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

[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.

[Davek0974]

The 5mm cutter runs cleaner at 18000rpm and 1000mm/min. :)

Edge finish...


Nice pile of swarf...


I had the onion-skin set a little too tight and had to hold the parts in for part of the finish cut but that's easily fixed.

Couple of videos...

Running the 5mm roughing cut, I can't be sure if this was the fast or slow setting though.
https://youtu.be/I_gkfQ6zJKQ

Pre-finishing the sharp corners...
https://youtu.be/h2HGya_X3iU

Still need to sort out some chip management as the mess is unbelievable ;)

[Davek0974]

2 Jobs tested and in production :) 2nd one much less stress ;)

2010 screen-set, tool change routine...

On this job I did exactly the same as before but the first cutter seems to have run about 0.2mm lower than it should, made a bit more mess out of my bed but i'm not worried about that as it's buggered anyway ;)

The next two tool changes worked perfectly and did not gouge the bed.

Anything that can cause this?

I have verified the code and all parts are cut to the same depth.

[Clive S]

Anything that can cause this?

Human error or the tool slipped in the collet

[Davek0974]

Vaguely possible but why only slip 0.2mm and not just keep going as usual?

The second and third tools were spot-on which indicates the initial height sense was good, i think.

[lucan07]

If it did slip the torque from cutting and centrifual forces or heat generated in the tool could have locked it tight again.

One plus for leaving my cast iron bed for later use if I feck up a bit of MDF or even some Aluminium extrusion I won't be to upset but I don't want to replace a 1000x700x50mm cast plate that has been ground

[Ger21]

2 Jobs tested and in production :) 2nd one much less stress ;)

2010 screen-set, tool change routine...

On this job I did exactly the same as before but the first cutter seems to have run about 0.2mm lower than it should, made a bit more mess out of my bed but i'm not worried about that as it's buggered anyway ;)

The next two tool changes worked perfectly and did not gouge the bed.

Anything that can cause this?

Didn't you have this issue before?

[Davek0974]

Didn't you have this issue before?

That was when the coolant stopped and the cutter loaded up, i was also pushing much hared back then as the feeds/speeds were off.

This job was only 3mm aluminium, I was taking a full depth cut though. Odd that it was only the first cutter, which went back in later to do a final full depth pass around the edge.

I will have a look at the shank and see if there are any skid marks.

Also have another to make today.

[Davek0974]

Next run went fine, apart from a boo-boo ;(

I've seen this behaviour before on the plasma table - something goes wrong, you press stop on the Mach screen, I know your supposed to press feed-hold but i wanted something between e-stop and feed-hold as the coolant failed to come on (duff relay) so i knew it would load up and break and so pressed stop.

Fixed the issue, wound the code back to the last M05 stop and set next line.

Pressed cycle start and the cutter goes down where it is and shoots off to X+ at cut speed, snapping the tool off. It should have gone back to where it started last time and re-cut the partial slot and then finished normally.

Looking at the DRO's the X machine position is off by 226mm which i think is the setting that it was stopped at so now the cut start was not X5 as it should be but X-221 or something like that.

As i said, this has happened on the plasma and as here, the only way back is scrap the part, re-home and start again. I failed to note the X/Y positions for job location so i couldn't reset it and try again.

Some sequence of events throws Mach positions into a tizzy and it shits the bed. On the plasma no harm usually but on the mill = broken tool :(

Oh well, the next part finished perfectly, no bed gouging, if anything it was running too high now - the material miked up at 2.91mm, i programmed the cuts to 2.90mm and there was still a good skin left at the base. Something seems a little variable on height setting possibly?