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...
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 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.
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.
How to improve?? It looked better on the roughing cut ;)
Pre-finishing the fiddly loops, 2mm tool...
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.
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/
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?
Last edited by Davek0974; 02-04-2016 at 05:48 PM.
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:
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?
Last edited by Davek0974; 02-04-2016 at 06:10 PM.
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.
By Tenson in forum Gantry/Router Machines & BuildingReplies: 1Last Post: 21-09-2015, 07:54 PM
By fandango in forum Gantry/Router Machines & BuildingReplies: 14Last Post: 21-03-2014, 12:38 AM
By D.C. in forum Gantry/Router Machines & BuildingReplies: 28Last Post: 15-12-2012, 06:23 PM
By purple_rob in forum Gantry/Router Machines & BuildingReplies: 5Last Post: 03-08-2009, 10:08 PM
By Ross77 in forum Gantry/Router Machines & BuildingReplies: 9Last Post: 03-06-2009, 07:34 PM