Hi,
OK, I have used the Mach3Plasma post, and it works. Why not just use that?
You may have noticed that Mach3 toolpaths, with very few exceptions, run in Mach4 and vice versa. The only time Mach4 fails to run Mach3 Gcode
is when one of the shortcuts for which Mach3 was famous for is invoked and Mach4 refuses to play ball. It usually means tweaking the Gcode so that it meets
the more formally defined Fanuc21i for which Mach4 is almost a dead ringer.

Craig

Craig
Relative to, “ OK, I have used the Mach3 Plasma post, and it works. Why not just use that? ”, are you suggesting using the Mach3 Plasma post in Mach4? Or are you saying simply use Mach3 and forget, using Mach4 all together? 

Chuck

Hi,

are you suggesting using the Mach3 Plasma post in Mach4? Or are you saying simply use Mach3 and forget, using Mach4 all together?

My intent was to say use Mach4 but just use the Gcode file that was generated for Mach3. In 99.999% of cases a Mach3 file will run in Mach4 and vice versa.

Craig

Craig,
I tried that and it did not work, but I think it might’ve had something to do with how I have Mach4  configured for spindle start and stop. I need to look into this. 

Chuck

Hi,
this is the Gcode generated by Fusion using the Mach3 Plasma post:

N10 G90
N15 G71

(2D Profile1)
N20 G0 X22.67 Y-2.5
N25 M3
N30 G4 P1.
N35 G1 X27. Y0. F1000.
N40 G3 X-27. I-27. J0.
N45 G3 X27. I27. J0.
N50 G1 X22.67 Y2.5
N55 M5


(2D Profile2)
N60 G0 X184.83 Y-117.5
N65 M3
N70 G4 P1.
N75 G1 X180.5 Y-120.
N80 G2 X180. Y-120.5 I-0.5 J0.
N85 G1 X-180.
N90 G2 X-180.5 Y-120. I0. J0.5
N95 G1 Y120.
N100 G2 X-180. Y120.5 I0.5 J0.
N105 G1 X180.
N110 G2 X180.5 Y120. I0. J-0.5
N115 G1 Y-120.
N120 G1 X184.83 Y-122.5
N125 M5

N130 M30
And there is nothing about it which is alien to Mach4. The only thing is that it uses M3 followed by a G4 P1 to turn the torch on. Have you a properly configured M3
in your profile?

Craig

Craig,
I think our messages are getting crossed in the mail.

Relative to, “ Have you a properly configured M3”

I think that’s what my problem is.

Do you have any insight on how I need to configure M3 for Mach4?

Chuck

Hi,

I have just generated another toolpath for a somewhat smaller part. I ran the Mach3Plasma post and have run the code on my mill. It runs fine, but obviously the spindle turns on
rather than a plasma, but the code runs fine with the correct clearance for the width of the cut.

As to what constitutes an decent m3....well.

Craig

OK, I need to find out how to get my spindle on/off, M3/ M5 configured properly in Mach4

Craig,
 As I understand, in Mach4 M62 and M63 were developed for more precise, laser cutting., Much more precise than M3 and M4.

I was hoping a post processor could be developed for Mark’s for using the M 62 and M63 commands.

Chuck

Hi,
I don't use either Laser or Plasma so I'm having to guess to a certain extent.

m62/m63 are for lasers. It turns the laser on, but ONLY when the machine has started to move, otherwise the laser would burn a spot right at the start. m63/m63 are not right for you.

First thing you may note is that I use lowercase m or lowercase g in all Gcode....because Mach's Gcode interpreter parses all Gcode to lowercase, strips out leading zeros and whitespace. Thus
M03 becomes m3, etc. When the interpreter encounters an M3 for instance its going to search for code starting m3. To make sure it finds it then use its preferred format, ie lowercase and without
leading zeros. Note that I often still use whitespace to separate items for readabilities sake, but should in truth remove whitespace as well so g1x16.67y45.67f556 not g1 x16.67 y 45.67 f556.

When Mach encounters an m3 it will search in the macros folder of the current profile, if it does not find it it will search 'up the file tree' until it does. Normally this means that Mach will
use the built in m3 that turns the spindle one. Presumably the built-in m3 will turn on the SpinOn signal and generate the required PWM to meet the prevailing S word etc. In your case you want
m3 to turn on the torch so you will have to write your own m3() function and put it in the macros folder of your profile. Thus Mach will find and execute your macro BEFORE it searches to find the built-in one.

I would guess you need to code something like:
Function m3()
1) g31 probe the surface of the material
2) Back off the surface of the material by 20mm or so
3) Activate the torch turn on relay.
4) Wait until the ARC_OK signal is received from the plasma. If an ARC_OK signal is not received within 5 seconds....bail ARC_FAIL_YOU_BLOODY_PLONKER.
5) descend to pierce height
6) Wait for the pierce delay
7) Return....this signals that the torch has fired, arc stabilised, pierced and is now ready to cut.

And your m5 would be something like:

Function m5()
1) De-activate the torch relay
2) Lift off the material by 20mm
3) Return

Craig

PS: the ARC_FAIL_YOU_BLOODY_PLONKER is optional!