problem, the issue will be maxing out the power of your router/spindle if you try and cut too deep in one pass. For both the 1/8" and 1/4", going to higher rpm (and also increasing the feed-rate by the same fraction) will give a better surface speed and is likely to give a better finish, *BUT* getting the chips out becomes much harder at the higher material removal rates. I use a compressed air blast directed as close as I can to the cutter tip to clear the chips, but with deep slots, sometimes it is best to pause the machine after a few passes, and use compressed air and a vac to clear the slots out before going deeper.
I'm going a total of 1/2 deep. I definitely need to raise my tool as it cutting way to deep now. I'm going to be printing me up some line locs to add to my machine so I can have compressed add blowing on it to cool and remove chips. Thank you for the help
Yes 1/2" deep is getting tricky to clear the debris out of the slot with an 1/8" bit. I have slotted a fair bit of 15mm thick (0.6") plate with 1/8" bit and it was a right pain! Although the 1/8" bit wastes the least material, if you can do the cut-outs with the 1/4", that would make life much simpler. As you are using Fusion 360, it may be worth considering a trochoidal toolpath for the slots (I think it is Adaptive Clearing in Fusion; I am not a Fusion user though). The trochoidal toolpath makes many small circle paths of light cuts and makes a slot wider than the bit, but does allow you to cut deeper each pass, so the overall cut rate is quite fast still. The really big advantage though is the slot that is cut is wider than the tool and makes clearing the debris out much easier.
I just ordered some 1/4 bits and was thinking about using adaptive clearing. I'll be changing everything over once I have free time. Would the same feed rate and speed apply to so profiles and boring of holes?
With a feed rate of 1000mm/minute for a 1/4" bit (and 10krpm), I usually use a Z plunge rate of 200mm/minute, but it does depend on what the particular bit (and machine Z-axis) can handle. If you can, it is best to ramp into cuts. For holes, where possible I use a helical tool path with a bit that is a smaller diameter than the hole, rather than trying to just plunge in as with a drill. With an adaptive clearing tool path, the radial width of cut is usually much lower than for slotting, so the effective chip-load may well be lower due to radial chip thinning. To get the chip-load back up and therefore the heat-clearing capacity, the feed rate needs to increase. If the bit is small and the tool path does lots of very small circles, the tricky balance is then finding a feed-rate that the machine can actually reach, given that machine acceleration is finite. For a 1/4" bit, there should be less of a problem and running at a radial cut width of 2mm will only mean about a 10% increase in feed rate is needed to restore the chipload seen with slotting (i.e. 1100mm/min, but 1000mm/min would still be fine in practice). You should be able to cut at a depth of around 6mm with a 2mm radial cut, but need to be careful with the tool path that the bit does not engage deeper on corners etc. For a 1mm radial cut width, then a feed rate of 1400mm/min would be better and in theory should be able to do the full 1/2" depth if you have a router something like the RoutER11, but it would be worth trying some more cautious test cuts first! With a 0.5mm radial cut width at the full 1/2" depth, the feed needs to be more like 1800mm/minute.
