Printable View
Same thing happened here when i was testing my belt grinder, the vfd and the 3kw motor. At the end i had to open the VFD and say "bye bye" to 6 capacitors which were connected to ground. Desoldered them and now all is allright. That with the Siemens micromaster 420. Luckily the Toshiba inverter have a button to lift the capacitors from ground in urban scenario.
To check if that's the case you just check using V meter if you have leak voltage on ground pin. Carefull!
I don't think it's earth current, the breaker is not an ELCB, just a plain MCB. The whole shop is run from an ELCB and that did not blow.
I also can't risk opening it up, it's brand new and if it will not work here, it will have to go back.
All is not lost ;)
Just had a reply from the supplier - that's what i call customer service!
Hidden away under a little plastic cover is a lever - pull it and it disconnects the internal EMC filters, he thought it worth a try. Popped out to shop, pulled the thingy and plugged it in - hey presto it powered up :)
Sounds like the same setup as Boyan mentioned above.
Didn't have time to run the PC up or start the spindle but at least the breaker didn't blow. I unplugged it, waited a minute and tried again and it worked ok again.
It's a promising note to end the day on at least.
Also have the new 5mm cutters - brilliant service from CutWell Ltd. Now I just need time, it's in short supply at the moment;)
I had same problem with mine but unfortunatly only just seen post else could have saved you some pain. . .:joker:
Very odd, I have two other VFD's in the shop now, once upon a time I had five on various machines, none caused this issue.
Maybe the issue is worse on newer drives with tighter EMC nonsense - the others are about 5 years old.
Hopefully get cutting again Saturday, have a little test piece lined up, got to sort the z axis calibration out first.
RESULT (at last) :) Double whammy tonight :)
I had 20 minutes tonight and also had a chat with the VFD supplier this afternoon...
Double-checked my settings in the VFD and following advice from the tech guy I run an autotune sequence with everything connected up - apparently this is 100% vital with sensorless vector drives.
Huanyang vs Schneider Altivar... Like comparing apples and grapes!
The spindle sounds much smoother and quieter, draws less current too! No annoying resonance effects at certain speeds either. Success 1.
Happy with the way it was running I reached for the tacho in the hope that the speed ranges would be better, well they were, a tiny bit anyway but not enough for me!
I visited spindle pulleys again and raised the minimum speed to 6000, the result was that made my calibration worse, much worse - this gave me the light-bulb moment of realising that if lifting the minimum above zero makes the issue worse then surely taking the minimum BELOW zero would make it better - and oddly enough, it DID!
In the end I have a minimum spindle pulley of -6,500 and a maximum of +24,000 - I now have calibrated speeds from 8,000rpm to 24,000rpm to within about 200rpm of the requested speeds from Mach3 - success 2.
Next I thought i'd see if it had any power - called an S100 from mach, and gingerly tried to stall the spindle by hand - this was easy with the Huanyang drive, but I tried as much as i dare without risking injury and could not get it to stall or even change speed much! OK, so running at 100rpm is unrealistic - it uses more current, and likely won't do the spindle much good but knowing VFD's a little I know the power is usually naff at low rpm's.
So, at this stage at least I would say it's in far better shape now.
Tomorrow hopefully should be recalibrating the Z axis and starting test cuts again. I might even risk an old cutter and set the speed at the correct value, I have a feeling it will work this time and not bog down and break.
Now you tell me good job I like apples just brought a 2.2kw HY VFD and spindle but at £146 delivered from UK with the eBay codes yesterday i don't think I would have got near the Scheider
£146 for spindle AND drive?? thats pretty darn cheap!
The Schneider was £148 delivered BTW
Yeah saw the 20% discount for everything on eBay so had to go for it only ran from 4-10pm found a HY chinese supplier with warehouse in UK near me in Leicester so did the deal can resell on ebay for that money and still not lose so gotta be worth a shot.
Don't threat I fit these all the time and think Dave had VFD which wasn't setup correctly or possibly faulty. Normally they work very well above 6000rpm.Quote:
Originally Posted by lucan07
Yes the Huanyang won't match Vector drives for torque, esp at low rpm but it's more than good enough for cutting wood an aluminium between 8000-24000rpm with smaller cutters which is where you'll mostly run it.
I agree, I have a strong suspicion it was a duff drive - setting it up wrong would not give the odd fact that I could not get a voltage reading on the 0-10v inputs when running - that is extremely suspicious.
Ok, getting somewhere now :)
I checked the Z axis calibration, microscopic tweak to steps-per but nothing major.
It turns out the reason my previous onion-skinning and tabbing failed was because of operator error - garbage in, garbage out! The metal i ordered was 5mm thick, I set that in CAM and tried to leave a 0.1mm skin or a 0.3mm tab.
In real life however the sheet was only 4.85mm thick - there was the missing skin and tab, I was telling it to go deeper than it really was - lesson learnt - don't ever trust what you order is what you get :)
Another possible source of error in the sub millimetre range was the probe touch-plate, it miked up at anything from 1.42mm to 1.51mm depending on where you place the micrometer. I have fixed this by scribing an area on the surface of the plate where it measures exactly 1.5mm - always using that spot should sort it out.
So, on to cutting stuff, I threw in my sacrificial 5mm 3-flute HSS cutter and set a lump of my 4.85mm ally on the bed.
In CAM i made a straight line 40mm long, 4mm deep, slot width, plunge in, 1mm DOC, speed at 8000rpm(where it bogged down before) and feeds ranging at 600, 800, 1000, 1200mm/min.
Result was perfect in all settings, no speed drop at all, perfect cuts.
Next test was the same job but this time 1.5mm DOC per pass, same speed ranges.
Result was 100% perfect, it didn't even know it was cutting!
A video of a 1.5mm DOC 1200mm/min, 4mm deep slot cut...
https://youtu.be/cL3Om6xMfK8
So, I am now going to risk a tool and try my job again, onion skin at 0.15mm to start with, I am expecting a failure as I don't think the sheets are really big enough for the job but who knows :)
Made it's first full-job :)
Yes, I know it's a failed part - i lost a cutter due to it hitting a hold-down bolt caused by my messing with the CAM so much I forgot which file was which :distress: I didn't want to add wasted metal to a wasted cutter so i reset the file and cut the next run over the first one.
Attachment 18069
Onion-skin was perfect, too thick and hard to remove at 0.15mm but i did manage to take the job right through all the post-finish drilling, counter-sinking and fettling just to prove the process.
OK, education time...
Poor quality on the finish passes, 2mm single-flute cutter, 0.6mm DOC, 450mm/min cut, 23,000rpm - chatter I think.
Attachment 18070
How to improve?? It looked better on the roughing cut ;)
Videos...
Roughing cut...
https://youtu.be/oSgf-0C5PHM
Pre-finishing the fiddly loops, 2mm tool...
https://youtu.be/nD4If43P3c0
Job took 43 minutes including tool-change, mostly the delicate finish cuts, I will look at these a bit more as something is off a little there I think.
Any pointers?
On the next run I'm going to take the skin down by 0.05mm and also put a sheet of paper or card under so I take the fine detail - holes and slots, down to 100% depth.
The pointers: i said it many times, and most disagreed. For perfect aluminum finish if the machine is normal, that combo gives me the best finish. I don't care about 12k rpm or 30 krpm. That combo for 3mm bits gives me best finish. On the yellow machine i could cut at 12krpm and 2500mm min at 1mm deep with 1/4 bit. But best perfect finish is around 600mm min/ hence 25 ipm/
Attachment 18071
Those settings are not far off where i was, I was a little slower feed and faster rpm, that may make a difference, don't forget there is a fair bit difference between a 1/8" and 2mm tool.
Thoughts over dinner...
1 - Make the final pass on the main parts with the 5mm cutter then isolate the small features and machine only those bits with the 2mm tool?
2 - Try the final pass with the 2mm at full depth but add a slow-down in the corners where it's biting the rads from the 5mm tool?
3 - something else?
On the finish pass question - I don't often use small cutters so don't know what the problem is. But 0.6mm DOC seems small for the finish pass ?
I generally use 6mm cutters and for finishing I leave 0.1mm roughing on the part - how much are you leaving?. Then I cut at 3mm DOC as this works well but I could probably do anything up to 10mm DOC as you're hardly removing any material on the finish.
Here is the finish on a 10mm part using this method:
Attachment 18072
I left 0.1mm from the roughing pass.
The 2mm cutters are spec'd to 3mm DOC but I still have concerns where they hit the rads from the 5mm tool and also have to plough into the corners a bit to create the sharp internals. Maybe my option 2 above would work?
Looking at figures there is a fair difference between the finishing pass and the sharp corners -
Lets go for a 2.5mm DOC this time, just below the cutters limit and half the final depth...
Finishing the edge wants 23,000rpm and 670mm/min feed
Ploughing out the rads and creating the sharp corners - basically a slotting cut - wants 18,500rpm and 180mm/min feed
So quite a change, all other parameters being left fixed, sounds like a path rule in SheetCam might work there?
That would be a 25% speed reduction and setting feed to 28%.
The machine made it's first saleable parts today :)
I did sacrifice two 2mm cutters, here's how...
On the part in the OP, there is a little square notch, first from the left along the top edge, it's about 4mm square and as such was not roughed out by the 5mm tool on the first pass. I set the code for a 2.5mm deep cut on the finishing pass with the 2mm tool and added a reduction to feed with CAM rules, it worked nicely until the tool reached that notch when it died.
I then increased the before and after feed change in CAM so the rate slowed well before and after the notch - ping went another tool. I then reverted back to 0.6mm per pass and 450mm/min rate as before and it sailed through. Still got that slightly poor surface finish though.
So, it seems despite what HSM says, even on severely reduced settings, you cannot slot 2.5mm deep with a 2mm tool.
Now, in light of the slow finish passes and the fact that it did seem to handle the 5mm rads with a CAM rule and 2.5mm DOC, is it worth singling that feature out and running a pre-finish run on it like I did with the loops??
Apart from that, I'm not happy with the paraffin/oil mix, seems to be affecting my hands a bit, I have found a suitable retail item - MilliCut J40 from Cutwell, its a veg oil based product.
Has anyone got there mill in an enclosure? I'm finding the floor is covered in chips about a 4' radius around the little bugger from the roughing passes - the 2mm tool just makes dust.
Next step get the processing nailed down and make them profitable too, let the bugger start earning its keep!Quote:
Originally Posted by 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.:unconscious: :cheerful:
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.
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.
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.Quote:
Originally Posted by Davek0974
What's Max thickness Ali can you cut with plasma.?
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.
What kind of feedrates would you cut 19mm Ali with.? Is this using 45A plasma.?Quote:
Originally Posted by Davek0974
Attachment 18088
Attachment 18089
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.
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.
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.
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.
The 5mm cutter runs cleaner at 18000rpm and 1000mm/min. :)
Edge finish...
Attachment 18107
Nice pile of swarf...
Attachment 18106
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 ;)
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.
Human error or the tool slipped in the colletQuote:
Anything that can cause this?
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.
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
Yeah i also have a cast iron bed but its only ever for use as a sub-bed, the part that has been mauled is only 15mm Eco-cast plate so i'm not bothered too much, will likely end up taking a skim off it anyway.
Only reason I didn't use mine is I don't like shredded wheat enough to eat three, or the fact that after having it ground flat advised to leave it on steel base, either part I could find a couple of mates and man handle up a flight of stairs into my flat but together they're almost 0.4 of a ton and can wait until I move again and have my workshop at ground level.
Didn't you have this issue before?Quote:
Originally Posted by Davek0974
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.Quote:
Originally Posted by Ger21
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.
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?
Any time you press Stop, you MUST re-home the machine before doing anything else.
And I'd highly recommend using Run From Here, unless you know exactly what state mach3 is in when you use Set Next Line.