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

1. 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.

2. Originally Posted by irving2008
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:

3. 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. :)

4. Originally Posted by irving2008
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:

5. Originally Posted by Robin Hewitt
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!

6. Originally Posted by irving2008
nothing whizzes anywhere.. just snaps off flush with the end of the collet!
Well at least we agree on that bit, same thing happens with larger sizes :whistling:

I did try an accidental fast cut once...

I was using CamBam and cutting an outline in 1/2" x 6" HE30 alloy bar. Rather than drill hold downs I used a CamBam facility to leave tabs around the bottom edge. 'Easy to saw out after and clean up with a file', I thought.

Didn't notice in the G-code that when it lifted and passed ove the tabs it was using G0's with the tool still 10mm deep in the slot previously cut.

I would have changed them to G1's if I'd spotted it, but I didn't.

Of course the groove forming cuts above had side loaded the tool and bent it. Riding free in the slot the tool found itself zooming through a slot it didn't exactly line up with.

Chip loading was minimal but the horrible graunching sounds resulted producing great gouges which were reflected in the clean up pass.

I even thought about hitting the abort button because I knew it still had 2 laps to go and I wasn't sure it was going to make it.

Maybe if I'd had 4 times the revs I'd have gotten away with it?

There was a problem with that.

The quill splines had been rattling when I was whittling a 5" x 1.25" iron bar so I added grease. Heavy clay loaded grease.

Shut it up a treat. Unfortunately I hadn't reckoned on the taper roller bearings being unshielded. Then I had a problem with the phase converter cutting out on over current when I wound the speed up.

As soon as I realised what was going on I flushed the quill through with engine oil until it ran oil coloured rather than black. Top speed again became an option.

I have been speed limited, maybe faster feeds will now be possible, I shall play.

OTOH 10mm/s still sounds very silly :heehee:

Page 3 of 3 First 123

#### Posting Permissions

• You may not post new threads
• You may not post replies
• You may not post attachments
• You may not edit your posts
•