Does M5 Break Blending?

More
14 Jan 2016 13:46 - 23 Jan 2016 23:37 #68368 by Paul
Does M5 Break Blending? was created by Paul
On my plasma table, I am working on the idea of turning off the torch before the end of the cut. Using SheetCAM to produce the code, it will insert an M05 at the point I specify before the end. While watching the actual cut, I see a noticeable stop at the M05 and then the torch moves to the end and lifts.

Should I config and use an M63 to turn off the relay that fires the torch. Would that help give me a torch off with out the stop/hesitation?

Thanks for any direction...

Paul
Last edit: 23 Jan 2016 23:37 by Paul.

Please Log in or Create an account to join the conversation.

More
14 Jan 2016 15:55 #68382 by andypugh

Should I config and use an M63 to turn off the relay that fires the torch. Would that help give me a torch off with out the stop/hesitation?


It should do.

It is relatively easy to try it as a dry-run with sample G-code without actually reconfiguring anything.

Please Log in or Create an account to join the conversation.

More
14 Jan 2016 17:21 #68396 by Paul
Thanks Andy,

I assumed I would need to tie the pin for the torch relay to a motion.digital-out-XX pin in order to control it with a M63

I will try things out next chance I get. Thank you...

Please Log in or Create an account to join the conversation.

More
14 Jan 2016 17:30 #68398 by andypugh
You need to reconfigure to have the output _do_ anything, but LinuxCNC will drive the HAL pin and not care that is isn't connected to anything.

Please Log in or Create an account to join the conversation.

More
15 Jan 2016 08:47 - 15 Jan 2016 08:49 #68434 by Rick G

Should I config and use an M63 to turn off the relay that fires the torch. Would that help give me a torch off with out the stop/hesitation?

That is what I am doing on my plasma table.
To see the difference try...
%
g64p.001 q.001
f100
g0 x0y0
m3
g1 x4 y0
m5
g1 x8 y0
m3
g1 x12 y0
m5
g1 x16 y0
%

and then ...
%
g64 p.001 q.001
g0 x0y0
m62 p0 ;turn on 
g1 x4 y0
m63 p0 ; turn off
g1 x8 y0
m62 p0 ;turn on 
g1 x12 y0
m63 p0 ; turn off
g1 x16 y0
%

Couple of things, you will want to turn the torch on with M62 Pn and then off with M63 Pn.
Also there needs to be a G movement after the M62 / M63 command for it to take effect.

15. M62 - M65 Digital Output Control

M62 P- - turn on digital output synchronized with motion. The P- word specifies the digital output number.

M63 P- - turn off digital output synchronized with motion. The P- word specifies the digital output number.

M64 P- - turn on digital output immediately. The P- word specifies the digital output number.

M65 P- - turn off digital output immediately. The P- word specifies the digital output number.

The P-word ranges from 0 to a default value of 3. If needed the the number of I/O can be increased by using the num_dio parameter when loading the motion controller. See the Motion Section for more information.

The M62 & M63 commands will be queued. Subsequent commands referring to the same output number will overwrite the older settings. More than one output change can be specified by issuing more than one M62/M63 command.

The actual change of the specified outputs will happen at the beginning of the next motion command. If there is no subsequent motion command, the queued output changes won’t happen. It’s best to always program a motion G code (G0, G1, etc) right after the M62/63.

M64 & M65 happen immediately as they are received by the motion controller. They are not synchronized with movement, and they will break blending.
Note
M62-65 will not function unless the appropriate motion.digital-out-nn pins are connected in your hal file to outputs.

linuxcnc.org/docs/html/gcode/m-code.html#mcode:m62-m65

You will then have to edit your SheetCam post processor to use M62/M63 instead of M3/M5.

Rick G
Last edit: 15 Jan 2016 08:49 by Rick G.
The following user(s) said Thank You: Paul

Please Log in or Create an account to join the conversation.

More
15 Jan 2016 11:21 #68441 by Paul
Thanks Rick!

A possible wrinkle for me is that I setup my table to hold motion using an and2 component for both the arc-ok signal and motion.spindle-on pin. Can I use the m62/m63 method and still achieve a hold if I loose the arc-ok signal?

I was going to experiment with this yesterday, but didn't get the chance. Maybe today...

Thanks again...

PK

Please Log in or Create an account to join the conversation.

More
15 Jan 2016 12:30 #68443 by andypugh

A possible wrinkle for me is that I setup my table to hold motion using an and2 component for both the arc-ok signal and motion.spindle-on pin. Can I use the m62/m63 method and still achieve a hold if I loose the arc-ok signal?


You just need to net the and2 input that currently connects to the spindle-on pin to the same signal as the motion.digital-out-00 pin.
The following user(s) said Thank You: Paul

Please Log in or Create an account to join the conversation.

More
15 Jan 2016 12:54 - 15 Jan 2016 13:00 #68446 by Paul
Cool - Thanks Andy!

Edit: That also sounds like I will need to reprogram all existing jobs because those M3/M5 jobs won't run as the new and2 inputs won't be satisfied. Not all current jobs *need* the torch off early.

:whistle: I wonder if I can do simple find and replace of M3/M5 lines with the M62/M63 commands...? I'm not sure that is a safe route :blink:

PK
Last edit: 15 Jan 2016 13:00 by Paul.

Please Log in or Create an account to join the conversation.

More
15 Jan 2016 14:14 #68450 by Todd Zuercher
You could also make a filter script that automatically replaces them when Linuxcnc loads the g-code file.
linuxcnc.org/docs/2.6/html/config/ini_co...l#sub:FILTER-Section
The following user(s) said Thank You: Paul

Please Log in or Create an account to join the conversation.

More
15 Jan 2016 17:21 - 15 Jan 2016 17:22 #68473 by Rick G

Edit: That also sounds like I will need to reprogram all existing jobs because those M3/M5 jobs won't run as the new and2 inputs won't be satisfied. Not all current jobs *need* the torch off early.


Not really. as Andy said I just use an and2 in hal, for the torch to light both M62 and M3 need to be active.
M63 or M5 will turn torch off.

I set the M62 in my light torch sub, (go to pierce height, light torch, go to cut height etc.)
You could also just command a M62 at the beginning of the existing programs and let the M3 and M5 do there thing.

Rick G
Last edit: 15 Jan 2016 17:22 by Rick G.

Please Log in or Create an account to join the conversation.

Time to create page: 0.144 seconds
Powered by Kunena Forum