[johndjmix]

So, ive learned to make good bolt holes you need to slow the speed way down, and turn THC off. Well, I modified the candcnc POST for sheetcam, and well...it works. I combined code from a few files to make this. Still messing with it but its made a BIG difference in cut quality of small holes.

Here it is:

function OnAbout(event)
ctrl = event:GetTextCtrl()
ctrl:AppendText("johns CNC plasma Settings!!!\n")
ctrl:AppendText("plasma MP1000-THC post processor\n")
ctrl:AppendText("\n")
ctrl:AppendText("Modal G-codes and coordinates\n")
ctrl:AppendText("Comments enclosed with ( and )\n")
ctrl:AppendText("M03/M05 turn the torch on/off\n")
ctrl:AppendText("Incremental IJ - set in mach2\n")
ctrl:AppendText("The torch is referenced at cut start and every 500mm of movement thereafter\n")
ctrl:AppendText("Designed for use with Mach3 and CandCNC MP1000-THC and Floating head Touch-n-Go\n")
ctrl:AppendText("Post variables:\n")
ctrl:AppendText("refdistance - set the distance between each reference\n")
ctrl:AppendText("switchoffset - set your net switch offset amount \n")
end


--post.SetOptions(post.ARC_SEGMENTS)


-- created 1/1/06
-- Based on plasma1.post



function OnInit()

post.SetCommentChars ("()", "[]") --make sure ( and ) characters do not appear in system text
post.Text (" (Filename: ", fileName, ")\n")
post.Text (" (Post processor: ", postName, ")\n")
post.Text (" (Date: ", date, ")\n")
if(scale == metric) then
post.Text (" G21 (Units: Metric)\n") --metric mode
else
post.Text (" G20 (Units: Inches)\n") --inch mode
end
post.Text (" G53 G90 G40\n F1\n")
minArcSize = 0.2 --arcs smaller than this are converted to moves

dist = 9999999
refdistance = 10* scale
--Put your switch offset value here
switchoffset =.3704
lastz = 0
-- set the radius when to go slow and turn off thc
-- radius's above this number will be cut normally
-- Not sure exactly what the slowradius number represents
-- It cant be the radius of the circle in inchs???
-- But i can see if you want it to work on smaller holes RAISE the slowradius
slowradius = 8 * scale

-- Speed you want it to go when it slows down. .3 = 30% normal speed
slowspeed = .3
end

function OnNewLine()
post.Text ("N")
post.Number (lineNumber, "0000")
lineNumber = lineNumber + 10
end


function OnFinish()
endZ = safeZ
OnRapid()
endX = 0
endY = 0
OnRapid()
post.Text (" M05 M30\n")
end

function OnRapid()
dist = dist + math.hypot(endX-currentX , endY-currentY)
post.ModalText (" G00")
post.ModalNumber (" X", endX * scale, "0.0000")
post.ModalNumber (" Y", endY * scale, "0.0000")
post.ModalNumber (" Z", endZ * scale, "0.0000")
post.Eol()
end

function OnMove()
dist = dist + math.hypot(endX-currentX , endY-currentY)
post.ModalText (" G01")
post.ModalNumber (" X", endX * scale, "0.0000")
post.ModalNumber (" Y", endY * scale, "0.0000")
post.ModalNumber (" Z", endZ * scale, "0.0000")
post.ModalNumber (" F", feedRate * scale, "0.0###")
post.Eol()
end

function OnArc()
dist = dist + math.hypot(endX-currentX , endY-currentY)
radius = math.hypot(endX - arcCentreX,endY-arcCentreY) * scale
-- johns mod to slow down feedrate and turn thc off for tight holes
if (radius < slowradius) and (math.abs(arcAngle) > 0.5) then
--feed = (radius / slowradius)
feed = slowspeed
if(feed < slowspeed) then feed = slowspeed end
feed = feed * feedRate
post.ModalText (" m101")
post.Eol()
else
feed = feedRate
post.ModalText (" m102")
post.Eol()

end


if(arcAngle <0) then
post.ModalText (" G03")
else
post.ModalText (" G02")
end
post.NonModalNumber (" X", endX * scale, "0.0000")
post.NonModalNumber (" Y", endY * scale, "0.0000")
post.ModalNumber (" Z", endZ * scale, "0.0000")
post.Text (" I")
post.Number ((arcCentreX - currentX) * scale, "0.0000")
post.Text (" J")
post.Number ((arcCentreY - currentY) * scale, "0.0000")
post.ModalNumber (" F", feed * scale, "0.0###")
post.Eol()
end


function OnPenDown()
if(dist >= (refdistance/scale)) then
dist = 0
-- modaltext (" G00")
-- text(" Z")
-- number (pierceheight * scale, "0.0000")
-- eol()
post.ModalText(" G28.1 Z")
post.Number(3 * scale, "0.00")
post.Eol()
post.ModalText(" G92 Z0.0\n")
post.ModalText (" G00")
post.Text(" Z")
post.Number (switchoffset, "0.0000")
post.Eol()
post.ModalText(" G92 Z0.0\n")
post.ModalText (" G00")
post.Text(" Z")
post.Number (pierceHeight * scale, "0.0000")
post.Eol()
else
post.ModalText (" G00")
post.Text(" Z")
post.Number (pierceHeight * scale, "0.0000")
post.Eol()
end
if (preheat > 0) then
post.Text ("\n G04 P")
post.Number (preheat,"0.###")
post.Eol()
end
post.Text ("\n M03\n")
if (pierceDelay > 0) then
post.Text (" G04 P")
post.Number (pierceDelay,"0.###")
post.Eol()
end
end


function OnPenUp()
post.Text (" M05\n")
if (endDelay > 0) then
post.Text (" G04 P")
post.Number (endDelay,"0.###")
post.Eol()
end
end


function OnNewOperation()
post.Text (" (Process: ", operationName, ")\n")
if (plungeRate <= 0) then
post.Warning("WARNING: Plunge rate is zero")
end
if (feedRate <= 0) then
post.Warning("WARNING: Feed rate is zero")
end
end

function OnToolChange()
post.Text (" M06 T")
post.Number (tool, "0")
post.ModalNumber(" F",feedRate * scale,"0.#")
post.Text (" (", toolName, ")\n")
end

function OnNewPart()
post.Text(" (Part: ",partName,")\n");
end

function OnDrill()
OnRapid()
OnPenDown()
endZ = drillZ
OnMove()
OnPenUp()
endZ = safeZ
OnRapid()
end

[xalky]

Hey John; Awesome! Does it work as a regular post when no small holes are present? In other words, could this post be used on all files or just those with small holes?

If this is perfected, you should name it, and submit it to sheetcam, and CandCNC support for submission. I'm sure it would be much appreciated by all.

Thanks
Marcel

[Torchhead]

Hey John; Awesome! Does it work as a regular post when no small holes are present? In other words, could this post be used on all files or just those with small holes?

If this is perfected, you should name it, and submit it to sheetcam, and CandCNC support for submission. I'm sure it would be much appreciated by all.

Thanks
Marcel

Problem: Any M command or the THC ON/OFF will cause a "stutter" (pause) in the motion if it comes in the cut path. There are fundamental limitations in MACH that cause this. Not something that you can work around in a POST, Also while detecting small holes and doing an automatic THC OFF has value, it does not cover an even more valuable way to do that with other features (corners, sharp turns, lead outs, etc) .

The THC ON in MACH delay has been solved by putting in the ability in the DTHCII to disable it's outputs but leave the THC Function ON in MACH stopping any Z motion.

Then we needed a transparent way to do that in the middle of a cut not using an M command and suffer the pause. I have been working with MACH to resolve that and I am happy to say that is working well in our Beta testing.

The final piece is to have a way to define an "action point" in SheetCAM to be able to make it break the toolpath and be able to insert cut commands like lowering the feedrate. turning on/off the DTHC signals or (for the lucky guys with new Hypertherms) change the Cut current. It is just a matter of time before we have this piece working.

It is premature to announce anything specific but I will tell you that in a short amount of time there will be a FULL solution from CandCNC. Those of you that haunt my support forum or have your Yahoo profile setup to receive Special Announcements on the forum will be rewarded this week with a couple of eye-openers.

We have a policy at CandCNC about "ideas" for products or even our current development having seen what happens to most projects that get announced too soon. We announce when we have a working product that is ready to move to production.

Stay tuned.....

TOMcaudle
www.CandCNC.com

[xalky]

I can't wait Tom: I just received the HyT connect kit and the rs485 kit for the Hypertherm. In the process of hooking all that up now. Maybe it'll all be ready by the time of your announcement.

Will there be a new post for sheetcam or will all the new features be enabled thru Mach? OR a little of both?

[Torchhead]

I can't wait Tom: I just received the HyT connect kit and the rs485 kit for the Hypertherm. In the process of hooking all that up now. Maybe it'll all be ready by the time of your announcement.

Will there be a new post for sheetcam or will all the new features be enabled thru Mach? OR a little of both?

There will be:

New version of MACH (upgrade)
New Version of SheetCAM
New set of plug-ins, screens and manual

I will build an installer and instruction file to do MOST of the stuff for you.