if you can get your drill coordinates in a text file,
write a little VB-script with reads the file and
executes the movements.

Thomas

Its easy to write this VB-Script?....I'm noob on codes and programing, i use rhinocam to make the g-codes and a little bit of codes "by hand"....my biggest experience on writing code is on MachTurn.

Ya-Nvr-No

All the cylinder system is already setted, the return is automatic whem the screw is flat on the panel... i was thinking on using dwell to make the delay, but i found on configuration a delay on M8, that is perfect for this "screw" head   My only problem is with offset  

You put the offset on the mach3 config, right?....Them you only put the G54 and G55 with the coordinates of the holes?

Return stroke of your cylinder on a M08 might happen but what turns off the model command M08 other than a M09 or M30? (you have to reset it to use it again) will work but its not industrial robust or efficient. Good luck and have fun.  

You put the offset values in "fixture offsets" you just have to know the difference between the spindle and your cylinder center lines.

I used a limit switch to return the cylinder, i just need a pulse to activate the system, the rest is made by an arduino with some basic program 

I don't remeber my last tests, but if my memory is right the delay ou M8 activate the relay and after a few seconds they "reset" the comand, i think i have the code here of my tests...

Thanks!!!

And Thanks to everyone who posted here helping me with this problem! 

I found here one of the codes i was testing there, i'm using M9 to cancel the M8, but i think this code is before i found the delay on M8, this week i will test again:

"%
N1 G17 G21
N2 G00
N3 T1 M6
N4 G90 G00 X200. Y0. S4851 M3
N5 Z6.
N6 G81 X200. Y0. Z-10.866 F1000. R2.5
N7 G80
     G55 G0X-170Y-83Z0 M8
N8 M9
N9 G00 Z6.
N10 G81 X150. Y0. Z-10.866 F1000. R2.5
N11 G80
     T2 X150. Y0. Z0. M8
N12 M9
N13 G00 Z6.
N14 G81 X100. Y0. Z-10.866 F1000. R2.5
N15 G80 M8
         M9
N16 G00 Z6.
N17 G81 X50. Y0. Z-10.866 F1000. R2.5
N18 G80 M8
         M9
N19 G00 Z6.
N20 G81 X0. Y0. Z-10.866 F1000. R2.5
N21 G80 M8
         M9
N22 G00 Z6.
N23 M5
N24 M30
%"

Quote from: TPS on December 07, 2014, 04:54:33 AM

if you can get your drill coordinates in a text file,
write a little VB-script with reads the file and
executes the movements.

Thomas

Its easy to write this VB-Script?....I'm noob on codes and programing, i use rhinocam to make the g-codes and a little bit of codes "by hand"....my biggest experience on writing code is on MachTurn.

if you need some help to do this VB-script just let me know.

Thomas

Thanks TPS! 

This week i will test all the sugestions here 

Hi guys,

I tried your sugestions but the machine goes crazy, i go on fixtures offset on the "config" menu, put G54 X0 Y0 Z0, on the G55 i put X150 Y50 and Z0 (my mach3 is in millimeter), then i put the G54 and them G55 on the second step, and the machine goes to the center of the machine, goes to X3000 Y1200 or something like that, them i go to the "fixtures offsets" screen and the values change to this crazy numbers...i'm not understanding what's happening  

Fixtures offsets is the only way to do that?....I have to make this work fast and simple...

This is the code i tried:

"%
N1 G17 G21
N2 G00
N3 T1 M6

G54

N4 G90 G00 X200. Y0. S4851 M3
N5 Z6.
N6 G81 X200. Y0. Z-10.866 F1000. R2.5
N7 G80
    G0X-170Y-83Z0 M8
N8 M9
G55
N9 X200. Y0. Z-10.866 F1000. R2.5
N7 G80
   G0X-170Y-83Z0 M8"

Still not sure what your trying to do as your using the same Z move to do two things? Wont one of the heads run into something while they are both going up and down at the same time?

but as far as your numbers I would think your mixing imperial fixture offsets with metric gcode movements
150" * 25.4 = 3810mm and 50" * 25.4 = 1270mm ( that's why your seeing the huge movements)
you might want to make sure you setup units are in metric or use the equivalent value (just some more math).


%
N1 G17 G21
N3 T1 M6
G90
G54
G0 Z6.
S4851 M3
X200. Y0. M8
N6 G81 Z-10.866 F1000. R2.5
N7 G80
M9
G55
X200. Y0.
G1 Z-10.866 F1000.
G0 Z6.
G54
X200 Y0
m30
%


Set your G55 to X100 Y50 and save fixture

Move to the Point of Origin X0Y0 on your material. then Zero the xy axis(that will set the g54 to 0,0)  the example just drills 1 hole then offsets the head and drills another hole in the same spot to prove the offsetting works correctly.



N3 T1 M6

G54

G00 X200. Y0. S4851 M3
N5 Z6.
N6 G81 X200. Y0. Z-10.866 F1000. R2.5
N7 G80
 
(Switch to G55 to offset to the 2nd head)

G55

N9 G81 X200. Y0. Z-10.866 F1000. R2.5
N7 G80
   
G54 ( go back to the original fixture offset)

G0 X0 Y0  (Go back to the original Point of origin)

M5 M9
M30
%

NOW do not get confused by what you see in the toolpath as it does NOT exactly show what the machine is going to do. Just follow the machine tool as it does the job IT will be correct.

NOW as teh first test "I" would drill all the holes first THEN switch to the G55 and finish all the rest.

Then when you get a good grip on using fixture offsets you could try the flip flopping of fixtures at each hole.

Test each senario to SEE which one finishes in the least amount of time.

It may surprise you, (;-) TP