Fanuc 16i-MB on Robodrill - a couple of issues!

Hi All,

I've recently acquired a Robodrill with a Fanuc 16i-MB controller and have already hit some problems. I have tried searching the forum, but can't quite find what I need or answers were sent via PM so I can't see the resolutions.

Problem 1:
Helical interpolation - I get the "Alarm 021 - illegal plane axis command" despite the format of the G2/G3 movement looking correct and G17 active. I see talk of this being either a missing option or just a parameter change and need to work out which is the case for me. All threads I could find on this ended in a secret pm!? :(

Problem 2:
Jerky movement is 3D surface machining - I need to use High Speed Machining (G05 I believe?), but the controller does not recognise it? Does this mean I don't have this option or just another parameter? How can I find out?

Any help would be very much appreciated! :)

Best Regards
Aussie CNC

Ok, the 1st issue is fixed after a little more digging on here. Parameter 9930 bit #3 set to 1 fixes the problem. Why wouldn't they be setup like this from the factory??

I found the following thread very useful:
http://www.cnczone.com/forums/fanuc/...rameter-2.html

Still struggling with the high speed machining function though, and I little more confused after more reading and testing:

G05 P2 (high speed linear interpolation on)
G05 P0 (function off)
..........This gives me "improper gcode" error, but cannot be used with circular interpolation anyway!? :(

G05 P10000 (High Precision Contour Control)
..........This gives me "improper gcode" error! :(

G05.1 Q1 (Al contour control/nano contour ON)
G05.1 Q0 (function OFF)
..........This gives me the same "improper gcode" error

G05.4 Q1 (High Speed HRV function ON)
G05.4 Q0 (function OFF)
..........This runs, but makes little difference?

G08 P1 (Advanced Preview Control ON)
G08 P0 (function OFF)
..........This runs, but makes little difference?

Anyone doing any high speed cutting on a Robodrill that can share their experience? :)

if you read the top sticky thread 'GE Fanuc & FANUC proprietary posts' you will see it's not a good idea to post option parameters on this forum and the administrator does not like it.

as for 'why would they be set up like this from the factory'........... options are, well, ......... optional. If you want something extra the option needs to be purchased from Fanuc. Your machine simply does not have those options which results in the improper g-code alarm(s).

This thread will probably end in a secret PM also ;-)

Hi,
Thanks for your reply. I guessed HSM would be an option but not helical interpolation, and as I bought this machine second hand, I have no idea of which options it should have!? It seems I can't edit my post to remove the parameter details!? Can an administrator remove anything they feel I shouldn't have posted please?

At this stage I'd just like to know the solution to my HSM issues, as in which G05 or other code someone else is using and whether I need to investigate the purchase of that option!?

I suppose I could be asking too much, but I have seen similar slow/jerky movements solved on other machines (eg Haas, Okuma etc) with the use of a HSM option!?

On Fanuc pretty much everything is an option. Even the manual pulse generator is an option. Of course there are many things required for basic operation and those are provided at the factory. Helical Interpolation is generally not provided unless requested. Same for High Speed Machining. I'll send you a secret PM...... ;-)

A quick update for those that may search later.....

G05.1 Q1 gave me what I was looking for, but the twist is that you have to turn this on before Tool Length Comp (G43).
The format I found worked for me was:

G91 G28 Z0
G90
N1 T12 M6 (12.0 MM DIA MILL)
G90 G40
S10000 M3
G54 G0 X-7.838 Y-11.152
G05.1 Q1
G43 H12 Z10.
G0 Z2.
G1 Z-1. F1000
X-2.182 Y-5.495 F2000
X5.495 Y2.182
....
cutting
....
G05.1 Q0
G28 G91 Z0
G28 G91 X0 Y0
G90
M05
M09
M30

Hope this helps someone else at some point!

Hi fordav11 you can help me ?

I have same problem abot High Speed G5.1. I use Robodrill with a Fanuc 16i-MB controller.
Cam 3d does some F cut to F8, I set it to F1000.
Most of the time that f decreases in the arc.
What parts of the parameters can I modify?
I am using Robodrill T14ia control 16ima.

Thanks.

picture https://ibb.co/nc3SLHK