Rapid move, corner rounding?

[Ydna]

There's a definite "rounding off" of corners when multiple rapid motion movements are set back to back. Very noticeable when making a rapid +Z move then a rapid +X move, followed by a G1 -Z. The control automatically places an exact stop before running the G1 block, but doesn't stop and instead rounds off the rapid moves by some tiny amount.
...Is this setting 85?

If not, I'm wondering if the rapid roundoff zone is adjustable some other way. Just trying to tinker

[Geof]

How old is your machine? There are differences, below is from an older manual:

Setting 85 and Parameter 134 both affecr corner rounding. Also you can use G187 in a program to override the Setting 85 value.

This is from a more recent manual:

G187 Setting the Smoothness Level (Group 00)
G-187 is an accuraccy command that can set and control both the smoothness and max corner rounding value when cutting a part. The format for using G187 is G187 Pn Ennnn.
P Controls the smoothness level, P1(rough), P2(medium), or P3(finish).
E Sets the max corner rounding value, temporarily overriding Setting 85 "Max Corner Rounding".
Setting 191 sets the default smoothness to the user specified "rough," "medium," or "finish" when G187 is not
active. The "medium" setting is the factory default setting. NOTE: Changing setting 191 to "Finish" will take longer
to machine a part. Use this setting only when needed for the best finish.
G187 Pm Ennnn sets both the smoothness and max corner rounding value. G187 Pm sets the smoothness but
leaves max corner rounding value at its current value. G187 Ennnn sets the max corner rounding but leaves
smoothness at its current value. G187 by itself cancles the E value and sets smoothness to the default smoothness
specified by Setting 191. G187 will be cancelled whenever "Reset" is pressed, M30 or M02 is executed, the
end of program is reached, or E-stop is pressed.

[WallyL7]

I think he is talking about "rapid" moves here, geof. I don't believe that setting 187 does anything for the rapid moves. I know that my newer VF-3SS cuts crazy corners with similar moves to what he is talking about. Never Never never use less than .1" of Z clearance and you should be fine.

We used to get away with .05" of Z clearance on the older Haas', but Z.1 is the new Z.05...lol

[Matt@RFR]

Originally Posted by WallyL7 I know that my newer VF-3SS cuts crazy corners with similar moves to what he is talking about. Never Never never use less than .1" of Z clearance and you should be fine.

Exactly. My '07 VF-2ss will do the same thing with clearance planes of less than .100".

If you really wanted to save time in a cycle, I think the only way to do it is to program all G1 Z moves at your max feedrate. That should let you keep your clearance planes down lower and not lose any time unless it's a BIG retract.

[Andre' B]

That is the basic difference between a rapid and a feed rate move.

Any control has a servo loop update rate, which is how often it checks the measured position and speed against the calculated position and speed and spits out new commands to correct for errors. These loop times are normally something between a 1000 and 10000 times per second. The lower end on the general run of the mill machines and the upper end on machines designed for high speed hard milling.

Since the update rate is fixed the faster things are moving the longer the distance moved between corrections. Feed rate moves are limited to speeds which will make sure the control can keep the tool within some given distance from the programmed path.

In a rapid move path accuracy is not as important as in feed rate moves and so it is traded for more speed.

[Wizzard of H]

The servo update rate has nothing to do with this rounding.
It is all controlled by the mathematics of the planned motion.
If this is a recent brushless control, the G-code positions are picked up at 1 Khz.
The interpollated data for servo is picked up at 4 Khz.
And the torque in the motor is updated at 16Khz.
There is one parameter that is used to decide how close a rapid move must be before the next move can start - it is 101, 102, and 103.
The units are encoder feedback.

[Ydna]

The manual likes to leave out distinctions between G1 and G0 when it comes to some of those settings which control movement (like G187) which is why I asked. I wondered if there was some way to easily control it, naturally for things like tool clearance like everyone correctly assumed.

Yesterday I was trying to draw a comparison for somebody, between the "continuous path" roundoff movements that robots perform, and the rounding off of rapid segments that the CNCs perform. Different robots do it differently, but most transform the movements into an arc segment based on a number you give it for the radius. But then Fanuc's robots come along and want a % value, which is "percent of the programmed speed at which point the roundoff arc will start" and that is blended between any two consecutive motion commands even if the speeds aren't the same. So it's not as much a perfect arc segment as it is an ellipse segment (I like math as much as the next guy, but HOLY GOD!). Anyway the Haas rapid roundoff is definitely speed dependent, or at least when running 100% rapid, the only time you'd want it to bother rounding off? That would make sense.

ah well....back to the drawing board!