New machine bogging down / missing steps

[James123]

Hello there,

I have recently got my machine up and running and im having problems with it bogging down and stalling the steppers.

The problem seems to mainly be on the x axis, though i think i may of missed a few steps on the Y. The X is driven by a 3.1Nm stepper direct drive onto mod 1 rack with 20 tooth pinion, the Y is the same but has 2 motors left and right. I skimmed the bed a few days ago and it seemed to run fine, then i tried cutting some plywood yesterday. The program i ran was quite large and ran for about 2 hours until it obviously bogged down and started to cut where it shouldent of, upon closer inspection it had missed a few steps earlier on in the program.

I made a simpler program today to do each part indivually but it bogged down on the deepest passes on the first part, then it stalled on the next part, i ran the program again and it stalled at the same point (as soon as it had to cut some plywood) i then replaced the cutter and it managed to get through it. I am using 4mm Chinese carbide cutters cutting 12mm birch plywood, 2.2Kw water cooled spindle at 12000 RPM, the passes were 4mm deep with 5mm on the 3rd pass to make sure it cut all the way through. the channels are clogging up as the extraction does not have enough suction to get deep into the channel and there only 4mm, i thought this was the issue and was hoping it would be ok if i switched back to 6mm cutters but then it stalled on a 8mm deep pass that was clean and open as it had a recess next to it.

Im not trying to do hard machining, i used 6mm cutters doing 6mm deep passes with my old machine with a wood router and it cut fine. The new z axis assembly and gantry are heavier than on my old machine, about 55kg now, so i am thinking that running direct with no gearbox may be the issue, but it seems to jog about at 6m/min and not loose steps, (im machine at 2m/min)and it ran the bed skiming program fine, so is it more likely to be down to the cutting?

Im a bit lost with this at the moment so i thought i would put a post up on the forum and see if someone with better understanding could point out whats going wrong.

Many thanks

James

[Blackrat]

The stepper is straight into the pinion with no reduction box ? Is that right ?

[James123]

The stepper is straight into the pinion with no reduction box ? Is that right ?

Yes there is is no reduction, im starting to think this is probably the problem, it seemed ok on my old machine though, but i guess the extra mass combined with hitting a hard bit of plywood could be enough. It occured to me thT the x axis is cutting accross the grain, and the y is cutting down the grain, which might explain why the y axis seems ok.

Cheers

James

[EddyCurrent]

I think you are running the spindle too slow, 16500 to 18000 sounds better, also the depth of cut seems high, and your feedrate is too high.
So I would try this to see how it cuts; speed 18000rpm, depth of cut (with 4mm dia.tool) 2mm, feedrate 800mm/min.
If that works okay you can try to increase the depth of cut and feedrate until it starts to fail.


. . .but i guess the extra mass combined with hitting a hard bit of plywood could be enough. It occured to me thT the x axis is cutting accross the grain, and the y is cutting down the grain, which might explain why the y axis seems ok.

Plywood has grain going at 90 degrees to each other in adjacent layers so there is no 'with' or 'across' the grain.

[James123]

Cheers Eddy, i will try that tomorrow, i used to run at similar feed rates (2-3m/min) with my old machine, when i decreased feedrate it started overheating cutters due to decreasing the chip load, as i had to run the router at full speed to get full torque, so ill start with the numbers you suggested and check the cutter for over heating, im just a bit wary of running too slow feedrate/ too high spindle speed.

TBH i thought i was taking it gently, i used to take 6mm deep passes with a 6mm cutter with a wood router, and this spindle is more powerful... But ill try it shallower. Ive not used 4mm cutters before and yeah 12000 is a bit slow if there smaller then the cutting edge is not moving as fast as a 6mm cutter would, add that to me running too slow and i recon that could cause the problem.

Yeah your right, i do know this i work with birch ply a lot, just my brains a bit scrambled today...it does cut more cleanly on the surface when you cut down the grain though.

Thanks again

James

[EddyCurrent]

Yeah your right, i do know this i work with birch ply a lot, just my brains a bit scrambled today...it does cut more cleanly on the surface when you cut down the grain though.

I just thought, if the depth of cut is the same as the thickness of one plywood layer then yes, there will be a grain direction.

[James123]

I ran it today and cut a few more parts at 18000rpm, 1500mm/m feed rate and 2mm deep passes and it didnt miss any steps, ill finish it off tomorrow at 3mm deep and see how it does. It might just be that the plywood is really hard due to the cold, its not been much above 0 degress in my workshop for about a week now.

[EddyCurrent]

Sounds good, maybe you should invest in a wood burner, this is the one I use and it's great; http://tecnikstoves.co.uk/8-kilowatt-stoves

[JAZZCNC]

Give us some more info on system like motor wiring parallel or serial, voltage, micro stepping etc drives are running at to get better idea of system.

But still your going to want a ratio applying as 20t pulley direct drive means 63mm pitch which is way too high really and torque low so any stiction will have an affect which is why your bogging down. (2m/min shouldn't be a problem in plywood)
If you use 3:1 ratio you'll triple the torque and put the motors in an rpm range there more happy running and still get decent rapid speeds, well in excess of 10M/min.

[James123]

Ive cut more pieces today and had lots more missed steps on the x axis, i then realized the pinion was completely free on the x axis. The pinions are held with 2 M3 grub screws, one tightens onto the flat part of the stepper shaft. I have ordered some M3 cap head screws so i can get more tension into it, with the little grub screws i couldn't get that much tension into it as it was bending and twisting the hex key, i think this is the issue as it would also explain the small amount of missed steps i am getting with the Y axis, theirs 2 motors on the Y so if one came loose it would still be driven by the other.

Thanks Jazzcnc, The steppers are all wired in parallel, the supply voltage is 36V and i think i left it on 1/16th micro stepping in the end, Its not very smooth though you can really hear it when it accelerates and decelerates, I think im going to go for some reduction, ive been looking at the pulleys on CNC4YOU and i could get 3.333/1 ratio with a 15 tooth on the motor and a 50 tooth on a shaft to my 20 tooth pinion. What do people use for a shaft? Will M8 threaded rod work or should i go for some 8mm aluminum rod and tap one end to mount it onto a bearing? I think it should be possable to modify what ive already done and add in some reduction, ill try and work it out and do some drawings.

Yeah those stoves look great Eddycurrent , youve got me trying to think of ways to get a flu through my plastic roof... the problem is with my workshop is its got very little to hold the heat in, I think im just going to have to live with it for this winter at least.

Thanks again for your help guys!

James

[mike os]

Although I have limited CNC, I am generally considered fairly expert when it comes to wood...., my thoughts on the above

rule of thumb for cutting wood... depth of cut never greater than cutter diameter, to a maximum of shaft diameter... so 4mm = max 4mm cut, for say 10mm with 1/4(6mm) shank = 1/4 etc.... obviously this is a catch all and can be pushed, but with this you will generally not break tooling, burn material or blunt tooling with rubbing, damage collets, and allows for better chip clearance.... although at less than 6mm this will often be an issue with cuts more than 2x dia. and up to 1/2" at more than 3x dia deep

cutting speed is crucial with small cutters, at 4mm I would be running nearer 30000rmp and adjust depth and feed to suit... ie shallow & fast

[Blackrat]

ooer ... i cut 10-12mm with a 6mm bit , maybe i should lighten up a bit :D

[EddyCurrent]

cutting speed is crucial with small cutters, at 4mm I would be running nearer 30000rmp and adjust depth and feed to suit... ie shallow & fast

You'll probably pay a premium for a decent size spindle to run at this speed, mine can run at 24k but it was quite a bit more expensive than the 18k model.

[mike os]

24k is not bad tbh... more in reference to running at 12k.. :-)

[EddyCurrent]

I suggested 16500 to 18000 rpm earlier because that seems to be a sweet spot on my machine, (16500 especially) it gives a good finish on the smallest cutters in hardwood and less tool wear (cuts per second).

[mike os]

balancing cuter speed, DOC and feed is the key I think, but generally low cutter speeds (peripheral /curcumferencial speed- varies with diameter) is an important consideration... when I get consulted on poor performance/finish on router & spindle moulder work it is nearly always running too slow, usually because the operator is inexperienced or scared of the tool.... should not be a problem with CNC though I don't think

[James123]

Thanks guys, the missing steps issue turned out to be the pinions slipping, ill try running it at 24,000 rpm and higher feed rate and see if that improves the cut quality.