Just to let everyone on CNC zone I am a tech specialist with Torchmate. I am here to assist in anyway possible.

Hi.
I have to write a driver for a Torchmate plasma machine.
I have written dozens of drivers but all for Routers with Z movement and am having a bit of trouble wrapping my head around a plasma tool.
I am used to raising the tool to Safe Height, travelling to the start point and then plunging into the material.

Are G00/G01 Z moves not required for plasma tools?
Do you just G00 xy to start point, turn the tool on and then G01 xy moves to cut the job.
===================
Also, the machine in question seems to support Plasma and router /engraver tools with tool changing commands.
What happens if the job starts with a Plasme tool, and then callls for a router bit. Do you just start with G00/G01 Z moves at that point.

Hope im not being too vague.


Should have added, is there place to view example gcode for Torchmate machines

G00 (Move at full rapid speed) and G01 (move at a defined feedrate) are common G-code conventions. The same codes are used for plasma. If you have control of the Z in plasma then there are a few changes from doing router/mill type cuts:

G00 to position of pierce point at Z rapid height
G00 down to pierce height (variable based on tip and material)
Fire Torch using conventional M03 command. Torch firing is handled by Output relay.
Delay until you get a valid Arc Good signal or for X sec if no Arc Good avail
Move tip towards material and start XY moves.
At the end of the cut, turn the torch off, delay about 1/2 sec and lift the torch back to safe rapid height.

Since the gaps involved are .080 to .25 for piercing and .040 to .125 for most cutting (gap depends on the material and tip combo and the current you are cutting at). you cannot tolerate much material wappage or the pierce heights will be wrong. Too little gap shortens consummmable life and too much causes missed cuts. Usually some form of surface touch is used to maintain a constant tip to material gap. That part of the move is added before the M03 in the Z.

You can avoid some of this by using a "plate follower" system, (no Torch Height Control) but that has it's own set of problems.

I would like to see a single headed plasma/router machine with a ATC!

Are you tasked with writing g-code for this machine or are you writing a Driver? For what CAM package? It would take the form of a custom Post for their machine.

Torchmate has their own control software and plasma specific CAM as well as similar products for Router. At you need is to develop your artwork in any CAD or Drawing package and transfer in DXF format.

I am confused as to why you need to write a "driver". This is not quite like doing a printer driver or Windows device driver.:confused:

I work for a semi popular software company where people design artwork in our program and then can output to 1001 differant machines. By driver i mean just the part that creates the gcode output. We can and do output in DXF but the request was to create gcode output.

I am mainly used to dealing with routers. So typically we allways send the tool a user specified SafeHeight befor we do any XY moves and lower it to the surface at start point.
I am dealing indirectly with someone at Torchmate who asked us to remove the Z moves as they are unnecessary.
Its no problem for me to remove them. I was just wondering if this was the common procedure with plasma tools.
Is it OK to remove the 3 lines in blue below


M06 T1
G43 H1
G00 Z0.5 <----- I would normally go to safeheight
G00 X0.030 Y0.030
G01 Z0.0 <----- I would NORMALLY go to a user specified depth
M50
G01 X19.033 Y0.030 F90.000
G01 X19.033 Y18.820
G01 X0.030 Y18.820
G01 X0.030 Y0.030
G00 Z0.5 <----- I would normally go to safeheight
M51
G00 X0.000 Y0.000
M02

1. You don't normally have toolchanges in plasma
2. For systems without a full Z and using a THC not integated with the motion software, there is no need for Z moves. The THC takes care of everything including the lifting , piercing, delays and cutting height.
3. It normally triggers off the torch on/off commands.

Cutting with plasma takes a lot of different moves. If they say take out the Z's then I guess they will be handling all of the Z moves and your job is easy.

Tom Caudle
www.CandCNC.com

I am having problems with cutting 5/8 plate at 18"/min. i am getting a lemon shape from a 2.25" circle. Can any one help me. Using T3 hyper 1650 60 amp tip AV 148v.

Regards Carl

Carl,

I run an Hypertherm 1650 too. I recommend operating at a higher amperage i.e. 80 or 100A

Are both the X & Y motors equally calibrated? Has your tech support provided any help?

Tom

There are several factors that can cause poor circular cuts. You will want to do a series of point moves and make sure your table is accurate. In the configuration menu under feedrate/ramping the continous contour should be lower than your program cut speed; generally 80-90 %. What cad package did you create your dxf in? Check the set screws, do you have backlash?

Got the problem sorted out..........Loose grubscrews on geardrive. Oh well, we learn as we go. Had to be something easy as it has been cutting fine.

Tom, I have yet to buy some 80A consumables but I am waiting for a power upgrade before I sink my teeth into some 100A stuff