EMC2 and Acceleration setting

[Zig]

Strictly speaking not just an EMC2 question... here goes:

I am runing some micro tools on my mill. Everynow and then the tool will snap at the start of feed cycle. The runout of the spindle is not a problem. The PC is operating with a latency of under 20 000.
I suspect the acceleration may be too high and is causing the tools to get overloaded.

How to set up machine dynamics ( acceleration ) so that the tool is stressed least by the start of a feed cycle?

Does the acceleration have a bearing ( pardon the pun ) on the tool survival?

If this is not the correct forum to ask these questions please redirect me.

[wendtmk]

Sounds like your feed is too fast or your DOC is too much at the beginning of your run in the G Code. Have you tried a shallower DOC or a slower feed?

Mark

[acondit]

Backlash could also cause a heavier cut than the gcode would call for, because backlash could result in the tool not being where you expect it to be. With micro tooling it might not take very much.

Also, spindle acceleration (if the spindle is being started under machine control and movement begins before the spindle reaches the correct speed for the specified feed).

If you solve the problem, let us know what you find.

Alan

[Zig]

Micro tool behavior is quite different from conventional tool performance.
Everything seems to affect it sometimes catastrophically as far as the tool is concerned.

I am using an Alfred Jaeger spindle ( capable of 100KRPM with a run out of 8 micron at the tip of a 15 mm long tool ) and servo controls with linear scales ( 5 micron resolution).

The acceleration was set to 300 mm/s/s on all 3 axes. I have now brought it down to 200 mm/s/s.
The servo motors sound a bit quieter.I shall be doing some test milling over the next couple of days using 0.25mm end-mill tool.

Hope to have some more information soon.

[TDA]

Yes, acceleration can have a effect on tooling. What you should be running will depend on your machine and tooling. If it helps I have cut with a .005" (.127mm) endmill with an acceleration of 20" (508mm)/s/s.

They're are a great many issues when you start cutting with tools of this size. I would also check the height of the material being cut to see if you have one side of your material higher then the other (relative to your spindle head not the table or a level). Or better yet surface the material with your CNC before cutting it and KNOW that it is true to your spindle. And as already said check for backlash it will kill you too.

[Zig]

The machine is built with preloaded recirculating ball nut screws.
My expectation is that backlash is minimal ( have not measured it ).

The work table has been machined bythe spindle so the expectation is that the table/spindle are perpendicular.

I had just trammed the spindle a couple of days ago so that ought be OK.

What spindle speed and feed did you use with the 0.005" tool?

[TDA]

Not sure what you are cutting but even if I knew my table and spindle was good I would then have to question the material thickness. If you want to be on the safe side (at least for testing) I would still surface the material.

I think I was going 24KRPM (my max) at 6IPM (152mm/min) with a 2IPM (51mm/min) plunge I believe it was in a phenolic. I'll see if I can find the data. Something that a lot of our customers cut with is a 3 flute .010" (.254mm) cutting in mother of pearl. Those numbers I have: 24KRPM, 4IPM (102mm/min), with a 2IPM (51mm/min) plunge. Like I said though I don't know what you are cutting or with what tooling so that info is only so useful.

[acondit]

Originally Posted by Zig The machine is built with preloaded recirculating ball nut screws. My expectation is that backlash is minimal ( have not measured it ).

Is that a single ballnut with some oversize balls to adjust out the backlash or a double ball nut with anti-backlash adjustment.

Alan

[jmelson]

Originally Posted by Zig The machine is built with preloaded recirculating ball nut screws. My expectation is that backlash is minimal ( have not measured it ).

I have high-precision anti-backlash ballscrews on my machine (a Bridgeport mill, so probably a
lot more mass and slide friction than yours). I have measured the "backlash" and it is about .025
to .04 mm on the 3 axes. This is largely due to FLEX in the mountings of the ballscrew and nut, and a little due to rocking of the table when direction changes. So, just because you have anti-backlash screws does not mean there is no "lost motion" between the motor/encoder and the
linear slide. The measurement is easy to do.

Jon

[Zig]

John ( TDA),

The feed and spindle spped settings are not as much of a mystery as they used to be.

I adhere to the 1% to 2% ( of tool diameter ) per cutting edge chip load and tru to keep to an optimal spindle speed ( maximum speed at what sounds like minimum "rattle". In my case that is up to 70KRPM.

V tools are typically operated at 40KRPM and 350 to 400 mm/min.

Runout specified by manufacturer is 8 micron at 15mm tip length.

Alan,

Yes the preloaded ball nut is just as You have described it; a ball nut with somewhat oversize balls .


Jon,

No doubt there is nothing perfectly stiff. I use linear scale not a rotary shaft encoder. One step closer to God.


The issue in my mind at the moment is whether the initial jerk ( first derivative of acceleration ) could be the killer?

[jodhner]

With too much acceleration for the structure of the machine, the tool might not move initially, then suddenly catch up -- even without static backlash there can be higher order dynamical hysteresis. The solution would be accelerating the acceleration -- inches per second per second per second. Of course lowering the acceleration a lot would be a practical test, if not a solution.