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

[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.

[Davek0974]

RESULT !

Had a bit of time off work today so out in the shop :)

The new cut parameters seem to be perfect so far, the 5mm roughing cuts seem a bit off as i was seeing some chip-welding to the sides of the cut, this was at 2.5mmDOC an 1350mm/min @ 24000rpm, this was with coolant as well so its a bit wrong somewhere there, not sure if too much rpm, too much feed or something else, manuf states max rpm is 12000 so maybe i need to retune at that speed?

I made several alterations to the CAM and CAD by way of pre-finishing the sharp corners with the 2mm tool - this works great, then the final pass with the 2mm at 24000rpm 5mm DOC, 0.1mm WOC and 244mm/min feed spat out lovely little shards of swarf and not dust. Surface finish is now 100% quality.

The CAD/CAM changes also reduced my part time from 45mins+ to 20mins which is a considerable change, that includes tool change but not plate setting and bed clean-up.

Pictures later.