Error 907 Z Axis travel exceeded (RESOLVED)

All things related to Centroid Oak, Allin1DC, MPU11 and Legacy products

Moderator: cnckeith

mrichards
Posts: 34
Joined: Thu Feb 28, 2019 12:05 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Error 907 Z Axis travel exceeded (RESOLVED)

Post by mrichards »

Hi,

Trying to run a job, getting the 907 error, can't for the life of me figure out why.
I Touched off G54 Z0 using probe (loaded the probe using m6T2H2)
When I try to run the following job it throws a error at line N55 when I hit cycle start

Code: Select all

%
(T22  D=0.25 ZMIN=-0.18 - flat end mill - HELICAL - END MILL FOR STEEL - 4 FLUTE -  VARIABLE PITCH - 0.2500 DIA X 0.500 L)
(T120  D=0.25 TAPER=118deg - ZMIN=-0.2551 - drill - 1/4 Twist Drill)
N10 G90 G94 G17
N15 G20
(Drill1)
(begin job)
N20 G28 G91 Z0.
N25 G90
N30 T120 M6
N35 S1375 M3
N40 G54
N50 G0 X0.75 Y-0.75
N55 G43 Z0.6 H120
N65 Z0.2
N70 G98 G81 X0.75 Y-0.75 Z-0.2551 R0.2 F5.157
N75 X0.4688 Y0.
N80 X0.75 Y0.75
N85 X-0.75
N90 X-0.4688 Y0.
N95 X-0.75 Y-0.75
N100 G80
N105 Z0.6
(Circular1)
N115 G28 G91 Z0.
N120 G90
N125 M1
N130 T22 M6
(0)
N135 S3000 M3
N140 G54
N150 G0 X-0.4688 Y0.
N155 G43 Z0.6 H22
N160 Z-0.1
N165 G1 Z-0.18 F25.
N170 X-0.6625 Y0.025
N175 G3 X-0.6875 Y0. I0. J-0.025
N180 X-0.25 I0.2187 J0.
N185 X-0.6875 I-0.2187 J0.
N190 X-0.6625 Y-0.025 I0.025 J0.
N195 G1 X-0.4688 Y0.
N200 G0 Z0.2
N205 X0.4688
N210 Z-0.1
N215 G1 Z-0.18 F25.
N220 X0.275 Y0.025
N225 G3 X0.25 Y0. I0. J-0.025
N230 X0.6875 I0.2188 J0.
N235 X0.25 I-0.2188 J0.
N240 X0.275 Y-0.025 I0.025 J0.
N245 G1 X0.4688 Y0.
N250 G0 Z0.6
N260 G28 G91 Z0.
N265 G90 G53 X0. Y0.
N270 M30
(end job)
%
If I graph the job no error is thrown
There is plenty of room in Z travel to get to the job Z-min, let alone Z0.6.
All the offsets look good as far as I can tell. If I jog to Z0 (G54) the tool is touching the work.
If I single block through the program I get the error at line N55. When the job halts I can immediately issue "Z0.6" at the MDI and the move is executed without problem.

The Fusion 360 post created the following line:

Code: Select all

N55 G43 Z0.6 H120
After the error, I was wondering if the problem was that the H120 comes after the Z0.6 (trying to move before knowing the tool height?) so I modified the file to:

Code: Select all

N55 G43 H120 Z0.6
I also tried:

Code: Select all

N55 G43 H120 
N56 Z0.6
It made no difference.
Side question; is it typical to issue the H value in the same line after the Z move?

Any Ideas?

Thanks.
Attachments
Screen Capture.JPG
report_0008DC111213-0916201004_2020-12-07_16-00-46.zip
(843.13 KiB) Downloaded 22 times
------------
Mark
cncsnw
Posts: 1892
Joined: Wed Mar 24, 2010 5:48 pm

Re: Error 907 Z Axis travel exceeded

Post by cncsnw »

Interesting. At first glance, I do not see the reason for the error message.
- The Z+ software travel limit is +0.495 (above home)
- The Z- software travel limit is -3.940 (below home)
- The G28 Z position is +0.495 (above home, at the travel limit)
- The G54 part zero location Z coordinate is -0.13847.
This means that a tool with no offset would have to go -0.13847" down from home to reach Z0 (or 0.4615" up to reach Z0.6)
- The H120 offset value is -1.7215.

Therefore, to get to Z+0.6 in G54 with H120 active, the machine would need to move to -0.13847 - 1.7215 + 0.6 = -0.9830. That is within the travel limits.

The order of codes on the line generally does not matter. "G43 H120 Z0.6", or "G43 Z0.6 H120", or "Z0.6 H120 G43" all do the same thing.

You say the error appears "when you hit cycle start". Is that when you hit cycle start the first time, to begin running the job? Or is it the second time or third time, at one of the "Insert Tool" prompts that appears when the M6 tool change runs?

Do you get any different results if you step through the job with "Single Block" turned on?
cncsnw
Posts: 1892
Joined: Wed Mar 24, 2010 5:48 pm

Re: Error 907 Z Axis travel exceeded

Post by cncsnw »

I think the problem is that your M6 macro selected "G91" mode (in order to do the "G28 G91 X0 Y0 Z0" move to the tool-change position), but your CNC program assumed that it was still in G90 mode after the M6.

Because you end the tool change at maximum Z height and (inadvertently) in G91 incremental mode, the "Z0.6" move is trying to move above maximum Z height.

The M6 macro should save the positioning mode (system variable #4003) in a local variable, then restore it after the G28 moves are complete. Otherwise you are depending on your postprocessor to repeat every modal code after a tool change.
RogDC
Posts: 34
Joined: Wed Jan 01, 2020 2:40 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: Error 907 Z Axis travel exceeded

Post by RogDC »

Mark,
I have run into this a few times with a Vectric PP for the Precision Router smoothing and @Swords '3D Relief Fine Router ' smoothing .

What I have experienced is when using G54 WCS offset, when at G54 X-Y '0', I will continue to receive this condition until I jog the my gantry in a negative position to the G54 X-Y '0', then it will work as it should.

I haven't been able to identify what is causing the issue in my situation and when I try to reproduce it and take video of it, I'm not able to intentionally create the issue.
RogDC
Posts: 34
Joined: Wed Jan 01, 2020 2:40 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: Error 907 Z Axis travel exceeded

Post by RogDC »

cncsnw wrote: Mon Dec 07, 2020 6:00 pm

You say the error appears "when you hit cycle start". Is that when you hit cycle start the first time, to begin running the job? Or is it the second time or third time, at one of the "Insert Tool" prompts that appears when the M6 tool change runs?
When I have experienced the issue It occurs when I press Cycle Start after the "Insert Tool" prompt.
mrichards
Posts: 34
Joined: Thu Feb 28, 2019 12:05 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: Error 907 Z Axis travel exceeded

Post by mrichards »

cncsnw wrote: Mon Dec 07, 2020 6:06 pm I think the problem is that your M6 macro selected "G91" mode (in order to do the "G28 G91 X0 Y0 Z0" move to the tool-change position), but your CNC program assumed that it was still in G90 mode after the M6.

Because you end the tool change at maximum Z height and (inadvertently) in G91 incremental mode, the "Z0.6" move is trying to move above maximum Z height.

The M6 macro should save the positioning mode (system variable #4003) in a local variable, then restore it after the G28 moves are complete. Otherwise you are depending on your postprocessor to repeat every modal code after a tool change.
That was the problem. I had modified the m06 macro earlier in the day.
I added the following to fix it (which I poached from the sample on your website - thanks):

Code: Select all

#105 = #4003								;MDR - Save current positioning mode (G90/G91)
...
(rest of macro here)
...
G#105										;MDR - Restore positioning mode
N1000                                     						;End of macro  
cncsnw wrote: Mon Dec 07, 2020 6:00 pm Do you get any different results if you step through the job with "Single Block" turned on?
No error when single blocking through the program, nor when graphing. I assume because the m06 macro is not processed ahead
------------
Mark
Gixer
Posts: 37
Joined: Tue Jun 30, 2020 3:18 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 0324202376

Re: Error 907 Z Axis travel exceeded

Post by Gixer »

I have this same problem on my mill where abouts do you install the code is it installed before the M6 code or at the beginning of all the code.
Cheers.
%
O01001 (Clock Bracket Mount v5.5)
(T1 D=8. CR=0. - ZMIN=-30. - flat end mill)
(T17 D=8.5 CR=0. TAPER=118deg - ZMIN=-40. - drill)
N10 G90 G94 G17
N15 G21
N20 G28 G91 Z0.
N25 G90
(Drill4)
N30 T17 M6
N35 T1
N40 S3000 M3
N45 G54
N50 M8
N60 G0 X-10. Y7.5
N65 G43 Z15. H17
N75 Z5.
N80 G1 Z-30. F1000.
N85 Z-40.
N90 G4 P3.
N95 Z5.
N100 G0 X-65.
N105 G1 Z-30. F1000.
N110 Z-40.
N115 G4 P3.
N120 Z5.
N125 G0 Z15.
N135 G28 G91 Z0.
N140 G90
(2D Contour10)
N145 M9
N150 M1
N155 T1 M6
N160 T17
N165 S2500 M3
N170 G54
N175 M8
N185 G0 X-3.6 Y37.8
N190 G43 Z15. H1
N195 Z5.
N200 G1 Z1. F333.33
N205 Z-2.2
N210 G18 G3 X-4.4 Z-3. R0.8 F1000.
N215 G1 X-5.2
N220 G17 G3 X-6. Y37. R0.8
N225 G1 Y33.448
N230 X2.146 Y23.673
N235 G2 X4. Y18.552 R8.
N240 G1 Y4.
N245 G2 X-4. Y-4. R8.
N250 G1 X-18.5
N255 G2 X-26.5 Y4. R8.
N260 G1 X-48.5
N265 G2 X-56.5 Y-4. R8.
N270 G1 X-71.
N275 G2 X-79. Y4. R8.
N280 G1 Y18.552
N285 G2 X-77.146 Y23.673 R8.
N290 G1 X-69. Y33.448
N295 Y37.
N300 G3 X-69.8 Y37.8 R0.8
N305 G1 X-70.6
N310 G18 G3 X-71.4 Z-2.2 R0.8
N315 G0 Z15.
N320 G17
(2D Contour11)
N325 G0 X-3.6 Y37.8
N330 Z15.
N335 Z5.
N340 G1 Z1. F333.33
N345 Z-26.2
N350 G18 G3 X-4.4 Z-27. R0.8 F1000.
N355 G1 X-5.2
N360 G17 G3 X-6. Y37. R0.8
N365 G1 Y33.448
N370 X2.146 Y23.673
N375 G2 X4. Y18.552 R8.
N380 G1 Y4.
N385 G2 X-4. Y-4. R8.
N390 G1 X-18.5
N395 G2 X-26.5 Y4. R8.
N400 G1 X-48.5
N405 G2 X-56.5 Y-4. R8.
N410 G1 X-71.
N415 G2 X-79. Y4. R8.
N420 G1 Y18.552
N425 G2 X-77.146 Y23.673 R8.
N430 G1 X-69. Y33.448
N435 Y37.
N440 G3 X-69.8 Y37.8 R0.8
N445 G1 X-70.6
N450 G18 G3 X-71.4 Z-26.2 R0.8
N455 G0 Z15.
N460 X-3.6 Y40.8
N465 Z5.
N470 G1 Z1. F333.33
N475 Z-29.2
N480 G3 X-4.4 Z-30. R0.8 F1000.
N485 G1 X-5.2
N490 G17 G3 X-6. Y40. R0.8
N495 G1 Y33.448
N500 X2.146 Y23.673
N505 G2 X4. Y18.552 R8.
N510 G1 Y4.
N515 G2 X-4. Y-4. R8.
N520 G1 X-18.5
N525 G2 X-26.5 Y4. R8.
N530 G1 X-48.5
N535 G2 X-56.5 Y-4. R8.
N540 G1 X-71.
N545 G2 X-79. Y4. R8.
N550 G1 Y18.552
N555 G2 X-77.146 Y23.673 R8.
N560 G1 X-69. Y33.448
N565 Y40.
N570 G3 X-69.8 Y40.8 R0.8
N575 G1 X-70.6
N580 G18 G3 X-71.4 Z-29.2 R0.8
N585 G0 Z15.
N590 G17
N595 M9
N600 G28 G91 Z0.
N605 G90
N610 G28 G91 X0. Y0.
N615 G90
N620 M30
%
mrichards
Posts: 34
Joined: Thu Feb 28, 2019 12:05 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: Yes
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: none

Re: Error 907 Z Axis travel exceeded

Post by mrichards »

I have attached my mfunc6.mac file.
This is the based on the file created by swissi for use with Probeapp / F360.
if you look for "MDR" in the comments, you will see the couple changes I made:

At the beginning of the macro system variable #4003 is read and saved to user variable #105.
System variable #4003 holds the current positioning mode (G90 or G91)

At the end of the macro, the G#105 line restores the positioning mode.

I had caused problems by using a G28 G91 move during tool change, leaving G91 active after the tool change. The next attempted move after the tool change threw the 907 error, which is good as I would have crashed the machine otherwise.
Attachments
mfunc6.mac
(4.62 KiB) Downloaded 10 times
------------
Mark
Gixer
Posts: 37
Joined: Tue Jun 30, 2020 3:18 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 0324202376

Re: Error 907 Z Axis travel exceeded

Post by Gixer »

Thanks for the reply but i`m not sure where i should be looking for the code is it in the post Processor i use in fusion 360.
is it in this section i need to install the command for G90/G91.
Cheers.
// define home positions
var _xHome;
var _yHome;
var _zHome;
if (method == "G28") {
_xHome = toPreciseUnit(0, MM);
_yHome = toPreciseUnit(0, MM);
_zHome = toPreciseUnit(0, MM);
} else {
_xHome = machineConfiguration.hasHomePositionX() ? machineConfiguration.getHomePositionX() : toPreciseUnit(0, MM);
_yHome = machineConfiguration.hasHomePositionY() ? machineConfiguration.getHomePositionY() : toPreciseUnit(0, MM);
_zHome = machineConfiguration.getRetractPlane() != 0 ? machineConfiguration.getRetractPlane() : toPreciseUnit(0, MM);
}
for (var i = 0; i < arguments.length; ++i) {
switch (arguments) {
case X:
words.push("X" + xyzFormat.format(_xHome));
xOutput.reset();
break;
case Y:
words.push("Y" + xyzFormat.format(_yHome));
yOutput.reset();
break;
case Z:
words.push("Z" + xyzFormat.format(_zHome));
zOutput.reset();
retracted = true;
break;
default:
error(localize("Unsupported axis specified for writeRetract()."));
return;
}
}
if (words.length > 0) {
switch (method) {
case "G28":
gMotionModal.reset();
gAbsIncModal.reset();
writeBlock(gFormat.format(28), gAbsIncModal.format(91), words);
writeBlock(gAbsIncModal.format(90));
break;
case "G53":
gMotionModal.reset();
writeBlock(gAbsIncModal.format(90), gFormat.format(53), gMotionModal.format(0), words);
break;
default:
error(localize("Unsupported safe position method."));
return;
Gixer
Posts: 37
Joined: Tue Jun 30, 2020 3:18 pm
Acorn CNC Controller: No
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 0324202376

Re: Error 907 Z Axis travel exceeded

Post by Gixer »

I think i`m sorted now had part of the code missing from the Post Processor will be back if not that and i don`t know why it changed.
Post Reply