After touch off, torch goes to cut height not pierce height

[Turboram]

My system- home made 4x4 table, TD cutmaster 102, price avhc10 torch height controller, mach3, sheetcam.
The problem I am having is after my torch does a reference and gets ready to pierce, the machine goes from z-0 to z-.06 I stead of going to my pierce height. Essentially it zeros then goes and cuts right away. On most of my test cuts it seems to still pierce the plate alright at .06 but it blows back on the torch. Also I'm going through consumables rather quickly because of this. Am I supposed to include the pierce height into the number I enter for switch offset for the floating head? In my gcode after the reference I notice it zeros the Z but then the next line is g00 z0 then my cut height is the next line. What am I missing here?

[acourtjester]

You have not stated what programs you are using. In SheetCam you would set the tool up with a pierce height and a cut height and use a post processor that uses the floating head to find the metal surface. then take into account the amount of switch offset (also in the post processor) and zero the Z DRo then move to the pierce height, and fire the torch then drop to cut height. Here is a video on how to fine the switch offset.
https://www.youtube.com/watch?v=6CDml_kosbY
the second image shows the Price Post processor I edited for a Ohmic sensor (g31 floating head would use G28) and the switch offset location. Again mine is for a ohmic sensor yours would be larger, but this is where you put it after you find what it is.

cut.JPG (46.09 KiB) Viewed 889 times

[Turboram]

At the top of my post I mentioned all the equipment I'm using. I went into tools on sheetcam and set my heights just like I have read on all the forums. I am using the mach3 with scriber post because I was having issues with the price avhc10 post but that could have been my voltage issue I figured out. I also figured out the switch offset just as the video shows and entered it all in the post. Made sure the post I edited was the one selected. Loaded a gcode of a test plate zeroed the table where I wanted to cut the hit cycle start. While trying to watch the table and the dros it appears that my torch is not moving to the pierce height. It looks as though the reference zeros the z and it fires the torch and runs at the .06 cut height. Where in the gcode would I find the line for the pierce height. And what would it look like. Sorry for sounding stupid I'm new to this and I try to figure it out on my own but it has me stumped

[djreiswig]

This is not where you set the switch offset.

PS1.png (181.11 KiB) Viewed 882 times

What you changed to 0.002 is actually the format that the value is output as, not the value itself. There should be a place at the top of the post where the variable is assigned. Remember, values inside the post need to be in mm no matter what units you are using in SheetCam.
Also, 0.002 is a pretty small offset, unless you are using a proximity sensor.

[acourtjester]

Ok here is the top of the post
You may be correct, but that location has worked for me a long time.
On your comment on you must always use MM in the post processor then why is there the commands g20 and g21, it seems like SheetCam looks at the spects entered at time of setup where you signify MM or Inch for generating the G-code.
This Grasshopper would like to learn

switch offset3.JPG (33.15 KiB) Viewed 862 times

[acourtjester]

turboRam
you may try using the single step mode when running your G-code then you see each action in separate motions.
just click on Single then click on cycle start for each line of G-code to be executed. See what happened and them step to the next line (sometimes you need to click on cycle start more then one time to see things happen, not all line cause a movement).

step.JPG (44.65 KiB) Viewed 860 times

[Turboram]

Ok so I got some time to play with it after work today and I was able to figure a few things out. So my 50:1 divider I installed in my TD cutmaster 102 was not sending the right voltages to my price after playing with wire position on the connector for the price and checking the jumper inside the machine making sure it was on 50:1 it still didn't work. I ran raw arc voltage out the back and now the price is reading accurately based on the cut chart I received with the TD. So I loaded the price post processor and inter the switch offset just as I was instructed at the top. My switch offset comes out to .280 inches. I converted it to mm and that didn't run right it tried sending the z to 7 inches which is the .28 in mm. So I changed it in the post to .28 again and then the machine referenced properly.
I am beginning to understand the gcode a little more at a time. When I scroll through it after posting it to mach I noticed after it zeros the z the second time it stays at zero, then calls for the m3 command to fire torch. It's like it's ignoring the pierce height. I have entered the pierce height on the post where it says pierce height*scale =o.ooo. ( no idea if that is right or not) also entered the delay just below that where it says pierce delay. In sheetcam I entered both of those in the tool set up and operation setup.
When it pierces it's doing it right on the plate then moves up higher then the .06. to achieve the .06 I have to turn the voltage setting on the price down to 89 when the cut chart calls for 114. When I do this it maintains the .06 cut height and leaves pretty square edges but leaves a really jagged cut. If I leave it at the 114 I get I smooth cut but alot of edge angularity. Not sure where to go from here. Sorry about the super long post but this is everything I noted down tonight and what happened

[acourtjester]

If you look at the G-code the pierce height should be the line before the M3, don't worry about long posts as you give the info needed. Remember you are someone else eyes when working on a problem. I only enter the pierce and cut heights in the tool setting in SheetCam and not in the post processor. Now another thing the Price THC only comes into play after a short delay after you move to cut height, this is so the arc is stable.
I don't know if this video will help but here it is.
https://youtu.be/EyZJVMtzKzY

[djreiswig]

Ok here is the top of the post
You may be correct, but that location has worked for me a long time.
On your comment on you must always use MM in the post processor then why is there the commands g20 and g21, it seems like SheetCam looks at the spects entered at time of setup where you signify MM or Inch for generating the G-code.
This Grasshopper would like to learn
switch offset.JPG
switch offset3.JPG

I misread the line in the post. It doesn't have * scale in it like most numerical outputs, so that line isn't doing any calculating just outputting the value, but I still think since switchOffset is a variable the 0.002 is being used as a format. I'm not really sure how that works as you usually just use 0's and #'s for that.
SheetCam works in mm since Les is a Brit . The G20 & G21 are commands output for the machine controller. They don't affect how SheetCam works.
If you set inches in the settings then the variable scale is used to convert the output to inches. That's why a lot of the lines have a variable * scale.

[Turboram]

If you look at the G-code the pierce height should be the line before the M3, don't worry about long posts as you give the info needed. Remember you are someone else eyes when working on a problem. I only enter the pierce and cut heights in the tool setting in SheetCam and not in the post processor. Now another thing the Price THC only comes into play after a short delay after you move to cut height, this is so the arc is stable.
I don't know if this video will help but here it is.
https://youtu.be/EyZJVMtzKzY

This is the beginning of my gcode for the test piece I have been trying to dial in
G31 z -100 F15.85
G92 z0.0
G00 z 0.28 (switch offset)
G92 z0.0
G00 x 5.030 y2.7963 z 0
M03
G01 z 0.06 F 3.397
I thought that is what that line meant but was 100% sure so with the cut height and the pierce height entered in sheetcam why does the code put a zero for z instead of the . 19 pierce height that I enter in sheetcam?

[acourtjester]

This is the place that your pierce height should be it shows Z0 that is why Mach does what it does on you table, (just following orders).
here is a line from my G-code. you can see the Z is told to go to .150" could there be an error in your tool that you use, see above for my tool setting.
N3990 G00 X19.7048 Y6.9054 Z0.1500

[acourtjester]

Ok I emailed Les about a question I had which was along with the line in the G-code for Pierce height and he told me how to got around my question. But in doing so I think I can now say there may be a line missing from your post processor see attached image and the line is
post.ModalNumber (" Z", pierceHeight * scale, "0.0000") If you edit the post processor you can copy and paste this line in as shown then save with a different name like adding the date to its name. then use the edited post to make a G-code and see if the Z0 is now the amount in your tool setup.

line.JPG (51.82 KiB) Viewed 801 times

[Turboram]

Ok I emailed Les about a question I had which was along with the line in the G-code for Pierce height and he told me how to got around my question. But in doing so I think I can now say there may be a line missing from your post processor see attached image and the line is
post.ModalNumber (" Z", pierceHeight * scale, "0.0000") If you edit the post processor you can copy and paste this line in as shown then save with a different name like adding the date to its name. then use the edited post to make a G-code and see if the Z0 is now the amount in your tool setup.
line.JPG
line2.JPG

Yes I do have that line in my post processor. That is where I entered the pierce height is it supposed to be left as 0.000 after the word scale?

[acourtjester]

that is what is in the post processor I use, the pierce height should be in the tool setup in sheetcam itself.
very easy to check, make the change by editing the post processor and rename it with maybe a A after the original name. The create 2 G-code one with the old processor and one with the new and look at them both. That is what I show in the last image

[Turboram]

Ok by leaving the zeros alone on that line my code now populates the .19 pierce height where it's supposed to be before the m3 command. While cutting .25 HR mild steel I have to lower my volts from the suggested 114 to 88 to achieve a .06 cut height. This cause I very choppy cut at 80 amps and 40 ipm with I shielded tip. Does that sound normal? Or do you think the pierce height issue I was having with the torch piercing at z0 and then moving up to the .06 would cause the wackiness that was going on? Also what is your thc delay set to on your price controller before thc takes over?

[djreiswig]

You should be able to cut .25 with lower amp consumables than 80 amp. I have a Hypertherm 65 and I think I have cut .25 with 45 amp consumables. I don't have the chart handy, but if not 45 amps, then I think it would be on the low end of the 65 amp ones. Dropping your amps, using smaller consumables, and slowing down might help your cut quality. Also see if your thc is oscillating a lot.

[Turboram]

Well thanks for all the help guys. You have poi Ted me in the right direction, and I now have the table functioning properly in terms of cut and pierce heights. I know just need to spend time with different material thicknesses and get them saved and dialed in