M10/M11 + M3 & plasma

[Robertspark]

Going back to this thread http://www.cnczone.com/forums/uccnc-control-software/316888-feature-suggestion-m10-11-independent-m3.html

Could someone please give me the sequence of operations for the use of M10/M11 for plasma.

Reading that thread,

1) I need m3 to fire the torch as M3 will wait for the ArcOK signal before the pierce delay countdown starts.

2) I know that M11 will deactivate an output synchronously with motion (i.e. I can set sheetcam to overburn 10mm, and add a code snippet which will add M11, 10mm from the end of the cut)

The question is, do I need to add M10 in somewhere?

Can it be on the same line / the next line as M3 to fire the torch?

[in mach3, M10 & M11 were reversed (M11 turned the port on, M10 turned it off), and M11 would only become active providing motion had been given on the next line (i.e. a fudge was to add G0 B1 on the next line after M11, and then G0 B0 after M10 to turn the torch off)...... do I need anything like this? My overburn should take care of uccnc M11 to turn the torch off in sync with motion, but if I have M3 /n M10, the next line is normally G4 Pxxx for the pierce delay.... hence M10 may not be happy without a similar fudge)

[cncdrive]

Rob,

The M3 and M10 and M11 can be in the same line, because they are all macros,
if they are in the same line then they will execute in order from left to right.
There should be no problem with a G4 following a M10.

[beefy]

Hi Robert,

when I was testing UCcnc I found that I had to do M3 before M10 would work. And yes M11 has no meaning if M10 has not been done first. M10 simply turns on the laser output and M11 turns it off. The laser otuput can't be turned off if it hasn't already been turned on

You define output pins for both M3/M5 and M10/M11 (laser output) so then you have the issue of 2 separate outputs to fire the torch. I was (still am if I can find time) going to get around this in my custom THC which would take both inputs but "choose" which output to use for torch fire based on the info it was sent from my serial coms plugin. For example in a certain configuration my THC would listen to M3 to start the torch but listen to M11 to turn the torch off synchronously with motion a mm or two before the end of the cut. Likewise another configuration would listen to M10 to start the torch synchronously with motion. This would be good for when you are cutting open lines in thinner sheet and want to avoid the pierce divot.

Never really thought about how you can get around this with a stock standard UCCNC setup and and off the shelf THC. All my exploits were towards a custom designed THC communicating with UCcnc but I've been forced to put that on hold for now.

Keith.

[shad]

M11 would only become active providing motion had been given on the next line

Hi Robert!
I think you mean synchronized with motion commands M10Px/M11Px or ExP1/ExP0. This is not macros. M10/M11 macros always issue short pause in motion when executed.
I think you have to use M11Px (where x - number of the torch on output, for example if you use Output#1 for torch start in the M3 macros, then Command will be M11P1).
In this case you will have fast cutter off without pauses.
One thing - currently this synchronized with motion commands M10Px/M11Px are supports in Mach3 - LPT port, ESS and UC400ETH controllers.
UC400ETH use own commands with UCCNC software. With Mach3 there is a little bug, but I hope Balazs will solve this.
--Andrew

[Robertspark]

Andrew, there are built in m codes into uccnc which have no pauses for thc motion, if you have a look in the manual, m10/m11 is built into uccnc as are the m200's so they implement without hesitation

Uccnc does not use the px part of the m11px / m10px.... but I came from smooth stepper which only had one m11 output toggle and the px part made no difference as it was coded into the ss setup / config which port you wanted to toggle.

Have a read if the uccnc manual and the mcodes as they have been well thought out and developed where mach3 unfortunately stopped (6 years ago ish)
Rob

[shad]

Oh, I think you said about Mach3. I forgot that this is UCCNC machine forum!!

[cncdrive]

WIth the UCCNC with the current release the M10/M11 macros produce no pause and no slowdown in the motion, they work perfectly syncronous to the motion buffer.
The THC on/off macros caused a slowdown and speedup in the motion in previous releases just like they do in Mach3,
but in the current release of the UCCNC they are also perfectly syncronous to the motion buffer, no more slowdown in the motion.

And Rob is right, the UCCNC has only a single dedicated sync (laser) output controllable with the M10 and M11 macros, the P parameter for the macro is not the port number,
but is a PWM duty cycle value, because the output is a 100kHz base frequency PWM, it gives a solid output if P is 255 or if P is not defined.
Why we produced only a single dedicated sync output is because for the pins which are engaged for this type of output must be masked out from the others,
so it is not possible to make all pins to work as sync outputs. In Mach3 it is possible, because LPT port is accessible from the PC side software directly,
without a motion buffer in between. And Mach3 with a motion controller the M10/M11 causes some delays, so they work only to some level, they are not perfectly syncronous,
there are delays, we could implement it the same way in the UCCNC, but we thought it is much better to have one sync output only, but that is then really syncronous.

Shad: I'm sorry, but I could not check your mach3 code yet, I got a Flu and was not too well in the last few days and my collegues were away on an Expo in the last few days,
but my collegue will check it soon as I sent him the code and description and will let you know the results asap.
So, you are right that Balazs will correct this issue, however not me Balazs ... there are 2 Balazs in our company and we are both programmers.

[shad]

Thanks for the detailed description!
Also do you planned to add ability to select Absolute for IJ Mode.
Just now my cutting program looks like this. I am use Absolute mode for easy way to make Arc Lost Cut Recovery on holes.

[cncdrive]

The screenset looking good.

Currently the UCCNC supports only incremental IJ center point for arcs,
there is yet no option for absolute mode.

[shad]

Oh, I am understand!
Can you add this function to the future request?
Thank you!