Questions on using a moving gantry style mini-mill...

[Davek0974]

Yep, already on that ;)

I just revisited the original plans for the part with the notch in it and it appears it's non-critical so I have altered it from 4mm wide and square to 5.1mm wide and half-round so the roughing tool will rip out most of it and I can try the 2.5mm DOC on the finish pass again - the 0.6mm cuts were where most of the time was eaten.

While it was running today I was also making other stuff so the time taken is not critical to a tight degree, once I get going I can finish one set of parts while the next is running - there are holes to drill and tap etc. Demand is not massive for these but crucially it means I don't have to send them out for laser cutting anymore.

I can also move another part I make from the plasma cutter to the mill as the quality is higher and finishing/clean-up time would be far less as plasma leaves a very rough edge on aluminium.

Just need to sort out a better bucket for the cooling water, possibly some sort chip management, and some better cutting fluid.

I might also try some low-speed tests just to see how low she can go.

[lucan07]

As regards your enclosure I don't use an enclosure as such but have screens in Acrylic for certain jobs to control chip/coolant ejection etc, very easy to cut and weld together using Dichloromethane.

I should mention got a great deal on load of 5mm acrylic, less than 30p a square ft.

[JAZZCNC]

I can also move another part I make from the plasma cutter to the mill as the quality is higher and finishing/clean-up time would be far less as plasma leaves a very rough edge on aluminium.

I would combine them and let the Plasma rough them out and finish them with the router using full depth finish pass. May need a Jig if cutting lots but will be worth the time to make in long run.

What's Max thickness Ali can you cut with plasma.?

[Davek0974]

Hi Jazz,

Can't combine, one is 5mm and the other is 3mm plus the bed is too small to take both parts ;)

The parts i have been getting working in this thread were never plasma'd - too much detail and the heat would warp them, laser cutting does distort but not as much, costs though - that's why I wanted to bring them in-house.

I could pre-cut the 3mm parts on the plasma, would save metal as i can only order square-cut sheet or blanks and these parts are triangular. Would then need to be a two-step fixing on the mill - fix through the internal aperture wastage and cut the outside then fix clamps and finish the internal details. Would still work though, these are simpler parts to make.

I can plasma 9.5mm if it needs piercing or 19mm if I can edge-start the cut. It's not the favourite flavour of metal for plasma cutting though.

[JAZZCNC]

I can plasma 9.5mm if it needs piercing or 19mm if I can edge-start the cut. It's not the favourite flavour of metal for plasma cutting though.

What kind of feedrates would you cut 19mm Ali with.? Is this using 45A plasma.?

[Boyan Silyavski]

This is Kyocera carbide micro bits feed and speed chart. They are definitely one of the sharpest and overall best bits around. So if you are using inferior -30% at least on all data.

Vc - cutting speed
f - chip load or feed per tooth
Fr- feed rate mm/min
D- diameter of carbide bit
U- number of teeth on cutter
p=3.14


Ae - side removal
Ap - face removal


1.
determine spindle speed rpm/min depending an operation/roughing, slotting, finishing/


RPM=(Vc*1000)/(p*D)
so
RPM=(150*1000)/(3.14*2)=~24k RPM, so you are spot on here




2.


Calculate feed rate mm/min:


Fr=f*U*RPM
so
Fr =0.024*2*24000=1152mm/min for slotting

=0.002*2*24000=96mm/min for finishing


That all on a mill with very good cooling and chip removal. Diameter depth and 30% tool engagement

So if you play with the second formula you could easily see why you can no make a nice finishing pass. cause for 800mm/min feed you will need to have the spindle at 8000rpm, not 24000.

Now lower some percent that you ar not cutting on a mill with jet cooling the bit...

And bear in mind that the first speed calc is most probably for roughing bit, because that's how typically is done, that's why seems so fast.

From my experience there is no big science here, i have tested cuts on various machines and the only thing that really differs is the depth of cut that could be achieved with a particular machine.

[Davek0974]

Thanks Boyan, all I do is plug the manufacturers cutter specs into HSM Advisor, set the cut details and move the feed rate to 30%.

I was not feeding at 800mm/min, don't forget my tools are only single flute.

The cut is a tricky one though as the corners are more like slotting and the rest is plain finishing so a mix of heavy and light cuts.

[Davek0974]

If my understanding is better, after a good chat with the guy that supports HSM Advisor, it seems I might be a bit over zealous with the settings?

Plugging numbers again, I get for the 2mm tool, 18,500 rpm, 1,200 mm/min feed, 0.5mm DOC and 0.065mm/t chip load.

Reasoning - the limiting factors are the larger rads in the sharpened corners - this becomes slotting - also the manufacturers chip load limit of 0.065mm/t was set to not be exceeded, that gave DOC as 0.506mm as part of a balanced result to meet those factors.

So my earlier run was 0.6mm - too deep, 23,000rpm - to fast, 450mm/min - too slow. It survived but took a long time and gave poor surface finish.

The tool cannot give a 2.5mm DOC with any setting due to the slotting factor - the tool exceeds 100% torque limits = snapping - this backs up what really happened when i tried it.

So it seems lighter, faster is a way forwards, might risk a tool and try it I think. Its more passes but travelling at 3 x the speed so should still be quicker.