Eastwood 2x2 "Drill option"

General
1

Hello All New Here,

I have a Eastwood 2x2 and I’m having an issue trying to program a Pierce only or “Drill” function to make a small hole so it can drilled to size later. Has anyone found a work around? I have tried to edit the code after post but it seems to want to ignore it in the controller. Does anyone have a list of what G code it can use? I have tried a G04 P___ to allow the torch to turn on and off before movement but it seems to ignore it.

Thanks For Any Input!

2

@AmgInd , your going to need to make sure your Eastwood pp has the OnDrill() function defined. Here is a plasma ‘drill’ example of it -

function OnDrill()
OnNewEntity()
endZ = drillZ
OnRapid()
currentZ, currentX, currentY = endZ, endX, endY
OnPenDown()
endZ = drillZ
OnMove()
OnPenUp()
endZ = safeZ
OnRapid()
end

The challenge with Eastwood plasma tables is that they typically use a Fangling F2100 or similar controller. That controller manages the pierce height, pierce delay, cut height, feedrate, plunge rate, and cutter compensation from controller input fields. Those parameters do not come from the gcode, the exceptions being feedrate can be overridden if the controller allows it (there is a setting), and cutter comp. You should normally run with NO cutter comp, G40, not G41. Sheetcam already accounts for cutter compensation with outside/inside/no offset toolpath choices.

For ‘drilling’, just use a sheetcam Drill Operation with your plasma tool. The drill op recognizes holes in the designated layer and just makes a pierce.

3

Thanks For The Reply,

I checked the PP in the editor. I do not see any Drill operations listed, just seems like basic operations. FYI I am using the 55132 Eastwood Elite CNC Plasma Sheetcam PP. ( That seems like the only option, I tried to upload a copy here but am a newb so not allowed). It looks like they are using the Starfire SF-2001C controller and I couldn’t find much information on its capabilities or a PP.

I’m Assuming that the option of “drilling” is not possible on this machine? I did check the setting on the machine and haven’t found how to disable built in cutter comp so that may be an issue with in the future. They don’t mention anything in the manual but I may be able to zero out the Kerf to “Bypass” it that way.

Thanks for any input.

4

edit your pp and change the line posting gcode “G41…” to “G40…”

function OnPenDown()
  --post.Text (“G41\nM07\n”) --Left kerf compensation, plasma cut off
  post.Text (“G40\nM07\n”) --no compensation, plasma cut ON
end

Add the OnDrill() function as is shown in prev reply.