Price CNC AVHC 10 Post Processor Help

buckmaster1967

Buckmaster1967
Hello,

Built from scratch a 6ft x 11ft water table, Nema34 single shaft 1600 oz, 3.5A & driver 7.8A . Dual motors on my gantry.

Z Axis, Nema23 Dual shaft,425oz-in, DM542A 50V+350W-36V, 7" Lead screw floating head.

Hypertherm 45 cutter, Masso 3 axis. Price HVHC 10 Hight Controller.

I have the table cutting decent . But with my lack of CNC experience, learning as I go. Using Inkscape and Sheetcam for all my cutting.

I think I built the table to heavy for thin cutting, lots of weight jerking around. But the reason I am here today my Price HVHC 10 Hight Controller.

With the Price Post processor loaded in Sheetcam. As soon as the table takes of, the Z drive goes up and bottoms out, making the gears jump. I have to hit STOP. The Z drive is going in the wrong direction. If I change the Post processor and use the MASSO post processor with THC. Everything cut decent, except for the torch moving before the torch lights. Not every time. For example. I was cutting out a 4ft x 3ft sign with a dog treeing and the family's name at the top, and welcome to the farm at the bottom. I had to make about 8 cuts of 3in or so where the torch moved before it lite. This is driving me nuts. Any help or advise would be appreciated here in WV, USA
 

masso-support

MASSO Support
Staff member
Hi @buckmaster1967

When you go into screen 6 of the AVHC10 and set the Arc ok, up and down to active do you see the inputs on Masso F1 screen change from normally low to high?

Cheers

Peter
 

buckmaster1967

Buckmaster1967
Hello, Yes. The commands show up when I test the unit, like they should. I end up setting the the Pierce delay in Sheetcam to .5s. and Over cut to 1.0". That helped me with the torch moving before it fires. And the Over Cut helps clean up the late fires, but I know this is not the correct answer

With the Price Post processor loaded in Sheetcam. As soon as the table takes off, the Z drive goes up and bottoms out, making the gears jump. I have to hit STOP. The Z drive is going in the wrong direction. So I can't use it.

I load Masso Plasma (with THC) Post Processor. The Z axes with Go up and down in about 1" of travel. Price HVHC 10 Height Controller. Says on channel 1, to adjust the Tolerance if the torch hunts, but no matter if I adjust it .01 or up to 9.0. The torch still hunts. Without a doubt, My lack of knowledge on the subject is the issue. Any help or suggestions would be appreciated.

Oh, If I go into the Masso Torch Height Control settings, and select (1, Without THC & Arc OK signal) the table cuts good, just no HTC.

If I select (2,Without THC but using Arc OK signal) the table cuts good, just no HTC.

If I select (3, Proma Compact THC Controller 150, the table HTC Controller works, but Z axles Hunts.
 

masso-support

MASSO Support
Staff member
Hi @buckmaster1967

Can you share the start of the Gcode file where the Z axis drives up. I think you will find that there is a G38.2 probing cycle causing the issue.

https://www.masso.com.au/masso-documentation/?section=g38-2-straight-probe-cycle

Please be aware that the Z value specified is a machine coordinate value and not a working coordinate which may be your problem with that.

With regards the hunting are you 100% sure you have the up and down around the right way because i imagine that that would make it hunt something wicked.

Could you also do a simple test. Move your Z axis to the center of it's travel and zero the Z axis. Then type G00 Z-1 and make sure the Z axis moves down. I assume you are using imperial otherwise use G00 Z-25.

If the axis moves up you have it configured backwards which will also be a problem and cause hunting.

Cheers

Peter
 

segoman-designs

SegoMan DeSigns
Quote from Buckmaster1967 on January 3, 2020, 12:41 am

Hello, Yes. The commands show up when I test the unit, like they should. I end up setting the the Pierce delay in Sheetcam to .5s. and Over cut to 1.0". That helped me with the torch moving before it fires. And the Over Cut helps clean up the late fires, but I know this is not the correct answer

With the Price Post processor loaded in Sheetcam. As soon as the table takes off, the Z drive goes up and bottoms out, making the gears jump. I have to hit STOP. The Z drive is going in the wrong direction. So I can't use it.

I load Masso Plasma (with THC) Post Processor. The Z axes with Go up and down in about 1" of travel. Price HVHC 10 Height Controller. Says on channel 1, to adjust the Tolerance if the torch hunts, but no matter if I adjust it .01 or up to 9.0. The torch still hunts. Without a doubt, My lack of knowledge on the subject is the issue. Any help or suggestions would be appreciated.

Oh, If I go into the Masso Torch Height Control settings, and select (1, Without THC & Arc OK signal) the table cuts good, just no HTC.

If I select (2,Without THC but using Arc OK signal) the table cuts good, just no HTC.

If I select (3, Proma Compact THC Controller 150, the table HTC Controller works, but Z axles Hunts.

I was curious if you have any updates on this?
 

buckmaster1967

Buckmaster1967
Quote from MASSO Support on January 4, 2020, 10:25 am

Hi @buckmaster1967

Can you share the start of the Gcode file where the Z axis drives up. I think you will find that there is a G38.2 probing cycle causing the issue.

https://www.masso.com.au/masso-documentation/?section=g38-2-straight-probe-cycle

Please be aware that the Z value specified is a machine coordinate value and not a working coordinate which may be your problem with that.

With regards the hunting are you 100% sure you have the up and down around the right way because i imagine that that would make it hunt something wicked.

Could you also do a simple test. Move your Z axis to the center of it's travel and zero the Z axis. Then type G00 Z-1 and make sure the Z axis moves down. I assume you are using imperial otherwise use G00 Z-25.

If the axis moves up you have it configured backwards which will also be a problem and cause hunting.

Cheers

Peter

Hello,



(Could you also do a simple test. Move your Z axis to the center of it's travel and zero the Z axis. Then type G00 Z-1 and make sure the Z axis moves down. I assume you are using imperial otherwise use G00 Z-25.) I did the test, and the Z axis moved down like it supposed to.

So, with out the HTC, the table cuts great. Cut out a 4ft x 3ft sign last night. Everything worked great. Except the Z axis .It goes to park and stays down when it is when the job is done. Blow water from my table. Sheetcam says to park all axis at (0).

Using the MASSO post processor with THC, I can get the Price Controller to to pierce the metal and start to cut, than raises about an inch above the metal and start to hunt, which I can calm down by adjusting the tolerance on the controller. It will quit hunting, but remain an inch above the metal. Not sure why it won't go to .06" like the setting in Sheetcam.

If I use the plasma AVHC10 post processor, as soon as I hit start, the Z Axis moves up and hits the limit. I found that it is going by the setting in the Sheetcam Job Options where the Rapid Clearance is set to ( 1.5" ) causing the axis to go from Home at 0 to 1.5. The Masso Post Processor , using the same settings goes to 1.5 after the torch goes down and touches the metal zeroing the Z axis then moving up to 1.5"

function OnAbout(event)
ctrl = event:GetTextCtrl()
ctrl:AppendText("plasma AVHC10 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\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 PriceCNC AVHC10\n")
ctrl:AppendText("Post variables:\n")
ctrl:AppendText("refdistance - set the distance between each reference\n")
end

-- revision 3/2/07
-- Removed final safety move. This is now done in SheetCam

-- revision 7/10/05
-- Added new arc handling

-- created 27/10/04
-- 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 S500\n")

switchoffset = 0.752
bigarcs = 1 --stitch arc segments together
minArcSize = 0.05 --arcs smaller than this are converted to moves
end

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

function OnFinish()
post.Text (" M05 M30\n")
end

function OnRapid()
if(math.hypot(endX-currentX , endY-currentY) < 0.001 and endZ < currentZ) then return end
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()
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()
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", feedRate * scale, "0.0###")
post.Eol()
end

function OnPenDown()

post.ModalText(" G31 Z -100")
post.ModalNumber (" F", 500 * scale, "0.0###")
post.Eol()
post.ModalText(" G92 Z0.0\n")
post.ModalText (" G00")
post.ModalNumber(" Z", switchoffset, "0.0752")
post.Eol()
post.ModalText(" G92 Z0.0\n")
post.CancelModalNumbers()
post.ModalText (" G00")
post.ModalNumber (" X", endX * scale, "0.0000")
post.ModalNumber (" Y", endY * scale, "0.0000")
post.ModalNumber (" Z", pierceHeight * scale, "0.0000")
post.Eol()

post.Text ("\n M03\n")
if (pierceDelay > 0.001) 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")
end

function OnComment()
post.Text(" (",commentText,")\n")
end

function OnToolChange()
post.Text (" M06 T")
post.Number (tool, "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

Without doubt, my ignorance of the subject in my biggest issues. I really appreciate all input. Learning everyday, but miles to go.
 

segoman-designs

SegoMan DeSigns
OK thanks for the reply.

I will be in the THC mode in a month or so myself. I'm still tuning motors and making controller cables.
 

buckmaster1967

Buckmaster1967
Quote from MASSO Support on January 20, 2020, 10:37 am

Hi @buckmaster1967
Can you share the Gcode file where the Z axis drives up. I think you will find that there is a G38.2 probing cycle causing the issue.

https://www.masso.com.au/masso-documentation/?section=g38-2-straight-probe-cycle

Please be aware that the Z value specified is a machine coordinate value and not a working coordinate which may be your problem with that.

Regards

Peter

Please see my earlier post . I did share my Gcode.
 

masso-support

MASSO Support
Staff member
Hi Buckmaster1967

I've looked through this thread several times and cannot see your Gcode file.

I can see where you copied the text from a post processor into post 10 but that is all I can see. The Gcode file isn't showing up for me. Could you please repost it.

Cheers

Peter
 

buckmaster1967

Buckmaster1967
Very sorry. This cut out perfect with Masso Post and no HTC. But with the Price Post, Z axis goes up, instead of down.

N0010 (Filename: Treeing Bigger Price Processor.tap)
N0020 (Post processor: Plasma PriceCNC AVHC10 THC zFloat With Pierce Delay- G31.scpost)
N0030 (Date: 20/01/2020)
N0040 G20 (Units: Inches)
N0050 G53 G90 G40
N0060 F1
N0070 S500
N0080 (Part: Treeing Curr Bigger)
N0090 (Process: Inside Offset, white, T3: 45 amp 16g steel - FINE CUT)
N0100 M06 T3 (45 amp 16g steel - FINE CUT)
N0110 G00 X21.8636 Y12.3991 Z1.2500
N0120 G31 Z -100 F19.685
N0130 G92 Z0.0
N0140 G00 Z0.8
N0150 G92 Z0.0
N0160 G00 X21.8636 Y12.3991 Z0.1500
N0170 M03
N0180 G04 P0.5
N0190 G01 Z0.0900 F150.0
N0200 G02 X21.9671 Y12.3291 I-0.1727 J-0.3667 F140.0
N0210 X22.0808 Y12.2033 I-1.4941 J-1.4658
N0220 G01 X22.0869 Y12.1960
N0230 G03 X22.2651 Y12.0002 I2.5464 J2.1375
N0240 G01 X22.2658 Y11.9995
 

Attachments

  • Treeing-Bigger-Price-Pocessor.tap
    121.1 KB · Views: 12

masso-support

MASSO Support
Staff member
Hi Buckmaster1967

I had to cut down your post as it was too long. When posting Gcode files please just upload the file rather than post the entire file as text. I saved it as a separate file but left the start in your post as there are several obvious issues.

I immediately notice some things about your Gcode.
N0100 M06 T3 (45 amp 16g steel - FINE CUT)

This line is a tool change which will cause the Z axis to drive to the top to prepare for a tool change. This appears to be what you are talking about.
N0120 G31 Z -100 F19.685

This line looks like a Mach3 probing command but is unsupported in Masso. Please use G38.2 for your probing cycle.

https://www.masso.com.au/masso-documentation/?section=supported-g-m-codes



Lastly the Gcode does not contain any THC commands M666 or M667 so the THC will not work with this code.

Hope this helps

Cheers

Peter
 
Top