Pierce start before Pierce height reached.

[Ribbedgiraffe]

I may be wrong but but mach's list of "M" commands states the M3 is clockwise spindle control but for plasma can be used to send a signal to trigger the torch on. See attached in port and pins under spindle setup M3 can be sent to output #1 and this turns on the torch relay on the table I have worked on.
Not a macro. That is what should happen on line 140 after it had gone to the pierce height of 0.100"
When I run the first 300 line of you g-code that is what happens

M03 is definitely firing the torch using a relay. BUT, During the M03 operation it is also pulling the M3 macro for setting torch height.

[WyoGreen]

I looked a little closer to the posted G-code and I was a little off on my interpretation.
Line N0100 moved the Z axis to 1.25"
Line N0120 moved the X and Y axis to the start point
Line N0130 lowerd the Z to a Pierce height of 0.1"
Line N0140 Fired the torch with the M03
Line N0150 Paused the torch for 0.6 sec.
Line N0160 raised the torch to .06" (which is the cut height)
and then the following lines move the torch around on the cut path.

So line N0130 should be a pierce height of 0.15", which might keep the metal from splashing back on the torch.

All in all, the post is probably ok other than the pierce height.

Steve

[acourtjester]

From what he said and the video he posted the torch is on the metal when it fires, not at pierce height.

[Ribbedgiraffe]

Line 140 M03 senses material height with a macro, and fires the torch when the torch comes in contact with the surface, this is where I'm getting so confused now.

[acourtjester]

here is a video I just made with your G-code, now I changed it a little I did not have it move out to the start point you had.
This was to save material on my part, in you G-code you start with the torch touching the metal you the move up (1.250") and then to the start of the cut.
It drops to .100 for the pierce then to 0.060" for the cut if your metal is warped you will be sitting on the metal at you pierce height.
https://youtu.be/Bo410wwa6wo
In the video I don't move from the point I set Z to zero so if the metal is warped the torch will not know.
You need to change your plan so you set Z to zero move up move to the cut start then use the floating head to find the metal surface to reset Z to zero. the move to pierce height and fire the torch.
That's my story and I'm sticking to it.

[exapprentice]

Well done Tom
great to see someone who is prepared to help, loads of very good info and insite in this thread
wish more would, its a very steep and long learning curve no matter how you go about it
glad I started the journey though

[Ribbedgiraffe]

Well done Tom
great to see someone who is prepared to help, loads of very good info and insite in this thread
wish more would, its a very steep and long learning curve no matter how you go about it
glad I started the journey though

I am very thankful for all the help I have received! Some great people here.
I've got about 10 more hours today trying to figure it out! Probably one of the most complicated tasks I have ever taken on, and have 0 experience with.

[Ribbedgiraffe]

You need to change your plan so you set Z to zero move up move to the cut start then use the floating head to find the metal surface to reset Z to zero. the move to pierce height and fire the torch.
That's my story and I'm sticking to it.

I'm sure you are spot on. I just need to figure out how to change it. This whole Macro thing has me confused , And I think I need to stop focusing on it.
I'm going to sit in the garage for a couple hours with a cup of coffee and beat my head against the keyboard. I'm sure ill be back (Hopefully with positive results)

If you cannot tell already, I am very thankful for all of your help!

[Ribbedgiraffe]

ok.. So I changed the post processor, trying to get around the code issue. Here is the Gcode sheetcam generated. The problem I'm having here is - When I start the program, and it moves to the start point the Z axis climbs all the way until it binds ( I assume this is line 120 looking for a home position, I DO NOT have a home switch.) I'm going to look at installing a switch today. (But that is a whole new adventure). Thoughts on this one?

N0010 (Filename: YJ Winch Top Plate.tap)
N0020 (Post processor: MP1000-THC.scpost)
N0030 (Date: 17/06/2016)
N0040 G20 (Units: Inches)
N0050 G53 G90 G40
N0060 F1
N0070 (Part: YJ Winch Top Plate)
N0080 (Operation: Outside Offset, 0, T10: Plasma, 0.061 in kerf)
N0090 M06 T10 F42 (Plasma, 0.061 in kerf)
N0100 G00 Z0.1575
N0110 X33.7449 Y8.5439
N0120 G28.1 Z0.12
N0130 G92 Z0.0
N0140 G00 Z0.0520
N0150 G92 Z0.0
N0160 G00 Z0.0250
N0170 M03
N0180 G04 P2
N0190 G01 Z0.1100 F42.0
N0200 G02 X33.5195 Y8.5234 I-0.1229 J0.1024
N0210 G01 X30.5195 Y11.0234
N0220 G03 X30.5000 Y11.0305 I-0.0195 J-0.0234
N0230 G01 X3.0000
N0240 G03 X2.9805 Y11.0234 I0.0000 J-0.0305
N0250 G01 X-0.0195 Y8.5234
N0260 G03 X-0.0305 Y8.5000 I0.0195 J-0.0234
N0270 G01 Y-0.0610
N0280 G02 X-0.0610 Y-0.0305 I-0.0305 J0.0000
N0290 G01 X33.5610
N0300 G02 X33.5305 Y-0.0610 I0.0000 J-0.0305
N0310 G01 Y8.5000
N0320 G02 X33.6905 Y8.6600 I0.1600 J0.0000
N0330 M05
N0340 G00 Z0.1575
N0350 X0.0000 Y0.0000
N0360 M05 M30

[acourtjester]

Just remember the we all started at O after a little time working with it you will start seeing things clearer.
I cannot be sure but I think your macro may be part of the post processor you are using. That is where the floating head routine would come in to play too.
this is what is in the post processor to handle the floating head routine. I'm sure there are similar ones in other post processors.

function OnPenDown()
if (preheat > 0.001) then
post.ModalText (" G00")
post.ModalNumber (" Z", cutHeight * scale, "0.0000")
post.Text ("\n G04 P")
post.Number (preheat,"0.###")
post.Eol()
end
post.ModalText (" G00")
post.ModalText ("\n G90F100\n")
post.ModalText (" G28.1 Z0.50\n")
post.ModalText (" G92 Z0\n")
post.ModalText (" G0 z0.16\n")
post.Text (" Z")
post.Number (pierceHeight * scale, "0.0000")
post.Text ("\n M03\n")
if (pierceDelay > 0.001) then
post.Text (" G04 P")
post.Number (pierceDelay,"0.###")
post.Eol()
end
end

I just copy and pasted this into a Mach 3 plasma post processor and remove the original "0npendown" section Rename the post processor for storage.
This will automatically put this in the G-code at the start of each cut so it will move Z to home (switch trip) and zero Z postition then move tot he pierce height.

[acourtjester]

You may have the Z home set to up not down that is done in the homing/limits under config.
put your Z in the middle of its travel and hit Z home (diagnostic page Ref Z) watch which way it goes if down its ok if up change the setting.
Plasma homes Z down mill home Z up??????

[acourtjester]

I see a few problems with the post processor you are using.
remove lines 140 & 150 change 160 to GoZ0.160. this will be your pierce height.
and change 190 to G01 Zo.060 f42 this will be your cut height

[Ribbedgiraffe]

Just remember the we all started at O after a little time working with it you will start seeing things clearer.
I cannot be sure but I think your macro may be part of the post processor you are using. That is where the floating head routine would come in to play too.
this is what is in the post processor to handle the floating head routine. I'm sure there are similar ones in other post processors.

function OnPenDown()
if (preheat > 0.001) then
post.ModalText (" G00")
post.ModalNumber (" Z", cutHeight * scale, "0.0000")
post.Text ("\n G04 P")
post.Number (preheat,"0.###")
post.Eol()
end
post.ModalText (" G00")
post.ModalText ("\n G90F100\n")
post.ModalText (" G28.1 Z0.50\n")
post.ModalText (" G92 Z0\n")
post.ModalText (" G0 z0.16\n")
post.Text (" Z")
post.Number (pierceHeight * scale, "0.0000")
post.Text ("\n M03\n")
if (pierceDelay > 0.001) then
post.Text (" G04 P")
post.Number (pierceDelay,"0.###")
post.Eol()
end
end

I just copy and pasted this into a Mach 3 plasma post processor and remove the original "0npendown" section Rename the post processor for storage.
This will automatically put this in the G-code at the start of each cut so it will move Z to home (switch trip) and zero Z postition then move tot he pierce height.

Ill try this now, I just spent the last few hours trying to get it back to where it was when I started..

[Ribbedgiraffe]

ok - So I've tried cutting and pasting the code into the post processor setting, Now it does not recognize the limit switch for material height.. Here is the code that was generated.

N0010 (Filename: YJ Winch Top Plate.tap)
N0020 (Post processor: Mach3 plasma scott h.scpost)
N0030 (Date: 17/06/2016)
N0040 G20 (Units: Inches)
N0050 G53 G90 G91.1 G40
N0060 F1
N0070 S500
N0080 (Part: YJ Winch Top Plate)
N0090 (Operation: Outside Offset, 0, T10: Plasma, 0.061 in kerf)
N0100 M06 T10 F42.0 (Plasma, 0.061 in kerf)
N0110 G00 Z0.5000
N0120 X33.7449 Y8.5439
N0130 G90F100
N0140 G28.1 Z0.50
N0150 G92 Z0
N0160 G0 z0.16
N0170 Z0.0990
N0180 M03
N0190 G04 P2
N0200 G01 Z0.1100 F42.0
N0210 G02 X33.5195 Y8.5234 I-0.1229 J0.1024
N0220 G01 X30.5195 Y11.0234
N0230 G03 X30.5000 Y11.0305 I-0.0195 J-0.0234
N0240 G01 X3.0000
N0250 G03 X2.9805 Y11.0234 I0.0000 J-0.0305
N0260 G01 X-0.0195 Y8.5234
N0270 G03 X-0.0305 Y8.5000 I0.0195 J-0.0234
N0280 G01 Y-0.0610
N0290 G02 X-0.0610 Y-0.0305 I-0.0305 J0.0000
N0300 G01 X33.5610
N0310 G02 X33.5305 Y-0.0610 I0.0000 J-0.0305
N0320 G01 Y8.5000
N0330 G02 X33.6905 Y8.6600 I0.1600 J0.0000
N0340 M05
N0350 G00 Z0.5000
N0360 M05 M30

[Ribbedgiraffe]

In the last string of code I posted, I switched line 140 to G31, away from G28. At least now it is trying to probe to find material height. Even doing this, the torch still fired right as the torch made contact with the work surface, the exact moment the limit switch triggered..

[Ribbedgiraffe]

ok... I feel like I'm finally getting somewhere.. The Macro is no longer necessary since I changed the post processor (Thank you acourtjester) The torch no longer fires while the Macro is trying to determine height. (This is a huge relief). I did have to make a change away from G28 in your provided post processor mod and switch to G31 command because this for some reason would not acknowledge my limit switch. BUT with this mod, I'm getting two Z axis commands on the same line, straight out of Sheetcam. (Hoping for an easy solution)
Here is the modified code I have in my post processor.

function OnPenDown()
if (preheat > 0.001) then
post.ModalText (" G00")
post.ModalNumber (" Z", cutHeight * scale, "0.0000")
post.Text ("\n G04 P")
post.Number (preheat,"0.###")
post.Eol()
end
post.ModalText (" G00")
post.ModalText ("\n G90F100\n")
post.ModalText (" G31 Z-3 F20")
post.ModalText (" G92 Z0\n")
post.ModalText (" G0 z0.16\n")
post.Text (" Z")
post.Number (pierceHeight * scale, "0.0000")
post.Text ("\n M03\n")
if (pierceDelay > 0.001) then
post.Text (" G04 P")
post.Number (pierceDelay,"0.###")
post.Eol()
end
end



NOW - Using this code, I'm getting 2 commands for the z axis, on Line 150 (See below) (I trimmed the code @ 200 since my issues are in piercing)

N0010 (Filename: Unmodified code.tap)
N0020 (Post processor: Mach3 plasma scott h.scpost)
N0030 (Date: 17/06/2016)
N0040 G20 (Units: Inches)
N0050 G53 G90 G91.1 G40
N0060 F1
N0070 S500
N0080 (Part: YJ Winch Top Plate)
N0090 (Operation: Outside Offset, 0, T10: Plasma, 0.061 in kerf)
N0100 M06 T10 F42.0 (Plasma, 0.061 in kerf)
N0110 G00 Z0.5000
N0120 X33.7449 Y8.5439
N0130 Z0.2500
N0140 G90F100
N0150 G31 Z-3 F20 G92 Z0
N0160 G0 z0.16
N0170 Z0.2500
N0180 M03
N0190 G04 P3
N0200 G01 Z0.1100 F60.0

ALSO, Using my new post processor, My pierce height and cut height's are very high, approx. .75" vs the .25" pierce and .11" cut (Set points). I did notice the head goes below 0 on the z axis when it is probing (Just under -.5" So when it comes up to cut, it is well over the set height, I assume this is why it is 3/4" over my material)

I feel like these are 2 fairly Small issues compared to what I started with (At least I would like to believe that for now, humor me)

[acourtjester]

Do you have your Z move attacked to the limit switch pin? I have all my home and limit switches using the same pin. The command G28.1 Z.5 is telling mach to check for Z home. If the switches are not hooked to Z home pin it will not work.
Now I am no expert on G-code but on line 150 it has Z twice remove the Z0 after the G92 Also line 170 is not needed the line before tells mach to go to Z 0.16" Good pierce height and line 200 should be G01 Z0.060 f60. Z0.110 is to high for cutting

[Ribbedgiraffe]

Do you have your Z move attacked to the limit switch pin? I have all my home and limit switches using the same pin.

This brings yet another question.. The limit Switch is connected to Slot 2 on the Gecko 540 (How this interfaces with Mach 3, I'm not sure yet). This is literally the only limit or home switch on the table. I have all the switches I need to install them, but I'm trying to make it run before I start changing things.

[Ribbedgiraffe]

Ok - I feel like I've got it (Fixed my height issues) Didn't change any wiring at this point.
But I'm wondering if I should start a new thread in sheet cam. I manually changed some of the code from the last post processor mod and was able to get the best cuts I've personally seen come off of this machine (And there were 0 tip issues after)

Here is my current code in my post processor.
function OnPenDown()
if (preheat > 0.001) then
post.ModalText (" G00")
post.ModalNumber (" Z", cutHeight * scale, "0.0000")
post.Text ("\n G04 P")
post.Number (preheat,"0.###")
post.Eol()
end
post.ModalText (" G00")
post.ModalText ("\n G90F100\n")
post.ModalText (" G31 Z-3 F20")
post.ModalText (" G92 Z0\n")
post.ModalText (" G0 z0.16\n") (Is this the offset for my limit/home switch for my floating head?)
post.Text (" Z")
post.Number (pierceHeight * scale, "0.0000")
post.Text ("\n M03\n")
if (pierceDelay > 0.001) then
post.Text (" G04 P")
post.Number (pierceDelay,"0.###")
post.Eol()
end
end

This is the G code that was created using the above post processor.

N0010 (Filename: Direct from PP Testsquare.tap)
N0020 (Post processor: Mach3 plasma scott h.scpost)
N0030 (Date: 19/06/2016)
N0040 G20 (Units: Inches)
N0050 G53 G90 G91.1 G40
N0060 F1
N0070 S500
N0080 (Part: Testsquare)
N0090 (Operation: Outside Offset, 0, T10: Plasma, 0.061 in kerf)
N0100 M06 T10 F42.0 (Plasma, 0.061 in kerf)
N0110 G00 Z0.5000
N0120 X5.1600 Y5.1905
N0130 G90F100
N0140 G31 Z-3 F20 G92 Z0 < I had to split this into two lines, see below.
N0150 G0 z0.16
N0160 Z0.0990
N0170 M03
N0180 G04 P2
N0190 G01 Z0.1100 F42.0
N0200 G02 X5.0000 Y5.0305 I-0.1600 J0.0000
(Removed Additional lines of code)


this is the G code that I modified to work. I modified the Cut and pierce height's manually so I could measure them on the machine, I will change them in sheetcam on the next run.

N0010 (Filename: Testsquare.tap)
N0020 (Post processor: Mach3 plasma scott h.scpost)
N0030 (Date: 19/06/2016)
N0040 G20 (Units: Inches)
N0050 G53 G90 G91.1 G40
N0060 F1
N0070 S500
N0080 (Part: Testsquare)
N0090 (Operation: Outside Offset, 0, T10: Plasma, 0.061 in kerf)
N0100 M06 T10 F42.0 (Plasma, 0.061 in kerf)
N0110 G00 Z0.5000
N0120 X5.1600 Y5.1905
N0130 G90F100
N0140 G31 Z-3 F20 -> This line was split from the above code as it was both on 1 line ( I don't know how to fix this, thoughts?)
N0145 G92 Z0
N0150 G0 z0.16
N0160 Z0.22 <Simple change in sheetcam
N0170 M03
N0180 G04 P.60 <simple change in sheetcam
N0190 G01 Z0.18 F42.0
N0200 G02 X5.0000 Y5.0305 I-0.1600 J0.0000
(Removed additional lines of code.)

[Ribbedgiraffe]

Now I am no expert on G-code but on line 150 it has Z twice remove the Z0 after the G92 Also line 170 is not needed the line before tells mach to go to Z 0.16" Good pierce height and line 200 should be G01 Z0.060 f60. Z0.110 is to high for cutting

I overlooked this part of your previous comment, It was a long couple days . Ill make the change in the PP and see where it gets me.

[Ribbedgiraffe]

I was missing a very important piece of code in the post processor. Without \n it will not create a new line of code.

function OnPenDown()
if (preheat > 0.001) then
post.ModalText (" G00")
post.ModalNumber (" Z", cutHeight * scale, "0.0000")
post.Text ("\n G04 P")
post.Number (preheat,"0.###")
post.Eol()
end
post.ModalText (" G00")
post.ModalText ("\n G90F100\n")
post.ModalText (" G31 Z-3 F20") < This should read post.ModalText (" G31 Z-3 F20\n")
post.ModalText (" G92 \n")
post.ModalText (" G0 z0.16\n")
post.Text (" Z")
post.Number (pierceHeight * scale, "0.0000")
post.Text ("\n M03\n")
if (pierceDelay > 0.001) then
post.Text (" G04 P")
post.Number (pierceDelay,"0.###")
post.Eol()
end
end


Im going to go play - Lets see what kind of problems I can create now!

[acourtjester]

Just think of all you have learned Problems are a pain but they help you understand thing better and you are very happy after.
I just posted a video in tips that will help you with floating head switch offset values.

[Ribbedgiraffe]

Just think of all you have learned Problems are a pain but they help you understand thing better and you are very happy after.
I just posted a video in tips that will help you with floating head switch offset values.

You are right, I've learned so much every time I've had an issue. I bought this table as a "running" unit (Minus plasma cutter), with a very basic crash course on how to cut with it. I was literally taught how to move a part from cad, to plasma cam and then to Mach 3 and how to change the Macro for pierce height. Not even an instruction on settings etc... after the last 4 days, I feel much better about making sparks with it.

My next adventure is going to be installing a torch height control, and ultimately I plan to use this table to make parts for a much better table.

Ill check out your video shortly!

Thank you for the help!

[tcaudle]

Mp1000 THC post puts in an auto touch off using a switch offset value in the POST (variable is "switchOffset = ##) If you run that WITH the custom M3 code then you will get double touch offs. The M3 macro is doing the same thing as the POST does . The values in the Mcode are static meaning if something changes you will need to edit the macro. A bad touch off will ruin lots of consumables (and you day)
You need to do a series of tests starting with a dry run with the torch (and ususally the THC) turned off and just have it touch off and raise up and measure the pierce height (stop motion or swtich to Single Step mode in MACH and watch one line at a time execute). You can go back to the regualr MACH3 Plasma if you want to keep the macro but the macro has to be right. If you cannot get a valid touch off before every pierce and the torch starts the arc at the wrong height the rest of the cut will go downhill!

Once you have the touch-off working flawlessly (every time) THEN try it with the torch on and you should get a decent cut on flat material. Once you are there THEN add the THC to the mix and leave it off unti.l you have started a cut then turn it on and see if it locks to a height.