Category: Basic Configuration
Here's a detailed HOWTO for this config, also added to the attachment together with modified gcodetools for this config.
Pasted from the README:
May,26, 2014, Peja, Republic of Kosovo Europe
by Toma
This is a fully functional configuration file for Linuxcnc to be used
with any and all of the "simple THC" systems on sale, like:
-Proma Elektronika Compact THC (tested and verified on production machines)
-Cand CNC LCTHC should work with minor editing of files mentioned and explained below
All that output "UP""DOWN""ARCOK" signals even those that normaly use 2 parallel ports
can be made to work with only 1 parallel port if you can manage the changes in wiring
and change the pins in the config files.
This setup is configured with slightly relaxed timings so can be used even on older
systems and systems with lattency problems with a bit of trial and error.
It is based on the "thc_300" config found bundeled with Linuxcnc but it is heavily
modified to my needs and since in it's original form it does not work due to feed errors.
Some more info.
The config works flawlessly so here are some functions that were already implemented and
some added.
0- IT does not need 2 parallel ports, just a single one. Granted you don't use limit
switches.
1- Absolutely noo need for Z axes anything, so remove anything related to Z axis in Gcode
since it will slow down the execution waiting for it, but it will not efect the axes,
the machine WILL function properly even if you have Z values.
2- The floating switch, if it trips while running in auto mode, it will force an E-stop
and halt the machine so try to make the floating switch as sensitive as posible, if the
nozle dives into material it will stop everything.
3- It will remember last position so even on power loss you can continue exactly where it
left. I added this since where i live power outs are very frequent so it is a life
saver (or material and time saver in this case).
4- If the plasma cutter stops for any reason (mine beeing heat due to running full time
doing 11meter cut 3 second pause and again 11 meters and..........10 hours a day) it
will stop movement and try to fire the torch several times and wait for ARCOK. To
continue just press F9 and do a right click and "run from here" over the highlighted
gcode line. The Z axis will again find the metal and move up and fire the torch and
continue as usual.
5- No need for a post processor at all, exept if you need "lead in and lead out",
so NO G38.2 or whatever, nothing. Everything works with M3, finding the metal, moving
to pierce height firing the torch and moving on.
I have added the "gcodetools" for "inkscape" with modications needed for outputing gcode
with only M3 and M5 for every cut.
Some tips on editing attached files :
-Use a text editor like "gedit" or "vi" or "nano" or "notepad" in windows, do not use
word procesors.
-Add a "#" sign (shift+3) without quotes in front of any line you dont need, and remove
the same sign in front of any line you need.
-Always have a copy of all config files set as "read only" for safety if something goes
wrong during editing.
Before you start, be sure to check the "parport addres" and the output pins for motor
drives in the "thc_parport.hal" file, see picture "thc_parport.hal.png".
The "thc_parport.hal" has only the outputs for motor controls ( step and direction pins )
with added lines for reverse direction of any of the axes if it need be. There are
settings for 4 axes although i use 3. Check your output pins and edit this file based on
your setup. The standard pin order should be (yours may vary) :
-pin 2 Xstep
-pin 3 Xdir
-pin 4 Ystep
-pin 5 Ydir
-pin 6 Zstep
-pin 7 Zdir
etc etc
Next change the pins in the "thc.hal" file to match the "UP","DOWN","ARCOK","TORCH ON" signals.
You need to check for positive or negative input signals and change that based on the break
out board you are using. See picture "thc_hal.png". There are already lines for positive AND
negative type inputs, you just need to omit the ones you don't need and remove # in front
of the ones you need.
Also you need to change the "scale" "velocity" and "acceleration" in "Axes Section" in
the "thc_toma.ini" file to mach your setup. See picture "thc_toma.ini.baseperiod.png" and
"thc_toma.ini.velocity.accel.png".
For "scale" i use "40" since i have full step drives connected to 200 step/rev
(1.8 degre/step) motors attached to 5mm/rev ballscrews. This is simple
math: steps per rev/mm per rev, in my case 200/5=40.
For "velocity" use anything between 30 and 100 that your setup can handle without
loosing steps or stalling. The value is mm per second so 30 is 1800mm/minute
and 100 is 6000mm/minute.
FYI do this for each AXIS separatly or just use a value that is below the maximum
your setup can handle to be on the safe side. For actual cutting on a plasma the
maximum usable speed is about 4200mm/minute for cutting a 1mm thick mild steel plate,
in this case that would be a value of 70 for "velocity".
For "acceleration", again depending on your setup, put 300 to 800, that is mm/s squared,
but for geting sharp corners you need at least 500 if cutting under 3mm thick
plates, 300 for 4 to 6mm thick plates and 100 if cutting anything over 10mm. But if
your setup can handle 300 and above just leave it there, do not change this.
This config also remembers last machine position so if the machine is not moved while
powered off, you can continue from where it left. This is done since where i live
power outs are a normal occurence.
Regards,
Tom
