Manual tool change + tool lengh touch off

More
10 years 3 months ago #77103 by hancock
Replied by hancock on topic Manual tool change + tool lengh touch off

orangecat wrote:

hancock wrote: I looked into my gcode and i found that after every tool change

Code:
N60 G43 Z15. H1


That's the problem. G43 H1 will reset the tool offset that the touch-off set, to be the tool offset stored in the tool table for tool 1.
By removing G43 H1, all should work well. I don't know if you want to move to Z15 at this point. Maybe not, in which case the entire line can be removed.


Thanks for all the help! It seems that it was indeed the problem. I removed the H and Z values before but the G43 was constantly resetting the offset. Took some time to figure out how to remove the code from the post-processor but know I can work again :woohoo:

And if anyone has the same problem, this is the line I removed from the "linuxcnc.cps"-post-processor:
Code:
writeBlock(gMotionModal.format(0), gFormat.format(43), zOutput.format(initialPosition.z), hFormat.format(lengthOffset));

Thanks again & great community!

Please Log in to join the conversation.

More
10 years 3 months ago #77159 by orangecat
Replied by orangecat on topic Manual tool change + tool lengh touch off
Great it's all working now.
For reference, because it's lost in the middle of this thread, the link to the manual tool change code can be found here:
forum.linuxcnc.org/forum/10-advanced-con...h-off?start=30#48235

Please Log in to join the conversation.

More
10 years 3 months ago #78147 by hancock
Replied by hancock on topic Manual tool change + tool lengh touch off
Hello,

It's me again and I stumbled upon another problem with the routine.

When I use a 1mm bit again during a file, I get the error that the "Move in line 120 would hit the positive limit of Joint 2".
The line 120 in the file "too-change.ngc" is:

G53 G1 F[#<_TravelFeed>] Z[#5183 - #<_ToolZLast> + #<_ToolZ>] ( return to where we were in Z, ajusting for tool length change )


As far as I understand it, the problem is that the newly adjusted hight of the Z-axis is somehow colliding with my limits but I have now idea why because when I run the program again, the Z-hight is correctly adjusted and I get no error.

I don't want to mess around in that part of the code but it would be great if I could get it to work properly because right now I have to remove all line pre the current step from my Gcode. The offset is still correct.

Thanks for any suggestions!
Cheers,
Hancock

Please Log in to join the conversation.

More
10 years 3 months ago #78148 by orangecat
Replied by orangecat on topic Manual tool change + tool lengh touch off
that code from earlier:

N60 G43 Z15. H1


really should have been replaced with:

N60 Z15.


that would (typically) move the tool above the work before a tool change so that a shorter tool wouldn't give a limit error when moving back.

Please Log in to join the conversation.

More
10 years 3 months ago #78149 by hancock
Replied by hancock on topic Manual tool change + tool lengh touch off

orangecat wrote: that code from earlier:

N60 G43 Z15. H1


really should have been replaced with:

N60 Z15.


that would (typically) move the tool above the work before a tool change so that a shorter tool wouldn't give a limit error when moving back.


I replaced the code in my post-processor so I don't have the "G43" and "H1" in my gcode anymore. But it still happens...

For example this is my code
Code:
% (CAGE) (T17 D=1. CR=0. - ZMIN=-0.5 - SCHAFTFRSER) (T21 D=0.5 CR=0. - ZMIN=-0.2 - SCHAFTFRSER) N10 G90 G94 G17 G91.1 N15 G21 N20 G53 G0 Z0. (0.5 SENKFRSEN) N25 M9 N30 T21 M6 N35 T17 N40 S42000 M3 N45 G54 N50 M9 N60 G0 X-6.495 Y-5.65 N65 G0 Z15. N70 Z1.95 N75 G1 Z0. F250. N80 X-6.47 N85 G3 X-6.445 Y-5.625 I0. J0.025 N90 X-6.545 Z-0.05 I-0.05 J0. F20. N95 X-6.445 Z-0.1 I0.05 J0. N100 X-6.545 Z-0.15 I-0.05 J0. N105 X-6.445 Z-0.2 I0.05 J0. N110 X-6.545 I-0.05 J0. N115 X-6.445 I0.05 J0. N120 X-6.47 Y-5.6 I-0.025 J0. F250. N125 G1 X-6.495 N130 G0 Z5. N135 X-0.022 Y5.638 N140 Z1.95 N145 G1 Z0. F250. N150 X-0.034 Y5.616 N155 G3 X-0.025 Y5.582 I0.022 J-0.013 N160 X0.025 Y5.668 Z-0.05 I0.025 J0.043 F20. N165 X-0.025 Y5.582 Z-0.1 I-0.025 J-0.043 N170 X0.025 Y5.668 Z-0.15 I0.025 J0.043 N175 X-0.025 Y5.582 Z-0.2 I-0.025 J-0.043 N180 X0.025 Y5.668 I0.025 J0.043 N185 X-0.025 Y5.582 I-0.025 J-0.043 N190 X0.009 Y5.591 I0.013 J0.022 F250. N195 G1 X0.022 Y5.612 N200 G0 Z5. N205 X6.517 Y-5.613 N210 Z1.95 N215 G1 Z0. F250. N220 X6.504 Y-5.591 N225 G3 X6.47 Y-5.582 I-0.022 J-0.012 N230 X6.52 Y-5.668 Z-0.05 I0.025 J-0.043 F20. N235 X6.47 Y-5.582 Z-0.1 I-0.025 J0.043 N240 X6.52 Y-5.668 Z-0.15 I0.025 J-0.043 N245 X6.47 Y-5.582 Z-0.2 I-0.025 J0.043 N250 X6.52 Y-5.668 I0.025 J-0.043 N255 X6.47 Y-5.582 I-0.025 J0.043 N260 X6.461 Y-5.616 I0.012 J-0.022 F250. N265 G1 X6.474 Y-5.637 N270 G0 Z15. N280 M5 N285 G53 Z0. (1.0 KONTUR 1) N290 M9 N295 M1 N300 T17 M6 N305 T21 N310 S42000 M3 N315 M9 N325 G0 X6.239 Y-6.903 N330 G0 Z15. N335 Z5. N340 G1 Z-0.05 F50. N345 X6.241 Y-6.896 Z-0.088 N350 X6.247 Y-6.875 Z-0.121 N355 X6.256 Y-6.844 Z-0.142 N360 X6.266 Y-6.807 Z-0.15 N365 X6.293 Y-6.711 F400. N370 G3 X6.224 Y-6.588 I-0.096 J0.027 N375 G2 X5.547 Y-5.944 I0.271 J0.963 F70. N380 G1 X1.753 Y-3.753 N385 G3 X1.637 Y-3.764 I-0.05 J-0.087 N390 G2 X-1.637 I-1.637 J1.889 N395 G3 X-1.753 Y-3.753 I-0.066 J-0.076 N400 G1 X-5.547 Y-5.944 N405 G2 X-7.443 Y-5.306 I-0.948 J0.319 N410 X-6.297 Y-4.645 I0.948 J-0.319 N415 G1 X-2.503 Y-2.454 N420 G3 X-2.455 Y-2.349 I-0.05 J0.087 N425 G2 X-0.817 Y0.488 I2.455 J0.474 N430 G3 X-0.75 Y0.582 I-0.033 J0.095 N435 G1 Y4.964 N440 G2 X0.75 Y6.286 I0.75 J0.661 N445 Y4.964 I-0.75 J-0.661 N450 G1 Y0.582 N455 G3 X0.817 Y0.488 I0.1 J0. N460 G2 X2.455 Y-2.349 I-0.817 J-2.363 N465 G3 X2.503 Y-2.454 I0.098 J-0.019 N470 G1 X6.297 Y-4.645 N475 G2 X6.693 Y-6.605 I0.198 J-0.98 N480 X6.224 Y-6.588 I-0.198 J0.98 N485 G3 X6.101 Y-6.657 I-0.027 J-0.096 F400. N490 G1 X6.073 Y-6.753 N495 X6.063 Y-6.79 Z-0.142 N500 X6.054 Y-6.821 Z-0.121 N505 X6.048 Y-6.842 Z-0.088 N510 X6.046 Y-6.849 Z-0.05 N515 X6.239 Y-6.903 N520 Z-0.2 F50. N525 X6.241 Y-6.896 Z-0.238 N530 X6.247 Y-6.875 Z-0.271 N535 X6.256 Y-6.844 Z-0.292 N540 X6.266 Y-6.807 Z-0.3 N545 X6.293 Y-6.711 F400. N550 G3 X6.224 Y-6.588 I-0.096 J0.027 N555 G2 X5.547 Y-5.944 I0.271 J0.963 F70. N560 G1 X1.753 Y-3.753 N565 G3 X1.637 Y-3.764 I-0.05 J-0.087 N570 G2 X-1.637 I-1.637 J1.889 N575 G3 X-1.753 Y-3.753 I-0.066 J-0.076 N580 G1 X-5.547 Y-5.944 N585 G2 X-7.443 Y-5.306 I-0.948 J0.319 N590 X-6.297 Y-4.645 I0.948 J-0.319 N595 G1 X-2.503 Y-2.454 N600 G3 X-2.455 Y-2.349 I-0.05 J0.087 N605 G2 X-0.817 Y0.488 I2.455 J0.474 N610 G3 X-0.75 Y0.582 I-0.033 J0.095 N615 G1 Y4.964 N620 G2 X0.75 Y6.286 I0.75 J0.661 N625 Y4.964 I-0.75 J-0.661 N630 G1 Y0.582 N635 G3 X0.817 Y0.488 I0.1 J0. N640 G2 X2.455 Y-2.349 I-0.817 J-2.363 N645 G3 X2.503 Y-2.454 I0.098 J-0.019 N650 G1 X6.297 Y-4.645 N655 G2 X6.693 Y-6.605 I0.198 J-0.98 N660 X6.224 Y-6.588 I-0.198 J0.98 N665 G3 X6.101 Y-6.657 I-0.027 J-0.096 F400. N670 G1 X6.073 Y-6.753 N675 X6.063 Y-6.79 Z-0.292 N680 X6.054 Y-6.821 Z-0.271 N685 X6.048 Y-6.842 Z-0.238 N690 X6.046 Y-6.849 Z-0.2 N695 X6.239 Y-6.903 N700 Z-0.35 F50. N705 X6.241 Y-6.896 Z-0.388 N710 X6.247 Y-6.875 Z-0.421 N715 X6.256 Y-6.844 Z-0.442 N720 X6.266 Y-6.807 Z-0.45 N725 X6.293 Y-6.711 F400. N730 G3 X6.224 Y-6.588 I-0.096 J0.027 N735 G2 X5.547 Y-5.944 I0.271 J0.963 F70. N740 G1 X1.753 Y-3.753 N745 G3 X1.637 Y-3.764 I-0.05 J-0.087 N750 G2 X-1.637 I-1.637 J1.889 N755 G3 X-1.753 Y-3.753 I-0.066 J-0.076 N760 G1 X-5.547 Y-5.944 N765 G2 X-7.443 Y-5.306 I-0.948 J0.319 N770 X-6.297 Y-4.645 I0.948 J-0.319 N775 G1 X-2.503 Y-2.454 N780 G3 X-2.455 Y-2.349 I-0.05 J0.087 N785 G2 X-0.817 Y0.488 I2.455 J0.474 N790 G3 X-0.75 Y0.582 I-0.033 J0.095 N795 G1 Y4.964 N800 G2 X0.75 Y6.286 I0.75 J0.661 N805 Y4.964 I-0.75 J-0.661 N810 G1 Y0.582 N815 G3 X0.817 Y0.488 I0.1 J0. N820 G2 X2.455 Y-2.349 I-0.817 J-2.363 N825 G3 X2.503 Y-2.454 I0.098 J-0.019 N830 G1 X6.297 Y-4.645 N835 G2 X6.693 Y-6.605 I0.198 J-0.98 N840 X6.224 Y-6.588 I-0.198 J0.98 N845 G3 X6.101 Y-6.657 I-0.027 J-0.096 F400. N850 G1 X6.073 Y-6.753 N855 X6.063 Y-6.79 Z-0.442 N860 X6.054 Y-6.821 Z-0.421 N865 X6.048 Y-6.842 Z-0.388 N870 X6.046 Y-6.849 Z-0.35 N875 X6.239 Y-6.903 N880 Z-0.4 F50. N885 X6.241 Y-6.896 Z-0.438 N890 X6.247 Y-6.875 Z-0.471 N895 X6.256 Y-6.844 Z-0.492 N900 X6.266 Y-6.807 Z-0.5 N905 X6.293 Y-6.711 F400. N910 G3 X6.224 Y-6.588 I-0.096 J0.027 N915 G2 X5.547 Y-5.944 I0.271 J0.963 F70. N920 G1 X1.753 Y-3.753 N925 G3 X1.637 Y-3.764 I-0.05 J-0.087 N930 G2 X-1.637 I-1.637 J1.889 N935 G3 X-1.753 Y-3.753 I-0.066 J-0.076 N940 G1 X-5.547 Y-5.944 N945 G2 X-7.443 Y-5.306 I-0.948 J0.319 N950 X-6.297 Y-4.645 I0.948 J-0.319 N955 G1 X-2.503 Y-2.454 N960 G3 X-2.455 Y-2.349 I-0.05 J0.087 N965 G2 X-0.817 Y0.488 I2.455 J0.474 N970 G3 X-0.75 Y0.582 I-0.033 J0.095 N975 G1 Y4.964 N980 G2 X0.75 Y6.286 I0.75 J0.661 N985 Y4.964 I-0.75 J-0.661 N990 G1 Y0.582 N995 G3 X0.817 Y0.488 I0.1 J0. N1000 G2 X2.455 Y-2.349 I-0.817 J-2.363 N1005 G3 X2.503 Y-2.454 I0.098 J-0.019 N1010 G1 X6.297 Y-4.645 N1015 G2 X6.693 Y-6.605 I0.198 J-0.98 N1020 X6.224 Y-6.588 I-0.198 J0.98 N1025 G3 X6.101 Y-6.657 I-0.027 J-0.096 F400. N1030 G1 X6.073 Y-6.753 N1035 X6.063 Y-6.79 Z-0.492 N1040 X6.054 Y-6.821 Z-0.471 N1045 X6.048 Y-6.842 Z-0.438 N1050 X6.046 Y-6.849 Z-0.4 N1055 G0 Z15. N1065 M9 N1070 G53 Z0. N1075 M30 %

Thanks a lot for your help and routine - other than that, it works like a charm!!

Please Log in to join the conversation.

More
10 years 3 months ago #78150 by orangecat
Replied by orangecat on topic Manual tool change + tool lengh touch off
OK. So the problem is very likely that there's a G53 Z0. before the tool change. which positions the tool at the machine Z coordinate of 0. If 0 is the limit of the machine's Z coordinate and If there's any change in tool height (the wrong way) then the tool change can't return the tip of tool to the exact same position after it's changed.

It should be safe to remove this G53 Z0. as it appears to be a part of the tool change routine and there's no X,Y movement that follows.

Alternatively you could just remove the offending line:

G53 G1 F[#<_TravelFeed>] Z[#5183 - #<_ToolZLast> + #<_ToolZ>] ( return to where we were in Z, adjusting for tool length change )

from tool-change.ngc .

Please Log in to join the conversation.

More
10 years 3 months ago #78152 by hancock
Replied by hancock on topic Manual tool change + tool lengh touch off
Thank you so much - this actually seems to have been the problem! T H U M B S U P ;)

Please Log in to join the conversation.

More
10 years 2 months ago #78330 by clunc
Replied by clunc on topic Manual tool change + tool lengh touch off
I was eager to do this, but while reconfiguring it, I guessed that it's designed to work for tool changes within one program; that is, it won't work as intended if M600 is called before the first, roughing, program and M6 is called in a second, separately loaded, finish program.

But it [was] only a guess [EDIT: and it was WRONG. Read on.]. Can you comment whether it's true or not? And if true, if an adjustment might be made to accommodate the different approach?

Thank you.

(I have to separate passes because the immensity of them put together is too much for the memory.)

Please Log in to join the conversation.

More
10 years 2 months ago #78333 by orangecat
Replied by orangecat on topic Manual tool change + tool lengh touch off
It's designed to work with tool changes across many programs:

send M600 command
load first file which should contain 1 or more M6 commands.
run it.
load next file which may contain 0 or more M6 commands.
run it.
repeat loading next files and running them until job is complete.

unless you issue another M600 command to indicate start of job, all following files are considered to be part of the same job and may contain M6 commands.

Please Log in to join the conversation.

More
10 years 2 months ago #78359 by clunc
Replied by clunc on topic Manual tool change + tool lengh touch off
@Orange Cat

Thank you. It is now transparent, even to this blockhead.

(And it is going to change my life...)

EDIT: It changed my life all right. :S It is Aug. 18. It was only two weeks ago that I got it working, preparatory to doing the first real job on a new machine. However, the rest of the preparations were equally intense, causing me to FORGET ALL ABOUT HAVING SET THIS UP! This is my Keystone-Kops account of chasing my tail trying to figure out WHY my machine seems possessed and acting on its own--moving to a location that's NOT EVEN IN MY CODE! :blush: Turns out transparency is a double-edged sword. (My memory's never been the same since watching Memento...)

Please Log in to join the conversation.

Time to create page: 0.127 seconds
Powered by Kunena Forum