Z on the same line with an ,I,J,or K.

[HEAVY METAL]

I'm getting a error at the control it is a fanuc control .

Is this a fanuc issue or a post edit. I don't want to post this thing point to point. Got me scratching my head. I 've tried a few things but no luck

 

 

N8054 G01 X.5958 Y.291 Z-.1612

N8055 G03 X.5934 Y.2959 Z-.1611 I-.0668 J-.0307~~~~~~~~~~~~~~~~~~~~~~~~~~~~

N8056 X.5749 Y.3303 I-7.3227 J-3.9044

[Matthew Hajicek - Singularity]

I believe not all controls will handle helical interpolation. Depending on what op you're doing we may be able to change settings to avoid it without going point to point. More info?

[?Mark]

What's the error? Running in High Speed mode by any chance?

[HEAVY METAL]

yes Mark

[Allan]

Helix is an option on the older controls 6M 10M 0M ect.

I've not had issues with any current machines running Helixes

 

Your code shows a very small arc move.

The change in X is .0024

The change in Y is .0049

The change in Z is only .0001

 

I would look in your control deninition under tolerances and set the minimum arc length to like .01" the default is something like .0005" (way too small IMHO)

 

In the arc settings set the error checking to length of arc.

 

 

 

Allan

[?Mark]

You likely have a helix option in regular mode then, but when in High Speed (hpcc or similar) mode it (helix) used to be a separate option. Turn it off and re-run it the program, see if that helps. If that's it then point to point is your only option when using high speed...

[HEAVY METAL]

Thanks Mark I try that the .Control is 16m

[HEAVY METAL]

Allen my control def was set to arc length but i loosened up the tol to .01 and will give it a try

[HEAVY METAL]

now my Question is should I run high speed mode (hpcc) or use filter in mastercam highspeed toolpaths and shut the high speed mode off in the control

[?Mark]

hpcc will allow you to run significantly faster and it'll make a huge difference while surfacing...but the programs will get a lot bigger with point to point moves...

[Allan]

Is it alarm #28?

 

For Fanuc 16i

 

Check parameter 8485 bit 2. If it is zero helical interpolation is disabled in hpcc mode. Change it to a 1 to enable it.

 

 

HTH

 

Allan

 

From the Fanuc Manual:

 

NOTE

1 G00, auxiliary functions, subprogram call (M98, M198), and macro

call M and T codes can be specified in the HPCC mode only when

bit 1 of parameter MSU No. 8403 is 1. If these codes are specified

when MSU is not 1, an alarm is issued.

(Alarm No.5012 for G00 and alarm No.9 for auxiliary functions and

subprogram calls)

2 To specify the following functions in HPCC mode, the following

parameters are required. Specifying any of the following functions

without setting the corresponding parameter causes an alarm.

Helical interpolation : Parameter G02 (No.8485*)

(Alarm to be issued: No.28)

Involute interpolation : Parameter INV (No. 8485)

(Alarm to be issued: No.10)

Scaling, coordinate rotation : Parameter G51 (No. 8485)

(Alarm to be issued: No.10)

Canned cycle, rigid tapping : Parameter G81 (No.8485)

(Alarm to be issued: No.5000)

[HEAVY METAL]

Allan it is a 16 m

the alarm is # 28

I'm going to see if I can find that parameter

[?Mark]

I think you're out of luck on this control.

[HEAVY METAL]

Parameter #8485 is not the same on the 16m.

[HEAVY METAL]

another question if I untick output 3d arc moves on the transition parameters in the highspeed toolpths will this take care of my problem or will the filter have to be off also on all toolpaths

[?Mark]

Filter off only when using hpcc should take care of it.