I just did a rush retrofit from Torchmate to Mach3 on a customer's Plasma burn table. All is well but all their burn files are missing the M3 and M5 to start and stop the "spindle" (torch in my case).
How do I issue an M3 whenever I am moving in a feed IE G1, G2, G3 and a M5 when leaving feed?

Thanks in advance,

Rocky (Fool_4)

 

YA should have thought about that before you converted it.   

  Many people have ran into that problem when wanting to convert a Torchmate machine.

There is NO easy way to do it short of a PLUGIN written to do that function.
Are you now using a Z axis and floating head to find the TOM (top of material) ?

(;-) TP

Torchmate was losing connection to the sig gen to the point of NEVER WORKING. This works save the one issue. Please do you know who might have this plugin?

Thanks.
 

The COM signal loss would have been an easy fix.  Currently there is NO plugin to do it that I am aware of.

Send me a short test file from the TM so I can test something.

(;-) TP

 
Dang .fgc files isst vertboten?!?!

here is a file with a monkeyed extension.

This customer has literally thousands of burn files they are not one bit happy to edit.

Isn't there a way to see the last g code issued and if a program was running and just fire off an m3 or m5 based on this? The arcok pausing the feed means no relying on ismoving or combined feed I am guessing?

I had to dig WAY back in the OLD notebook for this one(;-). In theory yes you can look at DRO(19)  (GcodeMode) and IF = 1,2or3 then DO a TOM routine and then fire the torch (DospinCW) . AND if Dro(19) = 0 then DoSpinStop() (shut off torch),  IN THEORY. THe problem is in real life MAch3 does not update that dro reliably and MOST times it never changes state. It will in single block mode running 1 line at a time but NOT in run mode processing 1000's of blocks. 

SO you loose control over the process.

NEXT problem the Torchmate files DO NOT have any Z axis motion code in them. That part was handled by the Torchmate Z controller based on THC values and Homed to Z  when the torch was off. You could do some fancy code in the M5 macro to send the torch up to the Zhome (Top of stroke) every time it turns off or to a safe Z value POSITION + SafeZ incremental.

BUT you still have the dro update problem. AS that info was NEVER important to users of Mill/router/Turn that update has a very LOW priority and updates when it has time (maybe) I have seen it run 100s of lines of code and never update.

NOW the answer for them is not in hardware but in Cam software. If I remember correctly it IS possible in SheetCam to do an auto import/export Plugin that can convert a BATCH of files to the Mach3 plasma post of choice.  THEN you NEVER have to worry about MAch3 failing a script again.

(;-) TP

(;-) TP

Here is the torchmate file converted By sheetcam to a Mach3 THC plasma cut file.

N0010 (Filename: Plate w Window.TAP)
N0020 (Post processor: MP1000-THC.scpost)
N0030 (Date: 13/07/2015)
N0040 G20 (Units: Inches)
N0050 G53 G90 G40
N0060 F1
N0070 (Part: Plate w Window)
N0080 (Operation: No Offset, Tool 0 -0.000000 deep, T6: Jet tool)
N0090 M06 T6 F120  (Jet tool)
N0100 G00 X0.4140 Y0.4059
N0110 Z0.1200
N0120 G28.1 Z0.12
N0130 G92 Z0.0
N0140 G00 Z0.0520
N0150 G92 Z0.0
N0160 G00 Z0.1200
N0170 M03
N0180 G04 P1
N0190 G01 Z0.0800 F10.0
N0200 G02 X0.4022 Y0.4177 I0.0004 J0.0122 F120.0
N0210 G01 Y1.2441
N0220 X1.5120
N0230 Y0.3803
N0240 X0.4022
N0250 Y0.4177
N0260 G02 X0.4081 Y0.4236 I0.0064 J-0.0004
N0270 M05
N0280 G00 Z0.5000
N0290 X0.0000 Y0.0040
N0300 Z0.1200
N0310 G28.1 Z0.12
N0320 G92 Z0.0
N0330 G00 Z0.0520
N0340 G92 Z0.0
N0350 G00 Z0.1200
N0360 M03
N0370 G04 P1
N0380 G01 Z0.0800 F10.0
N0390 X0.0110 Y0.0039 F120.0
N0400 X1.9032
N0410 Y1.6205
N0420 X0.0110
N0430 Y0.0039
N0440 Y0.0000
N0450 M05
N0460 G00 Z0.5000
N0470 X0.0000
N0480 M05 M30