Had a go using motorcalc sheet but does not look right.

[irving2008]

Clearly the value for G0 is different than that for G1.... what value do you have for G1?

Maybe I should make the spreadsheet deal with different speeds and accelerations for G0 and G1 and estimate the motor power based on which is worst case... As stated the value of 0.02 will produce an overestimate on the motor size for large routers or table-based machines but isn't too bad on a small lighter machines

[Robin Hewitt]

Clearly the value for G0 is different than that for G1.... what value do you have for G1?

Now there's a question! I'd just wired up the new drivers and ran the last job on the computer for a look see. The X axis is in reverse.

Probably 1.5 mm/s, I usually cut between 1-2 but I might drop to 0.8 for a plunge.

When the cutters get long and spindly, even slower.

[irving2008]

sorry Robin, just to confirm - is that acceleration or cutting speed? If you really meant 1.5mm/s^2 thats 100 seconds to go from rest to 150mm/s cutting speed which doesnt sound fast enough to me! I think you meant 1.5m/s cutting speed, but what I was looking for was the acceleration you are using with that.

[Robin Hewitt]

I think you meant 1.5m/s cutting speed, but what I was looking for was the acceleration you are using with that.

That was cutting speed.

There has to be a top speed where it is okay to slam it in to reverse without losing steps.

No point applying accelerations below that speed so I don't. The 1.5mm/s feed has no accelerations.

Incidentally, slowing the axes down to maintain feed rate for arcs and slopes is easy. I started out playing gradients but it's not necessary. Took a while for the penny to drop.

At the sharp end of the program, you eventually step X, Y, neither or 'X and Y'.

If 'X and Y' you increase the delay before the next step by root 2.

Simples :naughty:

[irving2008]

Ah right, so your max cutting speed is 1.5mm/s = 90mm/min? That still seems for too slow to be a useful cutting speed, esp for alloy.. even with your high speed spindle. I was expecting 500mm/min+, i.e. something around 10mm/sec

Increasing delay between steps by root 2 on an 'X and Y step' is a neat approximation to maintaining a constant tangential linear speed in a curve. :)

[Robin Hewitt]

I was expecting 500mm/min+, i.e. something around 10mm/sec

Well, maybe if the machine had another ton or so of cast iron to keep the toolpath sweet :heehee:

I suppose I could try it but suspect on a quarter ton machine I'd get horrible graunching sounds from a fat cutter and bits of shattered tool whizzing past my ears from the smaller sizes.

Have you actually tried cutting metal? :naughty:

(Slight exageration there, whenever the tool breaks it never seems to do anything more than drop off the shank, never whizzes anywhere) :whistling:

[irving2008]

Well, maybe if the machine had another ton or so of cast iron to keep the toolpath sweet :heehee:

I suppose I could try it but suspect on a quarter ton machine I'd get horrible graunching sounds from a fat cutter and bits of shattered tool whizzing past my ears from the smaller sizes.

Have you actually tried cutting metal? :naughty:

(Slight exageration there, whenever the tool breaks it never seems to do anything more than drop off the shank, never whizzes anywhere) :whistling:

Err yes... I don't know what you are cutting (stainless steel perhaps?), but 6082T6 on my small mill cuts fine with an 8mm cutter at a feed rate of around 5mm/sec (which is about as fast as I can turn the handles manually - 2 revs/sec) and I would expect a powered table to move faster than that.

Some rough numbers... 8mm cutter, 60m/min cutting speed for alloy = 2300rpm on spindle (I whack it up as fast as the belts let me which is 2580 I think)

The chip load for alloy is approx dia/150 for roughing, d/200 for finishing. Assuming roughing chip load is 8/150 = .05mm so the feed rate @2300rpm for a 4flute cutter is .05mm * 4 * 2300 = 460mm/min = 7.7mm/sec

The material removal rate is depth * width * feed rate = 1 * 4 * 460/1000 = 1.84cc/min

Power(kW) = specific cutting force * removal rate/1000 = 17 (for alloy) * 1.84 = 31W (~1/20HP) and the torque needed is P * 60/(2pi * revs) = 31 * 60/(6.28 * 2300) = 0.13Nm

Doing the same with a 50mm facecutter its 400rpm spindle speed, 533mm/min (8.9mm/sec) feed rate and slightly less power. I know this is too fast for me to do manually which is why my surface finish isnt as good as I'd like with the 50mm/4tip facecutter compared to the 25mm/2tip one.. I havent yet tried the obvious and taken two tips off the bigger cutter...

I've only broken drills and two 3mm endmills... and nothing whizzes anywhere.. just snaps off flush with the end of the collet!