Hi,
the tool rotates in one direction, the vast majority are Right Hand.

As to the direction around the perimeter that you traverse the cut is the difference between 'conventional
milling' and 'climb milling'. With older mills which have backlash you must use conventional milling only whereas
CNC mills with no backlash can use either. For various reasons climb milling is preferred IF your mill has the rigidity
and ZERO backlash.

Most CAM programs allow you to chose either conventional or climb milling toolpaths.

There is plenty on the net about climb/conventional milling.

Craig

Could you explain what backlash is? I've found some information on the internet, but I'm not sure I understand it completely.

How would I know if my machine has a backlash system?

Hi,
on a conventional lathe or a mill with ordinary hand wheels if you wind the wheel clockwise the axis
will move to the right, say. If you now wind the wheel counter-clockwise there will be a small zone
where the axis does not move until the 'backlash' is taken up and then starts to move to the left.
If you like backlash is the slack in the thread of the leadscrew. Just about all conventional machines
have it, more as they wear.

Modern CNC machines with preloaded ballscrews can be called zero-backlash, although an engineer might question
your definition, and as such have no measurable slack between the axis moving right  or left. Such machines
often use 'climb milling' toolpaths.

Craig

Ok, I think I have that figured out on my machine.

After a few cuts I noticed that I am getting a pretty thick bur on the edges of my cuts (1/16"), I used a baseline feedrate/rpm calc sheet to start, but being that the material I am using is somewhat unique I'm not sure what to be using.

Currently, I have my IPM = 45 and RPM = 21,000 - The material I am cutting is a mix of an  aluminum backer (0.013" THK), corrugated polypropylene plastic 0.2" THK), and an aluminum face (0.031" THK). I am using convention milling as well.

I did a mixed calc with Gwizard, and it gave me 23,000 RPM @ 34 IPM for both the backer and face aluminum, and 24,000 @ 121 IPM for the plastic core. Is it switching feedrates and rpms logical for this situation?

Hi,
unless you can be sure that the only cutting that will be done in any pass is the plastic core then keep the speed the same.
If for instance you up the speed but part way through the pass the tool engages with some of the aluminum. either top or
bottom, the tool will break.

If I understand the way you have proposed your question you are doing multiple passes to cut through the composite.
That will mean that only the very tip of the tool will be doing the cutting. When the tip of the tool is blunt it will have
to be replaced but the rest of it is perfect.

May I suggest trying to cut through the entire thing in one pass. The two layers of aluminum constitute a thickness of only 1/16 and
the plastic core is that soft it doesn't really matter. You'll have to cut more slowly, probably very slowly to start until you get a feel for what
can be achieved but even at only 15ipm would still be the same total time as three passes at 45ipm. At least this way you would see that more of the
tool is engaged and cutting.

Craig

Hi,
I came across this when I was making my mill.

I went to the scrap yard and got some big cast iron weights that had been used in a lift. It was a cheap source of big cast iron lumps.
What I did not know was that the cast iron was pretty rubbishy, I mean all they have to be is heavy, they don't have to be that good.

When I started milling them in the Bridgeport at work I found that the iron had quite a few inclusions which were very hard on the HSS tools
I was using. In my inexperience I tried to take light and shallow cuts to make the tools last. That was a mistake, it means that the tip of the
tool does all the work and the flanks of the tool do nothing. Re-spharpening is possible but as I was paying a company to do it it was dubious that
I was saving any money.

I found instead the best way to proceed was to take deep cuts, 1/2 to 3/4 inch deep but only 20-50 thousandths laterally. The old mill has HEAPS
of backlash, nearly 0.2 inch, the yoke must just about be worn right through, and so after my one mistake, I had to use conventional milling
sometimes called down milling. At least when the tool was worn out I'd got the best out of it.

If you are unsure about climb/conventional milling get yourself to the controls of an old Bridgeport with plenty of backlash. Put in a 1/2 endmill and some
steel in the vice and try climb milling. Make sure you are wearing a face shield!. When the mill 'climbs' into the cutzone and shatters the tool and/or dislodges
the steel in the vice you will understand the difference and what that can mean. You can read 100 books or look at 10 videos but 5 minutes at the controls
of a mill will teach in a manner that you'll never forget!

Craig

Worth noting that if you're cutting grotty metal like odd castings and steel with mill scale on it, conventional milling saves the edges of the bit to an extent. if the cut starts in the meaty bit of the metal it doesn't impact on the scale or the casting's crusty shell. Climb milling has the teeth of the bit cutting through the nasty bits every time and it fouls it up quite fast.

@joe Chinese steel has this sometimes including structural sections, big pockets of carbon or slag, horrible stuff.

at 21000rpm @ 13 IPM, with 0.17" per pass and its cutting like a charm, thanks for the advice.

What's a good indication that a bit is dull or bad?

Hi,
first indication is cut quality, followed by built-up-edge, followed by breakage.
The last two occur within seconds.

Craig

Hi,
the real killer for aluminum cutting tools is heat.....and I don't mean necessarily heat of the tool or workpiece. Its more about
the heat of the chips.

There are some excellent videos on you-tube about chip formation, every mechanical engineer has to be intimately familiar with this process
AND the calculations that result. I'm only very fair with the calculations myself.

Amongst the objectives of forming a chip is to have the energy of the shearing work to enter the chip rather than the workpiece or the tool. You'd
say that the chip is 'hot'. You will of course have seen 'blue' hot steel chips forming when drilling steel. The same thing happens with aluminum but
without the change in color. Also the melting point of aluminum is only about 780 C whereas steel is about 1480 C.

If by a combination of heat and pressure aluminum chips adhere to the edge of the tool the energy (heat) required for the now blunt tool, by virtue
of the rounded built up edge, to create fresh chips increases dramatically. This results in now very very hot aluminum chips and will have a great propensity
to stick to the already built up edge. Breakage is now imminent.

It is a similar line of reasoning that recutting chips must be avoided. When an aluminum chip is formed it gets hot, lets say 400C. Should that same chip
get recut by the next flute it will get hotter again....lets say 700 C. At that elevated temperature the likelihood of it sticking to the tool goes up hugely.
Thus if you use means like flood cooling or air to remove the chip from the cutzone, it will still get hot, 400 C, air or coolant doesn't change the physics
of chip formation, but air/flood will prevent the chip from getting recut. If you haven't given some thought to trying flood cooling, think again, and if you
decide you can't do it, think a third time until you do it.

Flood coolant or air will have significance for tool life. Lets say that a new and sharp tool will produce chips of 300 C at normal cutting parameters. As the tool
wears and becomes less sharp the temperature of the chips will go up, lets say to 500 C, at which point they adhere to the tool and that tool is now worn out.
If you have flood cooling or compressed air in operation you may be able to cool the chips to the extent that they do not adhere and can carry on using the tool,
extending its life.

I use very small (0.5mm) and tender two flute carbide endmills to cut a thick (0.42mm) copper layer on a circuit board. Without flood cooling I get about 1/2 hour
life for a tool with decreasing cut quality, burrs etc. WITH flood cooling I get about 10 hours, and MUCH BETTER cut quality.
I have had similar experience in aluminum. At 500m/min surface speed my 3mm two flute endmills will last a few minutes before BUE (built up edge) and
subsequent breakage. WITH flood cooling the same endmills last for hours and NO BUE!!

I know a lot of highly authoritative sources say don't use coolant on aluminum but I have found an immense increase in performance if I do.

Craig