What's new
What's new

Problems with G61.1 - Mazak alarm 807 Illegal Format

pauls_boutique

Plastic
Joined
Feb 7, 2020
Hello all. I’m trying to use the G61.1 command for the first time and I keep running into the same alarm. The program runs fine until I come across a line that has all X Y Z I J coordinates, at which point I get the (807 Illegal Format) alarm. The program also runs fine without G61.1 turned on. I’m running MasterCAM 2020 into a 2015ish Mazak VCU500C. Anyone have an idea what I’m missing?

Here’s the relevant parameters from the machine and the offending line of code. F96 was the only parameter I changed from default.

G03 X-1.5278 Y-1.8159 Z-.0284 I.0124 J.128


F3 = 1
F84 = 1
F96 = 01110110
 
Since Mazak describe G61.1 as follows.....

The geometry compensation function (G61.1) is provided to reduce conventional geometry
errors caused by delayed follow-up of smoothing circuits and servo systems.

Makes me wonder if a helical move may not be considered "conventional geometry". Just for giggles, comment out the Z move in your problem line and air cut to test.
 
Can you post the relevant section of your program? It will help understanding what's going on better.

Here's the chunk around it, it's part of an opti-rough toolpath.

Z.0386 F25.
X-1.5678 Y-1.8002 Z.0153
X-1.5463 Y-1.797 Z-.0072
X-1.5387 Y-1.7889 Z-.0184
X-1.53 Y-1.7738 F40.
X-1.5237 Y-1.7555 Z-.0284
G03 X-1.5341 Y-1.5165 I-1.8398 J.0394
G02 X-1.5359 Y-1.4478 I3.7995 J.1356
G01 X-1.5364 Y-1.4439 Z-.0264
X-1.5462 Y-1.4323 Z-.0184
G03 X-1.5689 Y-1.4412 I-.0069 J-.0158 F200.
X-1.5703 Y-1.4479 I.0158 J-.0069
G01 X-1.5734 Y-1.8001
X-1.5735 Y-1.8197 Z-.0283 F40.
G03 X-1.5278 Y-1.8159 Z-.0284 I.0124 J.128
G01 X-1.5264 Y-1.8112 Z-.0259
X-1.5268 Y-1.7966 Z-.0184
X-1.5382 Y-1.7144 F200.
G03 X-1.5623 Y-1.6928 I-.0248 J-.0034 F40.
G01 X-1.5679 Y-1.6927 Z-.0178
X-1.5848 Y-1.6922 Z-.0042
X-1.5873 Z.0316
Z.034 F500.

Since Mazak describe G61.1 as follows.....

The geometry compensation function (G61.1) is provided to reduce conventional geometry
errors caused by delayed follow-up of smoothing circuits and servo systems.

Makes me wonder if a helical move may not be considered "conventional geometry". Just for giggles, comment out the Z move in your problem line and air cut to test.

I was thinking something along these lines too, but I couldn't figure out how to get MasterCAM to not put the Z move in. There's plenty of other helixes in the program, but I don't think they have both X and Y coords. I'll give it a shot tomorrow, it happens about an hour into a 3 hour program.
 
No alarm if I take the Z move out of the offending line, it's the helixes causing the alarm. I'll try another program when I have time next week.
 
You can absolutely use G61.1 with helixes, I use G61.1 for all milling operations. I'm wondering if it's a rounding error as posted from that line. G61.1 is forcing the machine to follow the path more accurately, so if it sees it's going to violate the path or if the arc coordinates aren't perfect you will get alarms. Now the weird thing is, you normally wouldn't get an illegal format alarm like that, you'd get an illegal arc data alarm. It's only moving a 0.0001 in Z as well on that line as well which is strange.
 
For shits and giggles, I just posted out this simple helix milling operation of a 1" hole out of Esprit and ran it in the air on a VCN. No alarms.

N1 (SPIRAL HOLE)
T1 M6 (3/4 EM)
S2546 M3
G54
G0 G90 X.025 Y0.
G0 G43 H1 Z.1
G61.1
G1 G94 Z0. F20.37
Y-.1
G3 G17 X.125 Y0. I0. J.1
X.125 Y0. Z-.05 I-.125 J0.
X.125 Y0. Z-.1 I-.125 J0.
X.125 Y0. Z-.15 I-.125 J0.
X.125 Y0. Z-.2 I-.125 J0.
X.125 Y0. Z-.25 I-.125 J0.
X.125 Y0. Z-.3 I-.125 J0.
X.125 Y0. Z-.35 I-.125 J0.
X.125 Y0. Z-.4 I-.125 J0.
X.125 Y0. Z-.45 I-.125 J0.
X.125 Y0. Z-.5 I-.125 J0.
X.125 Y0. Z-.55 I-.125 J0.
X.125 Y0. Z-.6 I-.125 J0.
X.125 Y0. Z-.65 I-.125 J0.
X.125 Y0. Z-.7 I-.125 J0.
X.125 Y0. Z-.75 I-.125 J0.
X.125 Y0. Z-.8 I-.125 J0.
X.125 Y0. Z-.85 I-.125 J0.
X.125 Y0. Z-.9 I-.125 J0.
X.125 Y0. Z-.95 I-.125 J0.
X.125 Y0. Z-1. I-.125 J0.
X.125 Y0. I-.125 J0.
X.025 Y.1 I-.1 J0.
G1 Y0.
Z.1
G64
G53 Z0.
M5

That would also be equivalent to this operation using G2/G3 with a "P" command for the number of revolutions. Not relevant to our discussion, but just as an FYI.
G61.1
G1 G94 Z0. F20.37
Y-.1
G3 G17 X.125 Y0. I0. J.1
X.125 Y0. Z-1. I-.125 J0. P20
X.125 Y0. I-.125 J0.
X.025 Y.1 I-.1 J0.
G1 Y0.
 
You can absolutely use G61.1 with helixes, I use G61.1 for all milling operations. I'm wondering if it's a rounding error as posted from that line. G61.1 is forcing the machine to follow the path more accurately, so if it sees it's going to violate the path or if the arc coordinates aren't perfect you will get alarms. Now the weird thing is, you normally wouldn't get an illegal format alarm like that, you'd get an illegal arc data alarm. It's only moving a 0.0001 in Z as well on that line as well which is strange.

I just tried this simple program like the one you posted, same alarm on the first helix line. We're going to talk to Mazak about it sometime this week, we don't have any issues using G61.1 on our Makino.

O0001(HSTEST2)
G00G17G20G40G80G90
G91G28Z0.
N1T5M06(0.49945FLATENDMILL)
G00G17G90G54X0.Y0.S10000M03
G43H5Z6.
G94
G61.1
G05P2
G01Z3.1F500.
Z3.F60.
G03Y.2003I0.J.1001F120. <-----807 ILLEGAL FORMAT
Y-.2003Z2.95I0.J-.2003
Y.2003Z2.9I0.J.2003
Y-.2003Z2.85I0.J-.2003
Y.2003Z2.8I0.J.2003
Y-.2003Z2.75I0.J-.2003
Y.2003Z2.7I0.J.2003
Y-.2003Z2.65I0.J-.2003
Y.2003Z2.6I0.J.2003
Y-.2003Z2.55I0.J-.2003
Y.2003Z2.5I0.J.2003
Y-.2003Z2.45I0.J-.2003
Y.2003Z2.4I0.J.2003
Y-.2003Z2.35I0.J-.2003
Y.2003Z2.3I0.J.2003
Y-.2003Z2.25I0.J-.2003
Y.2003Z2.2I0.J.2003
Y-.2003Z2.15I0.J-.2003
Y.2003Z2.1I0.J.2003
Y-.2003Z2.05I0.J-.2003
Y.2003Z2.I0.J.2003
Y-.2003I0.J-.2003
Y.2003I0.J.2003
Y0.I0.J-.1002
Y.2003I0.J.1001
Y-.2003I0.J-.2003
Y.2003I0.J.2003
Y-.2003Z2.045I0.J-.2003
Y.2003Z2.09I0.J.2003
Y-.2003Z2.135I0.J-.2003
Y.2003Z2.18I0.J.2003
Y-.2003Z2.225I0.J-.2003
Y.2003Z2.27I0.J.2003
Y-.2003Z2.315I0.J-.2003
Y.2003Z2.36I0.J.2003
Y-.2003Z2.405I0.J-.2003
Y.2003Z2.45I0.J.2003
Y-.2003Z2.495I0.J-.2003
Y.2003Z2.54I0.J.2003
Y-.2003Z2.585I0.J-.2003
Y.2003Z2.63I0.J.2003
Y-.2003Z2.675I0.J-.2003
Y.2003Z2.72I0.J.2003
Y-.2003Z2.765I0.J-.2003
Y.2003Z2.81I0.J.2003
Y-.2003Z2.855I0.J-.2003
Y.2003Z2.9I0.J.2003
Y-.2003Z2.945I0.J-.2003
Y.2003Z2.99I0.J.2003
X-.1287Y.1534Z3.I0.J-.2003
X0.Y0.I.0643J-.0767
G01Z3.25F500.
Z6.
G05P0
G64
M19
G91G00G28Z0.
G28Y0.
G28X0.
G90
M30
%
 
Can you try running the code I posted in the air? That should determine if it's an issue with G61.1 itself or your post format.

Your code ran OK, so I reran mine without the G05 commands and that appears to be the cause of the alarm. I was under the impression that G61.1/G05 were tied together, but it looks like G05 is a high speed machining option that we don't have. Thanks for the help!
 
According to my Mazak Smooth programming manual, helical interpolation is not available in high speed smoothing mode / high speed machining mode G5 P2.
 
According to my Mazak Smooth programming manual, helical interpolation is not available in high speed smoothing mode / high speed machining mode G5 P2.

I just tried both variants of my test program with G05 P2 added and they both ran fine. You are not allowed to use most modal commands while G05 is active, such as G17/G18 for plane selection or G94/G95 for feed mode. That would give an illegal format. You also can't use cutter compensation, but there aren't many scenarios where finish milling would benefit from adding G05 anyway.
 








 
Back
Top