Thread: Hole ovality - Fanuc 18i Control

Hello,all!
We are working with Mitsubishi Vertical CNC Machining Center (Fanuc 18i control).
A problem is a hole ovality during circular interpolation XY. A possible backlash was checked and finded O.K.
It looks like either wrong parameter or servo turning.
Any help will be appreciated!
Thanks!
Sol.

Possibly a resolver or encoder connection problem. If there is any quick disconnect cables to the drives, check the cleanliness (oil, water, tarnished) of the pins and sockets in the connectors. With power disconnected of course.

Beyond general cleanliness in the control cabinet, you may have to call on qualified personnel.

Circular interpolating an oval is usually caused by a difference in servo following error between the X and Y servos.

The CNC digitally "counts" its way around a circle, but the servos are always following the CNCs digitally calcuated position with a little "following error". This error is proportional to the speed, and should be exactly equal on X and Y. If the FE is equal, you'll cut a perfect circle.

There is a helpful "servo tuning" screen available on the 18i. To get to this screen, press the "System" key, then the "Right arrow" key below the CRT (on the far right), then the SV.PARA soft-key, then the SV.TUN soft-key.

If your CNC doesn't display have this screen, you can go to parameter 3111 and put a "1" in bit #0 (bit on the far right). If that bit is a zero, the servo tuning screen is not displayed.

Another way to do it is to look at the actual servo following error using the diagnostics. Diagnostic #300 shows the actual following error of the servos. If you jog the X and the Y axes at the same speed, you should get exactly the same following error on each axis. If you don't, some digital servo settings must be adjusted.

If you find a difference between the X and Y following error, I suggest that contact Fanuc or the machine tool builder before you mess around with the digital servo parameters.

it can also be cutter comp programming error

Did this Just show up? How bad is it? I have seen parts rocking in a fixture cause this before. Like Pi said could also be a programing issue. One other thing, what do the quadrant marks look like?

Some more info. would be helpful.

Dave

Has anyone used a G51 scaling command lately? It could still be active.

If you don't get an inch of slide motion (in either axis) when you program a one inch move, look to see if G51 is active. You can cancel it with a G50 in MDI mode.

Hi!
Thanks to all for the replies.
I'm going to check those useful ideas on the machine.
Sol.

There are 3 main causes for the ovality:
- scale mismatch
- servo mismatch
- poor squarness
The scale mismatch means that the machine executes bigger movement in one axis then in the other. The result will be oval with bigger dimension along one of the machine axes. The treatment - pitch error compensation for the machine.

The servo mismatch will produce the oval which is at certain angle to machine axes. I you will change the cutting direction (CW versus CCW) you will get the mirror image of this oval.

The treatment - adjust the axes gain to get the same following error (servo lag).

The poor squarness will give you once more the oval at certain angle to the machine axes, but in this case its "direction" will not change with while changing cutting direction.

The treatment - correct mechanical squarness of the machine.

All those (and many other) machine parameters can be examined in 10 minutes running the Renishaw Ballbar test.

Probe

what kind of machine? glass scales? what did you fix for the backlash? sounds to me like a mechanical problem persists.

Maybe you need to leadin and out on a arc, without doing this you will have an out of round hole.