Circular interpolation slowdown on Fanuc 16i controller

Hello! First post on the forum.
We have multiple Fanuc Robodrills, however the one in question is rather old, a T14iA with a 16i controller. When running a program with G03 the feedrate varies wildly during the arcs, rather than staying at a consistent speed. On the newer Fanucs with 31 controllers, they run the same program smoothly with consistent feedrates, leading to faster cycle times.

The newer Robodrills do show AICC active while running, but I'm not sure if that is what's causing this. Is there a parameter I should be looking for that's inhibiting the 16i machine's feedrate?

Thank you.

does it make round circles?

It does. The tool path is correct and looks the same as if ran on the newer machines, it's just not smooth and consistent feed like on the other machines. For example if it mills circular passes at 50 ipm, when the end mill approaches 9 or 3 oclock points of the circle it may slow down to 20 or 30 ipm, and looks a bit jerky with the movements.

Hi zelostos,

How are you feeding the program? I was running drip feed at 9600 baud and was data starved slowing down the feed rate. Have turned it up to 19200 and now all is fine. this was 3D contouring. Same Machine as you!.

I have the same issue on a t14ia. I made a couple threads about it (please note in the 2nd thread, there was an idiot member clogging up the replies, try to ignore it):

16i-ma robodrill "high speed milling" choppy and slow

Robodrill slows when going around (some) corners.


I also have a similar issue on the same machine, where the machine will show a .0001 distance to go after arriving at the programmed position, see here: Yet another robodrill problem - Distance to go .0001 on milling profile?


Your issue goes away when using g5.1, in my experience. Your machine may or may not have the option enabled.



If you ever run into the distance to go .0001 thing when running high speed tool paths, I've found that the issue is "resolved" if I change G0 to G1. In that picture on that thread, you can see that the line it completed was a G03, with the next line being a rapid in Z. If i change it to a feed in Z, the machine continues on.

Kenre said:

Hi zelostos,

How are you feeding the program? I was running drip feed at 9600 baud and was data starved slowing down the feed rate. Have turned it up to 19200 and now all is fine. this was 3D contouring. Same Machine as you!.

Click to expand...

Not drip feeding. We've run into too many issues in the past so we usually try to run directly from the machine memory.

dandrummerman21 said:

I have the same issue on a t14ia. I made a couple threads about it (please note in the 2nd thread, there was an idiot member clogging up the replies, try to ignore it):

16i-ma robodrill "high speed milling" choppy and slow

Robodrill slows when going around (some) corners.


I also have a similar issue on the same machine, where the machine will show a .0001 distance to go after arriving at the programmed position, see here: Yet another robodrill problem - Distance to go .0001 on milling profile?


Your issue goes away when using g5.1, in my experience. Your machine may or may not have the option enabled.



If you ever run into the distance to go .0001 thing when running high speed tool paths, I've found that the issue is "resolved" if I change G0 to G1. In that picture on that thread, you can see that the line it completed was a G03, with the next line being a rapid in Z. If i change it to a feed in Z, the machine continues on.

Click to expand...

Oof. Wish I hadn't read that second thread. It does seem like the same issue I'm having though, 16i controller circa 1997-1999 Robodrill. I gather you weren't able to find a solution other than the G05.1 workaround? Our two oldest machines don't seem to have that package.

barbter said:

FWIW....the G05 is only a turn-onable option. For the sake of program comparability between all machines, i would say it's well worth doing....

Click to expand...

You're saying it can be turned on? Is it through a parameter? I'd be willing to try it.

I thought I had posted a long reply, but I must have misclicked. In short, it only seems to slowdown on the specific block with the G03 code. My plunging helix also uses G03, but is consistent there. Bolded is where it slows.

T10 M6
M3 S2292
G00 G54 X-0.102 Y0
G43 Z0.5 H10
M8
Z0.17
G01 Z0.07 F20.
G03 Z-0.005 I0.1 J0
I0.1 J0
X-0.0944 Y-0.0383 I0.101 J0 F50.
X-0.0729 Y-0.0709 I0.0934 J0.0383
X-0.0404 Y-0.093 I0.0719 J0.071
X-0.002 Y-0.1011 I0.0396 J0.0934
G01 X-0.0004
G03 X0.0381 Y-0.0934 I-0.0003 J0.1018
X0.0708 Y-0.0717 I-0.0391 J0.0946
X0.0932 Y-0.0389 I-0.072 J0.0731
X0.1015 Y0 I-0.095 J0.0406
X0.0943 Y0.0396 I-0.1036 J0.0017
X0.0726 Y0.0735 I-0.0971 J-0.0382
X0.0393 Y0.0969 I-0.0756 J-0.0723
X-0.0003 Y0.1058 I-0.0425 J-0.0962
G01 X-0.002 Y0.1059
G03 X-0.0427 Y0.0982 I-0.0012 J-0.1055
X-0.0774 Y0.0754 I0.0395 J-0.0981
X-0.1007 Y0.0409 I0.0744 J-0.0754
X-0.1089 Y0 I0.0977 J-0.0409
X-0.1009 Y-0.041 I0.108 J0
X-0.0778 Y-0.0758 I0.1 J0.041
X-0.0431 Y-0.0994 I0.0769 J0.0759
X-0.002 Y-0.1081 I0.0424 J0.0998
G01 X-0.0003
G03 X0.0408 Y-0.0998 I-0.0004 J0.1088
X0.0758 Y-0.0766 I-0.0417 J0.101
X0.0895 Y-0.0603 I-0.0769 J0.078
X0.0997 Y-0.0416 I-0.0909 J0.0619
X0.1061 Y-0.0213 I-0.1012 J0.0433
X0.1085 Y0 I-0.108 J0.023

zelostos said:

You're saying it can be turned on? Is it through a parameter? I'd be willing to try it.

I thought I had posted a long reply, but I must have misclicked. In short, it only seems to slowdown on the specific block with the G03 code. My plunging helix also uses G03, but is consistent there. Bolded is where it slows.

Click to expand...

Hello zelostos,
Of course you won't see the issue with the helical moves, because they are full 360deg moves. From there on the moves are small arcs with a considerable Feed Rate. The issue is that the control can't accelerate the axes to that Feed Rate before it has to decelerate to the end point for the change of direction.

You will have to use a LOOK–AHEAD CONTROL, such as G08.

Regards,

Bill

angelw said:

Hello zelostos,
Of course you won't see the issue with the helical moves, because they are full 360deg moves. From there on the moves are small arcs with a considerable Feed Rate. The issue is that the control can't accelerate the axes to that Feed Rate before it has to decelerate to the end point for the change of direction.

You will have to use a LOOK–AHEAD CONTROL, such as G08.

Regards,

Bill

Click to expand...

Thank you, makes sense about the full movement. I've tried calling for a G08 P1, which is what my manual says, but the result is the same. How do I know if it's properly implementing look-ahead, and should that have smoothed out the feedrate variance?