We use cookies to personalize content, interact with our analytics companies, advertising networks and cooperatives, and demographic companies, provide social media features, and to analyze our traffic. Our social media, advertising and analytics partners may combine it with other information that you’ve provided to them or that they’ve collected from your use of their services. Learn more.
My feed&speed chart for 2mm 1F says 410mm/min at Dewalt speed #3.
Chip thickness = 0.02mm per tooth (runout / tool deflection need to be accounted for as well)
Say you did aim for 410mm/min and 0.02mm per tooth, but the system flex a little, perhaps 0.2mm.
That allow the bit to “bounce” and real chip thickness will vary and most likely exceed the ideal thickness. Uneven cut is the result and greater chance for bit breaking. I have broken a few bits this way during my learning curve
Straight plunge I dont go faster than 150mm/min but that is with 3-6mm bits, I expect a smaller diameter bit to be less “bouncy”. Helical circles do cut faster but I dont have the speeds on hand. (
Cut do look a little rough, how did it sound during cutting?
I got that
The close-up of the round hole show an uneven circle which suggest some chatter/bouncing. 1F have a uneven load distribution since only one flute is in contact / let go / re-engage and if it is allowed to jump around it could look like that. (Over-aggressive cutting from the bit point of view)
The rectangle pockets, are they intended to be true rectangles or are the “dimples” to the left by design?
Do you know which type of alloy that angle is made from? I know that the stuff from Home Depot seems brittle and doesn’t mill nearly as nicely as 6061.
Plausible, if you have the time or desire- try cutting same circle 4 times, one for each feed rate.
50/40/30/20ipm. I would expect the quality of the cut to improve a fair bit with lower IPM.
If you have a good speed in which the bit is happy/vibration is low you will see even slices/chips.
A flat end mill will be much better carving alu vs ball mill because edge engagement is less. (talking material removal, not finish pass)
A 2mm end mill should easily take 2-3mm depth per pass with the proper width per cut (typically 40% of diameter) and feed rate. For pocketing this equal helical ramp until depth is reached.
Lubrication helps for sure, I only use a mister (air and alcohol) but dry is not a no-no either
With a good and consistent chip thickness (rigid) and an optimum width per cut you can go deep. Provided the rig si rigid enough depth is limited by removal rate. 1mm DoC => 2mm DoC => 2x removal rate etc. The added engagement is only higher on the vertical cutting edge.
It handle the calculus for determining the optimum feed & speeds for their 1F ProAlu range, but may apply to other similar end mills aswell.
What is relevant is the approx speed and feed rate, where speed is tip (rotating) velocity and feed rate is…feed rate.
Take the 2mm 1F you have as an example:
500m / min surface speed (rotation) => 80k RPM
Obviously the Dewalt won’t do that so let us use speed #3 => 20400 RPM
20400 RPM x 1F x Chip Thickness = feed rate
20400 RPM x 1F x 0.02 = 408mm/min
Note that the 0.02 figure also need to take into the account runout and tool deflection. A 2mm bit with a 8mm cutter length will deflect.
FWIW - this data sheet is not universal but can relate to other similar end mills. It is not “the rule” either, just an approximation on where to start.
With a good RPM/feed rate only the length of the cutter and and machine rigidity will limit the effective cut per depth allowed. Ultimately this is what will determine real MRR.
You are welcome, I am no guru though but travelled the same road you are embarking last year. Getting the understanding on how chip thickness / feed rate works / calculate really helped the cut quality.
To simplify the datasheet linked to earlier, simply choose your RPM, multiply with number of flutes and target chip thickness. This will be your feed rate. Small diameter tools => higher RPM typically.
Regarding lubrication, alu can handle dry runs quite well but cut quality / tool preservation will be better with lubrication/cooling. I use a simple eBay mister which run on low pressure air, and denatured alcohol is mixed into the air stream. The alcohol evaporate which provide some cooling of the material. You can also use a mix of water/alcohol as fluid as you have a metal base for yours. Mine is wood so I run alcohol only.
Mass producing belt tension brackets? Give them a run in a tumbler to get the edges down
It’s on mine.