Post Processor for Mach 3 Plasma Table

[Anonymous]

i need a plasma post for mach3 with thc and touch and go setup. ppllleeeaaasseee help.

[skidsolo]

could you please expalin touch and go setup? We would like to see a sample file your machin will run also.

[Anonymous]

http://proma-elektronika.com/index.php/en/tips/plasma-detekcja-materialu
this is using the G31 macro.
G31 Z-100 F300 this lowered the head from wherever it was sitting and stopped when the probe switch closed.
G92 Z0 Set offset to zero.
G00 Z20 This moved the head back up by the amount of float head travel I have.
G92 Z0 Set offset to zero.
G00 Z1 This raised the head a further millimetre.
Here is the g28.1 ex.
G28.1 version

'M3 Macro for TOM G31 Version
Cfr = GetDro(18)
Code"G28.1 Z0 "
While Ismoving()
Wend
Code"G92 Z0"
While Ismoving()
Wend
Code"G0 Z .080" 'Switch offset
While Ismoving()
Wend
Code"G92 Z0.000"
While Ismoving()
Wend
COde" G0 Z0.120" 'Pierce Height
While Ismoving()
Wend
SetDro(18,Cfr)
While Ismoving()
Wend
DoOemButton(110) 'Fires Torch reset THC height
END

[Anonymous]

I'm also after the same post processor for Fusion360 using the waterjet/Laser/Plasma contour toolpath in CAM. 

basically before each M3 (Cut) it needs G31 to probe plate, G92 probe offset (mine is set at -3) and then move Z to 0. 

[skidsolo]

Would it be possible to post a complete program as well?

[Anonymous · Accepted solution]

Here is a simple program for a 50mm square with a 30mm hole in the centre.

N5 (Program posted with PlasmaG31 Post.pst)
N10 G0  Z10.0000 (RAPID HEIGHT)
N15 G0  X37.2237  Y25.0000
N20 G31 Z-100 (PROBE FOR PLATE)
N25 G92 Z-3.0 (PROBE OFFSET)
N30 G0  Z3.0000 (PIERCE HEIGHT)
N35 Z3.0000
N40 M3(PLasma On)
N45 G4 P1.0000 (PIERCE DELAY)
N50 G1  X38.0368  Y24.1868  F1500.00
N55 G3  X40.0000  Y25.0000  I38.8500  J25.0000
N60  I25.0000  J25.0000
N65  X38.0368  Y25.8132  I38.8500  J25.0000
N70 G1  X37.2237  Y25.0000
N75 M5 (Plasma Off)
N80 G0  Z10.0000 (RAPID HEIGHT)
N85 G0  X-2.7763  Y0.0000
N90 G31 Z-100 (PROBE FOR PLATE)
N95 G92 Z-3.0 (PROBE OFFSET)
N100 G0  Z3.0000 (PIERCE HEIGHT)
N105 Z3.0000
N110 M3(PLasma On)
N115 G4 P1.0000 (PIERCE DELAY)
N120 G1  X-1.9632  Y-0.8132
N125 G3  X0.0000  Y0.0000  I-1.1500  J0.0000
N130 G1  Y50.0000
N135  X50.0000
N140  Y0.0000
N145  X0.0000
N150 G3  X-1.9632  Y0.8132  I-1.1500  J0.0000
N155 G1  X-2.7763  Y0.0000
N160 M5 (Plasma Off)
N165 G0  Z10.0000 (RAPID HEIGHT)
N170 M30

[skidsolo]

Do the Z values in this section of code remain constant for all parts/operations? Can I fix these number in the post so they always remain the same?

N20 G31 Z-100 (PROBE FOR PLATE)
N25 G92 Z-3.0 (PROBE OFFSET)
N30 G0  Z3.0000 (PIERCE HEIGHT)

[Anonymous]

With my setup these values do remain constant. The Pierce Height & The Pierce Delay are variables in the LazyCam Post, I don't vary the height but the delay is varied depending on the thickness of the material being cut.

[Anonymous]

For anyone interested, After a lot of head scratching and trials & error (I have very little programming experience), here is my modified version of the torchmate post processor. This works on my Mach3 controlled plasma table which uses the G31 touch and go setup.  I have added 5 User Defined Properties in the Fusion post window to customise Safe Z Height, G31 Probe Offset, Peirce Height, Peirce Dwell & Cut height. No guarantee it will work for everyone but it does work on my setup.

[El8ias]

Loading in the cnc based plasma cutter this week and using Fusion360 w/ Mach3. A plasma post processor would be very much appreciated. Let me know if you need beta testers towards this endeavor. 

[Anonymous]

I have found a few bugs with the previous Post Processor I made. I have since discovered a better solution for my CNC Plasma table is to use the Torchmate Plasma Post Processor in Fusion (useZ disabled in parameter list). For this to work with Mach3 a couple of macro's need to be added/modified the M50.m1s & M51.m1s in the macros/profile folder (in my case "C:\Mach3\macro\plasma) need to be modified/replaced and the Custom Plasma screen set will need to be loaded as well, peice time, cut height etc can then be adjusted from the custom Mach3 screen. Attached are the macro's and screenset I am currently using with Mach3.

[Anonymous]

I had your post processor working great on my homemade plasma table, Thank you. But just updated fusion360 and now when I post using this same post processor the third line in the code is N30 M8 which for some reason turns on the torch on my machine. Once it does its first touch n go it turns on and off like it should. Before the update the third line was N30 M9. I looked up M8 is to turn on the flood coolant on and M9 is to turn it off. Any suggestions?  Do I have mach3 set up wrong? I've tried to find some where in the tool library in fusion360 where I have something with the plasma and coolant configured wrong with no luck. I've had to go in and modify the g code manually to change it back to M9 to get me by.

[Anonymous]

---

@Anonymous wrote:

I had your post processor working great on my homemade plasma table, Thank you. But just updated fusion360 and now when I post using this same post processor the third line in the code is N30 M8 which for some reason turns on the torch on my machine. Once it does its first touch n go it turns on and off like it should. Before the update the third line was N30 M9. I looked up M8 is to turn on the flood coolant on and M9 is to turn it off. Any suggestions?  Do I have mach3 set up wrong? I've tried to find some where in the tool library in fusion360 where I have something with the plasma and coolant configured wrong with no luck. I've had to go in and modify the g code manually to change it back to M9 to get me by.

---

Hi, I just checked & mine is also now adding a M8 instruction since the fusion update. I had a look through the code and the torchmate post processor has a coolant lookup table, this is due to it being used for both milling a profile cutting but I Think the problem is with the Tool Library in Fusion360. in tool library the post processor tab Milling tools etc have a coolant selection for post processing but cutting tools do not, It seems to me since the update cutting tools have defaulted to flood coolant but there is no coolant drop down selection or parameters to turn it off. Hopfully someone at autodesk can look at this issue. Saying that my table still works fine, a M8 should not turn on you torch, I would say you have a setup or a wiring issue with your machine or Mach3. I suspect you possibly have the same output assigned in Mach for flood coolant and spindle/torch.

Brad

[KerimY]

Hello All,

We are working on the Mach3 Plasma post processor and we would be happy to get some feedback from you before we put it into the library.

Please use the link below to discuss and download it from the Ideastation.

https://forums.autodesk.com/t5/hsm-ideas/post-processor-for-mach-3-plasma-table/idi-p/6702918

[ff_carson_stone]

I know this is an old post but does anyone have troubles with the pierce feature with the mach3 post? I am not getting any pierce height changes after torch fire and am unable to change the pierce delay to anything between 0 and 1 second. Any chance someone using a modified post to correct this would mind sharing it? Thank you in advance!

[Anonymous]

I did not have any trouble with the height change after piercing. If i'm
not mistaken the code was for metric and I had to change it over to US?
could be an issue.

I had a limit switch go bad and constantly give me a changing Z 0, so I
was changing it in fusion when I posted the code.

[Anonymous]

Sorry, I was not able to upload my post driver by email. Hope its attached now.

[ff_carson_stone]

Thank you! That Post solved all of my Z axis issues!