[samu]

I have a 3 axis vertical machining center with fanuc o-md controller. When the tool path is a small radius or a sharp corner at high feed (about 100 ipm) difference between programmed tool path and actual tool path is quite big. (about 1/32"). I know that a part of this error is caused by acceleration/deceleration parameter. But can i improve accurancy by changing servo tuning parameter. Actually, parameters are the same for all 3 axis. Loop gain 2500, proportionnal gain -816, integer gain 91. I have some notion in process regulation but i am a new with servo tunning.

[ben_heinman]

You might want to check your ACD(automatic corner decel), COV (automatic corner override), MDR (minumin decel ratio) parameters.

[SIG]

I've got the same problem.

[brandou10l]

do you know what motor model you are using??
i could give some better suggestions if i knew
its written on the motor itself, problably an alpha series the model will be followed by the alpha symbol
you have to keep the values on the x,y the same or it will not cut strait
try reducing the acceleration parameter until it starts overshooting,
this is supposed to be done with an oscilliscope
but i just put my hand on the table or the column and when you feel a jolt/vibration when it stops it usually means it overshooting then add small increments until it stops
this will help reduce the corner rounding
you should backup you parameters before you go messing with it

[samu]

servo model is alpha6/3000
-is automatic corner override active only in g41/g42 mode??

-is there a parameter to set to activate automatic corner override or MDR???

There is parameter #580 AOVLE (end point deceleration distance of automatic override at inside corner part. Set the operating range Le)
and parameter #581 AOVLS (end point deceleration distance of automatic override at inside corner. Set the operating range Ls)
Wath is difference between these two parameters???

If ther is a very small radius in an inside corner, do the controller handle it like an inside corner??

[brandou10l]

#580 is the distance to the corner when its slows down at the reduced rate
#581 is the distance after the corner before it speeds back up
about the small radius yes only if the angle is greater than the value you specify in the parameter
acd does only work in g41/42 and 1/2 tool dia for comp value
it does not work if 0 is specified

in order to get accurate high feed cuts you need controller with lookahead control
yours might have it lok and c if the manual specifies a g08p1 to turn it on
and a g08 p0 turns it off
this function would control the error to a high accuracy regardless of the feed
if not the next best thing is to manually slow the feed around small radaii and for sharp corners use the g61 mode

[brandou10l]

the 580 parameter value is with no decimal

example value of '45' is .0045 inches/.045mm