It's begun....

[Washout]

Even quicker update: looks like all parallel cables are not equal, as I have just replaced that for the old one and all is now well - test job ran without any e-stops :-)

Now for some cutting.......

[JAZZCNC]

Even quicker update: looks like all parallel cables are not equal, as I have just replaced that for the old one and all is now well - test job ran without any e-stops :-)

Now for some cutting.......

When having any problems with signals first place I always go is the Parallel Cable and swap it for a known good one.

Pleased your sorted.!

[Washout]

Thanks Dean,

I ran a couple of jobs yesterday: one was some text in plywood for a sign, which was long but ran fine. The other was a first go in aluminium doing some roughing 3D work (I'm using Vectric 2 and 3D for my toolpaths).

The aluminium didn't do too well and I'm pretty sure I'm being a plank with regards feeds and speeds. Material is 6082 as per previous posts and I was running a Carbide 2Flute End Mill @ 12000rpm and 1200mm/min with 2mm DOC and 30% stepover (maybe a bit aggressive on the DOC?) and was blowing air. Anyway the machine seemed to hold up well i.e. nothing broke but was grumbling a lot so I hit Feedhold and saw that the edges in the pocket were clean, but it was obvious the cutter was trying to erode its way through rather than cut as there was a good "weld" of aluminium on the cutter and a "lip" around the edge of the pocket.

My guess is my feed rate is too low (possibly rpm to high) and I'm re-cutting chips?

What was cut didn't have visible chatter marks on the walls of the pocket, so I'm tentatively confident the rigidity is OK (2 ballscrews does indeed help :) ).

Will have a play later with a less aggressive DOC and high feed rate, but if anyone has their own feeds/speeds I can try then it may save me some time in trial and error.

Chris

[Jonathan]

Assuming that's a 6mm cutter, then the feedrate and speed you posted should be fine. With only 30% stepover you could actually increase the feedrate slightly due to chip thinning, but I'd leave it for now. I tend to agree that rigidity shouldn't be a problem.

You're problem is almost certainly the lack of coolant. Air will help to cool the cutter, but not much compared to coolant (i.e. mainly water). Also, with no lubricant the co-efficient of friction is greater, so more heat is generated. You'll probably find that even a small amount of coolant will do the trick, or if you've not got any then WD40 works well on aluminium. I certainly wouldn't advise using it regularly though as it wont be good for the bearings.

If you think the rigidity of the machine is a problem, as a general rule don't change the feed or speed, instead lower the depth or width of cut. The reason is if you've chosen the 'correct' feedrate and rpm, then the chipload will be a particular value which you want to maintain. If you just change the feedrate or the spindle speed the chipload will change.

[JAZZCNC]

If you think the rigidity of the machine is a problem, as a general rule don't change the feed or speed, instead lower the depth or width of cut.

Agree with Jonathan keep playing with DOC and you'll find the sweet spot for your machine. Be aware it will also change depending if your Full slot cutting or Side cutting so often you'll need to find a balance depending on the job and how much it goes in or out of full/side cutting.

A good clue to cutting correct is to check heat of material and chips.? When your cutting correct the Chips will be scorching hot but the material just slightly more than warm.
When your more experienced you'll here the sound and know if your close to cutting correct but at the moment these sounds will probably be
making you nervous and weary.!! . . .Put some ear plugs in and listen to it you'll not be quite so on edge and it dampens mechanical noises and lets you hear cutting sounds better.!!

Also Set your VFD to display Amp's rather than RPM this will give clue to how well cutter is coping, also shows when cutters getting worn while jobs running. If Amps are low while cutting then this gives a clue that you can probably take deeper cuts.

Regards sticking then Mix some paraffin and old engine oil in a squirt bottle and give the cutter a blast every now and again to help with sticking but when you have found the correct chip load blown air is enough to clear chips and stop re-cut/sticking. I never get sticking and for most Jobs only use blown air with few squirts of coolant, for jobs where finish matters then I run a mister system. (just can't bloody breath when it's at full chat.!!)

Now test it properly for accuracy and cut the Aztec calendar.!! . . . That sorts the Baggy fanny's from the tight chuff's .. Lol

[Washout]

Thanks Jonathan as ever.

I'll try with some liquid coolant next and see how that goes - reason I thought I was being a numpty in the F&S dept. is that most calculators are throwing up higher feeds generally e.g. 18-1900 mm/min, which I can try but that sounds aggressive, although maybe its not aggressive enough?

Must try and remember where I got my last batch of mills from, I'm likely to be placing some more orders ;-)

[Washout]

Lol - I'll have a crack at the Aztec calendar soon I promise :-)

You're right the sound is a little disconcerting - was even louder than my bloody noisy compressor ;-)

[Jonathan]

If the coolant doesn't help then take a picture / video and that should make things more obvious...