Re: EMC for lasercutting /urgent

[Max Heise <mahe-at-bandstahlschnitte.de>]

Hi List, Ray, Paul and Jacob

I had the same difficulties here and got around that by writing a
perl script which inserts a G4P0.8 before I "misuse" M3, M4, M5, M7 or M8 as
general purpose IO. However this is not optimal and using free M commands would
be much better. In addition to that it is only possible to controll 3 pins for
you use. If you modify the source code to do this I'd be very interested. Coding
this would involve changing source code from the interpreter on down in almost
all the EMC modules.

If you use the laser be sure to put G61 in your NC program or all your corners
will be rounded smoothly ;-) (looks funny) 

Homing of the just the limit switches is achieved by defining or undefining of
#define NO_HOME_SWITCH 
#define NO_INDEX_PULSE 
#define NO_LIMIT_SWITCH
in extstgmot.c for servos which stg boards, if you use steppers use this as an
example and alter the stepper sources accordingly. And please do not forget to
give back and upload the changes to the CVS repository.

If you do pulse modulation, do you want to switch the laser on/off (which is
done in older laser sources) or do you want to adjust the laser power according
to a signal (a sin for example) ? And just out of curiosity: Which laser
source brand do you use: Rofin, Trumpf, Feha, Spectra Physics and what power ?
And what material do you want to lasercut ? The pulsing could be done in a RT
module which does the modulation on an unused port for the on/off or on and
DAC e.g. for the sin signal and which could be controlled by rt-fifos. Then only
the TkEmc GUI would have to be changed.

If you want to automagically home, play with RS274_STARTUP_CODE in
the [EMC] section of you ini file or use G28/G30 in your NC program and read the
following part from the RS274NGC_NEW documentation:
<quote>
3.5.8 Return to Home - G28 and G30
Two home positions are defined (by parameters 5161-5166 for G28 and parameters 5181-5186 for G30). The parameter values 
are in terms of the absolute coordinate system, but are in unspecified length units.
To return to home position by way of the programmed position, program G28 X- Y- Z- A- B- C- (or use G30). All axis words 
are optional. The path is made by a traverse move from the current position to the programmed position, followed by a traverse move 
to the home position. If no axis words are programmed, the intermediate point
is the current point, so only one move is made. 
</quote>
Note that you still have to home once the EMC is started to get green letters.

Changing the TkEmc is not so hard. If you have a bit of programming practice
you will easily understand the source. I recommend reading Practical Programming
in Tcl and Tk (if you have some spare time left ;-) (~750 pages)).

Regards
Max

> I think with your help offered (thanks for this) I
> will make it. But first, the main problem we should
> focus on is this delay in axis movement after a M3/M5
> or M8/M9 command. I wonder if the "signaling" to the
> GUI of these comands have anything to do with it? If
> this is the problem could an other M command be used
> for switching the laser? To use an "open" M command
> for switching the laser is preferebly anaway. So, how
> can we find out what causes this delay, and how to
> overcome it???


-- 
Max Heise <max.heise-at-gmx.net>
Student Mechatronik/Automatisierungstechnik
PGP public key from:
http://www.fht-esslingen.de/~mahemt01/pgp50i.pub or any keyserver