Another plasma component...

mkardasi wrote:

phillc54 wrote:

Non-sense! Can never have too much acceleration, just ask any car guy! Kidding aside yes, I'm able to out accelerate the arc, my fly weight gantry allows me 1.3G in X/Y which is why I see things that others, who have more iron to throw around, do not.

Wow, that's quite a bit more than HT's target of 40-50 mG.

Ooof. I didn't know that plasma was that low. Thought it might be similar to a quality machining center. Do you have a document that you can point me to, Phil?

Somewhere Tommy said 700-900 mm/sec/sec for acceleration. but it is a function of moving mass. My gantry is light too.
Some light hearted discussion here
forum.linuxcnc.org/30-cnc-machines/31509...pinion-drive?start=0

phillc54 wrote:

..... than HT's target of 40-50 mG.

where do you get that one from?

the number you will read occasionally from Jim colt on plasma spider is 0.3g

not 0.04-0.05g

that is just a an optimum target although, if the planner used S-curve acceleration or even a slightly modified trapezoidal acceleration profile then the acceleration could be improved (of stepper drive systems) but that is for another thread

if you read up on jolt / jerk (mm/s/s/s or in/s/s/s) which is basically the rate of change of acceleration you will understand that for stepper motors the gap between the first and second step (and last and second last step) of the acceleration profile that is where you limiting acceleration comes from.

servo motors are unaffected by this because they have an inbuilt following error allowable which gives some flexibility (smoothing of the sharp trapezoidal profile)

if stepper motors miss steps they

phillc54 wrote:

I am not really interested in jerk or steppers v servos, I am interested in what works for plasma cutting.

YMMV

Its physics ... you have to consider it all, understanding only part of something does not explain why it does what it does and appreciate what you need to do to improve things.

good luck, you obviously know what you want to know or think you need to know.

wish I were that confident.

Guys

Just another data point. I did quite a bit of power supply and driver changing to get the max performance that my steppers are capable of in the quest for maximum acceleration. What I found was that when I got my X & Y acceleration above about .3 g coupled with the known TP jerk problems my system could out run the arc on tight direction changes (45A, 220 ipm, 1.95mm steel). I mostly cut art work with mostly compound curves so I stress all of these problems. I spent a lot of time chasing this and finally gave up and limited my acceleration to .3 g ( about 100 in/s^2) in both the PID and the stepgen. Maybe some day I will have another go at it. The cut quality does improve once you get into the .2 g or greater acceleration.

John

acceleration is a bit pointless without direction (why do you NEED any specific acceleration number)....

first define what you want to cut?
material (ms/as/aluminium)
thickness (whatever)

then define what do you want to cut it with?
Amperage
what consumables? (fine-cut, 30a in a 45a machine) whatever

this should give you a feedrate number, and if you have a range of materials you cut decide what your preferred is (define a bit more than "everything" in the cut charts..... I mean are you really going to cut 0.8mm AND 12mm (1/2")?.... seriously!
let's say like me you are going to do mild steel, 2mm, 4mm and 6mm.... but obviously anything that is within your machines capacity remains an option

now think about the accuracy you expect.... inside corners, arcs and maybe outside corners are your consideration here.... if you cannot loop your outside corners.....

your limiting factor will always be your kerf as you ain't going to get tighter than that but also the trailing arc or cut (15 degrees I think is the norm at the recommended feedrate (it may be 5-7.... I forget....)

the trailing arc you can improve on by slowing down as it will catch up..... half the feedrate.... the trailing arc angle will be half that at the recommended feedrate ..... also on thin material it won't be that evident ... because of the kerf to thickness relationship.

there is also the good side of the cut (outside cut.... clockwise.... inside cut .... anticlockwise cut direction... good side on the left of the cut).... this still has a bevel 3-5 degrees at the recommended feedrate from memory..... worthwhile remembering regarding precision cut parts....

all these considerations regardless how trivial they are to you .... may actually form part of what you consider to be your acceptable precision.... and your acceptable level of acceleration.

the minimum recommended hole diameter tends to be 2xthickness (maybe 3x) for plasma .... anything less than this.... dimple (not pierce!!!) and drill.

if you need to reamer a hole.... dimple + drill (yes I have mounted bearings in an interference fit reamered hole as a hobby user adapter plates for a CNC mill conversion) as the edge of the cut will be hard and not help your drill bits and expensive precision reamers.

so back sort of on topic.... say you decide that the smallest hole will be 6mm dia (3x2mm mild steel plate).... allowing for a 1mm kerf this is actually a 5mm dia gcode path.... kerf may get a bit wider in practice .... say 1.5mm given we are going to slow down to the recommended 60% of linear feedrate so we are now at 4.5mm dia.

hell, for argument's sake say the smallest arc I ever want to cut is 2mm radius at 60% linear federate in mild steel with a 2mm thickness with a 45A plasma cutter with 45A consumables so the federate recommended from the book is 5560mm/min and ~7000mm/sec (hypertherm 45 non xp using duramax torch or original machine torch)

say 7000mm/min worst case..... 60% allowable federate for arcs and corners says it can drop to 4200mm/Min (70mm/sec). .... the minimum arc is 2mm or 2.5 or 3mm.....

ACC = vel^2 / radius.... (physics)

so the minimum acceleration I would need is 2450mm/s/s [0.25G] (for a 2mm arc radius), or 1960mm/s/s [0.2G]for a 2.5mm arc, or 1633mm/s/s [0.17G] for a 3mm arc

anything more than these acceleration figures don't actually help the cut really....

another interesting consideration is to cut a 4mm circle in gcode at a feedrate of 60% of the recommended linear feedrate how much lead-in and over-cut do I really need if I am using a torch with instant off in sync with motion M63 + delayed (overcut) m5...

at 4200mm/min or 70mm/s you will need a minimum acceleration distance of 1mm at 2.5G......

seems like in my case 2.5G would be a nice comfortable number to have as a target .... anything over this is not beneficial.... and may actually be detrimental..... yup detrimental because I would be placing undue stress on my components and system to achieve no benefit....

why you may wonder (or not if you cannot be bothered).....

YMMV.....

say I am running steppers and they have a step resolution of 0.05mm/step .... other than being course what does this mean????

well for acceleration it means that in 1 step it has to accelerate from rest to 0.25G... and at the end of the acceleration profile it has to decelerate from 0.25G to zero acceleration again in 1 step


time is the important criteria here.... how long is the first step.... at 2.5G this would be 0.006388766 seconds.... the jolt / jerk is therefore 383,485.6581mm/s/s/s

at 0.3G this would be 504,876.7751mm/s/s/s

which is ~30% more stress I would be placing on my components than needed

hopefully this is useful to someone as at least a consideration..... I'd go so far as to say that I would like the acceleration to be adjustable..... I clearly don't need 2.5G acceleration if I am cutting 4mm or 6mm or greater materials... so why not make the acceleration adjustable to a degree....

Acceleration can be set in LinuxCNC when the machine is idle
(not running GCode) via the ini pins.

PCW wrote:

Acceleration can be set in LinuxCNC when the machine is idle
(not running GCode) via the ini pins.

And a quick and dirty way of playing with it would be to load sim_pin via your ini file
linuxcnc.org/docs/devel/html/man/man1/sim_pin.1.html

This will open a separate window and is very useful for tuning and experimenting as you no longer need to shut down, edit your ini and restart.

PCW wrote:

Acceleration can be set in LinuxCNC when the machine is idle
(not running GCode) via the ini pins.

yes all CNC applications use a static acceleration for the planner. to be fair it would only change relative to the material being cut and the tollerance

although it doesn't change the acceleration, G64 is an interesting parameter to customise for a specific material and accuracy of cut which in turn will affect your feedrate relative to how close you require the part cut.... in the above example I was happy with a 2mm arc radius .... and therefore tolerance so I could set g64 (P&Q parameters) for this parameter and the planner would keep to this allowable tolerance..... if the part was set too accurate.... feedrate would drop and dross would be the result with an increased kerf...

linuxcnc.org/docs/html/gcode/g-code.html#gcode:g64

something else to consider or be aware of that it may be job specific.... set it too low for a high feedrate job and it'll cut poorer than you think